Solidworks 2006 Fundamentals


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Solidworks 2006 Fundamentals

  1. 1. Solidworks 2006 Fundamentals Solidworks 2006 Fundamentals Infrastructure Sketch Solid Features Surfaces Assembly Design 2D Drawing Design Table & Equation A- 1Version 1- May07 Written by Dickson Sham
  2. 2. Solidworks 2006 Fundamentals General User Interface File Name Menu bar (all commands) Feature Manager (to switch the layout of toolbars) Toolbars Folder for surfaces (commonly-used (3 hidden inside) Geometry area/ commands only) Working area Folder for solids (one visible inside) Lights on model Dimmed features (hidden) Specification Tree (all Global coordinate (never features stored be changed) in historical order) A- 2Version 1- May07 Written by Dickson Sham
  3. 3. Solidworks 2006 Fundamentals General Type of Documents The common documents are: A) A part document (. sldprt) , which contains information how the model is built B) An assembly document (.sldasm), which contains the relative positions of components A C) A drawing document (.slddrw), which can be a part drawing or an assembly drawing C B A- 3Version 1- May07 Written by Dickson Sham
  4. 4. Solidworks 2006 Fundamentals General Display Settings To improve the 3D surface accuracy: •Select “Tools->Options...” on the menu bar, then open the tab page Document Properties •Then Select “Image Quality” •Increase the value for HLR/HLV resolution To change the background color of the geometry area: •Select “Tools->Options...” on the menu bar, then open the tab page System Options •Then Select “Colors” •Change the colors of “Viewpoint Background” , “Top Gradient Color” & “Bottom Gradient Color” A- 4Version 1- May07 Written by Dickson Sham
  5. 5. Solidworks 2006 Fundamentals General Change the view with the mouse A. Rotating enables you to rotate the model around a point. Click and hold the middle mouse button, Middle button then drag the mouse. B. Panning enables you to move the model on a plane parallel to the screen. Press and hold “Ctrl” key, then click and hold the middle mouse button, then drag the mouse. C. Zooming enables you to increase or decrease the size of the model. Press and hold “Shift” key, then click and hold the middle button, then drag the mouse up or down. A- 5Version 1- May07 Written by Dickson Sham
  6. 6. Solidworks 2006 Fundamentals Sketch Create a Sketch Build a Sketch:- 1. Click “Sketch” Icon 2. Select a plane or a planar face 3. Draw a profile (with lines, curves and/or centerlines) 4. Add geometrical constraints (relations) 5. Add dimensional constraints & modify the values 6. Click “Exit Sketch” icon A- 6Version 1- May07 Written by Dickson Sham
  7. 7. Solidworks 2006 Fundamentals Sketch Toolbars in sketch Project external curves/sketches/edges onto the active sketch Get the intersection curve between “external curves/ sketches/edges/faces” and the active sketch plane A- 7Version 1- May07 Written by Dickson Sham
  8. 8. Solidworks 2006 Fundamentals Sketch Construction Geometry Construction geometry is created within a sketch to aid in profile creation. Only standard geometry will be used for creating solids or surfaces (Fig.1) Construction geometry is shown in dashed format. To convert an element into a construction element, select it and activate the option” for construction”. You can also toggle any construction elements from construction to standard by deselecting the option. Construction geometry Fig.1 A- 8Version 1- May07 Written by Dickson Sham
  9. 9. Solidworks 2006 Fundamentals Sketch Constraining the sketch • Dimensional Constraints • Geometrical Constraints (click the icon, then select the element(s)) (multi-select the two elements by pressing “CTRL” key and click the icon) • Perpendicularity • Length • Horizontal/Vertical • Distance • Concidence • