• Share
  • Email
  • Embed
  • Like
  • Save
  • Private Content
Solid Cam 2009 Milling User Guide
 

Solid Cam 2009 Milling User Guide

on

  • 8,004 views

 

Statistics

Views

Total Views
8,004
Views on SlideShare
8,004
Embed Views
0

Actions

Likes
2
Downloads
160
Comments
2

0 Embeds 0

No embeds

Accessibility

Categories

Upload Details

Uploaded via as Adobe PDF

Usage Rights

© All Rights Reserved

Report content

Flagged as inappropriate Flag as inappropriate
Flag as inappropriate

Select your reason for flagging this presentation as inappropriate.

Cancel

12 of 2 previous next

  • Full Name Full Name Comment goes here.
    Are you sure you want to
    Your message goes here
    Processing…
  • useful thanks
    Are you sure you want to
    Your message goes here
    Processing…
  • nice
    Are you sure you want to
    Your message goes here
    Processing…
Post Comment
Edit your comment

    Solid Cam 2009 Milling User Guide Solid Cam 2009 Milling User Guide Document Transcript

    • SolidCAM 2009 The Leaders in Integrated CAMPower and Ease of Use - the winning combination SolidCAM 2009 Milling User Guide ©1995-2009 SolidCAMWW W. S O L I D C A M . C O M All Rights Reserved.
    • SolidCAM 2009Milling User Guide ©1995-2009 SolidCAM All Rights Reserved.
    • ContentsContents1. SolidCAM Basics1.1 Installing the SolidCAM Software .................................................................................................... 24 1.1.1 System requirements................................................................................................................. 24 1.1.2 Supported CAD systems ......................................................................................................... 24 1.1.3 SolidCAM Single License installation .................................................................................... 25 1.1.4 SolidCAM Network License Installation .............................................................................. 291.2 Basic Concepts ..................................................................................................................................... 311.3 Starting SolidCAM............................................................................................................................... 311.4 SolidCAM Interface ............................................................................................................................ 32 1.4.1 SolidCAM Manager .................................................................................................................. 32 1.4.2 Coordinate System .................................................................................................................... 351.5 Getting Help ......................................................................................................................................... 362. CAM-Part2.1 Starting a new Milling CAM-Part ...................................................................................................... 38 2.1.1 New Milling Part dialog box.................................................................................................... 39 2.1.2 The structure of the CAM-Part.............................................................................................. 40 2.1.3 Milling Part Data dialog box ................................................................................................... 402.2 Coordinate System............................................................................................................................... 41 2.2.1 Defining the Coordinate System (CoordSys)........................................................................ 41 2.2.2 CoordSys dialog box ................................................................................................................. 42 2.2.3 Defining the Coordinate Systems for 3-axis CNC-machine .............................................. 48 2.2.4 Defining the Coordinate Systems for 4-axis CNC-machine .............................................. 49 2.2.5 Defining the Coordinate Systems for 5-axis CNC-machine .............................................. 50 2.2.6 Coordinate System definition methods ................................................................................. 51 2.2.7 CoordSys Data dialog box ....................................................................................................... 525
    • 2.2.8 SolidCAM Coordinate System ................................................................................................ 542.3 CoordSys Manager .............................................................................................................................. 552.4 Stock and Target Model...................................................................................................................... 57 2.4.1 Stock model ............................................................................................................................... 58 2.4.2 Target model .............................................................................................................................. 60 2.4.3 Common controls for Stock model and Target model dialog boxes ................................ 60 2.4.4 Associativity of Stock and Target models............................................................................. 612.5 Tool Options ........................................................................................................................................ 632.6 Mac Options ......................................................................................................................................... 652.7 Work Material ....................................................................................................................................... 652.8 CNC-Controller and Axis Type......................................................................................................... 66 2.8.1 Axis type ..................................................................................................................................... 662.9 Default GCode numbers .................................................................................................................... 682.10 Part Settings ........................................................................................................................................ 70 2.10.1 Units .......................................................................................................................................... 70 2.10.2 Interoperational tool movements ......................................................................................... 71 2.10.3 Update Stock calculation ....................................................................................................... 72 2.10.4 Synchronization....................................................................................................................... 75 2.10.5 Automatic CAM-Part definition ........................................................................................... 76 2.10.6 Machining Process .................................................................................................................. 78 2.10.7 Tool path simulation............................................................................................................... 79 2.10.8 GCode generation................................................................................................................... 80 2.10.9 Template defaults .................................................................................................................... 84 2.10.10 Tool coolant ........................................................................................................................... 86 2.10.11 Gouge check .......................................................................................................................... 862.11 Compressed CAM-Part .................................................................................................................... 87 2.11.1 Compressed CAM-Part file format ...................................................................................... 87 2.11.2 Creating a new compressed CAM-Part ............................................................................... 87 2.11.3 Converting CAM-Parts to Compressed mode ................................................................... 88 2.11.4 Opening/Closing Compressed CAM-Parts........................................................................ 88 6
    • Contents2.12 Managing CAM-Parts ....................................................................................................................... 902.13 CAM-Part Documentation .............................................................................................................. 97 2.13.1 Documentation Editor ........................................................................................................... 972.14 Tool sheet documentation................................................................................................................ 99 2.14.1 Capturing the CAM-Part image ............................................................................................ 99 2.14.2 Definition of tool sheet parameters .................................................................................. 100 2.14.3 The output file ....................................................................................................................... 103 2.14.4 Show Last Tool Sheet ........................................................................................................... 1072.15 Milling STL CAM-Part ................................................................................................................... 108 2.15.1 Starting a new Milling-STL CAM-Part .............................................................................. 108 2.15.2 Coordinate System definition.............................................................................................. 110 2.15.3 Stock model definition ......................................................................................................... 111 2.15.4 Target model definition........................................................................................................ 1112.16 Support of DriveWorks.................................................................................................................. 1123. Tools3.1 User-Defined Tool Types ................................................................................................................. 116 3.1.1 End mill .................................................................................................................................... 117 3.1.2 Ball nose mill............................................................................................................................ 118 3.1.3 Bull nose mill ........................................................................................................................... 119 3.1.4 Dove tail mill ........................................................................................................................... 120 3.1.5 Face mill.................................................................................................................................... 121 3.1.6 Slot mill ..................................................................................................................................... 122 3.1.7 Taper mill ................................................................................................................................. 123 3.1.8 Engraving tool ......................................................................................................................... 125 3.1.9 Tap tool..................................................................................................................................... 126 3.1.10 Lollipop mill .......................................................................................................................... 127 3.1.11 Thread mill ............................................................................................................................. 129 3.1.12 Thread taper .......................................................................................................................... 131 3.1.13 Drill ......................................................................................................................................... 1317
    • 3.1.14 Center drill ............................................................................................................................. 132 3.1.15 Spot drill ................................................................................................................................. 134 3.1.16 Chamfer drill .......................................................................................................................... 135 3.1.17 Reamer .................................................................................................................................... 136 3.1.18 Bore ......................................................................................................................................... 137 3.1.19 Shaped Tools ......................................................................................................................... 138 3.1.20 Add new tool types ............................................................................................................... 138 3.1.21 Tool type options .................................................................................................................. 1393.2 Tool Libraries ..................................................................................................................................... 1403.3 Working with the Part Tool Table ................................................................................................... 1413.4 Working with the Current Tool Library ......................................................................................... 1423.5 Managing Tool Libraries ................................................................................................................... 143 3.5.1 Edit Tool Library .................................................................................................................... 143 3.5.2 Create Tool Library................................................................................................................. 143 3.5.3 Copy Tool Library................................................................................................................... 144 3.5.4 Delete Tool Library ................................................................................................................ 1453.6 Tool Table dialog box ....................................................................................................................... 146 3.6.1 Tools Filter ............................................................................................................................... 146 3.6.2 Tool range ................................................................................................................................ 147 3.6.3 Show.......................................................................................................................................... 148 3.6.4 View .......................................................................................................................................... 149 3.6.5 Edit ............................................................................................................................................ 1493.7 Managing tools ................................................................................................................................... 1523.8 Tool data ............................................................................................................................................. 156 3.8.1 Tool Topology page ................................................................................................................ 157 3.8.2 Default Tool Data page .......................................................................................................... 161 3.8.3 Tool Message page .................................................................................................................. 164 3.8.4 Holder page.............................................................................................................................. 165 3.8.5 Tool Coolant page................................................................................................................... 166 3.8.6 Shape page................................................................................................................................ 167 8
    • Contents3.9 Tool Holding system ......................................................................................................................... 169 3.9.1 Tool Holders dialog box ........................................................................................................ 169 3.9.2 Tool Holder Geometry definition ........................................................................................ 173 3.9.3 Tool Holder segments ............................................................................................................ 173 3.9.4 Using Tool Holders ................................................................................................................ 1753.10 Shaped Tools .................................................................................................................................... 177 3.10.1 Shaped Tools dialog box ...................................................................................................... 177 3.10.2 Shaped tool geometry definition ........................................................................................ 180 3.10.3 Shaped Tool segments.......................................................................................................... 180 3.10.4 Using Shaped tools ............................................................................................................... 1823.11 Feed and Speed defaults ................................................................................................................. 1844. Geometry4.1 Introduction ....................................................................................................................................... 1884.2 Drilling geometry............................................................................................................................... 189 4.2.1 Defining a Drilling geometry ................................................................................................ 189 4.2.2 Editing a Drilling geometry ................................................................................................... 190 4.2.3 Drill Geometry Selection dialog box ................................................................................... 190 4.2.4 Around 4th Axis Drill Geometry Selection dialog box .................................................... 1944.3 3D Model geometry .......................................................................................................................... 197 4.3.1 Defining a 3D Model geometry............................................................................................ 197 4.3.2 Editing a 3D Model geometry .............................................................................................. 1984.4 Wireframe geometry ......................................................................................................................... 199 4.4.1 Defining the Profile/Pocket geometry ................................................................................ 199 4.4.2 Defining the Working Area ................................................................................................... 200 4.4.3 Defining the Slot geometry ................................................................................................... 200 4.4.4 Defining the Section geometry ............................................................................................. 201 4.4.5 Defining the Limit geometry................................................................................................. 2024.5 Editing chain geometries .................................................................................................................. 2039
    • 4.5.1 Geometry Name ..................................................................................................................... 203 4.5.2 Configurations ......................................................................................................................... 203 4.5.3 Adding a Chain ........................................................................................................................ 203 4.5.4 Managing chains ...................................................................................................................... 204 4.5.5 Chain direction ........................................................................................................................ 205 4.5.6 Selecting single entities ........................................................................................................... 205 4.5.7 Automatic selection ................................................................................................................ 209 4.5.8 Chain buttons .......................................................................................................................... 211 4.5.9 Options ..................................................................................................................................... 212 4.5.10 Gap control ............................................................................................................................ 212 4.5.11 Add Multi-Chain ................................................................................................................... 213 4.5.12 Mark Open Edges dialog box ............................................................................................. 2134.6 Chains Selection dialog box ............................................................................................................. 215 4.6.1 Chains Direction dialog box .................................................................................................. 217 4.6.2 Chain sorting ........................................................................................................................... 2184.7 Managing geometries ........................................................................................................................ 220 4.7.1 Synchronization of the Wireframe geometry ..................................................................... 221 4.7.2 Synchronization of the 3D Model geometry ..................................................................... 224 4.7.3 Boolean operations ................................................................................................................. 2265. Operations5.1 Adding an operation.......................................................................................................................... 2305.2 SolidCAM Operation Interface ....................................................................................................... 231 5.2.1 Operation name ...................................................................................................................... 233 5.2.2 Template ................................................................................................................................... 235 5.2.3 Info ............................................................................................................................................ 245 5.2.4 Operation buttons................................................................................................................... 245 5.2.5 Calculator ................................................................................................................................. 247 5.2.6 Geometry page ........................................................................................................................ 250 5.2.7 Tool page .................................................................................................................................. 252 5.2.8 Levels page ............................................................................................................................... 257 10
    • Contents 5.2.9 Technology page ..................................................................................................................... 264 5.2.10 Advanced Technology page ................................................................................................ 264 5.2.11 Link page ................................................................................................................................ 272 5.2.12 Miscellaneous parameters page........................................................................................... 2725.3 Working with operations .................................................................................................................. 275 5.3.1 Add Operation ........................................................................................................................ 275 5.3.2 Add Operation from Template ............................................................................................. 276 5.3.3 Add Operations from Process Template ............................................................................ 276 5.3.4 Add Machining Process ......................................................................................................... 277 5.3.5 Create Template ...................................................................................................................... 277 5.3.6 Edit ............................................................................................................................................ 277 5.3.7 Calculate/Calculate All........................................................................................................... 277 5.3.8 GCode/GCode All ................................................................................................................. 277 5.3.9 Calculate & GCode All .......................................................................................................... 278 5.3.10 Tool Sheet .............................................................................................................................. 278 5.3.11 Simulate .................................................................................................................................. 278 5.3.12 File ........................................................................................................................................... 278 5.3.13 Operation Group .................................................................................................................. 278 5.3.14 Cut/Copy/Paste.................................................................................................................... 279 5.3.15 Rename ................................................................................................................................... 279 5.3.16 Change tool ............................................................................................................................ 280 5.3.17 Change tool data ................................................................................................................... 280 5.3.18 Info.......................................................................................................................................... 281 5.3.19 Delete/Delete All ................................................................................................................. 281 5.3.20 Suppress/Unsuppress .......................................................................................................... 2815.4 Managing Operations in the SolidCAM Manager tree ................................................................ 284 5.4.1 Operation Sequence ............................................................................................................... 284 5.4.2 Undo Sequence........................................................................................................................ 284 5.4.3 Split............................................................................................................................................ 284 5.4.4 Expand tree .............................................................................................................................. 286 5.4.5 Collapse tree............................................................................................................................. 28611
    • 5.4.6 Show/Hide Tools in tree ....................................................................................................... 286 5.4.7 Show/Hide CoordSys in tree ................................................................................................ 287 5.4.8 Automatic Sort ........................................................................................................................ 2885.5 Operation Transformations ............................................................................................................. 290 5.5.1 Operation transformations .................................................................................................... 291 5.5.2 Options ..................................................................................................................................... 292 5.5.3 Transformations table ............................................................................................................ 292 5.5.4 Transformation buttons ......................................................................................................... 2935.6 Fixture ................................................................................................................................................. 298 5.6.1 Fixture dialog box ................................................................................................................... 2996. 2.5D Milling6.1 Profile Operation ............................................................................................................................... 302 6.1.1 Levels page ............................................................................................................................... 303 6.1.2 Technology page ..................................................................................................................... 303 6.1.3 Link page .................................................................................................................................. 3266.2 Face Milling Operation ..................................................................................................................... 335 6.2.1 Geometry page ........................................................................................................................ 335 6.2.2 Technology page ..................................................................................................................... 338 6.2.3 Link page .................................................................................................................................. 3496.3 Contour 3D Operation ..................................................................................................................... 351 6.3.1 Technology page ..................................................................................................................... 351 6.3.2 Link page .................................................................................................................................. 3556.4 Pocket Operation ............................................................................................................................... 357 6.4.1 Geometry page ........................................................................................................................ 358 6.4.2 Levels page ............................................................................................................................... 359 6.4.3 Technology page ..................................................................................................................... 360 6.4.4 Link page .................................................................................................................................. 3816.5 Pocket Recognition Operation ........................................................................................................ 397 6.5.1 Geometry page ........................................................................................................................ 397 12
    • Contents 6.5.2 Levels page ............................................................................................................................... 403 6.5.3 Technology page ..................................................................................................................... 404 6.5.4 Link page .................................................................................................................................. 4086.6 Drilling Operation ............................................................................................................................. 409 6.6.1 Tool page .................................................................................................................................. 409 6.6.2 Levels page ............................................................................................................................... 411 6.6.3 Technology page ..................................................................................................................... 4126.7 Drill Recognition Operation ............................................................................................................ 437 6.7.1 Geometry page ........................................................................................................................ 437 6.7.2 Levels page ............................................................................................................................... 442 6.7.3 Technology page ..................................................................................................................... 4466.8 Thread Milling Operation ................................................................................................................ 447 6.8.1 Tool page .................................................................................................................................. 447 6.8.2 Levels page ............................................................................................................................... 448 6.8.3 Technology page ..................................................................................................................... 449 6.8.4 Link page .................................................................................................................................. 4526.9 Slot Operation .................................................................................................................................... 453 6.9.1 Technology page ..................................................................................................................... 454 6.9.2 Pre-drilling geometry generation .......................................................................................... 4616.10 T-Slot Operation.............................................................................................................................. 463 6.10.1 Tool page ................................................................................................................................ 464 6.10.2 Technology page ................................................................................................................... 465 6.10.3 Link page ................................................................................................................................ 4706.11 Translated Surface Operation ........................................................................................................ 471 6.11.1 Technology page ................................................................................................................... 471 6.11.2 Link page ................................................................................................................................ 4827. 3D Milling7.1 3D Milling Operation........................................................................................................................ 484 7.1.1 Geometry page ........................................................................................................................ 48413
    • 7.1.2 Technology page ..................................................................................................................... 497 7.1.3 Roughing .................................................................................................................................. 498 7.1.4 Hatch roughing........................................................................................................................ 513 7.1.5 Contour roughing ................................................................................................................... 513 7.1.6 Plunging pattern ...................................................................................................................... 513 7.1.7 Semi-Finish/Finish ................................................................................................................. 514 7.1.8 Semi-Finish/Finish strategies................................................................................................ 520 7.1.9 Linear Finish strategy ............................................................................................................. 520 7.1.10 Offset Cutting Finish strategy............................................................................................. 524 7.1.11 Spiral finish strategy ............................................................................................................. 527 7.1.12 Circular Pocket finish strategy ............................................................................................ 531 7.1.13 Constant Z Finish Strategy.................................................................................................. 533 7.1.14 Constant Step over strategy................................................................................................. 540 7.1.15 Pencil milling ......................................................................................................................... 545 7.1.16 Tolerance page ....................................................................................................................... 5497.2 3D Engraving Operation.................................................................................................................. 551 7.2.1 Technology page ..................................................................................................................... 551 7.2.2 Tolerance page ......................................................................................................................... 5547.3 3D Drilling Operation ...................................................................................................................... 555 7.3.1 Geometry page ........................................................................................................................ 555 7.3.2 Tool page .................................................................................................................................. 556 7.3.3 Levels page ............................................................................................................................... 557 7.3.4 Technology page ..................................................................................................................... 5578. Machining Processes8.1 Introduction & Basic concepts ........................................................................................................ 560 8.1.1 Operation templates ............................................................................................................... 560 8.1.2 Parameters & Expressions ..................................................................................................... 561 8.1.3 Default sets .............................................................................................................................. 562 8.1.4 Machining Process Table ....................................................................................................... 5628.2 Creating Machining Processes ......................................................................................................... 563 14
    • Contents8.3 Defining Machining Process Table ................................................................................................. 564 8.3.1 Adding MAC file(s) ................................................................................................................. 5648.4 Machining Process Table Manager ................................................................................................. 566 8.4.1 Managing Machining Process Tables ................................................................................... 567 8.4.2 Machining Process Group Types.......................................................................................... 5698.5 Managing Machining Processes ....................................................................................................... 5718.6 Machining Process Define Manager ............................................................................................... 572 8.6.1 Operation Templates page..................................................................................................... 572 8.6.2 Define Operation Template .................................................................................................. 572 8.6.3 Managing Operation Templates............................................................................................ 573 8.6.4 Parametric field menu............................................................................................................. 575 8.6.5 Default Sets page..................................................................................................................... 576 8.6.6 Parameters & Expressions Tables ........................................................................................ 577 8.6.7 Add new parameter ................................................................................................................ 579 8.6.8 Variables and expressions ...................................................................................................... 579 8.6.9 Parametric tool definition ...................................................................................................... 5848.7 Using the Machining Processes ....................................................................................................... 5868.8 Inserting the Machining Process ..................................................................................................... 587 8.8.1 Choosing the tool.................................................................................................................... 5898.9 Machining Process Insert Manager................................................................................................. 590 8.9.1 Operation Templates Page..................................................................................................... 590 8.9.2 Default Sets Page .................................................................................................................... 591 8.9.3 Parameters Table ..................................................................................................................... 592 8.9.4 Operation Points ..................................................................................................................... 592 8.9.5 Parameters definition .............................................................................................................. 5929. Automatic Feature Recognition and Machining (AFRM)9.1 Introduction and Basic Concepts.................................................................................................... 5969.2 Preparation to Holes Recognition................................................................................................... 59815
    • 9.2.1 Definition of Coordinate Systems ....................................................................................... 598 9.2.2 Target model ............................................................................................................................ 5989.3 Start Holes Recognition .................................................................................................................... 5999.4 Holes Recognition User Interface ................................................................................................... 600 9.4.1 Holes Recognition Manager .................................................................................................. 600 9.4.2 Holes Recognition Toolbar.................................................................................................... 6019.5 Hole Feature Model........................................................................................................................... 603 9.5.1 Cylindrical Hole Feature segment......................................................................................... 604 9.5.2 Cone Hole Feature segment .................................................................................................. 604 9.5.3 Chamfer Hole Feature segment ............................................................................................ 605 9.5.4 Planar Hole Feature segment ................................................................................................ 605 9.5.5 Torus Hole Feature segment ................................................................................................. 605 9.5.6 Sphere Hole Feature segment ............................................................................................... 606 9.5.7 Compound Holes processing ................................................................................................ 606 9.5.8 Disconnected Holes processing............................................................................................ 607 9.5.9 Reaming recognition ............................................................................................................... 607 9.5.10 Hole Feature Shapes and Groups....................................................................................... 607 9.5.11 Hole Features page ............................................................................................................... 6089.6 Preparing Hole Features for machining ......................................................................................... 613 9.6.1 Undercut processing ............................................................................................................... 613 9.6.2 Undercut substitution............................................................................................................. 614 9.6.3 Segments Union ...................................................................................................................... 617 9.6.4 Machinable Hole Features ..................................................................................................... 619 9.6.5 Machinable Hole Feature conversion .................................................................................. 625 9.6.6 Machinable Hole Features page ............................................................................................ 6339.7 Feature Sets ......................................................................................................................................... 642 9.7.1 Creating Feature Sets .............................................................................................................. 642 9.7.2 Assigning Hole Features to Feature Sets ............................................................................. 642 9.7.3 Automatic CoordSys Positions definition ........................................................................... 643 9.7.4 Feature Sets page ..................................................................................................................... 645 9.7.5 Compatible/Incompatible Hole features ............................................................................ 645 16
    • Contents 9.7.6 Operating Feature Sets ........................................................................................................... 646 9.7.7 Defining the CoordSys Position origin location for the Feature Set .............................. 6479.8 Technology ......................................................................................................................................... 649 9.8.1 Choosing a Technological Solution ...................................................................................... 649 9.8.2 Choosing the tool.................................................................................................................... 650 9.8.3 Technology Page ..................................................................................................................... 657 9.8.4 Managing Technology ............................................................................................................ 6589.9 Generating Operations ..................................................................................................................... 6619.10 Technology Database ...................................................................................................................... 662 9.10.1 Global and Local Technology databases ........................................................................... 663 9.10.2 Technology Database interface........................................................................................... 664 9.10.3 Configurations page.............................................................................................................. 664 9.10.4 Current Configuration.......................................................................................................... 665 9.10.5 Solutions page ....................................................................................................................... 666 9.10.6 Conditions .............................................................................................................................. 667 9.10.7 Variables ................................................................................................................................. 670 9.10.8 Defining a new Technological Solution............................................................................. 673 9.10.9 Holes Recognition Functions.............................................................................................. 6749.11 Holes Recognition Settings ............................................................................................................ 676 9.11.1 System settings ...................................................................................................................... 676 9.11.2 Part settings............................................................................................................................ 67910. Simulation10.1 Introduction ..................................................................................................................................... 682 10.1.1 Simulation control panel ...................................................................................................... 682 10.1.2 Simulation modes.................................................................................................................. 684 10.1.3 Simulation controls ............................................................................................................... 68410.2 2D simulation mode........................................................................................................................ 685 10.2.1 Simulation toolbar................................................................................................................. 685 10.2.2 Simulation control panel ...................................................................................................... 68517
    • 10.3 VerifyPlus simulation mode ........................................................................................................... 687 10.3.1 Simulation toolbar................................................................................................................. 687 10.3.2 Buttons available in the Setup mode.................................................................................. 688 10.3.3 Buttons available in the Simulation mode ......................................................................... 69010.4 Host CAD simulation mode .......................................................................................................... 69110.5 3D simulation mode........................................................................................................................ 692 10.5.1 Simulation toolbar................................................................................................................. 692 10.5.2 Simulation menu ................................................................................................................... 69310.6 SolidVerify simulation mode .......................................................................................................... 695 10.6.1 Simulation control panel .......................................................................................................695 10.6.2 Simulation toolbar................................................................................................................. 696 10.6.3 Selection mode ...................................................................................................................... 700 10.6.4 Measurement ......................................................................................................................... 701 10.6.5 Updated Stock model ........................................................................................................... 701 10.6.6 Simulation menu ................................................................................................................... 70310.7 SolidVerify for 3D simulation mode ............................................................................................ 710 10.7.1 Simulation control panel .......................................................................................................711 10.7.2 Rendering of the simulation model ................................................................................... 711 10.7.3 Simulation toolbar................................................................................................................. 713 10.7.4 Simulation menu ................................................................................................................... 71310.8 Rest Material simulation mode ...................................................................................................... 71410.9 RapidVerify simulation mode ........................................................................................................ 715 10.9.1 RapidVerify control panel .................................................................................................... 715 10.9.2 Updated Stock Model........................................................................................................... 716 10.9.3 Simulation control panel .......................................................................................................716 10.9.4 Simulation toolbar................................................................................................................. 717 10.9.5 Simulation menu ....................................................................................................................71810.10 Machine Simulation....................................................................................................................... 719 10.10.1 Simulation menu ................................................................................................................. 720 10.10.2 Simulation windows ........................................................................................................... 732 18
    • Contents 10.10.3 Simulation toolbars ............................................................................................................. 741 10.10.4 CNC-machine definition parameters ............................................................................... 743 10.10.5 CNC-machine model definition ....................................................................................... 76012. SolidCAM Settings12.1 Introduction ..................................................................................................................................... 80012.2 User Directories settings ................................................................................................................ 801 12.2.1 User Directory for SolidCAM Parts .................................................................................. 801 12.2.2 User Directory for SolidCAM Tables ................................................................................ 801 12.2.3 Excel file for Threading tables ............................................................................................ 80112.3 Default CNC-controller settings ................................................................................................... 802 12.3.1 Post-processor files directory .............................................................................................. 802 12.3.2 CNC-controllers.................................................................................................................... 80212.4 Units settings .................................................................................................................................... 803 12.4.1 Metric/Inch ........................................................................................................................... 803 12.4.2 Approximation ...................................................................................................................... 803 12.4.3 Chain selection ...................................................................................................................... 804 12.4.4 Fillet size for last cut............................................................................................................. 805 12.4.5 Tool Start and Clearance Levels ......................................................................................... 80512.5 Synchronization settings ................................................................................................................. 806 12.5.1 Synchronization of CAM geometry with design model ................................................. 806 12.5.2 Synchronization tolerance ................................................................................................... 807 12.5.3 Synchronization of design model with original model ................................................... 807 12.5.4 Synchronization when design model configuration changes ......................................... 80712.6 Compressed CAM-Part settings .................................................................................................... 80812.7 Tool Settings ..................................................................................................................................... 810 12.7.1 Update Part Tool Table according to Machine Tool Table ............................................ 810 12.7.2 Print in documentation – Only used tools........................................................................ 810 12.7.3 Show in SolidCAM Manager............................................................................................... 810 12.7.4 Import tools ........................................................................................................................... 81119
    • 12.7.5 Set Tool as Permanent when user changes the tool number ......................................... 81112.8 Color settings ................................................................................................................................... 81212.9 Default Geometry Names .............................................................................................................. 81412.10 Interoperational tool movements ............................................................................................... 81512.11 AutoSave settings .......................................................................................................................... 81612.12 Automatic CAM-Part definition ................................................................................................. 817 12.12.1 Automatic Stock model definition ................................................................................... 817 12.12.2 Automatic Target model definition.................................................................................. 818 12.12.3 Definition of Coordinate System..................................................................................... 81812.13 Tool path simulation settings....................................................................................................... 81912.14 Machine simulation settings ......................................................................................................... 820 12.14.1 Directory for Machine simulation definition.................................................................. 820 12.14.2 Tool path coordinates ........................................................................................................ 820 12.14.3 Background.......................................................................................................................... 820 12.14.4 Enable collision control ..................................................................................................... 822 12.14.5 Solid verification ................................................................................................................. 822 12.14.6 Environment ....................................................................................................................... 82312.15 DNC settings ................................................................................................................................. 82312.16 Editors settings .............................................................................................................................. 82412.17 External program settings ............................................................................................................ 82512.18 Machining Process settings .......................................................................................................... 826 12.18.1 On MP insertion (for milling only) .................................................................................. 826 12.18.2 Operation name in SolidCAM Manager ......................................................................... 826 12.18.3 Update extra parameters on CNC-controller change ................................................... 82612.19 User interface settings................................................................................................................... 82712.20 CoordSys settings .......................................................................................................................... 82812.21 GCode Generation........................................................................................................................ 82912.22 Tool search ..................................................................................................................................... 833 20
    • Contents12.23 Internal Post-processor ................................................................................................................ 83312.24 SolidCAM Manager settings ........................................................................................................ 83412.25 Template defaults .......................................................................................................................... 83512.26 Miscellaneous settings................................................................................................................... 83512.27 Tool coolant ................................................................................................................................... 83612.28 Gouge check................................................................................................................................... 83611. GCode11.1 Generate ............................................................................................................................................ 83911.2 List .....................................................................................................................................................84011.3 Copy ..................................................................................................................................................84011.4 Print ...................................................................................................................................................840Appendix ................................................................................................................................................... 841Index ..........................................................................................................................................................84521
    • 22
    • SolidCAMBasics 1 SolidCAM is a powerful CAM product that has been designed especially for the shop floor. SolidCAM supports the complete range of major manufacturing applications including 2.5D Milling, 3D Milling, Turning, Turning with Driven tools and Wire EDM, in one integrated solution. Machining operations can be defined on 2D Design Drawings as well as on 3D Solid and Surface Models. SolidCAM also has a powerful general post-processor tool that enables the easy customization of the GCode file output to various types of CNC-controllers. This chapter discusses some basic concepts and terminology used throughout SolidCAM.  Installing SolidCAM  Starting SolidCAM  SolidCAM Basic Concepts  SolidCAM Interface  Getting Help
    • 1.1 Installing the SolidCAM Software1.1.1 System requirements Supported Operating Systems Microsoft® Windows Vista x32/x64 Business and Ultimate editions with Service Pack 1, Microsoft® Windows XP Professional with Service Pack 2 or 3, Microsoft® Windows XP Professional x64 Edition; CPU Intel® Pentium™, Intel® Xeon™, Intel® Core™, Intel® Core™2 Duo, Intel® Core™2 Quad, AMD® Athlon™, AMD Athlon™ X2 Dual-Core - class processor (emphasized processors are recommended); RAM 2 GB RAM or more (4 GB or more for x64 operating system is recommended for large CAM-Parts machining); Video A OpenGL workstation graphics card (512 MB RAM recommended) and latest driver; Other • Mouse or other pointing device; • CD drive; • Internet Explorer version 6 if you are using the SolidCAM Online Help; • For viewing the What’s New manual, Adobe Acrobat version 9 or higher is recommended.1.1.2 Supported CAD systemsThe following CAD systems are supported by SolidCAM 2009: • SolidWorks® 2006, 2007, 2008, 2009; SolidWorks® 64-bit version is supported. 24
    • 1. SolidCAM Basics • Autodesk® Inventor™ 2008, 2009; • Bentley Microstation/J Modeler; • Autodesk® Mechanical Desktop 2005; • Autodesk® AutoCAD® 2005.1.1.3 SolidCAM Single License installation 1. Insert the SolidCAM Installation CD into the computer CD drive; the installation starts automatically. You can also start the installation by running the Setup.exe file. This file is located in the SolidCAMXXXX/Disk1 folder on the SolidCAM Installation CD (XXXX stands for the current version of SolidCAM). 2. The Choose Setup Language dialog box is displayed. Choose English. When you have to install a localized version of SolidCAM, choose the appropriate language from the combo box. The installation procedure is continued. 3. The following message is displayed. Close all running applications and confirm the message with the OK button.25
    • 4. The Installing SolidCAM dialog box is displayed. Click on the Next button.5. The Choose Destination Location dialog box is displayed. This dialog box enables you to choose the destination folder for SolidCAM. You have to either confirm the default destination folder (C:Program Files SolidCAMXXXX) with the Next button or choose other destination folder with the Browse button and confirm it with the Next button.6. The Select Components dialog box is displayed. Choose the necessary SolidCAM components and confirm your choice with the Next button. 26
    • 1. SolidCAM Basics Make a note that Program Files component cannot be cleared. 7. The Select Program Folder dialog box is displayed. Confirm the default Program Folder name SolidCAMXXXX with the Next button. SolidCAM installation is continued. 8. When the installation is finished, the Choose Language dialog box is displayed. Choose English and click on the OK button. When you install a localized version of SolidCAM, choose the ap- propriate language from the combo box. 9. SolidCAM installs drivers for the hardware key. When the drivers are installed, the following message is displayed. Click on the OK button.27
    • 10. The Connection to CAD system dialog box is displayed. This dialog box displays all CAD systems that can be used by SolidCAM. Choose the appropriate Host CAD systems for SolidCAM. When SolidCAM has found only one CAD system available for connection, this dialog box is not displayed. Click on the Next button. SolidCAM is connected to the defined CAD systems. The following message is displayed. Click on the OK button.11. The following dialog box is displayed. Click on the Finish button. The installation is finished. 28
    • 1. SolidCAM Basics1.1.4 SolidCAM Network License InstallationSolidCAM enables you to install several SolidCAM copies through your network and use networklicensing to manage them. In this case, the SolidCAM Network hardware key has to be connectedto the server. The License Manager has to be installed on the network server computer, whichdistributes SolidCAM Licenses to client computers. When the SolidCAM software runs on a clientcomputer, it obtains the necessary license from the server. SolidCAM Network hardware key SolidCAM License Server SolidCAM Licenses SolidCAM Client ComputersSetting up the SolidCAM License ServerSolidCAM network licensing supports TCP/IP network protocol. 1. SolidCAM Network hardware keys are available in two configurations: for USB port or for LPT port. Connect your SolidCAM Network hardware key to the correct port of your server. 2. Install SolidCAM software on the server as explained in topic 1.1.3. During the installation, the necessary driver for the hardware key is automatically installed. 3. After the SolidCAM installation, the server must be restarted. 4. Install the License Manager software by running Lmsetup.exe application located in the ..SolidCAMXXXXUtil folder. 5. Check the IP address of the server in the network by clicking on the Start button located at the Windows taskbar and then choosing the Command Prompt item from the All Programs/Accessories submenu. The Command Prompt window is displayed.29
    • 6. Type the ipconfig command and confirm it with the Enter key. The IP address of the server will be displayed.Setting SolidCAM licenses on client computers 1. Install SolidCAM on client computer as described in topic 1.1.3. 2. Copy the NethaspTCPIP.ini file located in the ..SolidCAMXXXXUtil folder to the ..SolidCAMXXXXSolidcam folder. 3. Rename the copied file from NethaspTCPIP.ini to Nethasp.ini. 4. Open the renamed Nethasp.ini file in the Notepad editor. The [NH_TCPIP] section in this file contains the following string: NH_SERVER_ADDR = XX.XX.XX.XX; This parameter should define the IP address of the License Server. Type the IP address of the server instead of XX.XX.XX.XX, for example: 72.14.207.99. Save the Nethasp.ini file and close the Notepad application.After the License Manager is installed on the SolidCAM Licensing server and SolidCAM Licensesare configured on each client computer, SolidCAM software can be run. 30
    • 1. SolidCAM Basics1.2 Basic ConceptsEvery manufacturing project in SolidCAM contains the following data: • CAM-Part The CAM-Part defines the general data of the workpiece, including the model name, the Coordinate System, tool options, CNC-controller, etc. • Geometry By selecting Edges, Curves, Surfaces or Solids, define what and where you are going to machine. This geometry is associated with the native SolidWorks model. • Operation An Operation is a single machining step in SolidCAM. Technology, Tool parameters and Strategies are defined in the Operation. In short, Operation means how you want to machine.1.3 Starting SolidCAMTo start SolidCAM, click on the SolidCAM field in the main menu of SolidWorks and chooseMilling from the New submenu.SolidCAM is started.31
    • 1.4 SolidCAM Interface Coordinate System SolidWorks windowCAM ViewstoolbarSolidCAMManagerMachiningSolid model1.4.1 SolidCAM ManagerAfter the CAM-Part is loaded, the SolidCAM Manager is displayed in the left part of the screen.CAM-Part headerTool headerMachining Process headerGeometries headerOperations header } OperationsThe SolidCAM Manager tree is the main interface feature of SolidCAM. It displays completeinformation about the CAM-Part and contains the following headers: • CAM-Part header This header displays the name of the current SolidCAM CAM-Part. By right-clicking on it, you can display the menu to manage your CAM-Parts. The CoordSys Manager, Stock, Target, and Settings subheaders are located under the CAM-Part header. Double-clicking on this header displays the Milling Part Data dialog box. For more information on CAM-Parts, please refer to Chapter 2. 32
    • 1. SolidCAM Basics • Tool header This header displays the name of the current Tool Table. By right-clicking on it, you can activate the menu to manage the Tool Libraries. Double-clicking on this header displays the Part Tool Table. For more information on Tools, please refer to Chapter 3. • Machining Process header This header displays the name of the current Machining Process Table. By right- clicking on it, you can activate the menu to manage the MP Tables. Double-clicking on this header displays the Current Machining Process Table. For more information on Machining Processes, please refer to Chapter 8. • Geometries header This header displays all SolidCAM geometries not used in the operations. You can view the list of these geometries by clicking on the “+” icon near the Geometries header. You can display the geometries managing menu by right-clicking on the Geometries header. You can also open the relevant menu by right-clicking on each geometry name. Double-clicking on a geometry name displays the selected geometry. For more information on Geometries, please refer to Chapter 4. • Operations header This header shows you all the SolidCAM operations defined for the current CAM-Part. The operations managing menu is available by right-clicking on the Operations header. You can also open the relevant menu by right-clicking on each operation name. Double-clicking on an operation name enables you to edit the operation parameters in the operation dialog box. For more information on operations, please refer to Chapter 5.Item search in SolidCAM ManagerThe SolidCAM Manager search system works similarlyto a regular Windows searching functionality. To activateit, click anywhere in the SolidCAM Manager area andpress Ctrl+F. The Find dialog box is displayed, and youcan set the parameters for searching.33
    • Look in You may look for the required items in the whole CAM-Part or only in its operations, coordinate systems or geometries taken separately.Whole items only Select this check box if you want to check the availability of whole items as opposed to partial output.Match case This check box enables you to determine the case sensitivity of the search.Direction You may also decide whether the search results will be displayed from bottom to top or from top to bottom of the SolidCAM Manager tree.Find next Click this button if you want to view the search results one by one.Find all Click this button if you prefer to have all of the search results to be displayed simultaneously.General The whole line where the sought-for word appears is highlighted in the SolidCAM Managertree. When you close the Find dialog box, these lines remain highlighted. 34
    • 1. SolidCAM Basics1.4.2 Coordinate SystemThe Coordinate System is shown on the model. It defines the Coordinate Systemorigin for all the machining operations of the CAM-Part.For more information on Coordinate Systems, see topic 2.2.35
    • 1.5 Getting HelpSolidCAM Online Help enables you to get online help about various options in SolidCAM. The Helpis installed in the Documentation folder after the standard installation procedure.The Help is available via the SolidWorks Help menu. Click on the Help item in the main menu ofSolidWorks and choose the SolidCAM Help Topics, Milling items from the submenu.SolidCAM Help is fully context-sensitive. You can get a Help topic for each SolidCAM dialog box bypressing the F1 key. To get information about a specific dialog box area like field or button, click onthe question mark in the upper-right corner of the dialog box and then click on the field or buttonyou need. The Online Help is displayed and then the appropriate topic is explained.The Machining Portfolio is also available in the Documentation folder. This document provides anoverview of various features of SolidCAM. 36
    • CAM-Part 2At the stage of the CAM-Part definition, you have to specify all theinformation relevant to the machining project or workpiece you want tomanufacture. The CAM-Part folder includes all machining geometries,operation definitions and generated GCode files.The parameters and values defined at the CAM-Part level, such asCoordinate System, Milling levels and Tools will serve as default valuesfor separate machining operations. All specified parameters can bechanged in single operations.  Starting a new Milling CAM-Part  Managing CAM-Parts  Defining the Coordinate System  Defining the Stock model  Defining the Target model  CAM-Part Documentation
    • 2.1 Starting a new Milling CAM-PartAfter the SolidWorks model is loaded, do the following: 1. Click on the SolidCAM item in the SolidWorks menu. The SolidCAM main menu is displayed. 2. Choose the New option from the menu to define a new CAM-Part. 3. Choose the Milling type of new CAM-Part from the submenu. 4. The New Milling Part dialog box is displayed. When you start to program a CAM-Part, you have to decide on: • What type of CNC-machine you are going to use (3-, 4- or 5-axis); • Where you are going to clamp this part; • Where your Coordinate System positions are located (on a 4- or 5-axis CNC-machine, every clamping position is represented by the Coordinate System to which all additional positionings are related). 38
    • 2. CAM-Part2.1.1 New Milling Part dialog boxWhen you create a new CAM-Part, you have to enter a name for the CAM-Part and for the modelthat contains the CAM-Part’s geometry. • Directory In this field, you specify the location of the CAM-Part. The default directory is the SolidCAM user directory (defined in the SolidCAM Settings). You can enter the path or use the Browse button to define the location. The Use Model file directory option enables you to automatically create CAM-Parts in the same folder where the original CAD model is located. • Name In this field, you enter the name for the CAM-Part. You can give any name to identify your machining project. By default, the name of the design model is used. • Model name This field shows the name and the location of the SolidWorks design model that you are using for the CAM-Part definition. The default name is that of the active SolidWorks document. With the Browse button, you can choose any other SolidWorks document to define the CAM-Part. The chosen document is loaded into SolidWorks. Every time the CAM-Part is opened, SolidCAM automatically checks the correspondence of the dates of the CAM-Part and the original SolidWorks design model. When the date of the original SolidWorks model is later than the date of the CAM-Part creation, this means that the SolidWorks original model has been updated. You can then replace the SolidWorks design model on which the CAM-Part is based with the updated SolidWorks design model. After the Directory, Name and Model name fields are defined, click on the OK button to confirm the CAM-Part creation. The CAM-Part is defined and its structure is created. The Milling Part Data dialog box (see topic 2.1.3) is displayed.39
    • 2.1.2 The structure of the CAM-Part Cavity.prtThe Cavity CAM-Part includes the following data: Cavity • The Cavity.prt file located in the SolidCAM User directory. Cavity.SLDASM • The Cavity subdirectory containing all the data generated CAM.SLDPRT for the CAM-Part. DesignModel.SLDPRTSolidCAM copies the original SolidWorks model to the Cavity subdirectory and createsa SolidWorks assembly that has the same name as the CAM-Part (Cavity.sldasm). There are twocomponents in this assembly: • DesignModel.sldprt – a copy of the SolidWorks model file. • CAM.sldprt – a file that contains SolidCAM Coordinate Systems and geometry data.SolidCAM CAM-Part uses the assembly environment of SolidWorks. Thisenables you to create auxiliary geometries (e.g. sketches) without makingchanges in the original design model. You can also insert some additionalcomponents into the assembly file such as stock model, CNC-machinetable, clamping and other tooling elements.2.1.3 Milling Part Data dialog boxIn this dialog box, you specify all the information relevant to the machiningproject or workpiece you want to manufacture. The parameters andvalues defined at the CAM-Part level will later serve as default values formachining levels, etc. Naturally, all parameters can be changed in singlemachining operations. 40
    • 2. CAM-Part2.2 Coordinate SystemThe Coordinate System position defines theorigin for all machining operations of theCAM-Part. You can create multiple CoordSys Y-directionpositions and specify in each machining step X-directionwhich CoordSys you want to use for theoperation. The CAM-Part definition cannotbe completed if the Coordinate System is notdefined.The Coordinate System can be defineddirectly on the solid model. You can defineits origin location and axes orientation byselecting the model elements or by choosingthe already defined SolidWorks Coordinate Coordinate System OriginSystems.2.2.1 Defining the Coordinate System (CoordSys) Click on the Define button in the in the Coordinate System area of the Milling Part Data dialog box. If you define the first Coordinate System in the current CAM-Part, the CoordSys dialog box (see topic 2.2.2) is displayed. This dialog box enables you to define the Coordinate Systems. If the CoordSys that you define is not the first, the CoordSys Manager dialog box (see topic 2.3) is displayed. This dialog box enables you to manage your Coordinate Systems. You can also define new Coordinate Systems at the later stages of operation definition by clicking on the CoordSys button available in the Geometry page of the operation dialog box (see topic 5.2.6).41
    • 2.2.2 CoordSys dialog boxThis dialog box enables you to define a new 3-, 4-, and 5-axis CoordinateSystem directly on the solid model. The newly created Coordinate Systemautomatically receives the next sequential number. • Mac CoordSys number – this number corresponds with the built-in controller functions (for example, G54, G55, etc. in the Fanuc type controllers). It can be used for different clamping positions (Machine Coordinate Systems) in different operations on the CAM-Part. • Position – this number defines the sequential number of the CoordSys. For each Machine Coordinate System (Mac CoordSys), several Positions are defined for different positionings; each such Position is related to the Machine CoordSys. • In multi-sided machining on 4- and 5-axis CNC- machines, the SolidCAM post-processor uses the specific controller Macro language to create the positioning relative to the Machine Coordinate System. • For Machine Coordinate System, you have to define three points: the Origin, the X-direction, and the Y-direction. For the related position (e.g. for 4-axis CNC-machine), you have to define only the Origin and a point on the plane to rotate to; the rotation axis is defined by the type of the 4-axis (_4th_axes_around = X/Y in the MAC file).SolidCAM enables you to define the Coordinate System by one of the following methods:Select faceWhen you define the Coordinate System by selecting a face, the box surrounding the model iscalculated. For this box, SolidCAM generates a number of sketch points to facilitate the CoordSysdefinition. The points are located in the box corners, in the middle of each edge and in the centersof the planes (in the intersection point of the diagonals). 42
    • 2. CAM-PartThe face can be one of the following: • Planar face The Z-axis of the Coordinate System is normal to the selected face. • Cylindrical/Conical face The Z-axis of the Coordinate System is parallel to the axis of revolution of the specified cylindrical/conical face. Pick face Selecting this check box enables you to pick a face on the model for the Coordinate System definition. The selected model face is highlighted. Change to opposite/Change to original This button enables you to reverse the direction of the Z-axis of the Coordinate System.43
    • Place CoordSys origin to:• Corner of model box The upper plane of the model box is parallel to the XY-plane of the defined CoordSys. The CoordSys is located in the corner of the model box with the following coordinates (XMIN, YMIN, ZMAX). CoordSys Origin• Center of revolution face The origin is located at the intersection of the rotation axis of the part and the face of the model CoordSys box with the maximal Z-coordinate (the Z-axis is Origin directed along the rotation axis). Z• Top center of model box The CoordSys origin is placed in the center of the upper plane of the model, and the Z-axis of the CoordSys is normal to the selected face. CoordSys Origin• Corner box projection on the Z-level of the face The CoordSys origin is placed in the corner of the generated model box on the same Z-level with the selected face, and the Z-axis of the CoordSys is normal to the selected face. CoordSys Origin 44
    • 2. CAM-PartDefineThis option enables you to define the CoordSys origin and axes byselecting points. • Origin Select the origin point on the graphic screen. • X-direction Select a point relative to the origin that defines the X-axis. • Y-direction Select a point that defines the plane (the Y-axis is 90 degrees to the X-axis; the selected point defines the plane). After a point has been selected, the next button is automatically activated. If you miss the selection, you can at any time click the required button and continue automatically to the next button.Select Coordinate SystemSolidCAM enables you to choose the Coordinate System defined in theCAD model file as the SolidCAM Coordinate System.45
    • Normal to current viewThis option enables you to define the Coordinate System with the Z-axisnormal to the model view you are facing on your screen. You may bringthe model to the desired orientation by using the CAM Views toolbar orjust rotate it in an arbitrary fashion; then click on the Capture currentview CoordSys button, and the Coordinate System will be generatedrelative to the model view you are using. The CoordSys origin will lie inthe origin of the SolidWorks Coordinate System, and the Z-axis will bedirected normally to the chosen view of the model.You may change the location of the CoordSys Y-axis of theusing the placing options of the Select face Normal to current view CoordSysmode, and then choose the Normal to currentview mode to adjust the directions of theaxes to the current model view.Editing the Coordinate SystemAfter the face has been selected, you canedit the Coordinate System location bypicking entities on the model and change thedirections of its axes. X-axis of the Normal to current view Pick CoordSys • Pick origin This option enables you to define a new location for the CoordSys origin. The direction of the axes is not changed. • Pick XY origin This option enables you to define a new location for the CoordSys origin in the XY- plane by picking a point on the model. The Z-level of the CoordSys origin and the directions of the axes remain the same. • Pick X-direction This option enables you to choose a new direction for the X-axis by picking a point on the model. 46
    • 2. CAM-Part • Pick Y-direction This option enables you to choose a new direction for the Y-axis by picking a point on the model. Flip • Flip X&Y Click on this button to rotate the Z-axis 180 degrees by mutual replacing of the X- and Y-axes (X becomes Y, and Y becomes X). • Flip around X This button rotates the CoordSys 90 degrees around the X-axis. • Flip around Y This button rotates the CoordSys 90 degrees around the Y-axis. • Flip around Z This button rotates the defined CoordSys 90 degrees around the Z-axis. Delta This option enables you to move the CoordSys origin in the X-, Y-, and Z-coordinates relative to the point in which it was previously defined. Rotation around axis This option enables you to rotate the defined CoordSys a given number of degrees around the X-, Y- and Z-axes, but the rotation can only be defined around each axis separately. You cannot rotate the CoordSys around more than one axis simultaneously.47
    • 2.2.3 Defining the Coordinate Systems for 3-axis CNC-machineDuring the CoordSys definition for 3-axis CNC-machine, you have to define three points with theCoordSys dialog box. • Origin – Select the origin point (1st point) on the graphic screen. • X-direction – Select a point (2nd point) relative to the origin that defines the X-axis. • Y-direction – Select a point (3rd point) to finish the definition of the XY-plane.Use the mouse to define the origin, X- and Y-direction. You do not have to click on the X-direction orthe Y-direction button in the CoordSys dialog box, they are automatically selected after you definea point. Y-direction (third point) X-direction (second point) CoordSys origin (first point) Coordinate System definition ClampingFor the next Coordinate System, you also have to define three points. Y-direction X-direction (third point) (second point) CoordSys origin (first point) Coordinate System definition ClampingSolidCAM automatically assigns a new Position number to each Coordinate System. You can changethe Mac CoordSys number for a new clamping (Machine Coordinate System). 48
    • 2. CAM-Part2.2.4 Defining the Coordinate Systems for 4-axis CNC-machineWhen you define the Machine Coordinate System (Mac CoordSys) for the 4-axis CNC-machine,you have to define three points with the CoordSys dialog box: • Origin – Select the origin point (1st point) on the graphic screen. • X-direction – Select a point (2nd point) relative to the origin that defines the X-axis. • Y-direction – Select a point (3rd point) to finish the definition of the XY-plane.Use the mouse to define the origin, X- and Y-direction. You do not have to click on the X-direction orthe Y-direction button in the CoordSys dialog box, they are automatically selected after you definea point. Y-direction (third point) X-direction (second point) CoordSys origin (first point) Coordinate System definition ClampingTo add a new Position, you have to define only two points: • The point for the CoordSys origin. • The point on the plane to rotate to. If the rotation axis is X, you have to define the Y-direction. If the rotation axis is Y, you have to define the X-direction. X-direction (determined Y-direction automatically) (second point) CoordSys origin (first point) Coordinate System definition ClampingSolidCAM automatically assigns the new Position number to each CoordSys. You can change theMac CoordSys number for a new clamping (Machine Coordinate System).49
    • The rotation axis is automatically defined by SolidCAM according to the Axis type (see topic 2.8.1).The Shift and Rotation around parameters are calculated automatically.2.2.5 Defining the Coordinate Systems for 5-axis CNC-machineWhen you define the Machine Coordinate System (Mac CoordSys) for the 4-axis CNC-machine,you have to define three points with the CoordSys dialog box: • Origin – Select the origin point (1st point) on the graphic screen. • X-direction – Select a point (2nd point) relative to the origin that defines the X-axis. • Y-direction – Select a point (3rd point) to finish the definition of the XY-plane.Use the mouse to define the origin, X- and Y-direction. You do not have to click on the X-direction orthe Y-direction button in the CoordSys dialog box, they are automatically selected after you definea point. X-direction Y-direction (second point) (third point) CoordSys origin (first point) Coordinate System definition ClampingTo add a new CoordSys, you have to define three points. Y-direction (third point) X-direction (second point) CoordSys origin (first point) Coordinate System definition Clamping 50
    • 2. CAM-PartSolidCAM automatically assigns the new Position number to each CoordSys. You can change theMac CoordSys number for a new clamping (Machine Coordinate System).The rotation axis is defined automatically by SolidCAM according to the Axis type (see topic 2.8.1).The Shift and Rotation around parameters are calculated automatically.2.2.6 Coordinate System definition methodsCoordinate System definition using a sketchIn some cases, you cannot define the CoordSys origin position or thedirection of the axes without adding a geometry.Then you have to create a sketch that contains two perpendicular lines;the intersection point of the lines defines the CoordSys origin, and thelines define the X- and Y-axis directions. Y-direction CoordSysChoose the origin location at the intersection point of the lines originand define the axes directions. X-directionCoordinate System definition using a stock boxSolidCAM enables you to generate the stock box surrounding the modelautomatically with a defined offset (see topic 2.4.1). The top stock plane isparallel to the XY-plane of the Machine Coordinate System.Define the CoordSys in the stock box corner. Sometimes the model is located in the assembly in such a way that you need to rotate it before using the 3D Box option in order to calculate the optimal stock.51
    • 2.2.7 CoordSys Data dialog box • Position defines the sequential number of the Coordinate System. For each Machine Coordinate System, several Positions can be defined for different positionings; each such Position is related to the Machine Coordinate System. • X shows the X-coordinate of the CoordSys origin. • Y shows the Y-coordinate of the CoordSys origin. • Z shows the Z-coordinate of the CoordSys origin. • Machine CoordSys number defines the number of the Coordinate System in the CNC-machine. The default value is 1. If you use another number, the GCode file will contain the G-function that tells the machine to use the specified number stored in the controller of your machine. • The Tool start level defines the Z-level at which the tool starts. • The Clearance level is the Z-level to which the tool rapidly travels when moving from one operation to another (in case the tool does not change). • The CAM-Part Upper level defines the height of the upper surface of the part to be milled. • The CAM-Part Lower level defines the lower surface level of the part to be milled. Tool start level Rapid movements area Part Upper Clearance Feed movements area level level Part Lower level 52
    • 2. CAM-Part • The Tool Z-level is the height that the tool moves to before the rotation of the 4/5 axes to avoid collision between the tool and the workpiece. This level is related to the CoordSys position and you have to check if it is not over the limit switch of the machine. It is highly recommended to send the tool to the reference point or to a point related to the reference point. • The Plane box defines the default work plane for the operations using this CoordSys, as it is output to the GCode program. In the SolidCAM CAM module, you must always work on the XY-plane. Some CNC-machines, however, have different axes definitions and require a GCode output with rotated XY-planes. Choose one of the following options: • XY – the XY-plane is the work plane; the Z-axis is the depth (G17). • YZ – the YZ-plane is the work plane; the X-axis is the depth (G18). • ZX – the ZX-plane is the work plane; the Y-axis is the depth (G19). This option works correctly only when your post-processor has been customized to support this function. Please contact customer support for further details. • Shift is the distance from the Machine Coordinate System (Mac CoordSys) to the location of the Position in the coordinate system and the orientation of the Mac CoordSys. • Rotation is the angle of rotation around the main axes X, Y and Z. • For the first Position number related to a new Mac CoordSys number, the Shift and Rotation around parameters are always 0. • Shift and Rotation for other Position Numbers related to the same Mac CoordSys number are determined automatically. • The Edit CoordSys button enables you to change the CoordSys location or orientation of the axes with the CoordSys dialog box.53
    • • Create planar surface at Part Lower level This option enables you to generate a transparent planar surface at the minimal Z-level of the part so that its lower level plane is visible. This planar surface provides you the possibility to select points that do not lie on the model entities. It is suppressed by default and not visible until you unsuppress it in the FeatureManager Design tree. To unsuppress the feature, right-click on its entry under the CAM component in the FeatureManager Design tree and click on the Unsuppress button. This option is available only when the Coordinate System has been defined by selecting a face.2.2.8 SolidCAM Coordinate SystemSolidCAM changes the model orientation by setting the model to the Machine Isometric view.This orientation is suitable for machining on a CNC machine (with the Z-axis pointing verticallyupwards). Y Z Y Z X X SolidWorks Coordinate System SolidCAM Coordinate SystemUse the CAM Views toolbar to see the SolidCAM coordinate system.These views are related to the orientation of the selected CoordSysposition. 54
    • 2. CAM-Part2.3 CoordSys ManagerThe CoordSys managing commands are available in the CoordSys Manager dialog box after the firstCoordSys is defined. You can display the CoordSys Manager dialog box by clicking on the Definebutton in the Coordinate System area of the Milling Part Data dialog box or on the icon in theSolidCAM Manager tree. 1. Right-click on an item in the CoordSys Manager dialog box. 2. Choose a command from the menu.Add CoordSysThis command enables you to add a new Coordinate System to thecurrent CAM-Part.Edit CoordSysThis command enables you to change the data of an existing Coordinate System. It also enables youto change the CoordSys position. 1. Choose the Coordinate System you want to edit. 2. The CoordSys Data dialog box is displayed showing the default Coordinate System position values. The fields and values can be changed, if necessary. If you change the CoordSys position, you must recalculate the operations in which this CoordSys is used. You are also advised to review the simulation.Inquire CoordSysThis command enables you to view the relevant information about a particular Coordinate Systemposition, but you cannot edit the data.55
    • Delete CoordSysThis command deletes an existing Coordinate System. You can only delete Coordinate Systems ifmore than one CoordSys has been defined for the current CAM-Part. You cannot delete the firstMachine CoordSys and a CoordSys that is used for the operation (the Delete command in the menuis disabled in these cases). 1. Choose the Coordinate System you want to delete. The confirmation dialog box is displayed. 2. Click Yes to confirm.Rename CoordSysThis command enables you to rename the chosen Coordinate System.Default nameThis command enables you to return the Coordinate System name to the default value.Create/Delete Planar surfaceThis option enables you to create the planar surface at the Z-level of the model if you have notselected the Create planar surface at Part lower level check box at the stage of CoordSys datadefinition, or to delete the created planar surface if you have selected this check box.CoordSys visibilityThe Coordsys Manager dialog box enables youto control the visibility of Coordinate Systems.This feature simplifies the work when you havea number of coordinate systems.In the CoordSys Manager dialog box, clear thecheck boxes for the coordinate systems in orderto hide them. 56
    • 2. CAM-Part2.4 Stock and Target ModelStock model is the material placed on the machine before youstart machining the CAM-Part.The Stock model is used for: • SolidVerify, SolidVerify for 3D, VerifyPlus and Machine simulation; • For rest material calculation in 3D Milling operations. The stock model is not automatically associated with the solid model. If the model is changed and the stock is not correct any more, you will see it in the simulation; you can then replace the defined stock with the updated one. Note that the SolidVerify, SolidVerify for 3D and VerifyPlus simulations do not work without the Stock model defined.Target model is the final shape of the CAM-Part after themachining.The Target model is used for: • 3D simulation; • Rest material calculation; • Gouge checking in the SolidVerify simulation.During all machining operations, the remaining rest material isremoved so that the Target model can be obtained.Facet toleranceThe Facet tolerance parameter defines the accuracy of triangulation of the stock and target models,fixture or clamp.57
    • 2.4.1 Stock modelThe Stock model option enables you to define the actual material that hasto be removed. 1. Click on the Stock button in the Milling Part Data dialog box. 2. In the Stock model dialog box, choose the stock model definition mode and click on the Define button. 3. Select the geometry. 4. Confirm the geometry selection.Stock definition modes • The 2D Boundary mode enables you to define the 2D stock geometry with the chain of geometric elements (lines, arcs, splines, edges, etc.). Before selecting the stock material, you have to draw the boundaries of the stock material around the CAM-Part. When you choose this mode and click on the Define button, the Geometry Edit dialog box is displayed. • The 3D Model mode enables you to define the stock model via 3D model selection and is useful for casting machining. When you choose this mode and click on the Define button, the 3D Geometry dialog box is displayed. • The Box (Auto) mode enables SolidCAM to automatically determine the box surrounding the model. When you choose this mode and click on the Define button, the 3D Box dialog box is displayed. 58
    • 2. CAM-Part 3D Box dialog box This dialog box is used to select a 3D model to create a 3D box around the model. • The Name option enables you to define the name for the stock model. The default geometry name is assigned automatically and can be edited if necessary. • The Type option enables you to choose the type of model elements that will be selected: Solids (solid models), Surfaces, or Both. • The Expand box at option enables you to define how much access stock material you have in each direction of the stock material. • The CAD selection button enables you to pick the model with the Host CAD tools. • The Add box to CAD model button enables you to add the stock box to the CAD model. • The STL file mode enables you to define the stock model based on a STL file that exists in your system. When you choose this mode and click on the Define button, the Choose STL dialog box is displayed. This dialog box enables you to choose the STL file for the stock definition. Choose STL dialog box • The Name option enables you to define the name of the STL stock geometry. The default geometry name is assigned automatically and can be edited if necessary. • The STL File section shows the path to the STL file chosen for the stock geometry definition. • The Browse button enables you to display the browser dialog box from which you will choose the required STL file. • The Show button enables you to display the defined stock in the Rest material window of SolidCAM (see topic 2.4.3). • The Show on model button enables you to display the defined stock in the SolidCAM graphic area applied to the solid model (see topic 2.4.3).59
    • 2.4.2 Target modelThe Target model option enables you to define the final part after machining. 1. Click on the Target button in the Milling Part Data dialog box. 2. In the Target model dialog box, click on the Define 3D Model button to start the geometry selection. 3. Select the geometry with the 3D Geometry dialog box (see topic 4.3.1). 4. Confirm the Target model definition with the button.In future operations, you can use the Target model as a geometry.2.4.3 Common controls for Stock model and Target model dialog boxesNameIn this field, you can see the stock or target model name and choose the model from the previouslydefined 3D geometries.ShowClick on this button to show the Stock or Target model in the Rest material window of SolidCAM. Target model Stock model To control the quality of the Stock and Target models visualization, you can change the Facet tolerance in the Milling Part Data dialog box. The recommended value is 0.01 mm. A smaller tolerance will improve the quality and reduce the visualization speed. 60
    • 2. CAM-PartShow on modelClick on this button to see the selected Target model in the Host CAD window. Target model Stock modelSelf-intersectionsThe Check and fix button in the Self-intersections section enables you to check the model for self-intersections and fix them if they are found.When self-intersections are detected, the following message is displayed:Confirm it with the Yes button to fix the self-intersections.Note that the process of self-intersection fixing can take a long time to complete, depending on thecomplexity of the model.For more information on self-intersections, see topic 10.6.6.2.4.4 Associativity of Stock and Target modelsSolidCAM enables you to keep the associativity betweenStock/Target model and the SolidWorks model. When theSolidWorks model is updated, SolidCAM enables you to checkthe compliance of the Stock and Target model geometry to theupdated SolidWorks model. If the SolidCAM geometry is notsynchronized with the SolidWorks model, you can synchronize it.The Check synchronization command enables you to check thesynchronization status of the Stock/Target model geometry relative tothe SolidWorks model.61
    • If SolidCAM determines a misfit between the SolidWorks model and the Stock/Target modelgeometry, this geometry is marked with the synchronization mark .If the Stock/Target model geometry is not synchronized with the SolidWorks model, theSynchronize command enables you to update the Stock/Target model geometry according to theupdated SolidWorks model. 62
    • 2. CAM-Part2.5 Tool OptionsThe Tool options enable you to define additional data about the tools for your CAM-Part. You canenter the start and end position of your tool as well as the coordinates for tool changes on yourCNC-machine. After you click on the button, you can change the parameters in the Tool Optionsdialog box.The default values you receive in this dialog box are input from the MAC file of the selected post-processor.A sample from the MAC file is shown below. The first three values of each line are metric coordinatesand the last three values are in inches. ;Positioning dflt_start = 0.0000 200.0000 100.0000, 0.0000 7.8740 3.9370 dflt_end = 0.0000 200.0000 0.0000, 0.0000 7.8740 0.0000 set_z_chng = Y dflt_tool_chng = 0.0000 0.0000 0.0000, 0.0000 0.0000 0.0000In the Tool Options dialog box, you can edit the values for the currentCAM-Part. Start point This field determines the position of the first tool in the beginning of the milling. End point This field determines the position of the last tool in the end of the milling. • In most of the cases, the value in this dialog box will only affect the simulation. To affect the generated NC-program, the post-processor must use these values. • Normally, the new CNC-controllers do not need the start and end position. In the post- processor, you use the machine command to move to the machine reference point.63
    • Tool change XY This field defines the XY-coordinates of the tool change position. There are two options: • Default as in MAC file The XY-coordinates of the tool change position are defined by the end point of the operation that was executed before the tool change. • Define The XY-coordinates of the tool change position are defined by the user.Tool change Z This field defines the Z-coordinate of the tool change position. There are two options: • Default as in MAC file The Z-level where tool changes are performed is automatically read from the Tool start plane specified in the CoordSys Data dialog box (default input from MAC file). • Define The Z-coordinate of the tool change position is defined by the user.Feed type Defines the default type of feed used for the tool of this CAM-Part. There are two options: • Mm/Min – Millimeters per Minute; • Mm/Rev – Millimeters per Revolution. 64
    • 2. CAM-Part2.6 Mac OptionsIf the MAC file of your post-processor has extrafields (parameters) defined, they can be accessedthrough this field. In the Machine Options Listdialog box, you can enter unique informationrelated to the machine controller you haveselected. • In case of Numeric or Integer field type, the Numeric/Integer Value dialog box is displayed and you are prompted to enter a value. • In case of Logical field type, the Logical Value dialog box is displayed and you are prompted to choose between Yes and No. Refer to the GPPTool manual for additional information.2.7 Work MaterialThis option enables you to define the work material. Choose the work material from the list.The Work material field enables you to get Speed/Feed Defaults (see topic 3.11) based on thework and tool materials that you are using. If you choose the None option, the system will offeryou the internal standard value spin of 1000 rpm and the default feed for X, Y movement of100 mm/min.65
    • 2.8 CNC-Controller and Axis TypeSelect the CNC-machine controller. Click on the arrow next to the controllerfield to display the list of post-processors installed on your system.2.8.1 Axis typeThis field displays the CNC-controller type. This field cannot be edited; itis defined in the post-processor file.The axis type can be one of the following: • 3 axis; • 4_axis_around_X or 4_axis_around_Y; • 5 axis.The axis type defines the Coordinate System definition method:3 axisIn this type of machine, every siderequires a new clamping (new MachineCoordSys). For each Mac CoordSys, youhave to define the origin position, theX-axis direction and the Y-axis direction.4 axis • 4_axis_around_X This type is used for vertical machines with the 4th axis on the table along the X-axis. When defining the Machine CoordSys, you have to define the origin position, the X-axis direction and the Y-axis direction. For all additional positionings, based on this clamping, you have to define the origin position and the Y-axis direction only (the angle); the X-axis direction is determined automatically by the X-axis direction of the Machine CoordSys. 66
    • 2. CAM-Part • 4_axis_around_Y This type is used for horizontal machines with the 4th axis along the Y-axis. When defining the Machine CoordSys, you have to define the origin position, the X-axis direction and the Y-axis direction. For all additional positionings, based on this clamping, you have to define the origin position and the X-axis direction only (the angle); the Y-axis direction is determined automatically by the Y-axis direction of the Machine CoordSys.5 axisThis type is used for 5-axis CNC-machines. For the Machine CoordSys,you have to define the origin position, the X-axis direction and theY-axis direction. All additional positioning is related to this MachineCoordSys. Take care of the machine limitations (angles or undercuts). A message on the limit can be generated only during the GCode generation. In the definition process, it is not necessary to consider the kinematics of the CNC-machine. This is done in the last step when you generate the NC-program. • A CAM-Part created for a CNC-controller of 3-axis type cannot be converted to 4- or 5- axis type. • A CAM-Part created for the CNC-controller of 4-axis type can be converted to 3-axis type. • A CAM-Part created for the CNC-controller of 5-axis type can be converted to 3-axis type.67
    • 2.9 Default GCode numbersThe fields in this area are displayed according to a parameter defined in the MAC file. ; Program numbers get_prog_num = N or Y get_proc_num = N or YIf N – the field is not displayed.If Y – the field is displayed. get_prog_num = Y get_proc_num = NProgram numberThis field enables you to define the number of the main program that will be generated in theoutput NC-program.This field has ranges that are controlled from the MAC file parameters. prog_num_min = 1 prog_num_max = 9999 prog_num_dflt = 5000 68
    • 2. CAM-PartIn this case, the default number is 5000. You can change this value and type a number between 1and 9999. Typing any number beyond this range is followed with the message:Subroutine numberIn this field, you can define the number of the first subroutine in the generated outputNC-program.This field has ranges that are controlled from the MAC file parameters. proc_num_min = 1000 proc_num_max = 5000 proc_num_dflt = 1000In this case, the default number is 1000. You can change this value and type a number between 1000and 5000. Typing any number beyond this range is followed with the same message as above.In some machines (for example, Fanuc), the main program number and subroutine number cannotbe the same. SolidCAM does not warn you about this problem. In order to prevent this situation,you can set the main program range to 1 – 1000 and the subroutines range to 1001 to 9999 in theMAC file.69
    • 2.10 Part SettingsSolidCAM enables you to define a number ofparameters specific for the current CAM-Partusing the Part Settings dialog box.This dialog box is available by clicking on theSettings button in the Milling Part Data dialog boxor by double-clicking on the Part settings iconunder the CAM-Part header in SolidCAM Manager.2.10.1 UnitsThe Units page shows the measurement units usedin the current CAM-Part. 70
    • 2. CAM-Part2.10.2 Interoperational tool movementsThis page contains options that enable you tocontrol the interoperational movements (see topic5.2.8).For each new CAM-Part, these settings are copiedfrom the SolidCAM Settings (see topic 12.10) andcan be adjusted according to your preferences. SolidCAM enables you to change the settings even when a CAM-Part is opened.Part Clearance levelAll interoperational movements are performedthrough the Part Clearance level. This is the defaultoption.When you switch to the Part Clearance level mode, SolidCAM disables the Start level field in alloperations. All SolidCAM operations (except for Sim. 5 Axis operations) have to be recalculated.After the recalculation, all interoperational movements are implemented through the Part Clearancelevels of the appropriate Coordinate Systems.Operation Start levelWhen two neighboring operations use the same Coordinate System, Tool and Tool offset, theinteroperational movement between them is performed through the Operation Start level of thesecond operation.When you switch to the Operation Start level mode, SolidCAM enables the Start level fields in alloperations and defines the Start levels equal to the Part Clearance level of the related CoordinateSystems. All interoperational movements will be implemented through the appropriate Start levels.71
    • 2.10.3 Update Stock calculationThis page contains three tabs with Updated Stockmodel settings for the SolidVerify simulation (seetopic 10.6), Rest Material calculation (see topic 10.8)and SolidVerify for 3D simulation (see topic 10.7).SolidVerify tabThis tab enables you to define the Updated Stockparameters and options relevant for the SolidVerifysimulation. Update stock accuracy This section enables you to define the USM accuracy parameters for the SolidVerify simulation. • Tool facet tolerance This option controls the precision of the tool for the SolidVerify simulation. • Tool facet type In addition to changing the tolerance used for faceting, the application controls the manner in which the faceted tool representation approximates the tool by forcing the representation to be bigger or smaller than the actual tool. For example, if you want to know whether the tool gouged the target part, it would probably be preferable to have a tool representation that is guaranteed to lie outside the bounds of the actual tool. Internal. The tool representation lies within the actual tool. The vertices of the tool representation will lie on the surface of the actual tool and the facets will lie within the actual tool. External. The actual tool lies within the tool representation. The vertices will lie at distances up to the faceting tolerance from the surface of the actual tool. Mixed. This is a combination of the Internal and External modes. The vertices lie outside the actual tool but parts of the facets may lie inside it. This mode is the default and should be used unless there is a specific reason for using one of the other modes as it generates fewer facets and will therefore be faster. 72
    • 2. CAM-Part 5 Axis The Linear interpolate option enables you to perform the linear interpolation of 5-axis tool movement. The Max. interpolation angle value defines the angular tolerance for the interpolation. Update stock model method This section enables you to choose the method of Stock model updating. • Automatic Save updated stock model for every specified number of operations: SolidCAM automatically calculates and saves the Updated Stock model. The specified number enables you to define the quantity of intermediate USM files. For example: • if the specified number is 1, SolidCAM automatically saves intermediate USM files for each operation; • if the specified number is 2, SolidCAM automatically saves intermediate USM files for all even operations (2nd, 4th, 6th, etc.); • if the specified number is 0, SolidCAM does not save intermediate USM files. Save updated stock model for operations with a long tool path only: SolidCAM automatically estimates the time required for simulation of operations and saves the updated stock for those operations whose tool path is considered too long. • Manual SolidCAM enables you to manually save the updated stock model for a specific operation during the SolidVerify simulation. The simulation of the next operations can be performed on the updated stock model. Further 3D Milling operations can also use the saved USM for the cutting in Rest material areas. Automatically remove noise from input data During the faceting of Stock and Target models, the coordinates of facets generated by SolidCAM are often calculated as numbers of the float type with many digits after the point. These numbers cause problems during the SolidVerify simulation, such as self-intersections and gaps in model. The Automatically remove noise from input data check box enables you to use a smart rounding algorithm that removes the noise in facet coordinates so that the model is displayed properly. Note that the process of removing the noise may take a long time to complete.73
    • Rest Material calculation tabThis tab enables you to define the Updated Stockparameters and options used for the Rest materialcalculation in 3D Milling operations. Update stock accuracy This section enables you to define the USM accuracy parameters for the Rest material calculation. 5 Axis The Linear interpolate option enables you to perform the linear interpolation of 5-axis tool movement. The Max. interpolation angle value defines the angular tolerance for the interpolation. Current Stock model method This section displays the method of Stock model updating used for the Rest Material calculation. The setting of this section can be changed in the SolidVerify tab.SolidVerify for 3D tabThis tab enables you to define the Updated Stockparameters and options relevant for the SolidVerifyfor 3D simulation.The Updated Stock calculation parameters definedfor this type of simulation are similar to thosedefined for SolidVerify. Since in this simulationmode analytical surfaces are used instead of facetmodels used for SolidVerify, the Updated Stockmodel accuracy section is not relevant. 74
    • 2. CAM-Part2.10.4 SynchronizationThis page enables you to define the synchronization settings for the current CAM-Part when itsmodel configuration is changed.The Synchronization when design model configuration changes section provides you with thefollowing options: • Keep the geometry associative with the parent configuration This option enables you to keep the link between the geometry and the parent configuration. SolidCAM always keeps the geometry linked to the parent configuration (the configuration used for the geometry definition). When you switch between the model configurations, the geometry is not affected; synchronization is required only if the parent configuration is changed. Geometry Geometry Configuration #1 Configuration #275
    • • Associate the geometry with the current configuration This option enables you to establish the link between the geometry and the current configuration and perform the synchronization according to the current configuration. Geometry Geometry Configuration #1 Configuration #2 After such synchronization, the geometry is linked to the current configuration until you switch to another one.2.10.5 Automatic CAM-Part definitionSolidCAM provides you with a number offeatures aimed to automate the process of theCAM-Part definition. These features enable youto avoid a number of routine steps required to beperformed during the CAM-Part definition andperform them automatically.This page contains a number of settings relatedto the Automatic CAM-Part definition. For eachnew CAM-Part, these settings are copied fromthe SolidCAM Settings (see topic 12.12) and canbe adjusted according to your preferences.Automatic Stock model definitionThe Definition of Stock (as 3D box) option enables you to automatically define the 3D box stockmodel during the CAM-Part definition. The stock model is based on all solid bodies and/or surfacesof the DesignModel component of the CAM-Part assembly. 76
    • 2. CAM-Part • Define Stock by. This option enables you to choose the type of elements (solid bodies and/or surfaces) from the DesignModel model to use. • Expand box at. This option gives you complete control over how much access stock material you have in each direction of the stock material.The Add box to CAD model option enables you to add the stock model box to the CAD model.Automatic Target model definitionThe Definition of Target check box enables you to automatically define the target model duringthe CAM-Part definition. The target model is based on all the solid bodies and/or surfaces of theDesignModel component of the CAM-Part assembly.The Define Target by option enables you to choose the type of elements (solid bodies and/orsurfaces) from the DesignModel component of the CAM-Part assembly.Definition of Coordinate SystemWhen the Single CoordSys check box is selected, SolidCAM enables you to shorten the processof CoordSys definition by skipping the CoordSys Manager dialog box after the first CoordSysdefinition. This option is useful when defining CAM-Parts with only one Coordinate System.When the Single CoordSys check box is cleared, SolidCAM displays the CoordSys Manager dialogbox after the first CoordSys definition. The CoordSys Manager enables you to define an additionalCoordinate System. This option is useful when defining CAM-Parts with several Coordinate Systems.77
    • 2.10.6 Machining ProcessOn MP insertion (for milling only)Select the Perform auto calculation check boxin case you want the operations to be calculatedautomatically after the Machining Process isinserted into the CAM-Part.If you select the Ask before calculation checkbox, the message that enables you to confirmthe calculation is displayed. If this check boxis cleared, the calculation starts without priornotice.Operation name in SolidCAM ManagerThe setting of this field defines how theoperation names appear in SolidCAM Managerwhen a Machining Process Table is loaded anda Machining Process is added to the CAM-Part.When the Show group name check box is selected, the operation names are preceded with thenames of the operation groups and default sets defined in Machining Process Table Manager.Prismatic part_20-6_finish_wall Operation Default set Operation group name name name 78
    • 2. CAM-PartWhen this check box is not selected, only the operation names appear in the SolidCAM Managertree.2.10.7 Tool path simulationSolidCAM enables you to define the default simulation mode. • Use Host CAD simulation as default When this option is chosen, the Host CAD simulation mode is used as default for each new simulation session. • Remember last simulation option When this option is chosen, simulation starts in the last used mode.79
    • 2.10.8 GCode generationThis page enables you to define the parameters of the GCode generation.The Save GCode files box offers three optionsto define the parameters related to saving ofGCode files:In the CAM-Part directorySolidCAM saves the generated GCode files in theCAM-Part directory. The path to this directoryis displayed in the read-only field. This option isused by default.According to the MAC fileSolidCAM saves the generated GCode filesaccording to the parameters defined in the MACfile. The path to the directory that appears in theMAC file is displayed in the read-only field.In the GCode directorySolidCAM saves the generated GCode files in the specified GCode folder location. When theGCode generation is started, SolidCAM creates a new folder with the CAM-Part name in thespecified GCode directory and saves the GCode files there. If this folder already exists, SolidCAMuses it for the GCode output.This group box enables you to define the path for the GCode directory. You can enter the path orclick on the Browse button and choose the destination folder using the Browse For Folder dialogbox. If you have entered the path to a non-existing folder, the following message is displayed after the confirmation of the Part Settings dialog box: 80
    • 2. CAM-Part The Create button enables you to create the folder that will be used for GCode directory in the specified location. The Browse button displays the browser dialog box that enables you to choose another location that will be used for the GCode directory. If the new folder cannot be created, the following message is displayed: If the chosen folder has the read-only attribute, the following message is displayed after the confirmation of the Browse dialog box or the Part Settings dialog box:By default, the GCode directory location is not defined. You have to specify it when you choose theIn the GCode directory option for the first time. Create subfolders for split GCode files When split marks are detected in SolidCAM Manager during the GCode generation for the entire CAM-Part, SolidCAM creates a number of GCode segment files. Each such GCode segment file is created for one or several operations enclosed by split marks. These files are named with the CAM-Part name followed by the “-” sign and the order number of a split segment. Split marks are ignored in case of GCode generation for several operations. With the In the GCode directory option, SolidCAM creates separate CAM-Part GCode folders in the specified folder location. When the Create subfolders for split GCode files check box is selected, SolidCAM creates a separate folder for each GCode segment file and saves the GCode segments files there. The folder is created in the GCode folder of the CAM-Part in the specified GCode folder location. The name of the folder is the same as the GCode segment file name.81
    • When the Create subfolders for split GCode files check box is not selected, SolidCAM generates all the GCode segment files directly into the GCode folder of the CAM-Part in the specified GCode folder location. By default, the Create subfolders for split GCode files option is not selected. Create separate folders for each CAM-Part When this check box is selected, SolidCAM creates a folder for each CAM-Part and saves the GCode file there. Otherwise, the GCode files for all CAM-Parts are generated into the GCode directory.Additional control of GCodeWhen the Customize GCode file name check box is selected,you can alter the GCode file name and location. Whenyou click one of the GCode generation commands, theWindows-style Save GCode browser is displayed with thedefault CAM-Part name and location that might be edited. All the GCode files previously generated for the current CAM- Part remain in the specified folder.When this check box is not selected, the GCode is generated and automatically saved in the definedlocation. 82
    • 2. CAM-PartGCode generation for the entire CAM-PartThe Erase all previous GCode files check boxenables you to choose whether the old GCodefiles generated for this CAM-Part remain or areremoved when a new one is generated. This check box is not available if the Create a separate folder for each CAM-Part check box is not selected and when the Customize GCode file name check box is selected.GCode generation for separate operationsThe Erase all previous GCode files check boxenables you to choose whether the old GCodefiles generated for separate operations remainor are removed when a new one is generated. This check box is not available if the Create a separate folder for each CAM-Part check box is not selected and when the Customize GCode file name check box is selected.83
    • 2.10.9 Template defaultsThis page enables you define the default locationof the operation templates and to specify thedefault templates used for each new operation ofthe loaded CAM-Part. When a new CAM-Part is being created and defined, the Part settings for Templates and Defaults are copied from the SolidCAM Settings.SolidCAM Template DirectoryThis section enables you to define the default location for SolidCAMtemplates. You can define the path by entering it in the box or byclicking on the Browse button and choosing the location. In casethe chosen folder does not exist, the error message is displayed. • The Create button enables you to create the folder with the specified location and set it as the SolidCAM Template directory. • The Browse button displays the browser dialog box that enables you to choose another location for the SolidCAM Templates directory.The default Templates directory location is ..TablesMetricTemplates for Metric units and..TablesInchTemplates for Inch units.Operation default templatesThis section enables you to assign a default template to each operation type. It contains the followingtabs: • The 2.5D Milling tab lists the templates of 2.5D Milling operations. • The 3D Milling tab lists the templates of 3D Milling operations. • The HSM and HSS tabs list the templates of HSM and HSS operations. • The Sim. 4 Axis and Sim. 5 Axis tabs list the templates of Sim. 4 Axis and Sim. 5 Axis operations. 84
    • 2. CAM-PartEach tab contains a table that enables you to definethe default templates for each operation type.When the default template use is activated for aspecific operation (the check box in the operationtype line is selected), the Template column offersyou the list of available templates appropriate forthis type of operation.When the template use is activated for an operationtype, each new operation of this type will be loadedwith the data of the specified template.Templates activation/deactivationWhen you clear the check box in an operation typerow to deactivate the use of templates, the list inthe Template column is unavailable.When you select the check box to activate template use for an operation type, the search is performedin the SolidCAM Template Directory for suitable templates of this type. The names of the foundtemplates appear in the list, and the first of them is being chosen automatically. If no suitabletemplates are found, SolidCAM deactivates the use of templates for this operation.Changing the SolidCAM Template DirectoryWhen you change the path to the SolidCAM Template Directory, SolidCAM performs a search forsuitable templates for all the operations with the activated default template use. When a template forsome operation type is not found, SolidCAM deactivates the default template use for this operationtype. Found templates are added into the related list. The first found template name is displayed. The search for templates is not performed for the operation types for which the use of templates is deactivated.Creating sets of templates (working style)Consider a folder containing a set of templates. This set contains only one template for each operationtype, therefore, all operation types have assigned templates. The set of templates is customizedfor a specific application (e.g. Mold machining). Consider an additional folder containing a set oftemplates for another application.By switching between these folders for SolidCAM Template Directory, SolidCAM switches templatesfor all operation types. This enables you to choose a set of templates for a specific applicationquickly and easily.85
    • 2.10.10 Tool coolantThis page enables you define the tool coolantoptions that will be applicable to each new tooladded for use in the current CAM-Part.When a check box is selected, the related coolantoption is used.The coolant options available for use on thecurrent CNC-machine, according to the MAC-filesettings, are marked with asterisks (*).2.10.11 Gouge checkThis page enables you to control the gougechecking parameters at the CAM-Part level.The Check gouges on calculation check boxenables you to define the default state of thecorresponding edit box in the operation dialog box(see topic 5.2.12). This state is inherited by eachnew 2.5D Milling operation. 86
    • 2. CAM-Part2.11 Compressed CAM-PartSolidCAM provides you with the Compressed CAM-Part feature. SolidCAMThis feature enables SolidCAM to save all the CAM-Part data inone file compressed using the ZIP technology.SolidCAM saves all the CAM-Part data in ZIP archive file. ExtractedDuring the SolidCAM session, this file is extracted in the specific CAM-Parttemporary location and SolidCAM works with the extracted Open CloseCAM-Part data. When the CAM-Part is closed, the content of theZIP file has to be replaced with the updated CAM-Part data. When Compressedthe update process is finished, SolidCAM erases the extracted CAM-PartCAM-Part from the temporary location. • SolidCAM supports simultaneous work with both file formats: compressed CAM-Part and non-compressed CAM-Part. • Each newly created CAM-Part can be created either in the compressed mode or in the non-compressed mode, depending on SolidCAM Settings (see topic 12.6). • Each CAM-Part can be converted from open to compressed mode depending on the SolidCAM Settings (see topic 12.6).2.11.1 Compressed CAM-Part file formatThe SolidCAM Compressed CAM-Part format is ZIP SolidCAM Compressed CAM-Part(compatible with WinZIP application). This file hasthe *.prz extension and contains all CAM-Part data. SolidCAM CAM-Part SolidCAM CAM-Part folder2.11.2 Creating a new compressed CAM-PartWhen you confirm the CAM-Part creation in the NewMilling Part dialog box, SolidCAM creates the emptycompressed CAM-Part file in the location specifiedin the Directory field and with the name specifiedin the <Name> field. SolidCAM also creates the<Name>.prt file and the <NAME> folder in theSolidCAM Temporary folder.87
    • The SolidCAM Temporary folder is automatically created by SolidCAM. By default, this folder hasthe following path: C:Documents and Settings<user name>Local SettingSolidCAM Temporaryfiles. You can choose your own location for the SolidCAM Temporary folder via SolidCAM Settings(see topic 12.6).For example, the structure of the Shaft CAM-Part is the following: C:Program FilesSolidCAM2009User Shaft.prz C:Documents and Settings<User name>Local SettingsSolidCAM Temporary files Shaft.prt Shaft If the compressed CAM-Part already exists in the location defined in the Directorybox; you cannot define a new CAM-Part with the same name. SolidCAM offers you to choose an alternative name or location.After the CAM-Part definition, SolidCAM works with the CAM-Part data located in the SolidCAMTemporary folder. When the CAM-Part is being closed, SolidCAM updates the compressedCAM-Part with the CAM-Part data. After the update, the non-compressed copy is removed fromthe SolidCAM Temporary folder.2.11.3 Converting CAM-Parts to Compressed modeSolidCAM enables you to work with both types of CAM-Parts: compressed and non-compressed.Each non-compressed CAM-Part can be converted to the compressed mode in the opening process(according to the SolidCAM Settings). During this operation, SolidCAM compresses all CAM-Part data to the compressed CAM-Part. After these operations, SolidCAM removes the originalCAM-Part.2.11.4 Opening/Closing Compressed CAM-PartsWhen opening a compressed CAM-Part, SolidCAM extracts all its content into the SolidCAMTemporary folder and loads the non-compressed CAM-Part.When closing a CAM-Part, SolidCAM updates the corresponding compressed CAM-Part with thedata from the SolidCAM Temporary folder. After the update, the non-compressed data is removedfrom the SolidCAM Temporary folder.The smart algorithm of opening compressed CAM-Parts enables SolidCAM to prevent data loss incase the CAM-Part session was not completed correctly. 88
    • 2. CAM-PartIf the CAM-Part session was not completed correctly and the Compressed CAM-Part was notupdated successfully, the non-compressed data is not removed from the SolidCAM Temporaryfolder. In this case, SolidCAM finds the corresponding non-compressed data in the next CompressedCAM-Part and displays the following dialog box. • Continue with Compressed CAM-Part version The non-compressed data in the SolidCAM Temporary folder is updated with the content of the compressed CAM-Part. • Continue with SolidCAM Temporary folder version The compressed CAM-Part is updated with the non-compressed data from the SolidCAM Temporary folder. The Exit button enables you to cancel the operation and solve the problem manually.89
    • 2.12 Managing CAM-PartsUse the commands of the SolidCAM and CAM-Part menus to edit and manage existing CAM-Parts.NewThis command creates a new CAM-Part. According to SolidCAM Settings (see topic 12.6), theCAM-Part can be created either in the compressed mode or in the non-compressed mode.OpenThis command loads a CAM-Part (compressed and non-compressed) that has been previouslysaved. According to SolidCAM Settings (see topic 12.6), the non-compressed CAM-Parts canbe converted to the compressed mode. When you choose this option, the CAM-Parts browser isdisplayed. 90
    • 2. CAM-Part 1. Select the CAM-Part you want to load. 2. Double-click on the CAM-Part or select it and click on the Open button. The default type for the Files of Type filter is defined in SolidCAM Settings.If a CAM-Part was created with the previous SolidCAM version, the backup can be performedduring the CAM-Part opening, if necessary. The backup is created as a copy of the original file inthe Backup of <CAM-Part name> folder. You can also open CAM-Parts by double-clicking on the *.prt files in the Windows Explorer environment.Manage TemplatesThis command enables you to manage your operation and process templates using the TemplateManager dialog box.For more information on operation templates and process templates, see topic 5.2.2.CloseSolidCAM closes the active CAM-Part. The Compressed CAM-Part file is being updated, if necessary.91
    • CopyThis command creates an identical copy of a CAM-Part in another folder or drive for backup purposesor for making modifications without changing theoriginal. The Copy Parts dialog box is displayed. 1. Choose the drive from which you want to copy the original CAM-Part. 2. Choose the CAM-Parts you want to copy from the CAM- Parts list. 3. Transfer the list of the CAM-Parts you want to copy to the middle field by clicking on the Left to Right arrow. 4. Choose the drive and the directory you want to copy to. 5. Click on the Copy button. This feature is unavailable for compressed files; they can be copied with standard Windows tools.DeleteThis command enables you to delete a CAM-Part (compressed and non-compressed). ThePart to Delete dialog box is displayed.The Files of type filter enables you to displayeither compressed or non-compressed CAM-Parts. The default filter value depends onSolidCAM Settings. 1. Select the CAM-Part you want to delete. Use the Ctrl key to select several CAM-Parts together. 2. Click on the Delete button. 92
    • 2. CAM-Part 3. The confirmation dialog box is displayed: 4. Choose Yes to All to delete all selected CAM-Parts.Calculate CAM-PartsThis command enables you to calculate tool paths of all CAM-Parts (compressed and non-compressed) in the specified folder. The Calculate parts dialog box is displayed. 1. Click on the Add Directory button. 2. Choose the folder where the CAM-Part is situated via the standard Windows browser. 3. Click on the Calculate button to start the operation.You can also use the Delete All button to remove all the CAM-Parts from the specified folder.The compressed CAM-Part is extracted into the SolidCAM Temporary folder. The resulting non-compressed CAM-Part is opened by SolidCAM and calculated. The compressed CAM-Part is thenupdated and the non-compressed CAM-Part is removed from the SolidCAM Temporary folder.Change Model ReferenceSolidCAM enables you to change the reference to original SolidWorks model. This operation enablesyou to substitute the DesignModel component of the CAM-Part assembly with some SolidWorksmodel. 1. Choose the Change Model Reference command in the menu. The Change Model Reference dialog box is displayed.93
    • 2. Type the model name in the Model name edit box or choose the model with the Browse button. This button displays the browser dialog box that enables you to choose the SolidWorks model. 3. Confirm the dialog box. The following message is displayed. When the message is confirmed, the CAM-Part is closed, the CAM-Part Reference is updated, and then the updated CAM-Part is loaded again.CAM-Part DefinitionThis command enables you to view and edit the values, options and parameters of the currentCAM-Part. The Milling Part Data dialog box is displayed.CAM-Part PropertiesThis command displays the Milling part properties dialog box. This dialogbox provides you with information such as name and location of the CAM-Part and of the model used in the CAM-Part. 94
    • 2. CAM-PartSave AsThis command enables you to save the activeCAM-Part to the disk with a new name or in a newlocation.When this option is chosen, the Save As dialogbox is displayed. Save as Type This option enables you to choose the type of the CAM-Part: compressed or non-compressed. The default value of the Save as Type filter is the same as the type of the original CAM-Part. The conversion of the compressed CAM-Part to non-compressed is unavailable. Save as copy • When this option is not available, the saved CAM-Part is loaded instead of the current CAM-Part. • When this option is available, SolidCAM stays with the current CAM-Part.Recent CAM-PartsThis option displays a list of the lastnine CAM-Parts you worked with inSolidCAM. You can open the file byclicking on its name.95
    • Saving the updated stock in the STL formatSolidCAM parts can be machined in a sequence of stages on different CNC-machines, while theupdated stock model is shared between these stages.This functionality enables you to define a new CAM-Part basedon some other pre-machined CAM-Part, using the result ofmachining of the pre-machined part for the stock definition.Machining of a part can thus be performed in several stages,with one CAM-Part for each stage, by passing the machiningresults from one stage to the next through an updated stockmodel obtained after the last operation of each CAM-Part andsaved in the STL format. 1. Right-click on the CAM-Part header in SolidCAM Manager and choose the Save updated stock to STL command from the menu. 2. The Save updated stock to STL dialog box is displayed. Define the name and location for your file. The default name of the updated stock model STL file is inherited from the CAM-Part name. The default location of the STL file is the SolidCAM Part folder for regular SolidCAM Parts (*.prt). For compressed CAM-Parts (*.prz), the default location is that of the compressed CAM-Part files. 3. Click on the Save button. SolidCAM generates the STL file according to the HostCAD coordinate system. When the STL file is successfully generated, the notification message is displayed. 96
    • 2. CAM-Part2.13 CAM-Part DocumentationThis option enables you to document your tool list,operations sequence, etc. • Generate This option enables you to create the document. • Edit This option enables you to edit the document after it has been generated.2.13.1 Documentation EditorWith the documentation editor you can browse the generated CAM-Part documentation. Thetoolbar and the application menu on the top of the documentation editor work the same as in anytypical windows application.The left panel enables you to switch pages and the right page enables you to view and edit each page. • Cover page This page shows contents of the Cover page file defined in SolidCAM Settings. • Header page This page contains general information about the CAM-Part: the CAM-Part name, the program number, the amount of operations and the type of operations. To edit, simply click in the right field and make any changes or additions.97
    • • Tool Table page This page contains all the relevant information about the tools used in the CAM-Part: the tool number, the tool diameter, the corner radius, the tool type, the number of teeth and any other information that is relevant to each tool. To edit, simply click in the right field and make any changes or additions.• Operations table page This page contains the list of all operations in the CAM-Part.• Operation pages Under this page, there is a page for each operation name. This page gives you a detailed list of all of the fields you have chosen in the operation and their values. 98
    • 2. CAM-Part2.14 Tool sheet documentationThis option enables you to summarize the CAM-Part information by generating a tool sheetdocumentation in the RTF format.For each tool sheet project, SolidCAM creates theDoc folder in the CAM-Part directory for savingthe tool sheet file. In this folder, two subfolders areautomatically created: the Tools Images subfolderfor image files of the tools used in the partoperations, and the Images subfolder for imagefiles of the machined part.The tool sheet generation commands are availablein the right-click menu on the CAM-Part header inthe SolidCAM Manager tree.2.14.1 Capturing the CAM-Part imageThe Capture Image command enables you to create a part image captured from the SolidWorksgraphic area and save it in the PNG format. Later this image file can be attached to your tool sheet.When you choose this command, SolidCAM captures the image of the part as it is displayed in theSolidWorks graphic area. This image is saved as a PNG file in the Images folder.99
    • 2.14.2 Definition of tool sheet parametersThe Tool Sheet command is available for the entireCAM-Part (in the right-click menu available on theCAM-Part header) or for separate operations (in theright-click menu available on each operation entry).The Tool Sheet Extra Parameters dialog box isdisplayed. This dialog box enables you to define andmanage the content of the documentation file.ImagesIn this section, you can specify the logo and part imagefiles in the PNG format that will be attached to yourtool sheet. To attach a logo and/or a part image, clickon the button and choose a file from the standardWindows-style Browse dialog box.The attached logo appears in the upper right corner inthe document header. The attached images appear inthe separate Images page. 100
    • 2. CAM-PartParametersThis section contains the table that enables you to define your own variables and values to beinserted into the tool sheet. In the Label column, you specify the name of the parameter you wantto appear in the tool sheet; in the Value column, you can enter its value. In the Location column,you can specify where this parameter is supposed to appear in the documentation file, either in themain page or in the header.The buttons enable you to manage the table rows: • The button adds new rows to the table. • The button removes the selected row from the table. • The buttons move the selected rows in the table, changing their order.Part notesThis section enables you to add comments and notes related to your part. The note will appearunder the part image, in the main page of the tool sheet document.StyleThis section enables you to define the style of the output document.SectionsThis group enables you to define which elements of the information sheetwill appear in the output, by selecting the corresponding check boxes. • The Main page check box defines whether the main page will be included in the tool sheet.101
    • • The Images check box defines whether the Images page will be included in the tool sheet. The button displays the location of the part captured images in the Windows Explorer.• The Tool table check box defines whether the Tool table pages will be included in the tool sheet. The button displays the dialog box that enables you to specify the required tool data to appear in the Tool table summary by selecting check boxes.• The Operations summary check box defines whether the Operation summary page will be included in the tool sheet.• The Fixtures check box defines whether the Fixture page will be included in the tool sheet. 102
    • 2. CAM-Part2.14.3 The output fileThe output tool sheet file consists of the following sections:Main pageThis section summarizes the general information about the CAM-Part, including its graphicrepresentation and the comments you have added. Comment entered in the Parameters table (Location - Header) Part name Company logo Part definitionComment entered Part picturein the Parameters table(Location - Main page) Part notes Part properties103
    • Tool tableThis section displays the list of the tools used for the operations of the current CAM-Part, withtheir parameters and illustrations. 104
    • 2. CAM-PartOperations summaryThis section summarizes the operations defined for the current CAM-Part.105
    • FixturesThis section shows how the part must be fixed on the CNC-machine table. 106
    • 2. CAM-Part2.14.4 Show Last Tool SheetThis command enables you to display the last generated tool sheet for the current part, instead ofgenerating it anew. The Tool Sheet Extra Parameters dialog box is displayed so that you can view thedefined parameters of the last tool sheet generation.In this dialog box, you can edit only the Style and the Sections parameters to alter the documentappearance and define which sections of the last tool sheet you want to display.The Show button displays the generated tool sheet.107
    • 2.15 Milling STL CAM-PartThis functionality enables you to define the machining projects based on output of 3D scanningdevices in the STL format. The received STL file contains data on the shape and visual propertiesof the scanned real-world object upon which the machining project will be based. Such parts canbe machined using the SolidCAM 3D, HSM and 5-Axis milling capabilities. The peculiarity of suchprojects definition is that the STL graphic body cannot be divided into separate elements in the waya CAD design model can be. Therefore, the definition of such CAM-Part is different from a regularmilling project.2.15.1 Starting a new Milling-STL CAM-Part 1. Click SolidCAM, New, Milling-STL. 2. The New Milling Part dialog box is displayed and enables you to choose an STL file similar to the CAD design file chosen for CAM-Part definition. 3. In the Directory section, you need to specify the path to the location where the CAM-Part will be saved by entering manually or by clicking on the Browse button. 108
    • 2. CAM-Part 4. In the Model name section, click on the Browse button and choose the required STL file. 5. In the Name section, you need to enter the name for your machining project.When you confirm the New Milling Part dialog box, the Milling Part Data dialog box is displayedas for a regular milling project definition. The graphic body is displayed in the SolidWorks graphicarea. It can be zoomed and rotated.109
    • 2.15.2 Coordinate System definitionSimilar to a regular milling CAM-Part, the first definition stage is that of Coordinate System. Clickon the Define button in the Coordinate System section. Since you cannot select separate elementsof the STL graphic body, you can define the Coordinate System by entering the coordinates inthe Define mode (X,Y,Z) and/or by rotating the model into the required view and capturing in theNormal to current view mode (see topic 2.2.2). 110
    • 2. CAM-Part2.15.3 Stock model definitionWhen the Coordinate System is defined, a box is calculated surrounding the model. Using this box,you can define the Stock model with the 3D Box option (see topic 2.4.1).2.15.4 Target model definitionThe target model is defined by clicking on the Browse button in the Choose STL dialog box andchoosing the original STL file from the browser dialog box.When the CAM-Part is defined, you can add 3D Milling, HSM, HSS and 5-Axis operations for itsmachining.111
    • 2.16 Support of DriveWorksThe DriveWorks Design Automation software automates repetitivetasks and allows you to generate your design and manufacturing outputsautomatically. This software is integrated in SolidCAM enabling theautomation of the design-to-manufacture processes.The main principle of the DriveWorks functionality is creating rule-basedtasks for automatic modification of parameters of the parts. Based ona SolidWorks model with given parameters, DriveWorks enables you tocreate similar models with modified parameters and/or features (forexample, size changed, holes removed, etc.).When DriveWorks is used to modify a SolidWorks model on which a SolidCAM Part is based,DriveWorks copies the original model into a separate directory and performs the requiredmodifications. DriveWorks SolidCAM Original CAM-Part Original model Change Reference Model Copy of CAM-Part Modified model Synchronize & Calculate Modified CAM-Part 112
    • 2. CAM-PartAfter this stage, DriveWorks automatically starts SolidCAM, where the original part is copied intothe same location with the updated model. The copied CAM-Part is opened in SolidCAM and thereference model of the opened CAM-Part is automatically replaced with the modified model, thesynchronization is automatically performed and the operations are recalculated.In such manner, machining of new parts with different parameters and features can be performedautomatically using the defined modification rules.For more information about the DriveWorks software, visit www.driveworks.co.uk.113
    • 114
    • Tools andTool Libraries 3The tool commands can be used to create and manage tools and toollibraries in SolidCAM. You can save your programming time if you savethe tools you use most often in customizable tool libraries.The tool libraries can be based on machine tooling, materials or anyother personal criteria. When you define your machining operations,you can then load the tool, and all its parameters, feed and spin valuesare automatically copied into the operation.  Working with Part Tool Table  Working with Current Tool Library  Managing Tool Libraries  Defining tools  Tool types  Shaped tools  Tool holding system
    • 3.1 User-Defined Tool TypesFor easier identification and classification of tools, you can define your own tool types.SolidCAM offers you the following default tool types: • End mill • Ball nose mill • Bull nose mill • Face mill • Dove tail mill • Taper mill • Slot mill • Lollipop mill • Engraving tool • Center drill • Spot drill • Drill • Chamfer drill • Tap • Reamer • Bore • Thread mill • Thread taperUser-defined tool types can also be used to define new tools and to search tool libraries. 116
    • 3. Tools and Tool Libraries3.1.1 End millThis tool type is used for the definition of rough/finish end mills.The tools of this type are defined with the parameters shown in the image. Arbor Diameter TotalLength Outside Holder Shoulder Length Length Cutting Length DiameterThe diameter and the length of the cylindrical arbor are defined as Arbor Diameter and (TotalLength – Shoulder Length), respectively. The Shoulder Length value must be greater than or equalto that of the Cutting Length, and equal to or smaller than that of the Outside Holder Length.When a new tool is created, the default value of the Arbor Diameter is equal to that of the Diameter,and the default value of the Shoulder Length is equal to that of the Cutting Length.117
    • 3.1.2 Ball nose millA tool of this type is defined with the parameters shown in the image. Arbor Diameter TotalLength Outside Shoulder Holder Length Cutting Length Length Diameter Corner RadiusThe Corner Radius value of a Ball nose mill tool is equal to half the Diameter value and cannot bechanged.The diameter and the length of the cylindrical arbor are defined as Arbor Diameter and (TotalLength – Shoulder Length), respectively. The Shoulder Length value must be greater than or equalto that of the Cutting Length, and equal to or smaller than that of the Outside Holder Length.When a new tool is created, the default value of the Arbor Diameter is equal to that of the Diameter,and the default value of the Shoulder Length is equal to that of the Cutting Length. 118
    • 3. Tools and Tool Libraries3.1.3 Bull nose millA tool of this type is defined with the parameters shown in the image. Arbor Diameter TotalLength Outside Shoulder Holder Length Cutting Length Length Diameter Corner RadiusThe Corner Radius value of a Bull nose mill tool must be in the range from 0 to half the Diametervalue.The diameter and the length of the cylindrical arbor are defined as Arbor Diameter and (TotalLength – Shoulder Length), respectively. The Shoulder Length value must be greater than or equalto that of the Cutting Length, and equal to or smaller than that of the Outside Holder Length.When a new tool is created, the default value of the Arbor Diameter is equal to that of the Diameter,and the default value of the Shoulder Length is equal to that of the Cutting Length.119
    • 3.1.4 Dove tail mill Outside Arbor HolderThis tool type is used for dove tail slot machining. Diameter LengthA tool of this type is defined with the parameters Shouldershown in the image. Length Total Angle Length Cutting Length Corner Radius DiameterParameter limitations Parameter Range Angle 0° < Angle < 90° Corner Radius Corner Radius <= Diameter/2 Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length 120
    • 3. Tools and Tool Libraries3.1.5 Face mill Arbor Diameter Total LengthThis tool type is used for facemilling. A tool of this type isdefined with the parameters shown Shoulder Outsidein the image. Length Holder Length Cutting Length Angle Tip Diameter DiameterParameter limitations Parameter Range Tip Diameter Tip Diameter < Diameter Angle 0° < Angle < 90° Corner Radius <= Cutting Length Corner Radius Corner Radius <= Tip Diameter/2 Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length121
    • 3.1.6 Slot mill Arbor DiameterThis tool is used in a variety of applicationsfrom simple 2.5D undercut profiles all the wayup to machining cavities in Simultaneous 5 Axisoperations. The parametric definition of a slot Totalmill tool also enables you to define a cylindrical Length Outside Holdertool with a tool shank with a relieved diameter. LengthA tool of this type is defined with the parametersshown in the image. Corner Cutting Radius Length Diameter 122
    • 3. Tools and Tool Libraries3.1.7 Taper mill Outside Holder LengthThis tool type is supported in the calculations of Arborthe Sim. 5 Axis and 3D Milling Rough and Finish Diameteroperations. In 2.5D Milling operations such as AngleProfile and Pocket, only the bottom diameter istaken into account in the tool path calculation.This tool is used for milling internal or externalwalls with a constant draft angle. Total Length Shoulder Length CuttingA tool of this type is defined with the parameters Lengthshown in the image. ConeThe diameter and the length of the cylindrical tool Lengtharbor are defined as Arbor Diameter and (Total DiameterLength – Shoulder Length), respectively. TheShoulder Length value must be greater than or Tip Cornerequal to that of the Cutting Length, and equal to Diameter Radiusor smaller than that of the Outside Holder Length. • The default Arbor Diameter value is equal to that of the Diameter; • The Shoulder Length value is equal to that of the following expression: Cutting Length + (Outside Holder Length – Cutting Length)/2.To define the taper tool by Tip diameter or by Cone Length, select the appropriate check box nearthe Tip Diameter or the Cone Length edit boxes.When the Tip Diameter check box is selected, the Cone Length check box is unselected and therelevant edit box is disabled; the Cone Length value is thus automatically calculated.123
    • When the Cone Length check box is selected, the Tip Diameter check box is unselected and therelevant edit box is disabled; the Tip Diameter value is thus automatically calculated. Note that the Tip Diameter is the diameter of the virtual intersection of the conical shape with the bottom plane. Tip DiameterParameter limitations Parameter Range Tip Diameter Tip Diameter < Diameter Angle 0° < Angle < 180° Corner Radius <= Tip Diameter/2 Corner Radius Corner Radius < Cone length Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length 124
    • 3. Tools and Tool Libraries3.1.8 Engraving tool Arbor DiameterThis tool type is used for engraving. A toolof this type is defined with the parametersshown in the image. Total Length Diameter Outside Holder Shoulder Length Length Cutting Length Angle Tip Diameter Corner RadiusParameter limitations Parameter Range Angle 0° < Angle < 90° Corner Radius Corner Radius <= Diameter/2 Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length125
    • 3.1.9 Tap toolThis tool is used to machine the internal threadsin Drilling operations. It consists of two parts: Arbor Diametercylindrical and conical. A tool of this type is definedwith the parameters shown in the image. Total Length Outside Holder Length Chamfer Cutting Length Length Tip Diameter DiameterThe diameter and the length of the cylindrical tool arbor are defined as Arbor Diameter and (TotalLength - Shoulder Length), respectively. The Shoulder Length value must be greater than or equalto that of the Cutting Length, and equal to or smaller than that of the Outside Holder Length. Thedefault Arbor Diameter value is equal to that of the Diameter, and the Shoulder Length value is equalto that of the Cutting Length.Parameter limitations Parameter Range Tip Diameter Tip Diameter < Diameter Chamfer Length Chamfer Length < Cutting Length Pitch 0 < Pitch < min (Diameter, Cutting Length) Cutting Length Cutting Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length This tool can be used only in Drilling/3D Drilling operations. 126
    • 3. Tools and Tool Libraries3.1.10 Lollipop millThis tool is used in the Simultaneous 5 Axis operations. There are two shapes of the lollipop milltool: with conical shoulder and without one. A tool of this type is defined with the parametersshown in the image. Arbor Diameter Arbor Diameter Total TotalLength Length Outside Outside Holder Holder Shoulder Length Length Length Shoulder Cutting Cutting Length Length Length Diameter DiameterLollipop mill without conical shoulderWhen the Conical shoulder check box is not selected, SolidCAM enables you to define the tool withthe cylindrical shoulder.The diameter and the length of the cylindrical arbor are defined asArbor Diameter and (Total Length – Shoulder Length), respectively.The Shoulder Length value must be greater than or equal to that ofthe Cutting Length, and equal to or smaller than that of the OutsideHolder Length. The default Arbor Diameter value is equal to thatof the Diameter. The Shoulder Length value is equal to that of theCutting Length.127
    • Lollipop mill with conical shoulderWhen the Conical shoulder check box is selected, SolidCAM enables you to define the tool with theconical shoulder.The Arbor diameter value defines the upper diameter of the cone. The lower diameter of the coneis calculated automatically as the diameter of the circle resulting from section of the sphere by thehorizontal plane located at the Cutting length distance from the tool nose. The cone starts from theCutting length distance and continues till the Shoulder length distance. Therefore, the cone length isequal to the difference between the Shoulder length and Cutting length parameters.Parameter limitations Parameter Range Cutting Length <= (Diameter+sqrt(Diameter^2-Arbor Diameter^2))/2 Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Outside Holder Length <= Total Length Length 128
    • 3. Tools and Tool Libraries3.1.11 Thread mill Arbor DiameterThis tool is intended to machine the internal andexternal threads in Thread Milling operations.The following parameters define the geometry of Totalthread mill tools. Length Outside Holder Length Shoulder Length Thread Diameter Thread Cutting LengthPitchSolidCAM enables you to define the Pitch of the thread as a Metric value (MM) or as a number oftracks per inch (TPI).When defining the tool parameters in the Part Tool Table, you can define the Pitch in accordancewith international standards such as ISO, Whitworth, and so forth.In the Pitch/Standard field, choose the Table option and click on thearrow to open the list and choose the standard according to which youwant to define the thread pitch. This list is available only if the Threading table is defined in the SolidCAM Settings dialog box (see topic 12.2.3).When you choose one of the standards from the list, thecorresponding table is displayed in a separate window.129
    • Choose the required value and confirm with the OK button. You can open this table as an Excel file and edit its content. The path to the table file can be found on the User directories page of the SolidCAM Settings dialog box (see topic 12.2.3).SolidCAM provides you with a link to the Vardex software for thread milling tool selection fromthe Vardex tools library – TM Gen (www.vardex.com). This link enables you to define the thread milltool parameters and, based on this, it will search the Vardex library for the thread milling tools thatfit these parameters; you can then choose one of the offered tools for the operation.When the Vardex option is chosen in the Standard combo box, SolidCAM launches the Vardextool library wizard (TM Wizard). The wizard guides you through the steps to define the parametersof the tool you are looking for, selects a number of tools from the library that fit these parametersand then enables you to choose one of these tools. When the tool is chosen, it is imported into theSolidCAM tool library. 130
    • 3. Tools and Tool Libraries3.1.12 Thread taper ArborA tool of this type is defined with the parameters shown Diameterin the image. The Thread taper tool definition is similarto the Thread Mill tool definition (see topic 3.1.11). Total Angle Length Outside Holder Length Shoulder Length Thread Diameter Thread Cutting Length3.1.13 Drill Arbor DiameterThis tool type is used for the definition of drills, bores,reams, threading tools, etc. A tool of this type is definedwith the parameters shown in the image. Total Outside Length Shoulder Length Cutting Holder Length Length Angle DiameterThe diameter and the length of the cylindrical tool arbor are defined as Arbor Diameter and(Total Length – Shoulder Length), respectively. The Shoulder Length value should be greater thanor equal to the Cutting Length value, and equal to or smaller than the Outside Holder Length value.When a new tool is created, the default Arbor Diameter value is equal to that of the Diameter. Thedefault Shoulder Length value is equal to that of the Cutting Length.131
    • 3.1.14 Center drill ArborThis tool type is used for center drilling in Drilling Diameteroperations. A tool of this type is defined with theparameters shown in the image. Shoulder Angle Total Outside Length Holder Length Cutting Length Angle Tip Diameter Tip LengthWhen this tool is used in combination with the Use chamfer option, SolidCAM calculates thedrilling depth according to the following expression:Drilling Depth = Tip Length + Arbor Diameter/2 + cotan(Shoulder Angle/2) Arbor DiameterCutting Length Shoulder Angle Chamfer Diameter Drilling Depth Tip Diameter Tip Length Chamfer Diameter 132
    • 3. Tools and Tool LibrariesParameter limitations Parameter Range Tip Diameter Tip Diameter < Arbor Diameter Tip Angle 0° < Tip Angle < 180° Shoulder Angle 0° < Shoulder Angle < 180° Tip Length Tip Length <= Cutting Length Cutting Length Cutting Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total LengthThe length of the conical part defined by Tip Diameter and Tip Angle must be equal to or smallerthan the Tip Length value. The length of conical part can be calculated according to the followingexpression: Cone Length = Tip diameter/(2*tan( Tip angle/2)).133
    • 3.1.15 Spot drill Arbor DiameterThis tool type is used for center drilling andchamfering. A tool of this type is defined with the Diameterparameters shown in the image. Total Outside Length Holder Shoulder Length Length Angle Cutting LengthParameter limitations Parameter Range Angle 0° < Angle < 180° Tip Length Tip Length <= Cutting Length Cutting Length Cutting Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length Note that the Cutting Length edit box is unavailable. This value is calculated automatically according to the Diameter and Angle values. 134
    • 3. Tools and Tool Libraries3.1.16 Chamfer drill Arbor DiameterThis new tool type is used for chamfering. A toolof this type is defined with the parameters shownin the image. Total Length Outside Shoulder Holder Length Length Cutting Length Angle DiameterParameter limitations Parameter Range Corner Radius Corner Radius <= Cutting Length Angle 0° < Angle < 180° Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length135
    • 3.1.17 Reamer Arbor DiameterThis tool is used to machine precise holes in Drillingoperations. A tool of this type is defined with theparameters shown in the image. Total Outside Length Holder Length Cutting Length Chamfer Diameter LengthThe diameter and the length of the cylindrical tool arbor are defined as Arbor Diameter and(Total Length – Shoulder Length), respectively. The Shoulder Length value must be greater than orequal to that of the Cutting Length, and equal to or smaller than that of the Outside Holder Length.The default Arbor Diameter value is equal to that of the Diameter.Parameter limitations Parameter Range Cutting Length Chamfer Length <= Cutting Length <= Outside Holder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length 136
    • 3. Tools and Tool Libraries3.1.18 Bore Arbor DiameterThis tool type is used for boring inDrilling operations. A tool of thistype is defined with the parametersshown in the image. Total Outside Length Holder Diameter Length Shoulder Length Corner Radius Cutting Angle LengthParameter limitations Parameter Range Corner Radius Corner Radius <= Cutting Length Angle 0° < Angle < 90° Cutting Length Cutting Length <= Shoulder Length Shoulder Length Shoulder Length <= Outside Holder Length Outside Holder Length Outside Holder Length <= Total Length137
    • 3.1.19 Shaped ToolsThis tool type is used for the definition of shaped end/rough mills and drill tools. The tool shapeis defined by a sketch. The Tool Diameter defined in the Part Tool Table describes the cuttingdiameter of the shaped tool that will be coincident to the machining geometry.For more information on Shaped tools, see topic 3.10.3.1.20 Add new tool typesBased on one of the default tool types, you can create your own ones. 1. Click SolidCAM in the SolidWorks main menu and choose Tool Library, Tool type names. The Tool Type Names dialog box is displayed. This dialog box shows the user-defined tool type names and their actual SolidCAM default internal tool types. 2. In the Tool Type Names dialog box, right-click on an existing tool type name, e.g. End Mill. 3. Choose Add from the menu. 4. A new entry is created. Enter the name of the user-defined tool type. 5. By default, the new entry is of the Drill tool type. Right-click on the Drill field and select the relevant tool type from the list. 138
    • 3. Tools and Tool Libraries 6. When you finished making changes in the Tool type list, click on the Save button to confirm your changes. Double-click the tool type name to rename existing entries.3.1.21 Tool type optionsYou can manage the user-defined tool types in the list. 1. In the Tool Type Names dialog box, right-click an existing tool type name. 2. Choose the Add or Rename option from the menu.139
    • 3.2 Tool LibrariesThe tool libraries can be based on machine tooling, materials or any other personal criteria. Whenyou define your machining operations, you can then load the tool, and all its parameters, feed andspin values are automatically copied to the operation.The Part Tool Table is the tool library that contains all tools available for use in a specific CAM-Part.The Part Tool Table is stored within the CAM-Part.When you start a new CAM-Part and you want to copy the contents of a specific tool library intothe Part Tool Table of this CAM-Part automatically, specify its name in the MAC file of the CNC-machine. This file is called the Machine Tool Table. The Machine Tool table is defined in the MAC file by the following parameter: tool_table_name = name; where name (without an extension) is the name of the Tool Library located in the SolidCAM Tool Libraries folder defined in the SolidCAM Settings (see topic 12.2.2).Generally, the Machine Tool Table contains the tools situated in the Tool Magazine of the specifiedCNC-machine.SolidCAM enables you to define anynumber of Tool Libraries. Each tool Operation Operation Operationfrom the Tool Libraries can be importedinto the Part Tool Table. You can define Tool Tool Toolone Tool Library that has a top priority CAM-Partin the list for import: the Current Tool Part Tool TableLibrary. Tools imported at start Tools imported at user choise Machine Tool Table Current Tool Library Tool Library Tool Library Tool Library Tool Library Tool Library 140
    • 3. Tools and Tool Libraries3.3 Working with the Part Tool TableThe Part Tool Table is the tool library that contains all tools available for use in a specific CAM-Part.The Part Tool Table is stored within the CAM-Part.The Part Tool Table dialog box (see topic 3.6) enables you to manage the tools contained in the PartTool Table. 1. Choose the Part Tool table option from the right-click menu of the Tool header in SolidCAM Manager. 2. The Part Tool Table dialog box is displayed.141
    • 3.4 Working with the Current Tool LibrarySolidCAM enables you to manage your Current ToolLibraries using the right-click menu of the Tool header inSolidCAM Manager. • Set Tool Library This option enables you to set the Current Tool Library. You have to specify the type of the Current Tool Library (Milling, Turning or Turn-Mill) and choose the relevant Tool Library from the browser dialog box. The Current Tool Library is selected and displayed in the Tool Table dialog box (see topic 3.6). • Close Tool Library This option enables you to close the Current Tool Library. This option is available only when the Current Tool Library is already defined. • Show Tool Library This option enables you to display the content of the Current Tool Library. The Tool Table dialog box enables you to manage the tools in the Current Tool Library. This option is available only when the Current Tool Library is already defined. • Recent Tool Libraries This option displays the list of recently loaded Current Tool Libraries. You can open a file by simply clicking on its name in the list. The Tool Table dialog box is displayed. 142
    • 3. Tools and Tool Libraries3.5 Managing Tool LibrariesSolidCAM enables you to manage your Tool Libraries usingthe Tool Library menu available in the SolidCAM main menu.3.5.1 Edit Tool LibraryThis option enables you to display the content of the specific Tool Library.When you choose this option, the Load dialog box isdisplayed. 1. Select the name of the tool library you want to load. 2. Double-click on its name or select it and click on the Open button. The Tool Table dialog box is displayed. This dialog box enables you to manage the tools in the chosen Tool Library.3.5.2 Create Tool LibraryThis option enables you to define a new Tool Library. 1. Choose the Tool Library type (Milling, Turning or Turn-Mill) from the submenu.143
    • 2. Define the Tool Library name. 3. Confirm the Tool Library creation with the OK button. The Tool Library is created. The Tool Table dialog box is displayed enabling you to add tools to the new Tool Library. 4. Confirm the Tool Table dialog box with the OK button.3.5.3 Copy Tool LibraryThis option enables you to create an identical copy of a tool library in another folder or drive forbackup purposes or for making modifications without changing the original. The Copy Tool Librarydialog box is displayed. 1. In the left window, choose the drive and directory from which you want to copy the original tool library. 2. Select the tool library you want to copy. 3. Move the selection of tool libraries you want to copy to the middle window by clicking the Left to Right arrow. 4. Choose the drive and the directory into which you want to copy in the right window. 5. Click on the Copy button. 144
    • 3. Tools and Tool Libraries3.5.4 Delete Tool LibraryThis field enables you to delete tool libraries. The Delete dialog box is displayed. 1. Select the tool libraries you want to delete. Use the Ctrl key to select several tool libraries together. 2. Click on the Delete button. 3. The confirmation message is displayed: 4. Choose Yes or Yes to All to delete all selected tool libraries.145
    • 3.6 Tool Table dialog boxThe Tool Table dialog box containsstructured information about all toolsincluded in the specified Tool Library. Thisdialog box enables you to add new tools tothe Tool Library, remove tools from theTool Library, edit the tool definition, etc.The dialog box contains two pages: • View This page displays the tools of the Tool Library in a table format. • Edit This page enables adding of new tools or editing of existing tools in the Tool Library.3.6.1 Tools FilterSolidCAM enables you to filter toolsdisplayed in the Tool Table dialog box. • All All the tools are displayed. • Used Only the tools used in Operations of the current CAM-Part are displayed. • Unused Only the tools unused in operations of the current CAM-Part are displayed. The filter is available only for the Part Tool Table. 146
    • 3. Tools and Tool Libraries3.6.2 Tool rangeIf you work with large tool libraries, you canuse this option to reduce the number of toolsdisplayed. You can also search the tool table fortools that match your criteria. In the Range dialog box, enter the required properties of the tool. Enter only values that are different; leave the other fields unchanged.The User-defined tool type section enables you tochoose the type of tools you would like to havelisted in the tool library.The Rough tools only and Do not display roughtools options enable you to handle Rough tools(see topic 3.6.5) during the tools sorting. • The Rough tools only option enables you to display only rough tools in the tools list. • When the Do not display rough tools check box is selected, the tools marked as Rough are not displayed.The Tool number section lists results according to the tool numbers.The Diameter section enables you to choose the range using the diameter of the tools you wouldlike to have listed in the tool library. If, for example, you would like to list the tools with a diameterfrom 1 to 16, enter 1 in the From box and 16 in the To box.The Number of flutes section enables you to choose the range using the number of flutes of thetools you would like to have listed in the tool library. If, for example, you would like to list the toolswith 1 to 4 flutes, enter 1 in the From box and 4 in the To box.The Pitch section enables you to choose the range using the pitch of the tap tools you would like tohave listed in the tool library. If, for example, you would like to list the tap tools with the Pitch from0.5 to 1.5, enter 0.5 in the From box and 1.5 in the To box.The Arbor diameter section enables you to choose the range using the arbor diameter of the toolsyou would like to have listed in the tool library. If, for example, you would like to list the tools withan arbor diameter from 1 to 16, enter 1 in the From box and 16 in the To box.147
    • The Taper angle section enables you to choose the range using the taper angle of the tools youwould like to have listed in the tool library. If, for example, you would like to list the tools that havea taper angle from 20° to 30°, enter 20 in the From box and 30 in the To box.The Number of threads section enables you to choose the range using the number of threads of thetools you would like to have listed in the tool library. If, for example, you would like to list the toolswith 2 to 4 threads, enter 2 in the From box and 4 in the To box.The ID number section enables you to choose the range of the ID numbers of the tools you wouldlike to have listed in the tool library. If, for example, you would like to list the tools with an IDnumber from 10 to 100, enter 10 in the From box and 100 in the To box.The Corner radius section enables you to choose the range using the corner radius of the tools youwould like to have listed in the tool library. If, for example, you would like to list the tools that havea corner radius from 0 to 4, enter 0 in the From box and 4 in the To box.The Angle section enables you to choose the range using the angle of the tools you would like tohave listed in the tool library. If, for example, you would like to list the tools that have an angle from90° to 180°, enter 90 in the From box and 180 in the To box.The Chamfer length section enables you to choose the range using the chamfer length of the toolsyou would like to have listed in the tool library. If, for example, you would like to list the tools thathave a chamfer length from 2 to 5, enter 2 in the From box and 5 in the To box.The Tip diameter section enables you to choose the range using the tip diameter of the tools youwould like to have listed in the tool library. If, for example, you would like to list the tools that havea tip diameter from 5 to 10, enter 5 in the From box and 10 in the To box.The Tip length section enables you to choose the range using the tip length of the tools you wouldlike to have listed in the tool library. If, for example, you would like to list the tools that have a tiplength from 5 to 10, enter 5 in the From box and 10 in the To box.Click on the Execute button to start searching the tool library for the tools that meet yourrequirements. SolidCAM will return to the tool library and display the result of the range search.The Reset to defaults button returns you to the original program settings of this dialog box.3.6.3 ShowThis button enables you to display the selected tool. 148
    • 3. Tools and Tool Libraries3.6.4 ViewTool dataThis page displays the tool data in the tableformat. The table contains the followingcolumns: • Tool Number This column displays the number of a tool in the Tool Library. • ID Number This column displays the ID number of a tool. • User-defined tool type name This column displays the tool type. • Description This column displays the description of a tool.This page also displays the geometric parameters of a tool depending on its type.3.6.5 EditThis page enables you to edit the existingtools in the Tool Library (see topic 3.7).149
    • Rough toolsSolidCAM enables you to define rough tools of all the following types: • End mill • Bull nose mill • Ball nose mill • Face mill • Taper mill • Slot mill • Drill • Bore • Dove tail millThe Rough check box enables you to mark the tool as suitable forrough milling. The Rough status of the tool can be used for the toolssorting with the Range option (see topic 3.6.2).Tool unitsYou can assign different unit of measurement data for each tool in thetool library. The tool library can simultaneously store tools with Metricparameters along with those defined in Inches. This functionalityenables you to use tools defined in units different from those of theCAM-Part, without converting the tool parameters into the CAM-Partunits. You can choose the units for the tool diameter values and toollengths separately.The Mm and Inch buttons enable you to switch between the Metric andthe Inch system of measurement. 150
    • 3. Tools and Tool Libraries When a tool library created in a previous SolidCAM version is loaded, the following message is displayed: When you confirm this message, the Assign Units dialog box is displayed so that you can assign units for tools.Angular dimensionsThe button appears in theparameters with angular values.By clicking this button, you can switchthe angle value from the degrees/minutes/seconds format to the decimalformat and vice versa. In the first case,the edit box that displays the value isdisabled.When the value is displayed as a decimal,the edit box is available, and the valuecan be edited.151
    • 3.7 Managing toolsSolidCAM enables you to manage the tools in the tool library with the buttons at the bottom of thedialog box.All these commands are also available in the right-click menu. Permanent Tool If a particular tool is always used in the same magazine position in the machine, this tool can be marked as Permanent Tool. If you use the Tool Renumbering function, a tool marked as Permanent Tool is not renumbered. Add Tool This option enables you to add a new tool to the tool library. When you choose this option, the Tool Type dialog box is displayed so that you can choose the tool type. When you click on a tool to add it to the library, the Tool Type dialog box is closed automatically and the Part Tool Table is displayed again. 152
    • 3. Tools and Tool Libraries Change tool type This option enables you to add the type of the existing tool. When you choose this option, the Tool Type dialog box is displayed so that you can choose the required tool type. Copy Tool This option enables you to create a copy of an existing tool. Delete Tool This option enables you to delete the selected tool. Renumber Tools This option enables you to perform automatic tool renumbering. When the tool numbers in the list are not sequential increments of 1, this option enables you to renumber the tools sequentially by increments of 1. The tools can also be renumbered starting from a specific number that you choose. 1. Right-click on a tool in the list and choose the Renumber Tools command, from the menu, or click on the Renumber button at the bottom of the dialog box. 2. You are prompted to enter a new number for the first tool. The Sort by option enables you to assign numbers to tools according to the operation sequence or the Tool sequence. When you confirm the Tools Renumbering dialog box, the tools are renumbered accordingly, starting from the number of the first tool.153
    • 3. Recalculate the CAM-Part. The CAM-Part must be recalculated to ensure that the GCode contains the correct tool number for each operation. A tool marked as Permanent tool is not renumbered.Import Tool This option enables you to import tools to the Tool Library from the Current Tool Library or any other Tool Library. The Tool Libraries list is displayed. The Current Tool Library, which is the first in the list, is automatically chosen. You can choose the location of the Tool Libraries for the tools import. The Library name box enables you to choose the Tool table for the tools import. The File type box enables you to import tools from SolidCAM Tool libraries, Excel files and from CSV files. If the Current Tool Library is defined, it is automatically chosen as a source for tool import. The Tool list displays all the tools contained in the specified tool library. The right-click menu is available. The Copy to Table option imports the selected tools to the Tool Library. To import all tools from the list, click Copy all to Table. 154
    • 3. Tools and Tool Libraries Update to Machine tool table This option enables you to update the Machine Tool Table with the tools of an active Tool Library. This option is available only when: • The Tool Table dialog box is loaded outside the operation. • The Machine Tool Table is defined in the MAC file. The Update to Machine tool table dialog box is displayed. This dialog box displays the name of the Machine Tool Table. The Used Tools only option enables you to update the Machine Tool Table only with the tools used in operations. Update of the tools is affected by the Tool search parameters defined in the SolidCAM Settings. The system compares the tool parameters with corresponding check boxes selected and performs the update accordingly. Export all tools This option enables you to export all the tool data to an Excel-compatible file (*.xls, *.csv). Export selected tools This option enables you to export the data of the selected tools to an Excel-compatible file.155
    • 3.8 Tool dataSolidCAM enables you to define the Tool with the following data: • Geometric parameters; • Tool material; • Feed and Spin defaults; • Tool holder. Tool definition Tool material Speed and Feed Tool Holder Geometry definition L H R DThe Tool Data area displays the parameters of the selected tool. 156
    • 3. Tools and Tool LibrariesThe Tool Topology page contains the Topology data of the tool, such as diameter, length, angle,corner radius, etc.The Default Tool Data page contains the default Tool Material data, Feed and Spin data and diameterand length offset numbers.The Tool Message page contains fields, in which user messages are entered.The Tool Coolant page enables you to choose the coolant options that will be used by default forthe current tool.The Holder page enables you to define the tool holder by choosing it from the global or local tooltable and specifying the related parameters.The Shape page enables you to choose a shaped tool for the operation.3.8.1 Tool Topology pageTool numberThe Tool number is a numerical identifier of the tool, i.e. the numerical name of the tool, whosevalue has to be an integer. It enables you to define tool numbers according to the numbering systemthat you are used to. The Tool number is used in the GCode when the tool changes, the tool lengthand radius values for tool compensation (G4x) are read from the machine controller.The Max_Tool_Number parameter in the MAC file defines the total number of tools that can bedefined. In other words, this parameter defines the capacity of the cutter magazine of your CNC-machine.157
    • SolidCAM checks the total number of tools in the Part Tool Table during the following operations: • Adding, copying or importing tools; • Loading the CAM-Part; • Inserting Machining Process; • Creating new tools by AFRM.When the total number of tools exceeds the Max_Tool_Number, SolidCAM displays an errormessage.The Tools in list field displays the total number of tools defined in the Tool Library.ID numberYou can use any number, e.g. the catalog number of the tool to facilitate its identification. When a new tool is defined, SolidCAM sets the Tool number to the first unused number. This default Tool number can be changed. When you change the Tool number, make a note that this parameter has to be unique for each tool.If a particular tool always has the same number and cannot be changed, this tool can be marked asPermanent. For example, when the Tool number represents the number of a tool magazine pocketused for the tool, the Permanent mark means that the tool is always located in this pocket.If you use the Tool Renumbering function (see topic 3.7), a tool marked as Permanent is notrenumbered.DiameterThis field defines the cutting diameter of the tool.Corner Radius/AngleWhen the tool type is End mill/Ball nose mill/Bull nose mill, the Corner Radius field is displayed.When the tool type is Drill, the Angle field is displayed. 158
    • 3. Tools and Tool Libraries • Corner Radius This field defines the corner radius of the tool. There are three possibilities: R R D D D In Ball nose mills, the In Bull nose mills, the corner In End mills, the corner corner radius is equal to the radius is smaller than the radius is zero. radius of the tool. radius of the tool. • Angle This field defines the drill point angle of the tool (between 0.01 and 180 degrees). DArbor diameterThis field defines the diameter of the tool arbor. A Arbor diameter This parameter is relevant only for Slot, Lollipop and Taper tools.Thread diameterThis field defines the diameter of the thread of the Tap tool.Tip DiameterThis field defines the lower diameter of the conical part of the Tap tool.159
    • Chamfer lengthThis field defines the length of the conical part of theTap tool.Pitch Total LengthThis field defines the pitch of the Tap tool. The Pitch Chamfer Cutting Lengthis the distance between corresponding vertices of Lengthadjacent teeth of a thread. The Thread diameter, Tip Tip Diameter diameter, Chamfer length and Thread Diameter Pitch parameters are relevant only for Tap tools.LengthThis field defines the length of the tool. In milling calculations, the system does not use this data;the length of the tool is only the output to the GCode file. Total Length Cutting Length Outside Holder Length • Total The total tool length. • Outside Holder The length of the tool outside the tool holder. • Cutting The length of the cutting part of the tool. 160
    • 3. Tools and Tool Libraries • H Length Spindle The distance from the tool end to the CNC-machine spindle.Number of flutesThis field defines the number of teeth of the tool.This field is used when calculating the feed in the Feedrate type FZ. H length Tool Holder For Tap tools, the Number of flutes value is always 1. The value cannot be edited.DescriptionThis field enables you to enter a description of the tool (up to 40 characters).3.8.2 Default Tool Data pageTool materialThis field describes one or more of the following properties of the tool: • The Material of the tool (High Speed Steel, Carbide, etc.); • The Working conditions of the tool; • The Use of the tool (rough, finish, etc.).161
    • The Tool material is used to define the Speed and Feed defaults.When you choose the Tool material, the feed type is changed to FZ and the spin type to V. The Feedand Spin values are default system values since the Work material has not been defined yet. Loadingthe tool to an operation connects the Tool material to the Work material and the correct Feed andSpin values are loaded from the Speed/Feed defaults table.For Tap tools, the FZ value does not depend on the Tool Material. The Spin Rate value can becustomized for different Tool Materials. In this case, changing the Tool Material changes the SpinRate. Since the Spin Rate value is part of the formula of the F calculation, the F parameter valuehas to be recalculated.SpinThis field defines the spinning speed of the tool. It defines two spin values: • Spin Rate – Normal spin rate; used in rough milling. • Spin Finish – Finish spin rate; used in finish milling.The Spin finish check box enables you to optionally define different values for Spin rate and Spinfinish. When this check box is selected, the corresponding edit box is available so that you can editits value. When this check box is not selected, the specified Spin rate value is used for both roughand finish machining. For Drill and Tap tools, the Spin Finish parameter is not relevant.The spin value can be defined in two types of units: S and V.S is the default and it signifies Revolutions per Minute. V signifies Material cutting speed in Meters/Minute in the Metric system or in Feet/Minute in the Inch system; it is calculated according to thefollowing formula:V = (S * PI * Tool Diameter) / 1000 (for the Metric system);V = (S * PI * Tool Diameter) / 12 (for the Inch system).FeedThis field defines the feed rate of the tool. It defines three feed values: • Feed XY – Feed rate in the XY plane. • Feed Z – Feed rate in the Z direction. • Feed Finish – Feed rate used for finish milling. 162
    • 3. Tools and Tool LibrariesThe Feed finish check box enables you to optionally define different values for Feed XY and Feedfinish. When this check box is selected, the corresponding edit box is available so that you can editits value. When this check box is not selected, the specified Feed XY value is used for both roughand finish machining.For Drill and Tap tools, the Feed XY and Feed Finish parameters are not relevant.The feed value can be defined in two types of units: F and FZ.F is the default and it signifies Units per minute. FZ signifies Units per tooth and is calculatedaccording to the following formula:FZ = F/(Number of Flutes * S) For Tap tools, SolidCAM automatically calculates Feed Z (F and FZ) according to the following formulas: F=Spin Rate * Pitch FZ=PitchCalculated values are displayed in Feed Z field. These values cannot be changed. The F/FZ buttonsenable you to check the parameter values.3D Model - entry onlyWhen this check box is selected, the defined Feed Z is used for vertical movements only.When this check box is not selected, the defined Feed Z is used for all movements when theZ-coordinate changes. This option is available only for 3D Milling operations.Diameter offset numberThis parameter defines the number of the Diameter Offset Register of the current tool in theOffset table of the CNC-machine.Length offset numberThis parameter defines the number of the Length Offset Register of the current tool in the Offsettable of the CNC-machine.163
    • Second offset numberThis parameter defines the register number of the upper cutting face offset, in the offset table ofthe CNC-machine. This option enables SolidCAM to automatically take into account the minor sizedifferences between the defined tool and the one actually used for cutting the workpiece, if thereare any. You may choose not to use this option by clearing the check box. This option is available only for T-Slot operations.3.8.3 Tool Message pageIn this page, you can enter text messages for the GCode.The text strings entered in the Message 1 – Message 5 fields appear in the GCode file to help youeasily find information related to the tool in the GCode file when converting from one machine toanother. 164
    • 3. Tools and Tool Libraries3.8.4 Holder pageThis page enables you to choose the tool holder parts from the tool holders table (for moreinformation on the tool holders use, see topic 3.9).To activate the options, select the Use Holder check box. The tool adaptor is defined in the MAC file according to your CNC-machine. If the tool adaptor is not described in the MAC file, the first tool adaptor from the table is used.Global holders tableThe Tool Holders dialog box is displayed so that you can choose the tool holder components fromthe Global holders table. The selected tool is copied to the Local holders table related to the currentCAM-Part, and its parameters are displayed in the Tool adaptor and Tool extension fields after youconfirm the Tool Holders dialog box.Local holders tableThis option enables you to choose the tool holder component previously used in the current CAM-Part from the Local holders table. The Tool Holders dialog box is displayed. The parameters of theselected tool are displayed in the Tool adaptor and Tool extension fields after you confirm the ToolHolders dialog box.Shape EditThis option enables you to change dimensions of the selected clamping adaptor. The Tool Holdersdialog box is displayed. Click on the Edit page to modify the parameters of the tool holder.165
    • 3.8.5 Tool Coolant pageThis page enables you to choose the coolant options that will be used by default for the current tool.When a tool is chosen for use in a specific operation, the default coolant options are automaticallyapplied to the tool use in this operation. The tool coolant options can be changed for each operation.All the existing coolant types are listed with corresponding check boxes. When a check box isselected, the related coolant option is used.The coolant options available for use on the current CNC-machine, according tothe MAC-file settings, are marked with asterisks (*).The Minimum Quantity Lubrication edit box is enabled only when the correspondingcheck box is selected. The default value of this parameter is 0; the possible values are integers inthe range from 0 to 99999. When the entered value is out of range, the error message is displayed.When a new tool is defined, it is assigned the default tool coolant options according to the followingrules: • When a tool is created in the Part Tool Table, it is assigned the options according to the Part Settings. • When a new tool is defined not in context of CAM-Part (all the tool tables except for the Part Tool Table), it is assigned the options according to the SolidCAM Settings. 166
    • 3. Tools and Tool LibrariesWhen a tool is defined in the Part Tool Table with the coolant options not supported by the currentCNC-machine, a notification message is displayed when you confirm the Part Tool Table dialog box.The Yes button returns you to the Part Tool Table dialog box to edit the coolant options. The Nobutton confirms the defined coolant options and continues the process. The GCode will not begenerated for the tool coolant options that are not supported.3.8.6 Shape pageThis page enables you to choose the shaped tool from the local/global shaped tools table (for moreinformation on the shaped tools use, see topic 3.10).To activate the options, select the Use Shape check box.Global shaped tools tableThe Shaped tools dialog box is displayed enabling you to choose the shaped tool from the Globalshaped tools table. The selected tool is copied to the Local shaped tools table related to the currentCAM-Part, and its parameters are displayed in the Group name and Shape name fields after youconfirm the Shaped tools dialog box.167
    • Local shaped tools tableThis option enables you to choose the previously used in the current CAM-Part shape tool from theLocal shaped tools table. The Shaped tools dialog box is displayed. The parameters of the selectedtool are displayed in the Group name and Shape name fields after you confirm the Shaped toolsdialog box.Shape EditThis option enables you to change dimensions of the selected shape tool. The Shaped tools dialogbox is displayed. Click on the Edit page to modify the parameters of the tool.STLThis option enables you to export tools saved in the STL format. The Export Tool dialog box isdisplayed.Choose the required file and click on the Open button. 168
    • 3. Tools and Tool Libraries3.9 Tool Holding systemSolidCAM enables you to define a variety of tool holders }to help you check and prevent all possible collisions ofthe tool holding system with the workpiece. This featurealso enables you to see a more realistic simulation in theSolidVerify mode. Tool holding systemThe SolidCAM tool holder is defined by combining twocomponents. The first component is the tool adaptormounted in the spindle unit of the milling machine.The second component may consist of different typesof extensions and reductions like collet chucks, arbors,shanks and any other components that you may have. Tool adaptor Tool Extensions and reductions3.9.1 Tool Holders dialog boxThis dialog box enables you to define and operate your toolholders. 1. Click on the SolidCAM item in the SolidWorks main menu. 2. Choose the Tool Holders item from the Tool Library submenu.169
    • 3. The Tool Holders dialog box is displayed. A CAD model file is also displayed so that you can define the geometry of the new holders.Tool holder component tablesThe first list displayed above enables you to define and manage your tooladaptors. 1. Right-click on the item name in the table. 2. Choose a command from the submenu. • Add Holder Component This option enables you to define the geometry of the new tool adaptor that will be added to the table. The Holder Geometry dialog box is displayed. • Generate This option generates the sketch in the model file with the geometry of the selected tool adaptor. • Replace This option enables you to replace the existing tool adaptor geometry with a new one. The Holder Geometry dialog box is displayed. Select the new geometry. • Delete This option enables you to remove the tool adaptor part from the list. • Rename This option enables you to assign a new name to the tool adaptor. 170
    • 3. Tools and Tool Libraries • Copy This option enables you to create a copy of the existing tool adaptor.The second list enables you to define and manage groups of reductions andextensions such as collet chucks, arbors, shanks, etc. 1. Right-click on the group/component name in the table. 2. Choose a command from the submenu. • Add Group This option enables you to create a group of components and to define separate groups for tool holders components of the same type. • Add Holder Component This option enables you to define the geometry of the new component that will be added to the current group of the parts table. The Holder Geometry dialog box is displayed. • Generate This option generates the sketch in the model file with the geometry of the selected tool holder. • Replace This option enables you to replace the existing holder geometry with a new one. The Holder Geometry dialog box is displayed. Select the new geometry. • Delete This option enables you to remove the tool holder component from the list. • Rename This option enables you to assign a new name to the tool holder component or group.171
    • • Copy This option enables you to create a copy of the existing tool holder component.DescriptionSolidCAM enables you to type a brief description of the tool holder component (reduction orextension).Show pageThis page enables you to see a 3D model of the tool holder. In the graphic area of this page you can rotate, zoom and pan the 3D model of the tool holder. Use the following combinations: • Middle mouse button – Rotation of tool holder • Shift + Middle mouse button – Zoom of tool holder • Ctrl + Middle mouse button – Pan of tool holderEdit pageThis page enables you to edit the parameters of the selected tool holder component. 1. Select the tool holder component. 2. Switch to the Edit page to change the dimensions of the tool holder component.The interactive picture of the selected tool holder componentis displayed. The parameters pages are located below thepicture.SolidCAM divides the tool holder component into solidsegments like cylinders, cones or toruses. For each solidprimitive, SolidCAM determines the actual dimensions.For more information on this subject, see topic 3.9.3.You can change the dimensions of each segment with itsspecific page. 1. Select the segment on the picture or through the tabs below the picture. 2. Type the new value of the parameter in the value field. 172
    • 3. Tools and Tool Libraries3.9.2 Tool Holder Geometry definitionThis dialog box enables you to define the geometry of the tool holder component.Define chainThis option enables you to define a new chain of the component geometry.The Chain Options dialog box is displayed. In the model file displayed, you cansketch the shape of half the tool holder component and then define the chain.The direction of the chain does not matter. Note that the left side of the sketch is the bottom of the tool holder component and the right side is the top.Replace chainThis command enables you to replace a chain in the current chain geometry.Edit chainThis command enables you to update a chain in the current chain geometry.Reference pointThis option enables you to define the reference point through which the rotation axis of the toolholder component passes.3.9.3 Tool Holder segmentsSolidCAM determines three types of segments of the Holder Geometry.Cylinder Diameter • Diameter • Height Height173
    • Cone Angle • Top Diameter Top Diameter • Bottom Diameter Height • Height • Angle Bottom Diameter The following rules apply when parameters are changed: • Changing of the Angle causes Top Diameter change • Changing of the Bottom Diameter causes Height change • Changing of the Top Diameter causes Bottom Diameter change • Changing of the Height causes Bottom Diameter changeTorus • Top Diameter Top Diameter • Radius Start • Start Angle Angle • Sweep Sweep • Bottom Diameter Bottom Diameter Radius The following rules apply when parameters are changed: • Changing of the Radius causes Bottom Diameter change • Changing of the Top Diameter causes Bottom Diameter change • Changing of the Bottom Diameter causes Top Diameter change • Changing of the Start Angle causes Bottom Diameter change • Changing of the Sweep Angle causes Top Diameter change 174
    • 3. Tools and Tool Libraries3.9.4 Using Tool HoldersSolidCAM enables you to choose the tool holder component through the Tool Holders dialog box. Note that the tool adaptor section is inactive and you cannot select the adaptor type. SolidCAM enables you to define the Tool adaptor in the MAC file with the following string: mac_holder = BT45 If the parameter is not defined in the MAC file, SolidCAM will use the first adaptor from the list; the extenders are the same for all the adaptors. If all your machines use the same type of adaptor, you do not need to define the mac_holder parameter. In the table, drag and drop the requested adaptor to the first place on the list.In the Show area, SolidCAM displays the 3D model of the selected tool holder. In the graphic area of this page you can rotate, zoom and pan the 3D model of the tool holder. Use the following combinations: • Middle mouse button – Rotation of tool holder • Shift + Middle mouse button – Zoom of tool holder • Ctrl + Middle mouse button – Pan of tool holder175
    • Holders Edit dialog boxThe Holders Edit dialog box enables you to edit thedimensions of the selected tool holder component.This dialog box contains two tabs: Show This page displays a 3D model of the selected tool holder component. In the graphic area of this page you can rotate, zoom and pan the 3D model of the tool holder. Use the following combinations: • Middle mouse button – Rotation of tool holder • Shift + Middle mouse button – Zoom of tool holder • Ctrl + Middle mouse button – Pan of tool holder. Edit The interactive picture of the selected tool holder component is displayed. The tool holder component is divided into segments such as cylinders, cones and toruses. The Parameters table below the picture enables you to edit the actual dimensions of the tool holder component. 1. Select the holder’s element on the picture or through the parameter pages. 2. Type the new value of the parameter in the value field. 176
    • 3. Tools and Tool Libraries3.10 Shaped ToolsIn addition to three built-in tool types, SolidCAM enables youto use shaped tools. The geometry of these tools is definedwith a sketch. This way you can create your own database oftapered mills, T-shaped mills, etc.3.10.1 Shaped Tools dialog boxThis dialog box enables you to define and operate your shapedtools. Choose the SolidCAM item from the SolidWorks main menu. Choose the Shaped tools item from the Tool Library submenu. The Shaped Tools dialog box is displayed. A CAD model file is also displayed so that you can define the geometry of new shaped tools.177
    • Tool listThis field displays the database of shaped tools defined in SolidCAM. With this list you can defineand manage shaped tools. 1. Right-click on any item in the browser field of the Shaped Tools dialog box. The following menu is displayed. 2. Choose the specific command from the menu. • Add Group This option enables you to create a group of shaped tools. You can define separate groups for shaped tools of the same type. • Add Tool This option enables you to define the geometry of the newly shaped tool that will be added to the current group of the shaped tools table. The Shaped Tool Geometry dialog box is displayed. • Generate This option generates a sketch in the model file with the geometry of the selected shaped tool. • Replace This option enables you to replace the existing shaped tool geometry with a new one. The Shaped Tool Geometry dialog box is displayed. Select the new geometry. • Delete This option enables you to remove the shaped tool from the database. • Rename This option enables you to assign a new name to the selected shaped tool or group. • Copy This option enables you to create a copy of the selected shaped tool. 178
    • 3. Tools and Tool LibrariesDescriptionYou can place a brief description of the shaped tool here.Show pageThis page displays a 3D model of the selected shaped tool. In the graphic area of this page you can rotate, zoom and pan the 3D model of the shaped tool. Use the following combinations: • Middle mouse button – Rotation of tool • Shift + Middle mouse button – Zoom of tool • Ctrl + Middle mouse button – Pan of toolEdit pageThis page enables you to edit the parameters of the selectedshaped tool. 1. Select the Shaped tool. 2. Switch to the Edit page to change the shaped tool dimensions.The interactive picture of the selected shaped tool is displayed.The parameters pages are located below the picture.SolidCAM divides the tool into solid segments like cylinders, cones or toruses. For each solidprimitive, SolidCAM determines actual dimensions.You can change the dimensions of each segment in its specific page. 1. Select the tool’s element on the picture or through the parameter pages. 2. Type the new value of the parameter in the Value field.179
    • 3.10.2 Shaped tool geometry definitionThis dialog box enables you to define the geometry of the shaped tool.Define chainThis option enables you to define a new chain of the shaped tool geometry.The Chain Options dialog box is displayed. In the model file displayed, youcan sketch half of the shaped tool and then define the chain. The directionof the chain does not matter. Note that the left side of the sketch is the bottom of the tool and the right side is the top.Replace chainThis command enables you to replace a chain in the current chain geometry.Edit chainThis command enables you to update a chain in the current chain geometry.Reference pointThis option enables you to define the reference point through which the rotation axis of the shapedtool passes.3.10.3 Shaped Tool segments DiameterSolidCAM determines three types of segments of the Shaped ToolGeometry.Cylinder Height • Diameter • Height 180
    • 3. Tools and Tool LibrariesCone Angle • Top Diameter Top Diameter • Bottom Diameter Height • Height • Angle Bottom Diameter The following rules apply when parameters are changed: • Changing of the Angle causes Top Diameter change. • Changing of the Bottom Diameter causes Height change. • Changing of the Top Diameter causes Bottom Diameter change. • Changing of the Height causes Bottom Diameter changeTorus • Top Diameter Top Diameter Start • Radius Angle • Start Angle Sweep • Sweep • Bottom Diameter Bottom Diameter Radius The following rules apply when parameters are changed: • Changing of the Radius causes Bottom Diameter change • Changing of the Top Diameter causes Bottom Diameter change • Changing of the Bottom Diameter causes Top Diameter change • Changing of the Start Angle causes Bottom Diameter change • Changing of the Sweep Angle causes Top Diameter change181
    • 3.10.4 Using Shaped toolsSolidCAM enables you to choose the specific shaped tool using the Shaped tools dialog box.In the Show area, SolidCAM displays the 3D model of the selected tool. In the graphic area of this page you can rotate, zoom and pan the 3D model of the tool. Use the following combinations: • Middle mouse button - Rotation of tool • Shift + Middle mouse button - Zoom of tool • Ctrl + Middle mouse button - Pan of toolShape editThe Edit page of the Shaped tools dialog box enables you to edit the dimensions of the selectedtool.This dialog box contains two pages: Show This page displays a 3D model of the selected tool. 182
    • 3. Tools and Tool Libraries In the graphic area of this page you can rotate, zoom and pan the 3D model of the tool. Use the following combinations: • Middle mouse button – Rotation of tool • Shift + Middle mouse button – Zoom of tool • Ctrl + Middle mouse button – Pan of tool Edit The interactive picture of the selected shaped tool will be displayed. The tool is divided into segments like cylinders, cones and toruses. With the Parameters table below the picture, you can edit the actual dimensions of the shaped tool. 1. Select the tool’s element on the picture or through the parameter pages. 2. Type the new value of the parameter in the value field.183
    • 3.11 Feed and Speed defaultsThe Speed/Feed Default option enables the program Tool Materialto calculate the speed and feed rate according to the Work MaterialWork material and Tool material you are using.Choose the Speed&Feed Defaults item from theTool Library submenu. Speed/Feed DefaultsThe Speed/Feed Default dialog box is displayed.This dialog box enables you to define the Work Material and the Tool Material and to define thedifferent values of the Speed and Feed for each combination set. The dialog box shows the tree-control list of the existing Tool and Work Materials. The root items of the tree are the Tool Materials;for each tool material you can see the list of the Work Materials for which Speed/Feed default isdefined. The right area of the dialog box shows the Speed/Feed parameters for each selected pairof Tool material and Work material. 184
    • 3. Tools and Tool LibrariesAdd/Delete pageThis page enables you to operate the Tool and Work materials and define the Speed and feed valuesfor the combination of the tool and work materials.Right-click in the tool/work material list and choose the specific item from the menu. • Add Tool Material This option enables you to add the new Tool Material. The combination pairs of the new Tool material with the existing Work materials are automatically added. Type the name for the new Tool Material. • Add Work Material This option adds a new Work material. The Work material is added to all existing Tool material combinations. • Delete This option removes the selected Tool/Work material from the list. • Rename This option enables you to assign a new name to the selected Tool/Work material.185
    • Work material parametersIn this area, you have to assign the Speed and Feed values for the selected Tool/Work materialcombination.SolidCAM enables you to define the following values: • V Signifies the Rough Material cutting speed in Meters/Minute in the Metric system or in Feet/Minute in the Inch system. • V fin Signifies the Finish Material cutting speed in Meters/Minute in the Metric system or in Feet/Minute in the Inch system. • FZ XY Feed rate in the XY plane, in Units per tooth. • FZ Z Feed rate in the Z direction, in Units per tooth. • FZ fin Feed rate used for finish milling, in Units per tooth.Edit pageThis page enables you to edit the values of the Speed and Feed for each combination of the Tool/Work material.Click on the parameter you have to change and enter the new value. 186
    • Geometry 4Whenever you work in CAD, you use 2D wireframe curves and 3Dmodels to describe real life parts. With SolidCAM, you can turn thesemodels into GCode for any CNC-machine.A major step in the process from modeling to manufacturing is to tellSolidCAM what and where you want to machine. In SolidCAM, existingmodels are used to pass this information to the CAM module.  Defining a new Geometry  Drilling Geometry  3D Model Geometry  Wireframe Geometries  Managing Geometries  Geometry synchronization
    • 4.1 IntroductionSolidCAM enables you to turn 3D models, 2D and 3D sketches built with SolidWorks into GCodefor any CNC-machine. In this process of modelling to manufacturing, geometries have to be definedto determine where the model will be machined. Geometry 3D Wireframe Drill 3D Model Profile Faces Pocket Working Area Slot Limit SectionIn SolidCAM, you can define geometries in the operation dialog box; this enables SolidCAM tocheck if the geometry follows the necessary rules needed in this type of operation.The geometries defined in SolidCAM are associative to the SolidWorks model. Any change made tothe model or sketch will propagate to referenced SolidCAM geometry. 188
    • 4. Geometry4.2 Drilling geometryA Drilling geometry consists of one or more points (drillingcenters) that are defined by the X-, Y- and Z-values. Theycan be selected on models using a number of differentmethods.4.2.1 Defining a Drilling geometryIn Drilling operations, you have to define the coordinate points where SolidCAM will execute thedrilling cycles. The powerful selection tool enables you to define and edit drilling positions quicklyand easily.In the example above, the drilling points have been selected by their radius and Z-level on a 3D solidmodel. With automatic selection the distance between two drilling points is optimized to reducemachining time.The button in the Geometry page of the Drilling Operation andThread Milling Operation dialog boxes enables you to choose themode of the geometry definition. • The Plane mode enables you to define the geometry on the plane/face parallel to the XY-plane of the current CoordSys. Click on the Define button to display the Drill Geometry Selection dialog box (see topic 4.2.3). • The Around 4th axis mode enables you to select the drilling geometry wrapped on the solid model around the 4th axis. The Define button displays the Around 4th Axis Drill Geometry Selection dialog box (see topic 4.2.4). Revolution axis This method enables you to select only the holes whose axis intersects with the revolution axis of the CAM-Part. This method can be chosen when the appropriate CoordSys that enables the use of the 4th axis is selected.189
    • 4.2.2 Editing a Drilling geometryYou can add or remove drilling positions from previously saved drillinggeometries. 1. In SolidCAM Manager, right-click on a Drill geometry and choose the Edit option from the menu. 2. The Drill Geometry Selection dialog box is displayed. With the Select/Unselect option, you can add or remove drilling points.4.2.3 Drill Geometry Selection dialog boxFor Drilling operations, you have to define the coordinate points whereSolidCAM executes the drilling cycles.The powerful selection tool enables you to define and edit drilling positionsquickly and easily. Whenever you have to define a drilling geometry, theDrill Geometry Selection dialog box is displayed.NameThis option enables you to define the name of the geometry. SolidCAMoffers you the Default Geometry name (see topic 12.9) that can be edited.ConfigurationsThis option enables you to switch between SolidWorks configurations.Choose the necessary configuration for the geometry definition.Select/Unselect drilling centersUse the Select/Unselect mode to add and remove drilling positions fromthe geometry. The Undo/Redo button deletes or restores the last selection. 190
    • 4. GeometryAll the selected points are shown in the list at the bottom of the dialogbox. To remove a point from the list, right-click on the point name in thelist and choose the Delete option from the menu or choose the Delete Alloption to remove all of the points.Sequence of drill positionsYou can change the sequence of drill positions in the list by dragging anddropping. You can also define and edit the sequence of drill positions in the Drilling Operation dialog box (see topic 6.6.3).Selecting modes (Select centers by)You can add drilling positions to the current geometry using the followingoptions: • Pick position. You can define drilling positions one by one using the CAD point selection options. You can also type the coordinates into the X,Y,Z dialog box and confirm each drilling point by clicking on the Enter button. 1. Pick drilling center position – select the drilling point. 2. Confirm the selection by clicking on the Enter button. • 3 Points on circumference. Usually, all curves and arcs of imported models are converted into splines by the exporting CAD system. Due to the nature of spline curves or surface boundaries, you cannot pick a center position like you could on a circle or arc. SolidCAM calculates the center position of an arc defined by three points positioned on the spline edges. This facilitates the selection of drilling centers on spline surfaces. 1. Pick the first point – pick a point on the circumference of the circle or arc using the CAD point selection options or type the coordinates into the X,Y,Z dialog box and confirm. 2. Pick the second point.191
    • 3. Pick the third point. 4. SolidCAM calculates the center of the three points and displays the drilling position.• Multi-positions. With this option, you can select model faces. SolidCAM automatically determines all arcs/circles located on the selected face and defines the center points as drilling positions. You can also use the mouse to drag a box over the area of the model. SolidCAM automatically recognizes all arcs inside this area and defines the center points as drilling positions. The options you have selected in Filter affect the search when you apply the Multi-positions command. 1. Check whether the Filter options you have selected are correct. 2. Click on the solid model face. 3. SolidCAM starts searching the selected face for drilling positions and displays the search result.• All circle/arc centers. SolidCAM is searching the solid model for arcs and circles and adds all center points as drilling positions to the geometry. The options you have selected in Filter affect the search result when using the All command. 1. Check whether the Filter options you have selected are correct. 2. Click on the All circle/arc centers button to start the search. 3. SolidCAM starts searching the solid model for drilling positions and display the search result. 192
    • 4. Geometry • CAD selection. SolidCAM enables you to select the drilling geometry with the SolidWorks selection tools. 1. Check whether the Filter options you have selected are correct. 2. Click on the CAD selection button. The CAD selection button changes to Resume. 3. Select the geometry with SolidWorks tools. 4. Click on the Resume button.Selection filter (Filter for circle/arc selection)You can use various filters to search circles/arcs on the model for drillingpositions. SolidCAM selects only the drilling positions with the attributesset in the Filter options. You can select the following attributes: • Include arcs. If this check box is selected, SolidCAM also includes arc centers in the search for drilling positions. This option can solve the occasional problem caused by imported 2D sketches that have circle entities cut to halves. It also enables you to place drills in filleted corners. • All circles. SolidCAM is searching the model for circles. Arcs or broken circles are not included in the search result. • By Radius. You can limit the search by defining a radius value. Only arcs and circles with the given radius are selected and their center position is added to the drilling geometry. You can define the radius value on the model. Click on the By Radius button. In the Select radius by dialog box, you can choose how you want to pick the radius from your model. Select the corresponding option and pick the radius from an existing circle/ arc or use the 3 Points on circumference definition. • Z-Level. You can also limit the search to the Z-level. Only arcs and circles on the given XY-plane are selected and their center position is added to the drilling geometry. You can select the Z-level on your model. Click on the On Z-level button and select a point on your model using the point selection options. The Z-coordinate of the selected point is passed to the corresponding field.193
    • Selected circles/arcs • The No longer can be selected option enables you to select drills that were not selected previously. • The Show the center points option enables you to see the drills picked in the previous drilling geometry.4.2.4 Around 4th Axis Drill Geometry Selection dialog boxGeometry NameThis field enables you to define the name of the geometry. SolidCAM offers you the DefaultGeometry name (see topic 12.9) that can be edited.ConfigurationsThis field enables you to switch between SolidWorks configurations. Choose the necessaryconfiguration for the geometry definition.ModeYou can switch between the Select/Unselect mode to define or remove drilling positions from thegeometry. All the selected drilling positions are shown in the list at the bottom of the dialog box. 194
    • 4. GeometryType Pick face SolidCAM automatically selects all the holes starting from the selected face. The Full holes only option enables you to select only full diameter holes. Pick hole This mode enables you to select the holes around the 4th axis one by one.195
    • Pick 3 points This mode enables you to define the drilling geometry by selection of three points on the holes edge. CAD selection SolidCAM enables you select the drilling geometry with the SolidWorks selection tools.Drilling positions listThis list displays all the selected drilling positions, their angle aroundthe 4th axis and location along the revolution axis. The right-clickmenu is available.The Unselect/Unselect All options enable you to unselect the drillingpositions chosen for the operation.The Reverse option enables you to reverse the angle value 180°around the 4th axis.The Sort by Angle/Coordinate options enable you to sort the drilling positions in the list. 196
    • 4. Geometry4.3 3D Model geometryAny surface, solid or a combination of surfaces and solids can beselected as a 3D Model geometry. These models can be machined withthe 3D Milling operation in SolidCAM using various milling strategies.4.3.1 Defining a 3D Model geometrySolidCAM enables you to define the 3D Model geometry using the3D Geometry dialog box.NameThis option enables you to define the name of the geometry. SolidCAMoffers you the Default Geometry name (see topic 12.9) that can be edited.ConfigurationsThis option enables you to switch between SolidWorks configurations.Choose the relevant configuration for the geometry definition.TypeThis option enables you to define the type of objects that will be selected: • Solid – to select solid objects only; • Surfaces – to select surfaces only; • Both – to select both surfaces and solids.The default option is Both.CAD selectionThis option enables you to select the 3D geometry with the SolidWorks tools. When an object is selected in the CAD selection mode, the CAD selection button changes to Resume.197
    • List of selected objectsYou can select an object by clicking on it. When an object is selected, itsicon is displayed in the list in the bottom of the dialog box.To unselect the object, click on it again or right-click on its icon in the listand choose Unselect from the menu. To remove selection from all objectsin the list, click Unselect all.4.3.2 Editing a 3D Model geometrySolidCAM enables you to add, remove or replace entities in 3D geometriesthat have been previously defined. Actual changes in dimensions ortopology of your model must be performed with SolidWorks. 1. In SolidCAM Manager, right-click on the 3D Model Geometry icon. Choose the Edit command from the menu. 2. The 3D Geometry dialog box is displayed. 3. The default Type settings enable you to add solids and surfaces to your model. A click on a model object selects it; the next click removes the selection. You can also unselect objects by right-clicking on their icons in the list and choosing Unselect/Unselect all. 4. Confirm your selection by clicking on the button. Use the CAD selection mode to select the geometry with Host CAD tools. 198
    • 4. Geometry4.4 Wireframe geometryWireframe geometry has several subtypes, each with its own set of rules. All the subtypes use thesame interface to select the geometry.Chain geometries are defined by picking the following entities: edges of models, 2D curves, 3Dcurves, circles, lines and splines. Each chain is composed from one or more entities and defines anopen or closed contour. Wireframe Geometry Profile Working Area Limit Pocket Slot Section4.4.1 Defining the Profile/Pocket geometryChains for Profile Milling (see topic 6.1) can be either open or closed. You can machine one or moreprofiles in a single operation. Closed chain Open chainChains for Pocket Milling (see topic 6.4) must be closed. The first chain defines the contour of thepocket. All closed chains inside the first chain of each pocket are automatically treated as pocketislands. Overlapping chains are milled as separate pockets, not as islands. To select multiple pocketswith islands, continue adding chains to the geometry. Closed chain Closed chain with island199
    • 1. Select a chain to define the geometry. 2. Confirm the chain definition with the Apply button. 3. When you have completed the geometry definition, confirm the Geometry Edit dialog box (see topic 4.5) with the button.4.4.2 Defining the Working AreaWorking areas are used in 3D Milling (see topic 7.1) to constrain the machiningto certain areas of the 3D model. The working area is defined by a closed chain.The chain can consist either of selected points or of 2D/3D edges, curves orsplines. As in pocket geometries, working areas can be defined with internal chains, so that the islands are excluded from machining. In this example, the working area has been selected to machine the cavity. The external chain defines the outside boundary of the area. The internal chain excludes the parting surface from machining. 1. Select a chain to define the geometry. 2. Confirm the chain definition with the button. 3. When you have completed the geometry definition, confirm the Geometry Edit dialog box (see topic 4.5) with the button.4.4.3 Defining the Slot geometryChains for Slot Milling (see topic 6.9) can be either open or closed. You can machine one or moreslots in one operation. 1. Click on the edges or lines that make up your slot. 2. Confirm the chain definition with the button. 3. When you have completed the geometry definition, confirm the Geometry Edit (see topic 4.5) dialog box with the button. 200
    • 4. Geometry4.4.4 Defining the Section geometryIn the Slot (see topic 6.9) and Translated Surface (see topic 6.11) operations, you need to select aSection geometry. These 2.5D operations can be defined using 2D geometries only. Use sectiongeometries to define depth profiles for Slot and Translated Surface operations.Adding a Section geometry 1. In the Section Geometry dialog box, click on the Add button in order to add chains. The Chain options dialog box is displayed. 2. Select the edges or lines that make up your section and confirm by clicking on the button. 3. Click on the Pick Point button to pick the reference point. This point defines the level of the section relative to the upper level of the operation. 4. The Pick Z-Reference Point dialog box is displayed. Pick the point on the model and confirm with the button. 5. Confirm the Section Geometry dialog box with the button.201
    • Editing a Section geometryYou can edit the section or redefine the reference point of the section. 1. In SolidCAM Manager, right-click on the Section geometry and choose Edit from the menu. 2. In the Section Geometry dialog box, click on the Pick Point button to pick the reference point again or on the Edit/Replace buttons to edit or replace the section chain using the Chain Selection dialog box. 3. Click on the button to confirm your changes and close the dialog box.Spline ApproximationThis field enables you to define the Spline approximation tolerance for thechain selection.4.4.5 Defining the Limit geometryA Translated Surface Operation (see topic 6.11) can be defined using 2Dgeometries only. With Limit geometries you can define boundaries for thisoperation. 1. Select a chain to define the geometry. 2. Confirm the chain definition with the button. 3. When you have completed the geometry definition, confirm the Geometry Edit dialog box with the button. Section Limit 202
    • 4. Geometry4.5 Editing chain geometries To edit a chain, right-click on a geometry entry in SolidCAM Manager and choose Edit from the submenu. The Geometry Edit dialog box is displayed.4.5.1 Geometry NameThis option enables you to define the name of the geometry. SolidCAMoffers you the Default Geometry name (see topic 12.9) that can be edited.4.5.2 ConfigurationsThis option enables you to switch between SolidWorks configurations.Choose the relevant configuration for the geometry definition.4.5.3 Adding a ChainYou can add a chain to the existing set of chains in the current geometry.The new chain is added under the next sequential number. 1. Select the chain geometry using the Single entities (see topic 4.5.6) and Automatic selection options (see topic 4.5.7). 2. Confirm the chain definition with the button. or Use the Add Multi-chain button to automatically define a number of chains (see topic 4.6).203
    • 4.5.4 Managing chainsAll the selected chains are displayed in this dialog box. To edit thesechains, right-click on the Chain name and choose the appropriatecommand from the menu.ReplaceThis command enables you to update a chain in the current geometry.The old chain is deleted and you can define a new chain.InsertThis command enables you to insert a chain between two existing chains.EditThis command enables you to edit an existing chain. You can reverse the chain or undo the selectionsteps to change the chain.ReverseThis command enables you to reverse the direction of the chain.RenameThis command enables you to rename the geometry chain.Set CW/Set CCWThese commands enable you to set either clockwise or counterclockwise direction for the selectedchains.Mark open edgesThis option enables you to define the geometry for the Open Pocket machining by defining openedges on the conventional wireframe geometry. The Mark Open Edges dialog box is displayed (seetopic 4.5.12). This option is available only for Pocket operations (see topic 6.4).DeleteThis command enables you to delete a chain from the current geometry. 204
    • 4. Geometry4.5.5 Chain directionSome of the operations in SolidCAM use the Direction arrow Start pointdirection of the chain geometry to calculate the toolpath. In Profile Milling, for example, you have tospecify the tool side, which is relative to the directionof the selected contour. The selected edges or sketchsegments are highlighted. The arrow at the start pointof the chain indicates the direction of the chain.Use the Reverse command to reverse the directionof the chain during or after the chain selection, ifnecessary.4.5.6 Selecting single entitiesYou can define the geometry by selecting edges, sketch segments andpoints on the contour. The following options are available: • Curve This option enables you to create a continuous geometry chain by picking its successive entities. During the geometry definition, the gaps between selected entities are detected. They can be closed taking into account the Gap Minimum and Gap Maximum tolerances (see topic 4.5.10). 1. Pick start curve – select the first entity (a wireframe element or the solid model edge).205
    • 2. Pick next curve – select the next curve that belongs to the chain. If the detected gap is smaller than the Gap Minimum tolerance, it is being closed automatically by extending/shortening chosen entities up to their virtual intersection point. If the gap is greater than the Gap Minimum tolerance but smaller than the Gap Maximum tolerance, a message is displayed asking you if you want to close the gap. If you confirm the message, the gap is being closed automatically by extending/shortening chosen entities up to their virtual intersection point. If you cancel, the gap is not being closed, and the last entity is being unselected. In case the gap is larger than the Gap Maximum tolerance, the selected entity is not accepted, and the following message is displayed: 3. To complete the selection, click on the button. Associativity SolidCAM keeps the associativity to any edge or sketch entity. Any change made to the model or sketch automatically updates the selected geometry.• Curve + Close corners This option enables you to close the gaps between successive chain entities irrespective of the Gap Minimum and Gap Maximum values by virtually extending the entities up to their intersection. First selected entity Next selected entity Splines and arcs are extended by lines tangential to the arc/spline at its end point. 1. Pick start curve – select the first entity (a wireframe element or the solid model edge). 206
    • 4. Geometry 2. Pick next curve – select the next curve that belongs to the chain. When a gap is detected between these entities, the chain is continued by virtually extending the selected entities, according to the direction of the first entity, up to the virtual intersection point. If an intersection point cannot be found by extending either one or both selected entities, the following message is displayed: In case several possible intersection points exist, the point closest to the last vertex of the first selected entity is chosen. 3. To complete the selection, click on the button. Associativity When the model used for the geometry definition is modified, SolidCAM enables you to synchronize the geometry with the updated model. During the synchronization SolidCAM determines gaps areas created using the Curve + Close Corners option and regenerates the extension of the chain elements so as to close the gaps. • Point to point This option enables you to connect the specified points with a straight line. 1. Pick start point – pick a point on the model or enter the coordinates into the command line.207
    • 2. Pick next point – pick the following point (enter the coordinates into the command line), and the chain element will be created from the previous point up to this point. 3. To complete the selection, click on the button. Associativity SolidCAM does not keep the associativity to any selected point. SolidCAM saves the X-, Y- and Z-coordinates of the selected points. Any change made to the model or sketch does not update the selected geometry. You cannot select a point that is not located on a SolidWorks entity (if you need to select such a point, add a planer surface under the model and select the points on that surface). The following rules are applicable to virtual line selection with the Point to Point option: 1. When you select a virtual line between two edges, the line behaves as a spring. Whenever the model is changed and synchronized, the geometry is updated with the model. 2. When you select a sequence of several virtual lines, only the points connected to model edges or sketch elements are updated, but all the other points stay fixed at the defined X-, Y- and Z-positions.• Arc by points This option enables you to create a chain segment on an arc up to a specific point on the arc. 1. Pick start point – choose a Third point on the arc where you Second Point Point want the chain to start. If this is not the first point on the chain, go to step 2. 2. Pick next point – choose a First point on the arc between the Point first point on the arc and the third point on the arc. 3. Pick end point – choose a third point on the arc where you want the chain to end. 208
    • 4. Geometry Associativity SolidCAM does not keep the associativity to any selected arcs by points. SolidCAM saves the X,- Y- and Z-coordinates of the selected points. Any change made to the model or sketch does not update the selected geometry.4.5.7 Automatic selectionSolidCAM automatically determines the chain entities and closes the chain contour. The followingoptions are available:Auto-toThe chain is selected by specifying the start curve, the direction of thechain and the element up to which the chain is created. SolidCAM enablesyou to choose any model edge, vertex or sketch entity to determine thechain end.When the end item is chosen, SolidCAM determines the chain accordingto the rules of the chosen selection mode (Auto-general, Auto-Constant Zor Auto-Delta Z). The chain selection is terminated when the selected enditem is reached. End entityStart entity Selected chainIf the chosen end item cannot be reached by the chain flow, the chain definition is terminated whenthe start chain segment is reached. The chain is automatically closed. End entityStart entity Selected chain209
    • The confirmation message is displayed. The Auto-to option is useful if you do not want to define a closed chain, but an open chain up to a certain element. • Auto-general SolidCAM highlights all entities connected to the last chain entity. You have to select the entity along which you want the chain to continue. • Auto-constant Z This option identifies only entities on the same XY-plane with the previously selected chain entity. You are only prompted to identify the next chain element when two entities on the same Z-level are connected to the chain. The system tolerance for this option can be set in the SolidCAM Settings. 210
    • 4. Geometry • Auto-Delta Z You are required to enter a positive and negative Z-deviation into the Delta Z dialog box. Only entities within this range are identified as the next possible entity of the chain. 1. Pick start curve – select the start entity of the chain. 2. Pick point in chain direction – indicate the chain direction by choosing a point on the selected start entity of the chain. 3. You are prompted to select one of the possible curves if the system detects that more than one entity can be the next element of the chain. Indicate your choice. 4. When the system can close the chain, the confirmation message is displayed. Choose Yes to accept. If you answer No, you can continue the chain selection: for example, undo the last step or cancel the chain selection.4.5.8 Chain buttons • Undo step This button enables you to undo the last selection of a chain element. • Reverse This button enables you to reverse the direction of the chain you are currently working with. The direction is indicated by an arrow at the chain start point. • Accept Chain This button enables you to confirm the chain selection. • Reject Chain This button enables you to cancel the single chain selection.211
    • 4.5.9 OptionsSpline approximationThis field enables you to define the Spline approximation tolerance for the chain selection. Arcs onthe XY-plane are saved as arcs in the SolidCAM database; if you select an arc or spline that is noton the XY-plane of the actual part Coordinate System, SolidCAM will do the following: 1. Project the arc or spline on the XY-plane of the active CoordSys and divide it into segments according to the specified tolerance. Tolerance 2. In order to reduce the number of Tolerance Arc segments, SolidCAM tries to fit arcs on the segments generated in step 1 according to the specified tolerance Spline multiplied by 3.4.5.10 Gap controlThis field enables you to change the gap tolerances for the current geometry during the geometrydefinition.The automatic selection function for chain geometries uses certain tolerances to decide whethertwo consequent elements are connected or not. The behavior of this function depends on the gapbetween the entities. The Gap minimum and Gap maximum parameters define the range of gaptolerance values used for the chain geometry definition.The default values of these parameters are inherited from the SolidCAM Settings (see topic 12.4.3).In the Geometry Edit dialog box, you can edit the tolerance values during any stage of any chaindefinition (for example, at start of chain definition or during the chain definition). During thegeometry chains definition, SolidCAM uses these parameters in order to decide whether to connecttwo successive chain entities, if a gap between them is detected. 212
    • 4. Geometry • If the gap between the edges is smaller than the specified Gap minimum value, the system automatically continues the chain and closes the gap with a line. • If the gap is in the range between the Gap minimum and Gap maximum values, you are asked whether the gap should be closed. If you answer Yes, the gap is automatically closed with a line. • If the gap is larger than the Gap maximum value, the following message is displayed: When the message is confirmed, the last selected chain entity is rejected.4.5.11 Add Multi-ChainSolidCAM enables you to define a number of chains on the model byselecting its elements. The program automatically creates chains from theselected elements.For more information on Multi-chain selection, see topic 4.6.4.5.12 Mark Open Edges dialog boxThis dialog box enables you to mark the open edges on already selectedpocket chains by picking them. Closed edges Pocket geometry Open edge Open pocket213
    • Mark asThis section offers you the following selection modes: • Open When this option is chosen, picking a pocket geometry edge marks it as open. • Wall When this option is chosen, picking a pocket geometry edge marks it as closed (wall). • Toggle When this option is chosen, picking a closed edge marks it as open and the next picking marks it as closed, and so on.SelectThis section offers you the following selection methods: • Single entity When this method is chosen, you can pick single entities in order to mark them as open/closed. • From/To entities When this method is chosen, you can mark a segment of the pocket geometry by picking the start and the end entities.CAD SelectionThis button enables you to perform the selection using the CAD tools. The marking of open edges is available only for Pocket operations (see topic 6.4). 214
    • 4. Geometry4.6 Chains Selection dialog boxThe Chains Selection dialog box enables you to define a number of chains on the model by selectingits elements. The system automatically creates chains from the selected elements.Mode • Select – this mode enables you to select the elements to define the chains. • Unselect – this mode enables you to unselect the previously selected elements.Type • Edges SolidCAM enables you to choose model edges to build a chain geometry. • Text SolidCAM enables you to choose text to build a chain geometry. • Faces When this mode is chosen, SolidCAM enables you to pick a model face. All the loops of this face are collected and closed geometry chains are created. The Loops filter is applied to the collected loops to exclude all those that do not match the specified criteria.Selection FilterWhen this check box is selected, you can select only elements located on a specificZ-level. To define the Z-level, either enter the value in the dialog box or click on the On Z-Levelbutton and pick the level on the model.215
    • Loops filterWhen this check box is selected, the External loop and Internal loops check boxes are available.When the External loop check box is selected, all the internal loops are excluded from the pickedface and only the external loops are collected. External loopWhen the Internal loops check box is selected, all the external loops are excluded from the pickedface and only the internal loops are collected. Internal loopsWhen both these check boxes are selected, the system collects both internal and external loops fromthe picked face. This section is enabled only when the Faces mode is chosen. 216
    • 4. GeometryCAD selectionClick on this button to select the chains with the Host CAD tools.Get AllThis button enables you to select all of the model elements.Sort TypeWhen there is more than one chain, this option enables you to determine the chain you would liketo start from. The Sort chains dialog box is displayed (see topic 4.6.2).Chains directionThis option enables you to determine the cutting direction of each chain. The Chains Directiondialog box is displayed (see topic 4.6.1).View ChainsThis option enables you to see the chains before they are created.4.6.1 Chains Direction dialog boxThe Chains Direction dialog box enables you to determine the directionof the chain.Closed chains directionThis option enables you to determine the direction of closed chains. • External chains direction External chains are the outer borders of a pocket. You can determine if you want the chain to go clockwise or counterclockwise by choosing CCW or CW. • Internal chains opposite Internal chains are located within the boundaries of external chains. Selecting this check box, you can have the internal chains go in the direction opposite to that of the external chains.217
    • Open chains directionThis option enables you to determine the direction of open chains. • To center: the chain start point is the end of the chain furthest from the given center point. • From center: the chain start point is the end of the chain closest to the given center point.Selecting the Change center position check box enables you to choose the center position byentering the X- and Y-values or by picking a point on the model.If you do not change the center position, the CoordSys origin is used as center point.4.6.2 Chain sortingThe Chain sorting option enables you to define the order in which youwant the chains to be created.Sort by DistanceThe chain closest to the last chain is chosen using two options: • End to Start The next chain is the chain with the start point closest to the end point of the last chain. • Start to Start The next chain is the chain with the start point closest to the start point of the last chain.Sort by ValueThe next chain that is closest to the last chain in a given direction is chosen. • X start The next chain is the one in the X-direction. • Y start The next chain is the one in the Y-direction. 218
    • 4. Geometry • Reverse The direction of the chains changes (X-start: Left to Right; Y-start: Upward or Downward).Polar SortChains are selected around a specific point. If no point is chosen, the default point is the CoordSysorigin of the CAM-Part. • CW Direction The order of the chains is in clockwise direction around the point. • CCW Direction The order of the chains is in counterclockwise direction around the point. • Change center position The center position is chosen either by entering X-/Y-values or by picking a point on the model. • Start angle This field controls the angle between the start point of the chain and the point of rotation.219
    • 4.7 Managing geometriesYou can edit and manage your geometries using the Geometries header in the SolidCAM Managertree. Geometries used in machining operations can be edited through SolidCAM Manager: theyappear under the corresponding operation. SolidCAM also enables you to define and showgeometries inside the operation dialog box, so that you can select the geometry and machiningstrategy in one step. 1. In SolidCAM Manager, right-click on a geometry entry. The menu is displayed. 2. Choose a command from the menu.ShowThis command displays a 3D Model, Drill or Wireframe geometryhighlighted in the SolidWorks window.To exit from this mode, click on the button in the displayed Show Geometry dialog box.EditYou can change or update the selected geometry. If the tool path of an operation was calculatedbefore, it is deleted. You have to recalculate the operation after making changes to the geometry.Generate SketchThis command enables you to generate a SolidWorks sketch containing chains of the currentwireframe geometry. The sketch is generated in the CAM component of the SolidCAM Partassembly. This command is available only for wireframe geometries.CopyThis command enables you to duplicate the selected geometry. TheGeometry Name dialog box is displayed to define the name of thegeometry. 220
    • 4. GeometryCopy as Working areaThis command copies the selected geometry as a working area.SolidCAM generates a SolidWorks sketch containing chains of theselected geometry. The sketch will be generated in the CAM componentof the SolidCAM Part assembly. A new Working area geometry isdefined using this sketch.The Geometry Name dialog box enables you to define the name of thegeometry.Delete/Delete AllYou can delete geometries not used in any machining operation. These geometries are displayedunder the Geometries header. Any geometry used in operations appears under the respectiveoperations only and cannot be deleted unless the operation is deleted as well. The Delete all command is only available when you right-click on the Geometries header. It deletes all geometries not currently used in any machining operation. Whenever you click on a single geometry, the Delete command is available for the selected geometry only.Synchronize/Check synchronizationWhen the SolidWorks model is updated, you can check the compliance of the SolidCAM geometryto the updated SolidWorks model. If the SolidCAM geometry is not synchronized with theSolidWorks model, you can synchronize it.4.7.1 Synchronization of the Wireframe geometrySolidCAM Wireframe geometry is based on the SolidWorksmodel elements such as edges, vertices or sketches. SolidWorks Model SolidCAM Geometry based on the SolidWorks ModelWhen the SolidWorks model is changed, SolidCAMuses the synchronization algorithm to synchronize thegeometry with the updated SolidWorks model. SolidWorks Model has changed, SolidCAM Geometry SolidCAM Geometry has to is updated be updated221
    • Synchronization check SolidCAM GeometrySolidCAM marks all SolidWorks entities used for the Tag Taggeometry definition with tags. The list of these tags is saved.The tags enable you to establish a connection between theSolidCAM geometry and the SolidWorks model entities. Tag TagThe relations between the tagged SolidWorks geometry andSolidCAM geometry is saved in the geometry file (*.gem).SolidCAM enables you to check the synchronization statusautomatically or manually depending on the Synchronization SolidWorks Modelsettings (see topic 12.5).When you need to check the synchronization status of the geometry manually, do the following: 1. Right-click on an operation or geometry entry in SolidCAM Manager. 2. Choose the Check Synchronization item from the menu.SolidCAM checks all the geometry entities in the following method: • The SolidWorks model elements are compared geometrically to the relevant entities in the SolidCAM geometry file. • If a misfit is determined between the SolidWorks model and the SolidCAM geometry, this geometry is marked with the synchronization mark . • If there is a gap or overlapping entities, the geometry is also marked with the synchronization mark . The synchronization mark points to the problematic geometries and enables you to solve the problems with the geometries that were not synchronized. 222
    • 4. GeometryGeometry synchronizationWhen the geometry has to be synchronized (this geometry is marked with the synchronizationmark), do the following to synchronize it: 1. Right-click on a geometry entry in SolidCAM Manager. 2. Choose Synchronize from the menu.or 1. Right-click on an operation entry in SolidCAM Manager. 2. Choose Synchronize from the menu. The Synchronize & Calculate command enables you to synchronize the operation geometries and calculate the tool path.All of the geometries used in the operation are synchronized.During the synchronization, SolidCAM tries to update theSolidCAM geometry according to the updated SolidWorks model.SolidCAM finds the updated edges according to the saved tags dataand tries to re-create the geometry chain. SolidCAM recognizesgaps between geometry entities and closes them.223
    • SolidCAM closes the gaps by using the smallest number of entities. There are two methods ofclosing gaps: • If the original geometry entities are in the SolidCAM same plane with the Coordinate System, Geometry SolidCAM tries to close the gap with entities in the same plane only. • If the original geometry entities are not on a plane, SolidCAM is using a random search algorithm that closes the gap in the geometry. This search algorithm can SolidWorks Model find different solutions to close the same gap; this depends on the sequence of the entities involved in the loops that connect Gap area to the geometry entity.The geometry that cannot be updated is marked with an exclamationmark .You have to edit such geometries and manually update the problematicchains. SolidCAM does not find new chains that are not directly connected to old chains. The number of chains in the geometry remains the same. For example, SolidCAM does not find a new island in a pocket geometry.4.7.2 Synchronization of the 3D Model geometryThe calculation of the tool path for the 3D Modelgeometry is based on a facet model produced forthe whole SolidWorks model. SolidWorks Model SolidCAM GeometryWhen SolidCAM determines that the solid haschanged, it does not need to detect what haschanged; it simply recalculates the facet model. Updated SolidWorks Updated SolidCAM Model Geometry 224
    • 4. GeometrySynchronization checkSolidCAM enables you to check the synchronization status bycomparing the SolidWorks model and the SolidCAM 3D Modelgeometry. You can check the synchronization status automaticallyor manually, which depends on the Synchronization settings.When you need to check the synchronization status of the geometrymanually, do the following: 1. Right-click on an operation or geometry entry in SolidCAM Manager. 2. Choose the Check Synchronization item from the menu.If a difference is found, SolidCAM marks the geometry and relatedoperations with the synchronization mark .Geometry synchronizationWhen the geometry has to be synchronized (the one marked withthe synchronization mark), do the following to synchronize it: 1. Right-click on a geometry entry in SolidCAM Manager. 2. Choose Synchronize from the menu.or225
    • 1. Right-click on an operation entry in SolidCAM Manager. 2. Choose Synchronize from the menu. The Synchronize & Calculate command enables you to synchronize the operation geometries and calculate the tool path.All the SolidCAM geometries used in the operation aresynchronized.During the synchronization, SolidCAM recalculates the facetmodel.4.7.3 Boolean operationsSolidCAM enables you to perform a number of boolean operationsbetween working area geometries and boundaries.Choose the Boolean operations command from the right-clickmenu on the Geometries header.The Boolean Operations dialog box is displayed.Coordinate SystemThis field enables you to choose the Coordinate System where the sourcegeometries for the boolean operation are located. The resulting combinedgeometry is created in the chosen coordinate system.ConfigurationsThis field enables you to choose the SolidWorks configuration where thesource user-defined geometries for the boolean operation are located. 226
    • 4. GeometryOperation typeThis field enables you to define the type of the boolean operation. The following boolean operationsare available: Unite Source geometries This option enables you to unite selected geometries into a single one. All internal segments are removed; the resulting geometry is outer profile. Geometry 1 Geometry 2 Resulting geometry Merge Source geometries This option enables you to merge a number of geometries, created by different methods, into a single one. Geometry 1 Geometry 2 Resulting geometry Geometry 3 Subtract Source geometries This option enables you to perform subtraction of two geometries. The order of the geometry selection is important; the second selected geometry is subtracted from the first selected one. Geometry 1 Geometry 2 Resulting geometry227
    • Intersect Source geometries This option enables you to perform intersection of two geometries. Geometry 1 Geometry 2 Resulting geometryThe Accept button performs the command chosen in the Geometries section.GeometriesThe Geometries section displays all the available working areageometries classified by the definition method.This section enables you to choose the appropriate geometries for theboolean operation. Select the check box near the geometry name inorder to choose it for the boolean operation.When you click on the Accept button, the resulting geometry is displayedin the list under the Combined 2D header. SolidCAM enables you toedit the name of the created geometry. The newly created geometry isautomatically chosen for the further boolean operation. The resulting combined geometry is always a 2D geometry even if one or more of the input geometries is a 3D boundary.The right-click menu available on the list items enables you to perform the following operations: • The Accept button enables you to perform the chosen boolean operation with the selected geometries. • The Unselect all option unselects all the chosen geometries. • The Delete option enables you to delete combined geometries generated in the current session of the Boolean Geometries dialog box. 228
    • Operations 5In SolidCAM, an operation is a single machining step. A workpiece isusually manufactured using several machining steps and technologies.For each of these steps you can define a separate operation.An operation can be very complex, but always uses one tool, onemajor geometry and executes one machining type, e.g. 3D Milling,Profile Milling or Drilling. You can edit any single machining operation,change the operation sequence and generate the GCode, combineand split the operation list of your CAM-Part.  Adding an operation  Operation dialog box interface  Working with operations  Operation Transformations  Fixture
    • 5.1 Adding an operationThis command enables you to add a new operation to your CAM-Part. In SolidCAM, an operationis a single machining step. Normally, you manufacture a workpiece using several machining stepsand technologies. For each of these steps you can define a separate operation. An operation can bevery complex, but always uses one tool, one major geometry and executes one machining type, e.g.3D milling, profile milling or drilling.You can edit any single machining operation,change the operation sequence and generatethe GCode, combine and split the operation listof your CAM-Part. 1. In SolidCAM Manager, right- click on an operation. 2. Move to the Add Operation submenu and choose the type of operation you want to define. • When you add an operation by right-clicking on the Operations header, the new operation is added at the end of the operation list. • When you add an operation by right-clicking on an existing operation, the new operation is inserted after the selected operation. 230
    • 5. Operations5.2 SolidCAM Operation InterfaceSolidCAM operation dialog box interface has the following common areas: Operation name Template TechnologyGeometry parameters InfoTool parametersMachining levelsparametersTechnological parametersAdvanced TechnologyLink parameters Parameters pageMiscellaneous parameters Parameter illustration Operation buttons Technology The Technology box displays the chosen technology according to the operation type. Operation name The Operation name box displays the operation name and enables you to choose another already existing operation as a template. Template The Template box enables you to save the current operation as a template and to load another already existing template. Info By clicking on this icon, you can display a window that contains the information summary of the operation. In this window, the name of the operation, the Tool data and the Milling levels data are listed.231
    • Parameters pages and illustration The list on the left side of the dialog box enables you to switch between the following parameters pages: • Geometry This page enables you to define the geometry for the operation. • Tool This page enables you to define the tool for the operation. • Levels This page enables you to define the machining levels for the operation. • Technology This page enables you to define the technological parameters such as offsets, roughing and finishing data, depth type, etc. The Advanced Technology page contains the infrequently used parameters and options whose definition is required only in particular machining cases. • Link This page enables you to define the way how the tool approaches the material and retreats away. • Misc. parameters This page contains the miscellaneous parameters such as Message, Extra parameters, and so forth. In the bottom left corner of the dialog box, the illustration of a currently selected interface element is displayed to facilitate the definition of the corresponding parameter.Operation buttons At the bottom, the operation buttons are located. These buttons enable you to save and calculate the operation, start its simulation, etc. 232
    • 5. Operations5.2.1 Operation nameWhen you define a geometry and a tool, SolidCAM automatically enters the default name(e.g. 3DR_Profile_T1) based on the operation type, geometry name and tool number. 3DR_Profile_T1Operation type Geometry Tool abbreviation nameYou can edit the operation name, if necessary.SolidCAM uses the following operation type abbreviations for Milling operations:2.5D Milling • FM_ — Face Milling • F_ — Profile • F3D_ — Contour 3D • P_ — Pocket • D_ — Drilling • THM_ — Thread Milling • S_ — Slot • TSlot_ — T-Slot • TS_ — Translated Surface • PR_ — Pocket Recognition • DR_ — Drill Recognition233
    • 3D Milling • 3DR_ — 3D Roughing • 3DS_Lin — Linear 3D Semi-Finishing strategy • 3DS_Offs — Offset cutting 3D Semi-Finishing strategy • 3DS_Sp — Spiral 3D Semi-Finishing strategy • 3DS_Cir — Circular Pocket 3D Semi-Finishing strategy • 3DS_CZ — Constant Z 3D Semi-Finishing strategy • 3DS_Pen — Pencil Milling 3D Semi-Finishing strategy • 3DS_CS — Constant Step Over 3D Semi-Finishing strategy • 3DF_Lin — Linear 3D Finishing strategy • 3DF_Offs — Offset cutting 3D Finishing strategy • 3DF_Sp — Spiral 3D Finishing strategy • 3DF_Cir — Circular Pocket 3D Finishing strategy • 3DF_CZ — Constant Z 3D Finishing strategy • 3DF_Pen — Pencil Milling 3D Finishing strategy • 3DF_CS — Constant Step Over 3D Finishing strategy • 3DD — 3D Drilling operation • 3DE — 3D Engraving operationWhen you add a new operation, you can use an existing operation as a template for the newoperation. All values of the template operation are copied and you only need to edit some varyingparameters, e.g. select another geometry or redefine the surface offset value.Use the Operation name list to select the template operation. 234
    • 5. Operations5.2.2 TemplateSolidCAM enables you to create operation templates: once defined, an operation can be saved as atemplate and its data can be loaded into a new operation of the same type. The saved template datadoes not include the geometry which must be defined for each operation separately after loadingthe template. The saved template can optionally include the tool data.This section provides you with the following functionality:Saving TemplatesThe Save Template button enables you to save all of the current operation data (except for thegeometry) as a template.The Template Manager dialog box isdisplayed. This dialog box enables you todefine a name for the template. The defaultlocation offered by SolidCAM is defined inthe SolidCAM Templates Directory section ofthe Part Settings dialog box (see topic 2.10.9).The Operation Templates table displays alloperation templates located in the SolidCAMTemplates Directory, their types and thetechnology.The Include tool data check box enables youto include the tool data in the saved template.The saved tool data is used during the furthertemplate loading.235
    • Enter the name in the Template edit box to save a new template or choose an existing template fromthe table to overwrite it and click on the OK button. If a template with the defined name alreadyexists in the current location, SolidCAM displays the following warning message:When you confirm this warning by clicking on the Yes button, the existing template is beingoverwritten with the new one. When you click on the No button, the Save template dialog box isdisplayed again so that you can choose a different name for the template.Saving an operation as a template using SolidCAMManagerYou can also save an existing operation as operationtemplate by right-clicking on the operation name inSolidCAM Manager and choosing Create Templatefrom the menu.This command displays the Template Manager dialogbox that enables you to save the template data asdescribed above. 236
    • 5. OperationsLoading TemplatesThe Load Template button enables you to load an already existing template into the currentoperation. The Template Manager dialog box is displayed.This dialog box displays only the templates of type/technology suitable for the current operation.Choose the required template and click on the OK button. When the template is loaded, all thecurrent operation data is substituted with the data from the template.When a template is loaded into the operation, its name is displayed in the edit box in the Templatessection.When you place the mouse cursor over the edit box, the full path to the loaded template is displayedin a pop-up message.When any of the operation data is modified after loading the template, the template name in theedit box is marked with asterisk (*).237
    • Tool searchWhen an operation template is loaded, SolidCAM checks for tool data in the template. If the tooldata was saved in the operation template, the tool search is performed as follows: • When a tool used in the operation template is defined as Permanent, the tool search is performed according to the tool number only. First, the tool search is performed in the Part Tool Table. If the tool with the defined number is not found in the Part Tool Table, additional search is performed in the Current Tool Table. If a tool with the defined number is found in the Current Tool Table, it is being copied into the Part Tool Table and chosen for the operation. If it is not found in the Current Tool Table, the following error message is displayed: When you confirm this message, the operation dialog box is displayed again so that you can define a tool. • When the tool in the operation template is not defined as Permanent, the tool search is performed according to the tool parameters defined on the Tool search page of the SolidCAM Settings dialog box. The tool search is performed in the Part Tool Table. If a tool with the same definition as that used in the template is not found in the Part Tool Table, additional search is performed in the Current Tool Table. If a suitable tool is found in the Current Tool Table, it is being copied into the Part Tool Table and chosen for the operation. If it is not found in the Current Tool Table, a new tool with the parameters defined in the template is being added to the Part Tool Table and automatically assigned the first not used tool number. When you load a template with tool data into an operation in which the tool is already defined, the following message is displayed: When you confirm this message, SolidCAM replaces the tool defined in the operation with the tool defined in the template. 238
    • 5. OperationsCreating a new operation from an existing templateSolidCAM enables you create a new operation froman existing template. Right-click on an operation entryin SolidCAM Manager and choose Add Operation fromTemplate from the menu.The Template Manager dialog box is displayed. This dialogbox enables you to choose an existing template. In this case,the Template Manager dialog box displays all the templatesexisting in the SolidCAM Templates Directory regardless oftheir type/technology.When you confirm the dialog box by clicking on the OKbutton, SolidCAM inserts the chosen operation templateinto the SolidCAM Manager tree.The inserted operation is incomplete; it means that theoperation has no defined geometry and tool (if the initialoperation template used for the operation definition had notool). The incomplete operations are marked with red colorin SolidCAM Manager.Since the incomplete operations have no geometry, their tool pathcannot be generated. In order to completely define the operation,you have to edit it by defining the machining geometry and tool (ifnecessary).During creation of a new operation from an operation template,SolidCAM assigns the Machine Coordinate System #1 (Position #1)for the newly created operation. During the operation editing, thisCoordinate System can be changed.239
    • Process TemplateA Process Template is a template of a series of operations that execute a specific machining task.This functionality enables you to store a complete chain of technological operations as a templateand apply it for the machining of similar cases.Defining Process TemplatesTo create a process template, select in SolidCAMManager all the names of operations intended tobe included in the Template, right-click and chooseCreate Template.The Template Manager dialog box is displayed.This dialog box enables you to save the chosenoperations as a process template.All the process templates existing in the SolidCAMTemplates Directory are displayed. The processtemplates names are listed in the Template Folderssection under the Process Templates header. Thecontent of the templates is displayed in the OperationTemplates table.The Include tool data check box enables you to includethe tool data into the saved process template. 240
    • 5. OperationsTo save the selected operations as a new process template, enter a name in the Process name editbox or choose an existing process template from the Process Templates list and confirm by clickingon the OK button. If a process template with the defined name already exists in the current location,the following warning message is displayed:When you confirm this warning by clicking on the Yes button, the existing process template is beingoverwritten with the new one. When you click on the No button, the Template Manager dialog boxis displayed again so that you can choose a different name for the process template. The Template Manager dialog box provides you with the capability to create an empty process template and copy a number of operation templates from different process templates into this empty one.Using Process TemplatesSolidCAM enables you to insert operation templates containedin a process template into a CAM-Part and convert them intoregular SolidCAM operations. To insert a process templateinto the CAM-Part, right-click on the Operations header or onseveral selected operations in SolidCAM Manager and chooseAdd Operation from Process Template.This command displays the Template Manager dialog boxthat enables you to choose an existing process template to beinserted.241
    • During creation of a new operation from the process template,SolidCAM displays the CoordSys selection dialog box that enables youto choose the Coordinate System to be used in the created operations.The inserted operations are incomplete; it means that the operationshave no defined geometry and tool (if the initial operation templateused for the operation creation had no tool). The incomplete operationsare marked with red color.Since the incomplete operations have no geometry, their tool path cannot be generated. In order tocompletely define the operation, you have to edit it by defining the machining geometry and tool(if necessary).Managing operation/process templatesTo manage your operation and process templates, click Manage in the SolidCAM menu.TemplatesThe Template Manager dialog box is displayed.The Template Folders section contains the Templates and ProcessTemplates headers.When the Templates header is selected, all the operation templates located in the SolidCAM TemplateDirectory are displayed in the Operation Templates table.All the process templates located in the SolidCAM Template Directory are listed under the ProcessTemplates header. When a process template is selected, all the operation templates included in it aredisplayed in the Operation Templates table. 242
    • 5. OperationsManaging process templatesSolidCAM enables you to manage the processTemplates with the right-click menu available onthe Process Templates header or on each processtemplate.This menu provides you with the followingcommands: • New Process Template This command enables you to create a new empty process Template. • Rename This command enables you to rename an existing operation template. • Delete This command enables you to delete an existing operation template.Managing operation templatesSolidCAM enables you to manage operationTemplates with the right-click menu availableon the Operation Templates table entries. Thismenu is available for the standalone operationtemplates located in the SolidCAM TemplateDirectory and for operation templates includedinto process templates. • Create Process Template This command enables you to create a new process template; the current operation template is added to this process.243
    • • Copy This command enables you to copy the current operation template into the clipboard.• Paste This command enables you to paste the operation template from the clipboard. The operation template is inserted into the chosen location (either into the active process template or as a standalone operation template into the into the SolidCAM Template Directory).• Edit This command enables you to load the chosen operation template for editing. When a template is loaded, SolidCAM displays the appropriate operation dialog box with the template data. SolidCAM enables you to edit all the parameters and options of the template, except for the geometry and coordinate system. The Save Template button enables you to save the template data using the Save template dialog box.• Delete This command enables you to delete the active operation template. 244
    • 5. Operations5.2.3 InfoThe button at the right side of theoperation dialog box displays a windowthat contains the information summaryof the operation. In this window, thename of the operation, the Tool dataand the Milling levels data are listed.5.2.4 Operation buttonsSaveAll settings and parameters of the operation are saved on your disk. The tool path, however, is notcalculated. This button enables you to postpone the calculation or to calculate operations in batches.Use the corresponding commands of SolidCAM Manager to calculate the operation later on. In the operation list, all operations that have not been calculated are marked with asterisk (*).Save & CalculateAll settings and parameters of the operation are saved on your disk and the tool pathis calculated. After the calculation has been performed, you can exit from the operation dialog boxand return to SolidCAM Manager.245
    • There is no need to recalculate an operation if its changed parameters do not affect the tool path.These operation parameters include: • Tool Outside Holder Length • Tool Cutting Length • Holder • Operation name • Message • Extra parameters • FeedThere is no need to recalculate all the operations if the CNC-machine is changed, as long as thefollowing MAC parameters are not changed: • compensation • comp_by_zero_tool • comp_arc_arc • comp_arc_line • comp_line_line • comp_x_start • min_delt_arc_rad • zero_value • gen_procs • abs_zero_chng • full_gcode • init_cpos • set_dir • loops • eps_line • next_angleFor more information on these parameters, refer to SolidCAM GPPTool User Guide.SimulateThis button performs simulation of the cutting process. The operation must be calculated before this option can be used. 246
    • 5. OperationsGCodeThis button generates the temporary GCode file for the operation. The GCode file is generated intothe CAM-Part folder regardless of the defined settings. The generated GCode file is opened in thetext editor determined by SolidCAM Settings. When you close the operation dialog box, the file isremoved. Note that the operation must be calculated before this option can be used. To save the temporary GCode file, use the text editor functionality.Save & CopyThis button saves the current operation data and automatically creates a new operation with thesame parameters. The new operation is automatically opened for editing.Using the Save & Copy functionality, you can quickly create a new similar operation where mostparameters are identical.ExitThis button enables you to close the operation dialog box and return to SolidCAM Manager. Anychanges you made in the operation dialog box are lost if you exit the operation without prior saving.5.2.5 CalculatorSolidCAM enables you to use a built-in calculator to calculateparameter values. The Calculator is available for each numericparameter either by choosing the appropriate command from theright-click menu or by pressing the F2 key.The Calculator dialog box enables you to enter any expression(Expression edit box) and calculate its value (Result edit box).You can use the following symbols in the Expression edit box: • Addition (+) • Subtraction (-) • Multiplication (*) • Division (/)Parentheses are acceptable.247
    • When multiplication and division occur together in an expression, each operation is calculated asit occurs from left to right. When addition and subtraction occur together in an expression, eachoperation is calculated in order of appearance from left to right. Parentheses can be used to overridethe order of precedence and force some parts of an expression to be evaluated before others.Operations within parentheses are always performed before those outside. Within parentheses,operator precedence is maintained.SolidCAM enables you to use a set of standard mathematicalfunctions like sine, cosine, etc. in your formulas. Functions can beeither written manually in the Expression field or chosen from theFunctions list.The Functions button enables you to display/hide the Functionslist.Example: To calculate the value of the following formula: 152.8 / 2 tan (63/2) you have to write the expression: (158.8/2)/(tan(63/2)) The result (~129.56) is displayed in the Result field.To insert the calculated result into the field from where the calculator was started, click the OKbutton in the Calculator dialog box.SolidCAM standard functions sqrt() Returns a value specifying the square root of a number. sin() Returns a value specifying the sine of an angle. cos() Returns a value specifying the cosine of an angle. tan() Returns a value specifying the tangent of an angle. 248
    • 5. Operations abs() Returns a value of the same type that is passed to it specifying the absolute value of a number. The absolute value of a number is its unsigned magnitude. For example, and abs(1) both return 1. abs(-1) acos() Returns a value specifying the arccosine of a number. asin() Returns a value specifying the arcsine of a number. atan() Returns a value specifying the arctangent of a number. atan2(,) Returns a value specifying the arctangent of quotient first and second arguments. dist(,) and ang(,) dist(X,Y) (X,Y) Returns polar coordinates: distance and angle (in radians) of the point defined in Cartesian coordinates. ang(X,Y) 0 pow(,) Returns a value of the first argument raised to the power of the second argument. For example, pow(2,3) returns 8. log10() Returns a value specifying the base-10 logarithms of a number. ln() Returns a value specifying the natural logarithm of a number.249
    • sum3( , , ) Returns the sum value of three arguments. int() Returns the integer portion of a number. rad() Converts degrees to radians. deg() Converts radians to degrees.5.2.6 Geometry pageThis page enables you to choose the appropriate Coordinate System and to define the MachiningGeometry for the operation. 250
    • 5. OperationsCoordSysThis button enables you to define a Coordinate System for the operation.You can choose the Coordinate System forthe operation by picking it in the list or byclicking on the CoordSys button and selectingchains on the graphic screen. The CoordSysManager dialog box is displayed. Togetherwith this dialog box, SolidCAM displays thelocation and axis orientation of all CoordinateSystems defined in the CAM-Part.The Coordinate System can be chosen fromthe list or picked directly on the model.To get more information about the Coordinate System, right-click on its name in the list and choose the Inquire option fromthe menu. The CoordSys Data dialog box is displayed.After the Coordinate System selection, the model is rotated tothe appropriate orientation. The selection of the Coordinate System must be the first step in the operation definition process.After the Coordinate System has been chosen, define the maingeometry for the operation.If you have already defined geometries for this CAM-Part, youcan choose a geometry from the list. When you choose a Geometry from the list, the related Coordinate System is being chosen automatically.DefineThis button enables you to define a new geometry for the operation.ShowThis button displays the model geometry in the SolidWorks window.251
    • 5.2.7 Tool pageThe Tool page of the operation dialog boxenables you to define the tool and the relatedparameters for the operation.When the tool is defined, it displays thefollowing tool parameters: • Tool type • Number • Diameter • Corner radiusThe 3D View section displays the image ofthe chosen tool. This image can be zoomedand rotated.SelectThis button enables you to edit the tool parameters or define the tool for the operation. • When the tool is not defined for the operation, this button displays the View page of the Part Tool Table dialog box that enables you to choose the tool from the table or add a new one. Choose the tool from the Part Tool Table and click on the Select button. 252
    • 5. Operations • When the tool is defined for the operation, this button displays the Edit page of the Part Tool Table dialog box that enables you to edit the tool parameters and choose another tool from the list on the right or add a new one. The following pages are available: • The Tool Topology page (see topic 3.8.1) contains the Topology data of the tool, such as diameter, length, angle, corner radius etc. • The Default Tool Data page (see topic 3.8.2) contains the default Tool Material data, Feed and Spin data and diameter and length offset numbers. • The Tool Message page (see topic 3.8.3) contains the fields in which user messages are entered. • The Tool Coolant page (see topic 3.8.5) enables you to define the tool coolant options. • The Holder page (see topic 3.8.4) enables you to define the tool holder by choosing it from the global or local tool table and specifying the related parameters. • The Shape page (see topic 3.8.6) enables you to choose a shaped tool for the operation.253
    • DataThis button displays the Operation Tool Data dialog box. This dialog box displays the tool material,feed and speed parameters and the diameter and length offset numbers used in the current operation.When the tool is chosen for the operation, SolidCAM fills this dialog box with the default data ofthe selected tool. The Operation Tool Data dialog box enables you to edit the tool parameters forthe specific operation only. Tool Material This section describes one or more of the following properties of the tool: • Material (High Speed Steel, Carbide, etc.); • Working conditions; • Usage (rough, finish, etc.). The Tool Material is used to define the Speed and Feed defaults. When you choose the Tool material, the feed type is changed to FZ and the spin type to V. The Feed and Spin values are default system values since the Work material has not been defined yet. Loading the tool to an operation connects the Tool material to the Work material and the correct Feed and Spin values are loaded from the Speed/ Feed defaults table. 254
    • 5. Operations Spin This field defines the spinning speed of the tool by the following values: • Spin rate – normal spin rate; used in rough milling. • Spin finish – finish spin rate; used in finish milling. The Spin finish check box enables you to optionally define different values for Spin rate and Spin finish. When this check box is selected, the corresponding edit box is available so that you can edit its value. When this check box is not selected, the specified Spin rate value is used for both rough and finish machining. The spin value can be defined in two types of units: S and V. S is the default and it signifies Revolutions per Minute. V signifies the material cutting speed in Meters per Minute in the Metric system or in Feet per Minute in the Inch system; it is calculated according to the following formula: V = (S * PI * Tool Diameter) / 1000 (for the Metric system); V = (S * PI * Tool Diameter) / 12 (for the Inch system). Feed This field defines the feed rate of the tool by the following values: • Feed XY – feed rate in the XY-plane. • Feed Z – feed rate in the Z-direction. • Feed finish – feed rate used for finish milling. The Feed finish check box enables you to optionally define different values for Feed XY and Feed finish. When this check box is selected, the corresponding edit box is available so that you can edit its value. When this check box is not selected, the specified Feed XY value is used for both rough and finish machining. • Feed Link – feed rate used for tool path linking movements when the Hatch strategy is chosen. • Feed Lead in/out – the feed rates used for approach and retreat tool movements. The feed value can be defined in two types of units: F and FZ.255
    • F is the default and it signifies Units per minute. FZ signifies Units per tooth and is calculated according to the following formula: FZ = F/(Number of Flutes * S) 3D Model - Entry only When this check box is selected, the defined Feed Z is used for vertical movements only. When this check box is not selected, the defined Feed Z is used for all movements when the Z-coordinate changes. This option is available only for the 3D Milling operation.Diameter offset number This parameter defines the number of the Diameter Offset Register of the current tool in the Offset table of the CNC-machine.Length offset number This parameter defines the number of the Length Offset Register of the current tool in the Offset table of the CNC-machine.Second offset number This parameter defines the register number of the upper cutting face offset, in the offset table of the CNC-machine. This option enables SolidCAM to automatically take into account the minor size differences between the defined tool and the one actually used for cutting the workpiece, if there are any. You may choose not to use this option by clearing the check box. This option is available only for the T-Slot operation. 256
    • 5. Operations5.2.8 Levels pageThis page enables you to specify the Z-levels at which the tool movements are executed. The defaultinput values of these parameters are the CAM-Part values that you have specified in the CoordSysData dialog box.To define the Milling levels, enter the values or use the appropriate buttons to pick the Z-levels onyour 3D model.Start levelThis option defines the Z-level that can be optionally used for interoperational movements. The Start level button and the related edit box are available only if the Operation Start level option is chosen in Part Settings (see topic 2.10.2).The default Start level value is equal to the Part Clearance level value of the Coordinate Systemchosen for the operation.The Start level cannot be lower than the Operation Clearance level. If you are trying to save theoperation in which the defined Start level is lower than the Operation Clearance level, the errormessage is displayed:257
    • Clearance levelThis option defines the Z-level to which the tool retreats when it moves from one cut to another.Safety distanceThis option defines the distance to the Upper level at which the tool starts moving at the Z feed rateyou have entered for the tool. Movements from the Clearance level to this height are performed inthe rapid mode.Upper levelThis option defines the Z-level at which the machining starts.Lower level (Depth)This option defines the Z-level below which the tool does not mill in any milling strategy.Delta depthDelta depth is the offset for the cutting depth that can be changed with its associativity preserved.This parameter is always relative to the Depth defined for the operation.If the Delta depth value is positive, a blue arrow is displayed nearits field indicating a positive offset value (in the positive directionof the Z-axis).If the Delta depth value is negative, a red arrow is displayed nearits field indicating a negative offset value (in the negative directionof the Z-axis).The value of these parameters is the Z-coordinate. These parameters can be defined either byentering the value in the edit box or by picking a point on the solid model (except for Safetydistance). In the latter case, the parameters are associative to the solid model. Associativity enablesSolidCAM to be synchronized with the solid model changes. SolidCAM automatically updates theCAM data when the model is modified. 258
    • 5. OperationsDepth associativityThe following operation parameters are associative to the SolidWorks model. • Clearance level • Upper level • Lower levelSolidCAM enables you to define these parameters by picking the entities on the solid model. The Depth parameter used in some operations (Profile, Pocket, etc.) is indirectly associative. You have two possibilities: • To define Depth by manual input. • To define Lower level by picking on the model. In this case, Depth is calculated automatically. The associativity is established in Lower level. When either Upper level or Lower level is synchronized, Depth is updated.The associativity is saved only for the following picked items: • Vertex • Sketch point • Reference point • Part origin • Planar face parallel to the XY- plane of the current Coordinate System • Plane parallel to the XY-plane of the current Coordinate SystemThe Pick Lower level dialog box displays the Z-coordinate of the pickedpoint. If the value is associative to the model, the edit box is highlightedin pink.When the parameter is defined by picking model entities, SolidCAMdisplays the Z-coordinate of the picked point in the related edit box. Thebackground of the edit box changes. The value displayed in this edit boxis associative to the solid model.When you type in this edit box, the associativity is removed.259
    • The associative parameters are displayed in SolidCAM Manager under theoperation name.When the parameters are not synchronized, the parameters and the parentoperation are marked with the synchronization mark .The synchronization commands are available for operations in the right-click menu. • The Synchronize command enables you to synchronize the values of the parameters with the updated model. • The Synchronize & Calculate command enables you to synchronize the values of the parameters with the updated model and calculate the operation after the synchronization. 260
    • 5. Operations • The Check Synchronization command enables you to check the model for updates affecting the specified parameter. • The Break Z-Levels Associativity/Break associativity command enables you to break the associativity between Z-Levels parameters and the solid model. The confirmation message is displayed. • The Show command highlights the model entity with which the depth parameter is associated. The Show Geometry dialog box is displayed. The Exit button enables you to return to the normal model view.When the synchronization fails, SolidCAM marks the operation and theparameters with the exclamation mark.The parameters definition can be edited in the operation dialog box. Youhave to either type the necessary values or redefine the points on the model.In the first case, the associativity is removed.Interoperational tool movementsSolidCAM enables you to perform the interoperational tool movements either through the PartClearance level (same for all operations of the CAM-Part) or through the Operation Start level (canbe different from the Part Clearance Level and vary for each operation). Interoperational tool through Part Clearance level SolidCAM performs the interoperational movements through Part Clearance level when two neighboring operations use the same Tool (and Tool offset) and Coordinate System. Part Clearance Level Operation Clearance Level Operation Clearance Level Machining levels Safety distance Safety distance Rapid movements Feed movements261
    • Interoperational tool through Operation Start level You can change the level where the interoperational movements are performed for the specific operations when the same Coordinate system, Tool and Tool offset are used. This mode enables to reduce the rapid movements, especially between machining areas located significantly deeper than the Part Clearance level. In this mode, the tool performs interoperational movements at the Operation Start level, which can be different from the Part Clearance level. The Operation Start level can be specified separately for each operation. When the operation cuts are finished, the tool moves to the Operation Clearance level with the Rapid feed. Part Clearance Level Operation Start Level Operation Clearance Level Operation Clearance Level Machining Safety levels distance Safety distance Rapid movements Feed movements 262
    • 5. Operations If the Start level of the next operation is higher than the Operation Clearance level, the tool ascends to the Start level of the next operation, then performs XY-movement and descends to the Operation Clearance level of the next operation. All these movements are performed with the Rapid feed. The tool will then perform the rapid movement to the Safety Distance level of the first cut and start the descent to the first cut with the working feed. Next Operation Start Level Next Operation Clearance Level Previous Operation Clearance Level Safety distance Operation First cut Operation Last cut Rapid movements Feed movements If the Start level of the next operation is lower than the Operation Clearance level, the tool performs the XY-movements at the Operation Clearance level and than descends to Clearance level of the next operation without stopping at the Start level. All these movements are performed with the Rapid feed. The tool then performs the rapid movement to the Safety Distance level of the first cut and starts the descent to the first cut with the working feed. Previous Operation Clearance Level Next Operation Start Level Next Operation Clearance Level Safety distance Operation Operation Last cut First cut Rapid movements Feed movements263
    • All of these rules are relevant only when there is no Tool change, Tool offset change and Coordinate System change between the operations. If there are such changes, the Operation Start level is ignored and SolidCAM performs the tool movement through the Part Clearance level.5.2.9 Technology pageThis page enables you to define the technological parameters such as offsets, roughing and finishingdata, depth type, etc.5.2.10 Advanced Technology pageThis page contains the infrequently used parameters and options whose definition is required onlyin particular machining cases. 264
    • 5. OperationsAdvanced sortThis option enables you to define the machining order in case the operation geometry is composedfrom several chains. The button displays the Advanced Sort dialog box (see topic 6.6.3) that enablesyou to define the order of sorting of the chains included in the operation geometry.At the first stage, SolidCAM calculates the box surroundingeach chain. This box is used to determine the reference pointthat will be used for the advanced sorting. For Linear sortingstrategies, the reference point is automatically defined in thebox corner corresponding to the start position defined by thesorting strategy. For example, if the start position of the chosensorting strategy is the upper position (with the maximal X- andY-coordinates), SolidCAM automatically chooses the upperleft corner of the chain box to be the reference point. ForCircular sorting strategies, the reference point is automaticallychosen in the center of the calculated box.When the reference points are defined for all chains, SolidCAMperforms their sorting in the manner similar to the sorting ofthe drill positions. The resulting order of the reference pointsafter the sorting defines the order of the chains.Final cutsThis option enables you to divide the machined depth into two regions,each with its own Step down, when the Step down of the bottommostregion is smaller.The Final cuts dialog box enables you to define the parameters of thefinal cuts machining.When the Final cuts used check box is selected, Step downthe option is used.The Number of steps value defines the number offinal cuts. Step valueThe Step down value defines the distance betweentwo successive final cuts. Final cuts265
    • When the Final cuts option is used, SolidCAM performs the machining with the Operation Stepdown from the Upper level till the Depth calculated according to the following formula:Depth - Number of cuts * Step downFrom this depth, the machining is performed in a number of cuts determined in the Final cutsdialog box. The machining is performed in such manner until the full operation depth is reached. The Final cuts button is available only for Profile, Pocket and Contour 3D operations. In the Contour 3D operation, the Tool side must be set to Left or Right. When this option is used, the check box on the button is selected.Wall draft angleThis option enables you to perform the machining of inclined walls with a draft angle constantalong the entire geometry.When you click on the Wall draft angle button, the Wall Draft Angle dialog box is displayed.When the Wall draft angle check box is selected, the inclined wall machining is performed. 266
    • 5. OperationsThe Wall draft angle button is available only for Profile and Pocketoperations. In the Profile operation, the Depth type must be set toConstant or Define. When this option is used, the check box on the button is selected. External wall angle This parameter defines the draft angle of the wall measured from the Z-axis direction as shown. For the inclined wall machining, each cutting pass located at a specific Z-level is generated according to the specified External wall angle value. Island wall angle This parameter defines the draft angle of the island walls measured similar to the External wall angle parameter. This parameter is available only for the Pocket operation. For the inclined wall machining, each cutting pass located at a specific Z-level is generated according to the specified External wall angle/Island wall angle value.267
    • External corner typeThis option enables you to define how the cutting passes will be connected duringthe external corners machining. There are three ways to connect between the cuttingpasses:• Sharp corner The tool path is calculated to perform the machining of a sharp corner. This option affects only the machining of geometry sharp corners. Geometry• Conical fillet The tool path is calculated to perform the machining of the corner with a conical fillet; the radius of the tool path rounding increases from one pass to the next. This option affects only the machining of sharp geometry corners. Geometry 268
    • 5. Operations • Cylindrical fillet This option affects the machining of both of sharp and filleted corners of the geometry. The machining of sharp corners is performed similar to the Conical fillet option. For the filleted corners, the tool path is calculated to perform the machining of the corner with a cylindrical fillet; the radius of the tool path rounding is the same for all cutting passes. GeometryTrochoidal millingThis option enables you to replace the straightlines in a tool path by circular moves with aconstant radius. The Trochoidal button is available only for Profile, Pocket and 3D Milling operations. In the Profile operation, the Depth type must be set to Constant. In the 3D Milling operation, the Hatch or Contour strategy must be chosen. When this option is used, the check box on the button is selected.269
    • Potential benefits include: • Faster metal removal Making the constant circular curve the only direction change enables a high feed rate to be consistently maintained. • Longer tool life The cutting edge is in contact with the material through only about 5% of the cutter’s revolution vs. up to 50% for more conventional cutting. Cooling of the tool is improved.The Trochoidal dialog box enables you to define the parameters of trochoidal milling. • Radius This field defines the radius of the circle that describes the movement of the tool. • Step This field defines the distance between the centers of two adjacent circles that describe the tool movement. Radius Tool trajectory Step • Engagement angle This field defines the angle measured between two vectors describing the area of contact between the tool and the machined material. During the calculation, SolidCAM checks the engagement angle at each tool position defined by the Step parameter. If the engagement angle is greater than the specified Engagement angle value, SolidCAM at this position performs a circular tool movement with the radius defined by the Radius parameter. If the engagement angle is smaller than Engagement angle the specified Engagement angle value, SolidCAM does not generate a circular movement at this position; the tool moves to the next position. 270
    • 5. OperationsPlungingPlunging is a technology of removing material from a given areausing a special tool. Instead of milling the material, the tool movesup and down as in a drilling motion, travelling along the path typeyou choose. The Plunging button is available only for Profile and Pocket operations. In the Profile operation, the Depth type must be set to Constant. When the Plunging option is used, the check box on the button is selected.The Plunging dialog box is displayed. Step This field defines the distance between each two adjacent vertical plunging movements of the tool. Drill cycle type SolidCAM enables you to choose preferable drilling cycles for the plunging operation. 1. Click on the Drill cycle type button and choose the cycle type you want in the Drill cycle dialog box. 2. Click on the Data button and specify the parameters in the Drill options dialog box. For more information on the Drilling cycles, see topic 6.6.3.271
    • 5.2.11 Link pageThis page enables you to define the parameters of approach and retreat of the tool, linking betweentool paths, etc.5.2.12 Miscellaneous parameters pageThis page contains the miscellaneous parameters of the operation.MessageYou can type a message that will appear in the generated GCode file. G43G0 X-49.464 Y-38.768 Z12. S1000 M3 (Upper Face Milling) (--------------------------) (P-POCK-T2 - POCKET) (--------------------------) G0 X-49.464 Y-38.768 Z10. 272
    • 5. OperationsExtra parametersThis field is available only when special operation options have beenimplemented in the post-processor you are using for this CAM-Part.Click on the Parameters list button. The Operation Options dialog box is displayed with theadditional parameters defined in the post-processor.Gouge checkThis option enables you to perform gouge checking after the calculationof 2.5D Milling operations. During this checking, SolidCAM detectsall the gouges between the tool and the target model and informsabout the positions where these gouges occur.The Check gouges during calculation check box enables you toperform the gouge checking directly after the tool path calculation.You can also define the gouge checking tolerance in the correspondingedit box. If gouges are detected during this checking, SolidCAMinforms you about their location on the model by displaying thecoordinates in the Check gouges dialog box and dots showing thegouge positions on the model in the graphic area.273
    • In this dialog box, the check boxes enable you to control the visibility of the gouge positions on themodel. When a check box is selected, SolidCAM displays the corresponding gouge position on themodel with a cyan dot.When a check box is not selected, the related gouge position is not highlighted on the model. TheShow All button enables you to display all of the detected gouge positions on the model by selectingall of the check boxes. The Hide All button enables you to hide all of the detected gouge positionsfrom the model by clearing all of the check boxes.Approximation of arcsThis option enables you to control the process of arcs approximationat the operation level.The Approximate arcs by lines check box that enables you to controlthe existence of arcs in the GCode output for the current operation.When this check box is selected, SolidCAM approximates all tool path arcs by lines. The precisionof the approximation depends on the arc_max_chord and arc_max_angle parameters locatedin the MAC file; the resulting GCode does not contain arcs.When this check box is not selected, the resulting GCode might contain arcs. 274
    • 5. Operations5.3 Working with operationsSome of the operation commands affect all existing operations, others can only be applied to oneor more selected operations. SolidCAM produces different menus, depending on whether you right-click on the Operations header in SolidCAM Manager or on an existing operation in the list.In SolidCAM Manager, right-click on the Operations header. Theoperations menu is displayed.If you right-click on an existing operation, the operation commandsare displayed.5.3.1 Add OperationThis command enables you to add a new operation to your CAM-Part. In SolidCAM, an operationis a single machining step. Normally, you manufacture a workpiece using several machining stepsand technologies. For each of these steps you can define a separate operation. An operation can bevery complex, but always uses one tool, one major geometry and executes one machining type, e.g.3D milling, profile milling or drilling.You can edit any single machining operation, change the operation sequence and generate theGCode, combine and split the operation list of your CAM-Part.275
    • 1. In SolidCAM Manager, right- click on an operation. 2. Move to the Add submenu and choose the type of operation you want to define. • When you add an operation by right-clicking on the Operations header, the new operation is added at the end of the operations list. • When you add an operation by right-clicking on an existing operation, the new operation is inserted after the selected operation.5.3.2 Add Operation from TemplateThis command enables you create a new operation from an existing template.For more information on Operation Templates, see topic 5.2.2.5.3.3 Add Operations from Process TemplateThis command enables you to insert the operation templates contained in a process template intoa CAM-Part and convert them into regular SolidCAM operations.For more information on Process Templates, see topic 5.2.2. 276
    • 5. Operations5.3.4 Add Machining ProcessThis command enables you to use a previously created Machining Process in your CAM-Part.For more information on Machining Processes, refer to chapter 8.5.3.5 Create TemplateThis command displays the Template Manager dialog box that enables you to save operation dataas a template.When this option is applied to several selected operations, a process template is created with all theselected operations included.For more information on Operation Templates and Process Templates, see topic 5.2.2.5.3.6 EditThis command enables you to view or change the definition and parameters of an existingoperation. If you select this command, the corresponding operation dialog box is displayed and youcan change the operation definition.5.3.7 Calculate/Calculate AllBefore you are able to generate the GCode for your CNC-machine, you have to perform the toolpath calculation. Based on the geometries, machining strategy and technological parameters youhave defined and saved in the operations, SolidCAM calculates the movements of the tool. If you expect a long tool path calculation time, mainly in 3D Milling operations, it is advisable to define your operations, save them and postpone the tool path calculation. This function enables you to calculate large CAM- Parts with many operations in a batch routine e.g. overnight.5.3.8 GCode/GCode AllThe commands in this submenu enable you to generate, list, copy or print NC-programs.For more information on generating the GCode, refer to chapter 11.277
    • 5.3.9 Calculate & GCode AllThis command enables you to calculate all the operations in your CAM-Part and produce theGCode.5.3.10 Tool SheetThis option enables you to summarize the operations information by generating a tool sheetdocumentation.For more information on this option, see topic 2.14.5.3.11 SimulateYou can simulate and verify operations that have been saved and calculated.For more information on Simulation, refer to chapter 10.5.3.12 FileThis option enables you to append ASCII files with the GCode toyour CAM-Part.5.3.13 Operation GroupAn operation group in SolidCAM is a set of separateoperations with a defined sequential order. Theoperation group menu enables you to manageoperation groups.Define Operation GroupThis option converts the selected operations into an operation group.The Define New Operation Group dialog box is displayed. 1. Enter an operation group name in the Name field. 2. Choose the type from the list. 3. You can also enter the Description – a text string that describes the operation group.The selected operations are converted into an operation group. 278
    • 5. OperationsAdd Operation Group to Machining Process TableThis option enables you to insert the selected operation group into the current Machining ProcessTable.When the operation group is added, the following message is displayed:Remove Operations from Operation GroupThis option removes the selected operation from the operation group.Explode Operation GroupThis option turns the operation group into single operations.5.3.14 Cut/Copy/PasteSolidCAM enables you to cut, copy and paste operations. • The Copy command copies the selected operations into the clipboard. • The Paste command inserts the operations from the clipboard, after the selected operation. The pasted operations are marked by an asterisk; they must be calculated to obtain the tool path. If the clipboard is empty, the Paste command is unavailable. • The Cut command cuts the operations and copies them into the clipboard. When the operations are pasted from the clipboard, the source operations are removed.5.3.15 RenameSolidCAM enables you to rename a specific operation. Right-click onthe operation name in SolidCAM Manager and choose the Renamecommand from the menu.The Operation Rename dialog box is displayed. This dialog box enablesyou to assign a new name to the operation.279
    • 5.3.16 Change toolThis option enables you to change the tool used in a particular operation directly from SolidCAMManager. The Tool dialog box is displayed so that you can choose another tool.5.3.17 Change tool dataThis option enables you to edit the tool parameters such as tool material, feed and speed values,offset numbers used in a particular operation directly from SolidCAM Manager. The Operation ToolData dialog box is displayed so that you can edit the data.The All operations as first check box enables you to define the listed tool parameters in all operationsidentically to the first operation. 280
    • 5. Operations5.3.18 InfoThis option enables you to obtain the summary of a specific operationdirectly from SolidCAM Manager without opening the operation.The Info dialog box is displayed with the information of the selectedoperation. It contains Tool information (diameter, corner radius, taperangle and lengths); Operation Tool data (Feed and Spin parameters) andLevels (Upper level, Depth and Step down). The icon located in the title bar enables you to pin/unpin the Info dialog box.5.3.19 Delete/Delete AllThis command enables you to delete operations from the operation list of your CAM-Part. 1. Select an operation you want to delete. To delete several operations at a time, select them while holding the Shift or Ctrl keys. Right-click on the operations and choose the Delete command. 2. To delete several operations at a time, click Yes to all in the confirmation message.5.3.20 Suppress/UnsuppressSolidCAM enables you to suppress any operation in the CAM-Part,thus temporarily excluding it from the CAM-Part. When you suppressan operation, the operation does not participate in the calculation,simulation and GCode generation, as if the operation was deleted fromthe CAM-Part.In the SolidCAM Manager tree, the names of suppressed operationsappear in gray. The tool path check box is disabled for the suppressedoperations.The Suppress/Unsuppress command is available via the right-clickmenu, for a single operation or a list of operations.281
    • When the selected operations are not suppressed, right-click on the list of selected operations and choose Suppress. All selected operations are suppressed. When the selected operations are suppressed, the Unsuppress command available in the right-click operation menu unsuppresses the selected operations. When the list of selected operations contains both suppressed and unsuppressed operations, both Suppress and Unsuppress commands are available in the right-click menu. The Suppress command suppresses all the unsuppressed operations in the list. The Unsuppress command unsuppresses all the suppressed operations in the list.Editing suppressed operationsSolidCAM enables you to edit a suppressed operation. However,the Save & Calculate, Simulate and GCode buttons are unavailable. 282
    • 5. OperationsTool pathWhen an operation is suppressed, SolidCAM re-generates the CAM-Part tool path to exclude thetool path data related to the suppressed operations.The tool path stays unchanged till the parameters of the operation are updated.During the unsuppressing of the suppressed operation, the CAM-Part tool path is re-generated inorder to include the data of the unsuppressed operations.Suppressing linked operations 3D Drilling operation + 3D Milling operation When the Suppress command is applied to the 3D Drilling operation, the result is the following: • The 3D Drilling operation is suppressed; • The tool path of the related 3D Milling operation is removed and the operation appears marked with asterisk. When the Suppress command is applied to the 3D Milling operation, only this operation is suppressed. Both 3D Milling and related 3D Drilling operations must be selected in order to be suppressed together.283
    • 5.4 Managing Operations in the SolidCAM Manager tree5.4.1 Operation SequenceYou can change and rearrange the sequence of operations in theSolidCAM Manager. Drag the operation to its new place in the operationlist.5.4.2 Undo SequenceThis command enables you to undo your last change in the sequenceof the operation list.5.4.3 SplitThis command enables you to separate your list of operations beforethe GCode generation. If you place splits after operations and clickGCode All, separate NC-programs are generated for each operation orgroup of operations located between the corresponding splits. Eachsplit has a name and acts like a folder containing operations, fixtures,etc. In this example, you receive three separate GCode files for theoperations divided by the splits.Adding splits 1. Right-click on the operation after which you want to insert a split. 2. Choose the Split command from the menu. 3. Enter the split name in the Split dialog box. 3. The split is inserted.The (-) icon located near the split icon enables you to collapse/expand all the items (operations andfixtures) located under the split. 284
    • 5. OperationsManaging splits • Add This command enables you to add an operation to the list of operations that belong to the current split. • Add Machining Process This command enables you to add a Machining Process to the list of operations that belong to the current split. • GCode These commands enable you to generate and list GCode files for the operations that belong to the chosen split. The GCode file generated for each split is automatically saved in the CAM-Part folder.285
    • • User documentation These commands enable you to generate and edit the documentation that contains the data about the operations that belong to the current split. • Delete This command enables you to delete a split item. The confirmation message is displayed. Confirm it by clicking on the Yes button. • Rename This command enables you to edit the split name in the Split dialog box. • Suppress/Unsuppress This command enables you to suppress/unsuppress the split with all of its contents. Just like re-sequencing operations, you can move a split mark to another location in the operation list. Drag the split mark on the operation after which you want to insert it.5.4.4 Expand treeThis command enables you to open the operation list so that all the geometries used in eachoperation are displayed in the tree structure of SolidCAM Manager.5.4.5 Collapse treeThis command enables you to reduce the operation list so that only the operation names aredisplayed in the tree structure of SolidCAM Manager.5.4.6 Show/Hide Tools in treeThis command displays or hides the entries of tools used in the partoperations. 286
    • 5. OperationsThe right-click menu available on the tool entries enables you tochange the tool and manage the tool data for multiple operationswhere the same tool is used.Change toolThis option enables you to change the selected tool directly from SolidCAM Manager. The Tooldialog box is displayed so that you can choose another tool (see topic 5.3.16).Change tool dataThis option enables you to manage the tool data for multiple operations where the selected tool isused. The Operation Tool Data dialog box is displayed.The List operation section displays the list of operations that use this tool.The Show all operations using the current tool check box enables you to include in this list all ofthe CAM-Part operations in which the current tool is used. When this check box is not selected, theList operation section displays only the operations that belong to the current tool entry chosen inthe SolidCAM Manager tree.The All checked operations as selected one check box enables you to apply the parameters definedin the dialog box to all the checked operations.5.4.7 Show/Hide CoordSys in treeThis command displays or hides the entries of Coordinate Systemsused in the part operations.287
    • Indent according to Tools/CoordSysThis command available in the right-click menu on the operations header enables you to indent allthe operations in the CAM-Part according to the Tools/Coordinate Systems.5.4.8 Automatic SortThis command enables you to sort all of the operations that you created towork in a specific order. 1. Choose the Automatic sort item from the menu. The Automatic Sort Priority dialog box is displayed. 2. Choose the desired options. 3. Click on the OK button to confirm the operation. 4. All the operations are sorted in the specified order. If you click OK without choosing any of the options in the dialog box, the operations are sorted starting from tool number 1 and upward.Automatic Sort options: • CoordSys: operations are sorted according to the Coordinate System number. • Upper level: operations started on a higher level appear before operations started on a lower level. • Use center drill first: all tools tagged as center drills are moved to the top of the operation list. • Sort drill radius: drills can be sorted according to size, either from small diameters to large diameters or from large diameters to small diameters. 288
    • 5. Operations • Move drills to end: this option moves all drills not tagged as center drills to the end of the operation list. The following is the order of precedence if more than one option is chosen. 1. CoordSys 2. Upper level 3. Use Center drill first 4. Sort Drill radius 5. Move Drills to endUndo SortThis option returns the automatic sort to the original order.289
    • 5.5 Operation TransformationsWhen you transform an operation or a group of operations, commands such as move, copy, translateand rotate insert the corresponding G-function and cycle into the GCode file. You can check thedefined transformation during the tool path simulation. 1. In SolidCAM Manager, right-click on the entry of the operation you need to transform. 2. Choose the Transform option from the menu. 290
    • 5. Operations The Operation Transformations dialog box is displayed. The operation transformations are enabled only if your CNC-machine controller supports the corresponding function.5.5.1 Operation transformationsThis section offers you the choice of whether the originaloperation will be transformed or its copy will be added fortransformation and, in the latter case, enables you to define theplacing of the new operation in the SolidCAM Manager tree.The following options are available: • Edit operation transformations This option enables you to perform transformation of the selected operation. • New operation (add at current position in operations tree) This option enables you to add a copy of the selected operation and apply the transformation to the copied operation, without effect on the original operation. The transformed copy is inserted immediately after the original operation in the SolidCAM Manager tree. The original operation can be suppressed by selecting the appropriate check box in the Options section. • New operation (add at end of operations tree) This option also enables you to add a copy of the selected operation and apply the transformation to the copied operation, without effect on the original operation. The transformed copy is inserted at the end of the operation list in the SolidCAM Manager tree. The original operation can be suppressed by selecting the appropriate check box in the Options section.291
    • 5.5.2 OptionsThis section contains two check boxes that enable you to manage theoriginal operation: • Include original operation When this check box is selected, the original operation is included in the transforming action. • Suppress original operation When this check box is selected, the original operation is suppressed, and the transformation is applied only for the operation copy. This check box is available only when a new operation is added for transformation.5.5.3 Transformations tableThe transformations table lists the details of the defined transformation. • Operation name This column displays the list of operations to be transformed. In case of adding a new operation, the operation copy receives the Transform_ prefix with the sequential number of transformation. When an additional transformation action is defined on the existing transformation, the Transform_ prefix is added with the next sequential number, and the names of the previously transformed operations move under the new transformation. 292
    • 5. Operations • Transformation This column displays the type of transformation action to be performed on the selected operations. The following types of transformation are available: rotation, translation, mirroring and repeating the tool path using the fourth axis. • Description This column displays the details of transformation parameters defined for the current operations.5.5.4 Transformation buttonsThe buttons on the right represent the list of transforming actions that can beperformed on the chosen operations. Each button displays the related dialog boxthat enables you to define the parameters of the transformation.InitThis button cancels any transformation action that was performed on the operationsthat do not have inheritance (operation copy added for transformation). When youclick on this button to cancel the transformation defined for operations that haveinheritance, the following error message is displayed:If you want to cancel the transformation defined for operations with inheritance, exit the OperationTransformations dialog box and delete the operation copy in the SolidCAM Manager tree.293
    • RotateThis button enables you to define the tool path rotation around the Z-axis ofthe CoordSys origin or around the Z-axis passing through a defined point. Therotation can be performed using two options: • Delta Several rotations are performed from a start angle with a uniform delta angle. The Rotate Delta dialog box is displayed. 1. Enter the Number of Rotations. 2. Start angle – enter the start angle (+/-) relative to the positive X-axis. 3. Delta angle – enter the delta value (+/-) between two rotation steps. 4. Confirm with the OK button. • List This option copies the operation tool path to a list of angle locations defined by their angle relative to the positive X-axis. The Rotate list dialog box is displayed. 1. Enter the value of the angle and the number of rotations. 2. Click on the Add button to add the angle to the list of angles. 3. Confirm with the OK button. To edit an angle value in the list, click on the corresponding entry in the Value column and enter the new value. To delete an entry from the list, select it and click on the Delete Selected button. 294
    • 5. OperationsTranslateThis button enables you to copy the operation tool path to a rectangular matrix of locations (theMatrix option) or to a list of locations defined by their X-, Y- and Z-coordinates (the List option). • Matrix This option copies the operation tool path to a rectangular matrix of locations. When you choose this option, the Matrix dialog box is displayed. • Number of rows: enter the number of rows. • Number of columns: enter the number of columns. • X Step: enter the delta value between each two columns. • Y Step: enter the delta value between each two rows. • Rows first: the operation tool path is first copied horizontally, and then vertically in the defined matrix of locations. • Columns first: the operation tool path is first copied vertically, and then horizontally in the defined matrix of locations. • List This option copies the operation tool path to a list of locations defined by their X-, Y- and Z-values. The origin of the operation is moved to the absolute XYZ-position defined in the Translation List dialog box. 1. Enter the values of the absolute XYZ-position where the operation should be executed (separate the values by commas or spaces) or pick a point on the model. 2. Click the Enter button to add the position to the Translation list. 3. Confirm with the OK button. To edit a position in the translation list, select it, enter the new values for this position into the Offset value edit box and then click on the Enter button. To delete a position from the translation list, select it and press the Delete key.295
    • MirrorThis button enables you to mirror the operation tool path relativeto the X, Y or both axes. The point about which the operations aremirrored is either the CoordSys position or the Mirror/Rotate pointdefined in the operation. The Mirror dialog box is displayed. 1. Click on the corresponding button to define the axis around which the operations are mirrored: • X – mirrors around the X-axis. • Y – mirrors around the Y-axis. • XY – mirrors around both the X- and the Y-axes. • Reset enables you to clear the entry field. 2. Confirm with the OK button.4th AxisThis option enables you to execute 4-axis rotations of an operationtool path. After the 4th axis is rotated, the operation is executedagain. When you choose this option, the Rotate list dialog box isdisplayed. 1. Enter the value of the angle and the number of rotations. 2. Click on the Add button to add the angle to the list. 3. Confirm with the OK button.To edit an angle value in the list, click on the corresponding entry inthe Value column and enter the new value.To delete an entry from the list, select it and click on the Delete Selected button.SynchronizeThis button enables you to perform synchronization of the operation copies with their originaloperations, in case of changes to the original operations. Note that this button is available only forthe defined transformation with inheritance. 296
    • 5. OperationsWhen you click on this button, the Synchronization of operations technology dialog box is displayed. • Synchronize the technology of this operation with its original operation When the original operation has been edited, this option enables you to synchronize the operation copy with the performed changes. • Synchronize the technology of all operations with original operation When transformation is defined for multiple operations and the original operations have been edited, this option enables you to synchronize the operation copies with the changes made in the original operations.297
    • 5.6 FixtureSolidCAM enables you to define the Part Fixtures such as clamps, vises, jig plates, etc.This feature enables you to get a more realistic pictureduring the simulation and check possible collisionsbetween the cutting tools and fixtures. 1. Right-click on an operation entry in the SolidCAM Manager tree and choose Define Fixture. 2. The Fixture dialog box is displayed. This dialog box enables you to define the fixture geometry. 298
    • 5. Operations5.6.1 Fixture dialog boxDefine 3D ModelThis button enables you to select the 3D model for the fixture. The 3D Geometry dialog box isdisplayed.Show on ModelWith this button, you can highlight the selected fixture model in the SolidWorks window.299
    • ShowWith this button, you can display the Fixture in theRest Material window of SolidCAM.Self-intersectionsThe Check and fix button in the Self-intersectionssection enables you to check the model for self-intersections (see topic 10.6.6) and fix them if theyare found.When self-intersections are detected, the followingmessage is displayed:Confirm it with the Yes button to fix the self-intersections.Note that the process of self-intersection fixing can take a long time to complete, depending on thecomplexity of the model.When the fixture is defined, SolidCAM adds the Fixture item to the SolidCAM Manager tree.SolidCAM enables you to define any number of fixtures that can be used at different stages of theCAM-Part. 300
    • 2.5D Milling 6SolidCAM enables you to perform a number of standard 2.5Doperations like profile, pocket, slot machining, etc. These operationscan be performed using 2D sketches as well as solid models.Full tool path control and powerful algorithms ensure that yourmanufacturing will be performed in accordance with your plans.  Profile Operation  Pocket Operation  Drilling Operation  Slot Operation  Translated Surface Operation
    • 6.1 Profile OperationThis operation enables you to mill on or along a contour.The profile geometry can be either open or closed. In profilemilling you can optionally use tool radius compensation to theright or left side of the geometry. SolidCAM offers two typesof profiling: • Milling a single profile to the specified constant or variable depth in one step or in several user-defined down steps; • Milling concentric profiles to the specified constant or variable depth. This type of profiling generates several concentric profiles that start from the defined clear offset distance from the profile, and finishes on the profile geometry, thus clearing the area around the profile to a constant depth.In the Operations right-click menu, click Add Operation, Profile. The Profile Operation dialog boxis displayed. 302
    • 6. 2.5D Milling6.1.1 Levels pageThis page enables you to specify the Z-levels at which the tool movements are executed.6.1.2 Technology pageThis page enables you to define the technological parameters of the Profile milling.303
    • ModifyThe Tool side option enables you todefine the tool position relative tothe geometry. Left Right Center • Right: the tool cuts to the right of the profile geometry at the distance defined by the values set in the Modify offset section of the Modify Geometry dialog box. • Left: the tool cuts to the left of the profile geometry at the distance defined by the values set in Modify offset section of the Modify Geometry dialog box. • Center: the center of the tool moves on the profile geometry. The compensation cannot be used with this option. When the Zigzag option is used, the Tool side combo-box defines the tool location for the first cut. For each successive cutting pass, the tool position is changed relative to the geometry direction.GeometryThis button enables you to modify a geometry shared by severaloperations separately for each operation. The geometry modification is supported for Profile, Contour 3D, T-Slot and Translated Surface operations.Geometries shared by several operations can be modified separately for each operation. Thegeometry modification includes assigning different values to the Extension, Offset and Define Startparameters of the geometry, and also choosing which geometry chains are active in the operation (incase of multiple chain geometry). The modification is relevant only for the current operation anddoes not affect other operations where the geometry is used. 304
    • 6. 2.5D MillingThe Modify Geometry dialog box enables you to perform the geometrymodification for the current operation. • Tool side This option enables you to define the position of the tool relative to the geometry. • Chains This section displays the list of all geometry chains participating in the current geometry. The check box located near each chain name in the list enables you to include/exclude the chain from the geometry of the current operation. The right-click menu available on the elements of the list enables you to perform the following actions: • The Check All command enables you to check all the chains. • The Uncheck All command enables you to uncheck all the chains. • The Invert Check States command enables you to reverse the state of the check boxes. • The Reverse command enables you to reverse the direction of the chain. • The Reverse All command enables you to reverse the direction of all chains.305
    • • Start/End Extension This section enables you to define the extension for the selected chain. The Start and End parameters define the start and end extension lengths. The extension is performed tangentially to the chain entities at the start and end points of the geometry chain. The start and end elements are determined according to the chain direction. When a negative value is defined, SolidCAM shortens the chain by a distance measured along the chain elements and specified by the Start and End parameters. These parameters can be defined either by entering the values or by picking on the model (when the cursor is placed in the edit box). Start extension End extension Geometry chain The Apply to all button enables you to apply the extension defined for the selected chain to all chains of the geometry.• Modify offset This section enables you to define the offset for the Machining Geometry selected chain. Machining is performed at the specified offset. Modify offset 306
    • 6. 2.5D Milling Geometry chain Modify offset Modified chain SolidCAM enables you to define the Modify offset parameter by entering the value or by picking on the model (when the cursor is placed in the edit box). The Apply to all button enables you to apply the Modify offset value defined for the selected chain for all the chains of the geometry. The direction of the Modify offset Negative offset parameter for open contours is defined according to the chain Geometry chain direction. In case of a positive value, the offset is defined to the right side of the chain (according Positive offset to the chosen chain direction). In case of a negative value, the offset is defined to the left side of the chain (according to the chosen chain direction). For closed contours, a positive Positive offset Modify offset value defines the offset Geometry chain to the outside of the geometry; a negative Modify offset value defines the offset to the inside of the geometry Negative offset The Take 1/2 from selected offset option enables you to offset the chain by half of the defined offset value.307
    • In the part shown below the central pads should be machined with a single straight cutting pass located in the middle of the pad. After defining the geometry at the edge of the pad, the geometry is offset using the picked position at the opposite edge and the Take 1/2 from selected offset option. Modified geometry Picked offset position Geometry• Start position When the Default option is chosen, the start position is calculated automatically using the SolidCAM internal algorithm. When the Shift option is chosen, you to define the shifting of the start position for closed chains. The shifting of the start point is defined as a percentage of the chain length. You can define the start position shifting either by entering the Shift value or by picking the position on the model. For open chains, this section is disabled. The Apply to all button enables you to apply the Shift value defined for the selected chain to all closed chains of the current geometry. The Auto next button enables you to define the start points successively for all closed chains by picking the positions on the model. When this mode is activated, the first closed chain is highlighted, enabling you to pick the start position for it. When the position is picked, SolidCAM switches to the next closed chain and so on. The Resume button enables you to finish the automatic definition of the next start positions. The Set default button enables you to return the start position of the current chain to its initial state. When the Apply to all check box is activated, the Set default button returns the start positions of all chains to their initial state. 308
    • 6. 2.5D MillingCompensationWhen the Compensation check box is selected, the tool radius compensation options G4x of theCNC-controller are used in the GCode. • No compensation When the Compensation check box is not selected, SolidCAM generates a trajectory of the tool center as an offset by the tool radius from the geometry. Tool center trajectory Geometry This tool center trajectory is performed in the GCode. No compensation is used. • Radius compensation When the Compensation check box is selected, SolidCAM generates the trajectory of the tool center as an offset by the tool radius from the geometry. Tool center trajectory Geometry At the next stage, SolidCAM creates the tool path as the offset by the tool radius from the tool center trajectory. The offset is created in the geometry direction. Tool center trajectory Tool path The GCode is created for the tool path. The radius compensation is used in the GCode. The Offset value is equal to the Tool radius.309
    • • Zero Compensation SolidCAM calculates the trajectory of the tool center as the offset from the geometry. Tool center trajectory Geometry This trajectory is used in the GCode. The radius compensation is used. The Offset value is equal to 0. • Settings SolidCAM enables you to define the type of compensation used by the specific variable in the MAC file. Comp_by_zero_tool = N – the Radius compensation is used. Comp_by_zero_tool = Y – the Zero compensation is used. When the compensation is used for the tool path linked using the Zigzag option, SolidCAM takes into account the machining direction and the changes in the tool position relative to the geometry direction for each successive cut. The different compensation commands are used in the GCode output for even and odd cuts.Depth typeThis option enables you to choose the depth type for the profile. Constant SolidCAM generates a tool path with a constant depth as defined in the Milling levels area. 310
    • 6. 2.5D Milling Variable (Define) You can define a different depth at different profile points. 1. Choose the Define option. 2. Click on the Pick button. The Define depth dialog box is displayed. This dialog box enables you to control the points where the depth changes. The X,Y,Z dialog box enables you to enter the coordinates of the depth change points. Switch between the Select and the Unselect mode to define or remove points where the depth changes. The Undo button cancels or restores the last selection. You can specify a certain chain in the profile geometry using the combo box with the profile number and the Next Profile button. The Points field contains information about selected depth changing points. You can change the point properties by double-clicking the parameter in this area. • Profile No. – the Profile geometry chain number. • Z – the Z-coordinate of the profile depth at the specified point. • Type – the type of depth change: Vertical: the depth changes at specified points. Sloped: the depth changes gradually over the tool path segment. Depth change points Vertical type Sloped type Select the depth change point on the profile. The Depth dialog box is displayed. In this dialog box, specify the depth and the type of depth change.311
    • Helical This option enables you to enhance the productivity of profile machining by avoiding lead in/out movements at each Z-level and unnecessary rapid movements. With this option, the tool performs the spiral movements around the geometry with the continuous lowering along the Z-axis. For each turn around the geometry, the tool moves downward along the Z-axis according to the step down value. When the Profile depth is reached by the spiral movements, SolidCAM performs the last cut with the constant Z movement at the Profile depth level. Step downRest Material/ChamferThe Rest material option enables you to define parameters to removethe rest material left unmachined after previous operations. Rest MaterialThe Chamfer option enables you to machine chamfers with a Center drill tool. Rest material In Profile Machining, when a large tool is used around the profile, the tool leaves material in corners it cannot enter. The Rest material option enables you to remove the material from this area without defining a new geometry. 312
    • 6. 2.5D Milling The Rest Material dialog box is displayed. You have to define the following parameters: • Previous tool diameter – the diameter of the rough end mill used in the previous operation. The button enables you to display the Part Tool Table and select the previously used tool so that its diameter appears in the edit box. • Previous wall offset – the wall offset of the previous operation. • Extension – the overlap distance that you would like to start and end from the previous larger end mill. Extension Rest Material Milling type • Separate areas SolidCAM generates a profile tool path to clean areas that the previous tool could not mill. • Around profile SolidCAM machines the whole closed profile to mill the rest material.313
    • Chamfer This feature in Profile, Pocket and Contour 3D operations enables you to use a drill tool as well as a taper tool to add a chamfer to the edge of a part. In the Tool page of the operation dialog box, click on the Select button. The Part Tool Table dialog box is displayed. Choose a drill tool for the chamfering. In the Levels page of the operation dialog box, enter the size of the chamfer edge in the Profile depth field. In the Technology page of the operation dialog box, choose Chamfer from the Rest Material/Chamfer list and click the Data button. 314
    • 6. 2.5D Milling In the Chamfer dialog box, enter the following parameters: • Cutting diameter – the starting cutting diameter of the tool; • Feed – the feed rate you would like the tool to travel. Cutting Profile depth diameter (Chamfer length) (Profile depth) Chamfer height Cutting diameter When the Cutting diameter value is greater than the lower diameter of the taper tool cone, you can move the tool tip outside the chamfer. In such a way, the machining is performed by the conical part of the tool that can avoid the burr formation on the chamfer edge. If you choose to chamfer a part that ∅6 has a sharp corner, it is important that the cutting diameter is the same as the last tool used in that geometry so that the chamfer is ∅6 equal all around.Fillet size for last cutThis option enables you to add a radius to a sharp corner without theneed to change the geometry. This option is relevant for Profile, Pocket, Slot (Constant depth type) and the 3D Milling (Roughing and Constant-Z finishing) operations.315
    • • Internal This field defines the radius of internal Tool path corners. Geometry External • External fillets This field defines the radius of external corners. • The maximum external fillet size is defined in SolidCAM Settings (see topic 12.4.4). Internal • In the Profile operation, this fillets option is not available when the Tool side is set to Center.OffsetsSolidCAM enables you to specify the machining allowances that can beremoved either by profile finishing in the same operation or in anotheroperation. • Wall offset This option defines the offset that will remain on the wall of the machined part after roughing. Step down Wall offset Profile depth 316
    • 6. 2.5D Milling • Floor offset This option defines the offset that will remain on the floor of the machined part after roughing. When the Floor offset value is specified, SolidCAM performs the machining by the Z-levels defined with the Step down parameter. The machining is performed up to the Floor offset. Step down Profile depth Floor offset The Wall offset and Floor offset parameters are available only when the Rough section is activated.Clear offsetThis option generates several concentric profiles with constant depththat start at the defined clear offset distance from the profile and finishat the geometry of the profile, thus clearing the area around the profile.The Offset option defines the distance from the geometry at which the milling starts. The Offsetvalue must be equal to or greater than the Wall offset value. The tool starts milling the profile at thedistance defined by Clear offset and finishes at the distance defined by Wall offset.The Step over option defines the overlap of adjacent tool passes. It determines the offset betweentwo successive concentric profiles. Step over Clear offsetWalloffset Modify offset317
    • • The Zigzag option enables you to create the tool path for the Clear offset removal containing both climb and conventional movements. Clear offset tool path Profile geometry • The One way option enables you to create the tool path for the Clear offset removal containing only climb movements. Clear offset tool path Profile geometryRoughThis section enables you to perform the profile rough machining. Step down Profile roughing is performed in constant Step down Z passes. The Step down value defines the distance between each two successive Upper level Z-levels. The cutting passes are calculated using the Clear offset strategy with the specified Profile depth Offset and Step over parameters and taking into account the specified Wall offset and Floor offset parameters. 318
    • 6. 2.5D MillingFinishThis section enables you to perform the profile finishing. • Number of passes SolidCAM enables you to generate several finish passes to achieve the best surface quality. You can define the number of finish passes. • Extension/Overlap This option enables you to extend the profile in the positive profile direction. • Step down This parameter defines the distance between each two successive Z-levels. During the profile finishing, the machining of the floor area is performed first, then the finishing of the walls is performed. Step down The floor area is machined in a single cutting pass at the Profile depth level. This cutting pass is calculated using the Clear offset strategy with the specified Offset and Step over parameters and taking into account the Profile specified Wall offset. depth Offset Step over Wall offset Offset Step over319
    • The wall finishing is performed from the Upper level down tothe Profile depth in a number of steps defined with the Stepdown parameter.Equal step down Step downMachining of Profiles and Pockets starts from the Upper leveland is performed in a number of successive Z-levels till thespecified Depth. This option enables you to keep an equaldistance between all Z-levels.When the Equal step down check box is not selected, the Profiledistance between each two successive Z-levels is determined depthby the Step down parameter. If the machining depth is notdivisible exactly by the Step down value, the depth of the lastcut is smaller than the Step down value.When the Equal step down check box is selected, Step downan equal distance is kept between all Z-levels.Using this option, you have to specify the Max. Last cutStep down parameter instead of the Step down depthparameter. According to the Depth defined in theoperation and modified with the Floor offset andDelta depth parameters, SolidCAM automaticallycalculates the actual step down to keep an equaldistance between all passes, while taking intoaccount the specified Max. Step down so that it isnot exceeded. Max. The Equal step down option Step down is available only for Profile and Pocket operations. Actual Step down 320
    • 6. 2.5D MillingDepth cutting typeThis section enables you to define the direction of Z-levels machining and the connection betweenpasses.When the One way option is chosen, the cutting passes are orientedin the same direction and connection between them is performedthrough the Operation Clearance level. At the end of each pass thetool performs a retreat movement to the Operation Clearance level, ahorizontal movement at rapid feed to the start point of the next passand then descends to the Z-level of the next pass. The same cuttingdirection (climb or conventional) is kept along the whole tool path.When the Zigzag option is chosen, the tool path is performed in azigzag manner, with the tool path direction changing from one pass tothe next. The passes located at two successive Z-levels are connecteddirectly from the end of one pass to the beginning of the next pass. The Zigzag option cannot be used together with the Clear offset technology.Complete Z-level/Sort by chainsThese options enable you to define the order of Z-levels milling in the machining of several profilesin one operation. These check boxes are not available when the Zigzag option is chosen for Depth cutting typeand when the Helical or Define option is chosen for Depth type. The Sort by chains check box is available only when the Complete Z-level check box is selected and the Clear offset option is used with the One way option. When the Rough and Finish strategies are used together in the same Profile operation, the Complete Z-Level check box is not available.321
    • Rough machining When the Complete Z-Level check box is selected and the Clear offset strategy is not used, SolidCAM enables you to generate the following tool path: machining of all chains at a specific Z-level is performed; 1 when machining of this level is 2 3 completed, the tool moves down to 5 4 the next level, and so forth. 7 6 8 9 10 11 12 When the Complete Z-Level check box is not selected and the Clear offset strategy is not used, the machining is performed by chains: the tool completes the machining of a specific Z-level for a specific chain 1 and then moves to the next Z-level 7 2 of the same chain. When machining 8 3 of all the Z-levels of a specific chain 4 9 is completed, the tool moves to the 10 5 next chain. 11 6 12 When the Complete Z-Level check box is selected and the Clear offset strategy is used with the Zigzag option, SolidCAM enables you to generate the following tool path: the first chain at the upper cutting 1 level is machined in a zigzag cutting 2 pass, and then the next chain at the 3 same level is machined in a zigzag 4 movement. When all the chains of 5 the cutting level are machined, the 6 tool moves to the next cutting level, and so forth. 322
    • 6. 2.5D Milling When the Complete Z-Level check box is selected and the Clear offset strategy is used with the One way option, the Sort by chains check box is available. The tool path order depends on the state of this check box. • When the Sort by chains check box is not selected, SolidCAM enables you to generate the following tool path: the first chain of the first cutting level is machined in several equidistant profiles generated by the Clear offset strategy. When the machining of the chain is finished at the current cutting level, the next chain at the same cutting level is machined. When all the chains of this cutting level are machined, the tool descends to the next cutting level, and so forth. 3 2 1 6 9 5 8 4 7 15 12 14 11 13 10 18 17 16 • When the Sort by chains check box is selected, SolidCAM enables you to generate the following tool path: the first chain of the first cutting level is machined in several equidistant profiles generated by the Clear offset strategy. When the machining of the chain is finished at the current cutting level, SolidCAM performs the machining of the same chain at the next cutting level. When the chain is completely machined at all cutting levels, the next chain is machined in the similar manner. 3 2 1 12 4 11 5 10 6 9 15 8 14 7 13 18 17 16323
    • When the Complete Z-Level check box is not selected and the Clear offset strategy isused with the Zigzag option, SolidCAM enables you to generate the following toolpath: the first chain of the first cutting level is machined in a zigzag cutting pass, thenthe tool moves down to the next cutting level. When machining of the current chain iscompleted at all cutting levels, the next chain is machined in the similar manner. 1 4 2 5 3 6When the Complete Z-Level check box is not selected and the Clear offset strategy isused with the One way option, SolidCAM enables you to generate the following toolpath: the first clear offset cut (farthest from the geometry chain) is machined at theupper cutting level for the first chain. Then the tool descends to the next cuttinglevel and performs the first clear offset cut, and so forth. When the clear offset cut isfinished at all Z-levels, the machining of the successive clear offset cuts (closer to thegeometry chain) starts from the upper cutting level. When machining of all clear offsetcuts is finished for the current chain, the next chain is machined in the similar manner. 7 4 1 16 8 13 5 10 2 9 17 6 14 3 11 18 15 12 324
    • 6. 2.5D MillingFinish machiningWhen the Finish check box is selected, the Complete Z-level option is available if the Clear offsetstrategy is not used.When the Complete Z-Level check box is selected, the finishing is performed by Z-levels: machiningof all chains at a specific Z-level is performed; when machining of this level is completed, the toolmoves down to the next level, and so forth. 1 2 3 5 4 7 6 8 9 10 11 12When the Complete Z-Level check box is not selected, the finishing is performed by chains: the toolcompletes machining of a specific Z-level for a specific chain and then moves to the next Z-levelof the same chain. When machining of all the Z-levels of a specific chain is completed, the toolmoves to the next chain. 1 7 2 3 8 4 9 10 5 11 6 12325
    • 6.1.3 Link pageThis page enables you to define the parameters of tool approach and retreat relative to the machinedprofile.RampingThis section determines how the tool approaches the start point of the contour. Choose one of thefollowing descent types from the list: • Rapid generates a rapid descent (G0) from the Clearance level to the approach plane. Use this option when you know that there is no material in the descent path. • Feed causes the tool to move rapidly to the Upper level minus the Safety distance. Then the tool descends to the approach plane with the given Z Feed rate. Use this option when you know that there is material in the descent path. • Diagonal can be activated only if the Step down is equal to the Profile depth. It causes the tool to move rapidly from the Clearance level to the Upper level plus the Safety distance. Then the tool diagonally descends to the start of the profile geometry at the normal feed rate. The angle of the diagonal is automatically generated depending on the type of approach you choose.Pre-drilling geometry generationWhen the operation is defined and saved, SolidCAM automatically generates the pre-drillinggeometry. This geometry contains the points into which the ramping is performed. 326
    • 6. 2.5D MillingThe pre-drilling geometry can be generated only in the following cases: • The Normal/Arc/Tangent/Point strategy is used for the Lead in (when the None option is used, the pre-drilling geometry is not generated); • The Clear offset option is not used; • The One way option is used for Depth cutting type; • The Helical mode is not used for Depth type; • The Wall draft angle option is not used; • The Rest Material/Chamfer options are not used; • The Plunging option is not used.During the generation of the pre-drilling geometry, SolidCAM automatically collects the rampingpoints of the roughing tool path for all of the chains. For each chain, SolidCAM collects all theramping points where the vertical penetration into the material is performed. These points arelocated in the start point of the Lead in movement. Generally, for an open chain, SolidCAM has togenerate only one ramping point.Rampingposition Lead in327
    • In some cases, during the tool path generation for closed chains, the chain is machined in a numberof closed cutting passes. In such cases, SolidCAM generates more than one ramping position for onechain, and the number of positions depends on a number of cutting passes. For each cutting pass,one point is generated at the location where the vertical penetration into the material is performed. Lead in Ramping Lead in positionThe ramping positions are collected only for the rough cutting passes; the finish cutting passes areignored.The name of the generated geometry is composed of the nameof the initial Profile operation with the Drill_For_ prefix: Drill_For_ProfileName, where the ProfileName is the name of the initial Profileoperation. For example, for the Profile operation F_contour_T1, thepre-drilling geometry Drill_For_F_contour_T1 will be generated.The pre-drilling geometry appears under the Geometry header inSolidCAM Manager. This geometry is available for Drilling operationsonly. The pre-drilling geometry cannot be chosen in 3D Drillingoperations. 328
    • 6. 2.5D MillingAdjacent passes connectionThis option enables you to define the connection method for adjacentcutting passes generated using the Clear offset method with the Zigzagoption.The following options are available to define the passes connection: • Linear With this option, the tool movement from one cutting pass to the next is performed as a straight line connecting the end point of the first pass with the start point of the next pass. • Rounded With this option, the tool movement from one cutting pass to the next is performed as an arc tangential to the adjacent cuttings passes. The arc connects the end point of the first pass to the start point of the next pass.329
    • Lead in/Lead outThese options enable you to control the way the tool approaches theprofile and retreats away. • None The tool approaches the milling level and retreats away exactly adjacent to the start point of the profile. • Normal The tool approaches the profile and retreats away from/ to a point normal to the profile. The length of the normal can be set in the Value field. Lead in value • Arc The tool approaches the profile and retreats away with a tangential arc. The arc radius can be set in the Value field. The Data button is displayed and enables you to define additional parameters in the Arc Lead in Data/Arc Lead out Data dialog box. Lead in value Arc angle This parameter defines the angle of the Lead in arc segment. The default angle value is 90°; in this case, SolidCAM Angle Angle Distance generates a Lead in path of quarter arc. Lead in from Lead in from Center Distance 330
    • 6. 2.5D Milling Lead in from With the Arc Lead in option, the tool moves normal to the lead in arc at the arc start point. The following options are available: • Distance The tool starts milling at the specified distance from the arc start point. • Center The tool starts milling at the lead in arc center. Center of circle When this check box is not selected, the tool rapidly moves from the Clearance level to the Safety distance, enters the material in the center of the defined approach arc and performs the arc movement to the geometry start point at the first cutting level. When this check box is selected, the tool rapidly moves from the Clearance level to the Safety distance, enters the material in the center of the profile geometry and performs a linear movement to the geometry start point at the first cutting level. Approach movement Tool path Center of circle check box Center of circle check box is not selected is selected The retreat is performed in the same manner. • Tangent The tool approaches the profile and retreats away on a line tangent to the profile. The length of the tangent line can be set in the Value field. Normal Lead in value331
    • • Point The tool approaches the profile and retreats away from/to a user-defined position. From this position the tool performs a linear movement to the start point of the profile. When you choose this option, the Pick button is activated and you can select a position on the CAD model.Same as Lead inWhen this check box is selected, the strategy and parameters defined for Lead in are used for Leadout. When the Zigzag option is used, the lead in/out movements for all the cuts are calculated according to the direction of the first cutting pass, irrespective of the direction of the other cutting passes. During the tool path linking, SolidCAM connects the cuts that contain lead in and lead out movements in a zigzag manner and changes the direction of all even cuts to the opposite. Therefore only for odd cuts, the Lead in strategy is used for approaching and the Lead out strategy is used for retreating. For even cuts, the Lead in strategy is used for retreating and the Lead out strategy is used for approaching. Movements defined by Lead in strategy Movements defined by Lead out strategy 332
    • 6. 2.5D MillingKeep tool downThis option enables you to reduce the unnecessary tool movements through the Clearance level.When the Keep tool down check box is not selected, after the machining of the specific Z-level, thetool retracts up to the Operation Clearance level. At this level the tool horizontally moves to thestart position of the next cut and then descends to the next Z-level. Clearance levelWhen the Keep tool down check box is selected, after the machining of the specific Z-level, thetool retracts up to the height equal to the Safety distance from the machined cut, then horizontallymoves to the start position of the next cut at this level and descends to the next Z-level. Safety distance333
    • 334
    • 6. 2.5D Milling6.2 Face Milling OperationThis operation enables you to machine large flat surfaces with face mill tools.6.2.1 Geometry pageThis page enables you to define the machining geometry for the operation.The geometry for Face Milling operations is defined using the Face Milling Geometry dialog box.335
    • NameThis edit box enables you to define the geometry name.Base GeometryThis section enables you to choose the method of the Face Millinggeometry definition. • Model This option generates a rectangle located at the XY-plane and surrounding the Target model and selects it for the Face Milling geometry. The rectangle chain is displayed in the Chain List section. Face Milling geometry • Faces This option enables you to Face Milling geometry define the Face Milling geometry by face selection. The Define button and related combo-box enable you either to define a new faces geometry with the Select Faces dialog box or to choose an already defined geometry from the list. When the model faces are selected, SolidCAM generates a number of chains surrounding the selected faces. These chains are displayed in the Selected faces Chain List section. 336
    • 6. 2.5D Milling • Profile This option enables you to define the Face Milling geometry by selecting a chain. The Define button and related combo-box enable you either to define a new profile geometry with the Geometry Edit dialog box or to choose an already defined geometry from the list. The defined chains are displayed in the Chain List section. Face Milling geometryChain ListThis section displays all the chains chosen for the Face Milling geometry.Each chain entry in the list contains a check box. By clearing thischeck box, you can exclude the corresponding chain from thedefined geometry.The right-click menu is available on the chain entries in the list. • The Check All command selects all of the chain check boxes; all the geometry chains will participate in the current geometry. • The Uncheck All command removes the selection from all of the chain check boxes; all the geometry chains will be excluded from the current geometry. When the selection is removed from all of the chains in the list, the button that confirms the Face Milling Geometry dialog box is disabled. • The Invert Check Status command enables you to invert the selection status for all the chain entries; all the selected check boxes will be unselected and vice versa, all the unselected check boxes will be selected.337
    • The Merge button enables you to merge all the Face Milling geometry chains into a single chain. TheSeparate button enables you to divide a merged chain into its initial separate chains. Separate chains Merged chainModifyThis section enables you to offset the chain currently selected in the Chain List section. The Applyto all button enables you to apply the specified offset value to all the chains. Offset6.2.2 Technology pageThis page enables you to define thetechnological parameters of Face Milling. 338
    • 6. 2.5D MillingThe following technologies are available:Hatch technologyThe machining is performed in a linear pattern.The Overlap/Min. Overlap section enables you define the tooloverlapping between two successive passes. This section isavailable only for Hatch and Contour strategies. Equal step over This option enables you to generate the hatch tool path spaced evenly with the automatically calculated Overlap value, which is nearest to the specified Min. Overlap value but not smaller than this value. When this check box is not selected, the distance between the last pass and the one before it can be smaller than that between all of the other passes. Overlap Overlap When this check box is selected, the evenly spaced hatch tool path is generated. The overlap between two successive passes is not smaller than the specified Min. Overlap value. This option is available only for the Hatch strategy. Overlap Overlap339
    • The Data button displays the Hatch Data dialog box that enables you to define the parameters ofhatching. Hatch angle The following options to define the angle of hatching are available: • Automatic optional angle SolidCAM automatically calculates the optimal angle of hatching to expedite the machining. The tool path always follows the length of the face no matter what angle the machined surface is facing. 340
    • 6. 2.5D Milling You can change the angle by entering a different value in the Delta from optimal box. Delta angle Optimal direction • User-defined angle This option enables you to determine the angle of the tool path. Angle X Keep cutting direction This option enables you to control the cutting direction when moving around model contours. • Yes: the length of the tool path is not optimized. • No: a shorter, optimized tool path is generated by reversing some tool movements. The milling direction may change between climb and conventional milling.341
    • Cutting direction • One way This option enables you to create the tool path with only one-directional movements. One way • Zigzag This option enables you to create the tool path with bi- directional movements.Extension Zigzag During face milling, the tool path is extended over the edges of the machined face. The Extension section enables you to define the extension both along the tool path (the Along section) and across the tool path (the Across section). The extension can be defined either by percentage of the tool diameter (the % of tool diameter option) or by value (the Value option). Extension across the tool path Extension along the tool pathCorner • None The tool path is formed with sharp corners between one direction and the next. • Fillet This option connects each direction with a given radius allowing for a smoother transition between path directions. 342
    • 6. 2.5D MillingContour technologyThe machining is performed in a number of equidistant contours.The Data button displays the Contour Parameters dialog box. Start from • Inside This option enables you to work in a pocket area starting from the middle of the pocket and cutting towards the outside border of the pocket. • Outside This option enables you to work in a pocket area starting from the outside border of the pocket and cutting towards the middle of the pocket. Corner • None The tool path is formed with sharp corners between one direction and the next.343
    • • Fillet This option connects each direction with a given radius allowing for a smoother transition between path directions. The Min. corner radius parameter enables you to define the minimal value of the corner radius. If the given radius is too large for a specific corner, it produces the largest possible radius at that point. There are times were the fillet option might leave some material. This is particularly true if the given radius is large. • Loop This option ensures that the connecting points on the path are cleaned using a smooth transition. The tool path forms a loop in the corner, preventing an abrupt change of direction. • Sharp This option ensures that using a short and simple movement cleans the connecting points on the path. Although this produces a sharp movement by the tool, the path itself is slightly shorter than that in the smooth corner option. This can help cut down on machining time. This option is not recommended for high- speed cutting.Direction This option enables you to choose climb or conventional milling for the roughing operation. Climb Milling Conventional Milling 344
    • 6. 2.5D Milling Arc approximation This command enables you to create G2/G3 GCode output from Contour roughing operations. SolidCAM checks whether successive points of the calculated tool path can be connected using an arc or a circle. If arc or circle connection within the specified arc approximation tolerance can be made, you receive arc and circle interpolation commands G2 and G3 in the generated GCode. This feature can drastically reduce the number of lines in GCode files. Most CNC- controllers and machines work much faster on arcs and circles than on single tool path points or splines. Arc approximation increases actual feed rates on older CNC- machines and the machines work smoother. The Tolerance value defines the tolerance SolidCAM uses to position tool path points on arcs or circles. Adjacent tool paths connection This option enables you to choose the method with which the tool moves from one tool path to the next. • Linear The tool moves in a normal approach from one tool path to the next. • Rounded The tool moves in an arc path from one tool path to the next. The size of the arc is half the distance between tool paths. Extension The Contour tool path can also be extended over the machined face edges. The Extension section enables you to define the uniform extension of the tool path. The extension can be defined Extension either by percentage of the tool diameter (the % of tool diameter option) or by value (the Value option).345
    • One pass technologySolidCAM performs the face milling in one pass. The direction andthe location of the pass are calculated automatically according to theface geometry, in order to generate an optimal tool movement withthe tool covering the whole geometry.The Data button displays the One pass data dialog box that enablesyou to define the machining parameters.The Extension section enables you to definethe tool path extension over the face edges. Theextension can be defined either by percentage ofthe tool diameter (the % of tool diameter option) Extensionor by value (the Value option).OffsetsThis section enables you to define the offset that remains on the face floor after the roughingoperation (Floor offset).The Finish check box enables you to remove the remaining offset with the last cut (if the check boxis selected) or leave the offset unmachined for further operations (if the check box is not selected).Depth cutting typeThis option enables you to connect cutting passes by vertical zigzag movements. When a cuttingpass is machined, the tool moves down to the next cutting level and machines it in the oppositedirection. When the machining of all cutting levels is finished for a specific pass, the tool moves tothe next cutting pass and machines it in the same manner. This option is available only for the Hatch and One Pass strategies. 346
    • 6. 2.5D MillingThe behavior of these options depends on the state of the Cutting direction option defined in theHatch Data dialog box.When the Zigzag option is chosen for Cuttingdirection and the One way option is chosen for Depthcutting type, the tool performs the machining of acutting pass at a specific Z-level and then moves tothe beginning of the next cutting pass located at thesuccessive Z-level and continues the machining in thesame direction. The movement to the next cuttingpass is performed via the Clearance level.When the Zigzag option is chosen for Cuttingdirection and the Zigzag option is chosen for Depthcutting type, the tool performs the machining of acutting pass at a specific Z-level, then moves directlyto the next Z-level and then continues to machine thenext cutting pass in the reversed direction. 5When the One way option is chosen for Cutting 4direction and the One way option is chosen for Depth 10 3 9cutting type, the tool machines a cutting pass located 2 8at a specific Z-level and then rapidly moves via the 1 7Clearance level to the beginning of the next cutting 6pass at the same Z-level. When the Z-level is machinedin such manner, the tool starts the machining of thenext Z-level. In this case, SolidCAM preserves thecutting direction (either climb or conventional) for allof the cutting passes. 5When the One way option is chosen for Cutting 4direction and the Zigzag option is chosen for Depth 3cutting type, the tool performs the machining of 2all cutting passes at a specific Z-level in the same 1direction, and then directly moves down to machinethe passes at the next Z-level in the opposite direction. 6 7 8 9 10347
    • Reverse tool pathThe Reverse check box enables you to reverse direction of the tool path. When this check box isselected, the hatch tool path is performed in the opposite direction. Initial tool path Reversed tool path This option is available only for the Hatch and One Pass strategies.Sort cut orderThe Complete Z-level option enables you to define the order of the machining Z-levels, in casemore than one face is machined.For more information, see topic 6.4.3. 348
    • 6. 2.5D Milling6.2.3 Link pageThis page enables you to define the parameters of tool approach and retreat relative to the machinedgeometry.RampingThis field controls the way the tool plunges into the material inside the pocket.For more information, see topic 6.4.4.Lead inThis field controls the movement of the tool when it enters the pocket on the finishing cut.For more information, see topic 6.4.4.Lead outThis field controls the movement of the tool when it leaves the pocket on the finishing cut.For more information, see topic 6.4.4.Keep tool downThis option enables you to reduce the unnecessary tool movements through the Clearance level.Foe more information, see topic 6.1.3.349
    • 350
    • 6. 2.5D Milling6.3 Contour 3D OperationThe Contour 3D operation enables you to utilize the power of the 3D Engraving technology (seetopic 7.2) for the 3D contour machining. In this operation, SolidCAM enables you to prevent thegouging between the tool and the 3D contour.6.3.1 Technology pageThis page enables you to define thetechnological parameters of themachining.ModifyThe Tool side option enables you to Left Right Centerdefine the tool position relative tothe geometry. • Right: the tool cuts to the right of the profile geometry at the distance defined by the values set in the Modify offset section of the Modify Geometry dialog box. • Left: the tool cuts to the left of the profile geometry at the distance defined by the values set in Modify offset section of the Modify Geometry dialog box. • Center: the center of the tool moves on the profile geometry. The compensation cannot be used with this option. When the Tool side is set to Right or Left, all chains defined for the Contour 3D operation geometry must start at the same height.351
    • The Geometry button enables you to modify a geometry shared by several operations separately foreach operation.When the Compensation check box is selected, the tool radius compensation options G4x of theCNC-controller are used in the GCode.For more information, see topic 6.1.2.Tool referenceThis option enables you to define the point on the tool which is in contact with the machined 3Dcontour. • Tip With this option, the tool tip is in contact with the 3D contour; SolidCAM prevents the gouging between the tool and the 3D contour. Note that the tool axis always crosses the geometry. • Center With this option, the tool center is in contact with the 3D contour. In this case, SolidCAM does not check the gouging between the tool and the contour. 352
    • 6. 2.5D MillingTechnologyWhen the Tip option is chosen for the Tool reference definition, this section enables you to definethe technological parameters of the operation. Type This option enables you to perform the semi-finish and/or finish machining of the 3D contour. • Semi-finish The machining of the 3D contour is performed in several steps along the Z-axis. The vertical distance between two steps is defined by the Step down parameter. • Finish The 3D contour is machined to its final dimensions in one step down. • Both This option is used to machine the 3D contour first with a semi-finish cut and then with a finish cut. Step down This value defines the vertical distance between two successive steps during the Semi- finish machining of the 3D contour. • From Upper level SolidCAM performs a number of horizontal semi-finish passes at each down step, from the Upper level up to the defined Contour depth. Upper level 3D Contour geometry Contour depth353
    • • From surface SolidCAM performs a number of 3D semi-finish passes at each step down, from the chosen 3D contour to the defined Contour depth. 3D Contour geometry Contour depthThe Technology section is not available when the Center option is chosen for the Tool referencedefinition.OffsetsSolidCAM enables you to specify the machining allowances that can be removed either by profilefinishing in the same operation or in another operation.For more information, see topic 6.1.2.RoughThis section enables you to perform the profile rough machining.For more information, see topic 6.1.2.FinishThis section enables you to perform the profile finishing.For more information, see topic 6.1.2.Clear offsetThis section enables you to define the parameters of the Clear offset machining for the roughingand finishing passes.For more information, see topic 6.1.2. 354
    • 6. 2.5D MillingChamferThis option enables you to machine chamfers with a Center drill tool.This button is available only when the Right or Left option is chosen for the Tool side definition.For more information, see topic 6.1.2.6.3.2 Link pageThis page enables you to define the parametersof tool approach and retreat relative to themachined contour.Lead in/Lead outThese options enable you to control the waythe tool approaches and retreats from thecontour.When the Right or Left option is chosen forthe Tool side definition, the following Lead in/out options are available: • None • Normal • Arc • Tangent • PointWhen the Center option is chosen for the Tool side definition, the following Lead in/out optionsare available: • None • Arc • TangentFor more information about Lead in/out options, see topic 6.1.3.355
    • 356
    • 6. 2.5D Milling6.4 Pocket OperationIn pocket milling, you have to remove material from the interior of a closed geometry. SolidCAMoffers two types of pocketing: 1. When a profile geometry consists of one or more profiles and none of them are enclosed or intersect with one another, each is milled as a separate pocket without islands. 2. When a profile geometry consists of several profiles, any profile that is enclosed or intersecting with another profile is treated as an island. You can define an unlimited number of islands within a single pocket.When you click Add Operation, Pocket, the Pocket Operation dialog box is displayed.357
    • 6.4.1 Geometry pageThis page enables you to define the machining geometry for the operation.The geometry definition is performed using the Geometry Edit dialog box.Only closed contours are acceptable for the definition of geometry. Whenyou confirm an open chain definition in the Geometry Edit dialog box withthe button, the Close Chain dialog box is displayed.When you confirm this dialog box with the OK button, the chain is closedwith a line that connects the start and the end points of the chain. The Markline as open edge check box enables you to mark the connecting line as openedge to perform open pocket machining.When you click on the Cancel button, SolidCAM returns to the geometrydefinition and enables you to close the chain manually by the model elementselection. 358
    • 6. 2.5D Milling6.4.2 Levels pageThis page enables you to specify the Z-levels at which the tool movements and the operation areexecuted.Step down Step downSolidCAM uses the constant-Z passes for thePocket generation. The Step down parameter Upper levelenables you to define the distance between eachtwo successive Z-levels. Enter the tool’s cuttingdepth. Pocket depthEqual step downSelecting this check box enables you to keep an equal distance between all Z-levels.When this check box is selected, the Max. Step down parameter appears instead of the Step downparameter.For more information, see topic 6.1.2.359
    • 6.4.3 Technology pageThis page enables you to define the technological parameters of the Pocket machining.Pocket machining technology Pocket machining Hatch technologies Contour Hatch+Finish Plunging patternChoose the pocket machining technology from the list. • Hatch mills the pocket in a linear pattern. • Contour machines the pocket in a round pattern. • Hatch+Finish mills the pocket in a linear pattern and cleans up the profile on each cutting depth. • Plunging pattern: the tool moves up and down in a drilling motion, travelling inside the pocket.Click on the Data button to define additional parameters. 360
    • 6. 2.5D MillingHatch technologyThis technology enables you to machine the pocket in a linear pattern. This option is used in Pocket, Pocket Recognition and 3D Milling operations for Roughing (see topic 7.1.3) and Constant Z finishing (see topic 7.1.13).This technology creates a linear raster tool path up to the pocket contour.Click on the Data button. The Hatch Data dialog box is displayed.361
    • Hatch angle The following options to define the angle of hatching are available: • Automatic optional angle SolidCAM automatically calculates the optimal angle of hatching to expedite the machining. The tool path always follows the length of the pocket no matter what angle the pocket is facing. You can change the angle by entering a different value in the Delta from optimal box. • User-defined angle This option enables you to determine the angle of the tool path.Keep cutting direction This option enables you to control the cutting direction when moving around model contours. • Yes The length of the tool path is not optimized. • No SolidCAM generates a shorter, optimized tool path by reversing some tool movements. The milling direction may change between climb and conventional milling. 362
    • 6. 2.5D Milling Cutting direction • One way This option enables you to create the tool path with only one- One way directional movements. • Zigzag This option enables you to create the tool path with bi- directional movements. Zigzag Corner • None The tool path is formed with sharp corners between one direction and the next. • Fillet This option connects each direction with a given radius allowing for a smoother transition between path directions. Exit Material This option controls the tool movements between the working areas. • When this check box is not selected, the tool moves from one working area to the next through the full material around the island to get to the next working area as shown above. • When this check box is selected, the tool exits from the material and travels rapidly above the material to the next working area as shown above. The Lead in path is the Lead in you defined. This option is used in the Hatch and Contour strategies in Pocket, Pocket Recognition and 3D Milling operations.363
    • Contour technologyIn this technology, the tool moves on offsets parallel to the pocketcontour.Click on the Data button. The Contour Parameters dialog box isdisplayed. This option is used in the Pocket, Face Milling, Pocket Recognition and 3D Milling operationsfor Roughing and Constant Z finishing. Constant Z Pocket Milling Face Milling 3D Roughing Finishing Exit material This option controls the tool movements between the working areas. Connect islands This option enables you to keep the same cutting direction (conventional or climb milling) throughout the entire tool path where possible. This is particularly important in high- speed cutting. 364
    • 6. 2.5D Milling Start from • Inside This option enables you to work in a pocket area starting from the middle of the pocket and cutting towards the outside border of the pocket. • Outside This option enables you to work in a pocket area starting from the outside border of the pocket and cutting towards the middle of the pocket. Corner • None The tool path is formed with sharp corners between one direction and the next. • Fillet This option connects each direction with a given radius allowing for a smoother transition between path directions. The Min. corner radius parameter enables you to define the minimal value of the corner radius. If the given radius is too large for a specific corner, it produces the largest possible radius at that point. Some material can be left if the given radius is large. • Loop This option ensures that the connecting points on the path are cleaned using a smooth transition. The tool path forms a loop in the corner, preventing an abrupt change of direction.365
    • • Sharp This option ensures that using a short and simple movement cleans the connecting points on the path. Although this produces a sharp movement by the tool, the path itself is slightly shorter than that in the Loop option. This can help reduce the machining time. This option is not recommended for high-speed cutting.Direction This option enables you to choose climb or conventional milling for the roughing operation. Climb Milling Conventional MillingArc approximation This command enables you to create G2/G3 GCode output from Contour roughing operations. SolidCAM checks whether successive points of the calculated tool path can be connected using an arc or a circle. If arc or circle connection within the specified arc approximation tolerance can be made, you receive arc and circle interpolation commands G2 and G3 in the generated GCode. This feature can drastically reduce the number of lines in GCode files. Most CNC- controllers and machines work much faster on arcs and circles than on single tool path points or splines. Arc approximation increases actual feed rates on older CNC- machines and the machines work smoother. The Tolerance value defines the tolerance SolidCAM uses to position tool path points on arcs or circles. 366
    • 6. 2.5D Milling Adjacent passes connection This option enables you to choose the method with which the tool moves within the pocket from one pass to the next. • Linear The tool moves in a normal approach from one pass to the next. • Rounded The tool moves in an arc path from one pass to the next. The size of the arc is half the distance between passes.Hatch+Finish technologySolidCAM first machines the pocket on the actual stepdown with the Hatch technology and then makes a finalpath around the pocket contour.Click on the Data button. The Hatch Data dialog box isdisplayed. Hatching Final profiling367
    • Plunging pattern technologyPlunging is a technology of removing material from a given pocketusing a special tool. Instead of milling the material, the tool movesup and down as in a drilling motion, travelling along the path typeyou choose.Click on the Data button. The Plunging dialog box is displayed. Drill cycle type SolidCAM enables you to choose preferable drilling cycles for the plunging operation. 1. Click on the Drill cycle type button and choose the cycle type you want in the Drill cycle dialog box. 2. Click on the Data button and specify the parameters in the Drill options dialog box. For more information on the Drilling cycles, see topic 6.6.3. Clean condition This value determines the maximum percentage of material that will be removed based on the diameter of the tool. Minimal clean condition This value determines the minimum percentage of material that will be removed based on the diameter of the tool. 368
    • 6. 2.5D Milling Feeds The plunging feeds can be determined by the percentage of the tool and the diameter of the tool being used. • Full/Center If the full diameter of the tool is cutting, the feed and spin defined in the appropriate field are used. In the second field, you can determine a specific working diameter of the tool. If the working diameter from the center of the tool is greater than this value but smaller than the full diameter, the feed and spin rate that was entered in the appropriate field are used. • Overlap (%) If none of the above conditions have been met, the feed and spin are determined by the overlap of the tool.Open pocket machiningThis section is enabled only when the pocket geometry contains open edges. Extension During the open pocket machining, Open edge the tool path is extended beyond the open edges. The Extension section enables you to define the overlapping between the tool and the open edges; the overlapping can be defined as a percentage of the tool diameter (the % of tool diameter option) or as a value (the Value option). Extension369
    • Use profile strategy The Use profile strategy option enables you to perform the open pocket machining in a Profile manner. The tool path at a specific Z-level consists of several equidistant profiles starting from outside the model at the distance defined by the Extension parameter. The tool moves on offsets parallel to the pocket geometry. The following options enable you to define the tool path direction and linking. When the One way option is chosen, the tool finishes one profile pass, then rapidly moves (G0) to the safety distance and then to the start of the next cutting pass. The cutting direction (either climb or conventional) is preserved for each cutting pass. When the Zigzag option is chosen, the tool finishes one profile pass and then moves directly to the next pass. The machining is performed without leaving the material, thus constantly switching between climb and conventional milling.Approach from outside This option enables the tool to approach from outside of the material in the open pocket areas, if possible. Such approach enables you to decrease the tool loading when plunging into the material. This option enables you to perform the approach movement from the automatically calculated point outside of the material. The tool moves to the required depth outside of the material and then plunges into the material. 370
    • 6. 2.5D Milling Descend to cutting level with Rapid This option enables you to avoid vertical non-machining movements outside of the material performed with the working feed by direct rapid movement down to the cutting level. When this check box is selected, the tool descends from the Clearance level outside of the material directly to the cutting level (defined with the Step down parameter) using the Rapid feed. Then the horizontal movement into the material is started with the working feed. Upper level Rapid movement Cutting level When this check box is not selected, the tool descends from the Clearance level down to the Safety distance with the Rapid feed. From the Safety distance, the tool descends down to the cutting level (defined with the Step down parameter) with the defined feed and starts the horizontal cutting movements into the material with the working feed. Upper level Rapid movement Safety distance Feed movement Cutting level The Descend to cutting level with Rapid check box is available only when the Approach from outside check box is selected.371
    • Complete Z-level This option enables you to define the order of Z-levels machining when several pockets are machined in a single Pocket operation. 1 5 When the Complete Z-level check box is 2 6 not selected, SolidCAM machines all the 3 7 Z-levels of the first pocket and then starts 4 8 the machining of the next pocket. When the Complete Z-level check box is 1 2 selected, the machining is performed by 3 4 the Z-levels; SolidCAM removes material 5 6 at a specific Z-level in all pockets and then 7 8 moves to the next Z-level.OverlapEnter the Overlap of adjacent tool paths in the milling of the pocket.For example, with the tool diameter of 10 mm, the side step is 3.5 mm for the next tool movement. 0.5D 0.2D Overlap 0.5D Overlap 0.2DEqual step overThis option enables you to generate the hatch tool pathspaced evenly with the automatically calculated Overlapvalue, which is nearest to the specified Min. Overlap valuebut not smaller than this value.When this check box is not selected, the distance betweenthe last pass and the one before it can be smaller than thatbetween all of the other passes. Overlap Overlap 372
    • 6. 2.5D MillingWhen this check box is selected, the evenly spaced hatch tool path is generated. The overlap betweentwo successive passes is not smaller than the specified Min. Overlap value. Overlap OverlapFillet size for last cutThis option enables you to add a radius to a sharp corner withoutchanging the geometry.For more information on this option, see topic 6.1.2.OffsetsTo perform the rough machining of the pocket, you have to specify theoffsets on the pocket geometry that will be removed with the finishingcut. • Wall offset Enter the offset that will remain on the pocket wall after the roughing cut. • Island offset Enter the offset that will remain on the pocket islands after the roughing cut. • Floor offset Enter the offset that will remain on the pocket floor after the roughing cut.373
    • FinishThis section enables you to perform the finish machining of thepocket.The Wall check box enables you to perform finishing of the pocketwalls. Only walls and islands are finished on the contour. The pocketdepth is reduced by the specified floor offset.The Floor check box enables you to perform finishing of the pocketfloor. The finish cut is executed to remove the floor offset. Thespecified wall and island offset remain on the pocket contour. Wall finish This section field contains two options to control the material removal on the last finishing cut. • On offset The finish path is executed at an offset equal to the sum of the tool radius and the finish offset from the tool path of the last roughing cut. The result is a uniform cutting depth (side step) on Offset the last cut, since in the pocket corners the tool Offset is not drawn into the material. Offset • On geometry The last cutting pass is executed exactly on the pocket geometry. R R Offset Offset 374
    • 6. 2.5D Milling Depth This section enables you to choose how the wall finishing will be performed: at the whole depth or in a number of steps at each step down. Finish passes • Total depth When this option is chosen, the wall finishing is performed in a single cut at the whole depth. • Each step down Finish pass When this option is chosen, the wall finishing is performed in a number of successive cuts at each step down. The options of the Depth section are available only when the wall finishing is performed in the operation. When the Wall draft angle option is used in the operation, the Depth options are disabled and the wall finishing is performed in a number of successive cuts at each step down. Compensation When the Compensation check box is selected, the tool radius compensation options G4x of the CNC-controller are used in the GCode. For more information on this option, see topic 6.1.2.375
    • Rest Material/Chamfer • The Rest material option enables you to define parameters to remove the rest material left unmachined after the previous operations. • The Chamfer option enables you to machine chamfers with the Center drill tool. Rest material When a large tool is used around the Rest Material areas profile in Pocket machining, the tool Pocket leaves material in the areas that it cannot geometry enter. The rest material option enables you to remove the material from this area Island without defining a new geometry. geometry The Rest Material dialog box is displayed. In this dialog box, you have to define the following parameters: • Previous tool diameter – the diameter of the tool used in the previous operation. • Previous wall offset – the wall offset used in the previous operation. • Extension – the overlap distance that you would like to start and end from the previous Extension Rest Material larger end mill. 376
    • 6. 2.5D Milling Milling type When the Separate areas strategy is chosen, SolidCAM generates a profile or pocket tool path to clean areas that the pre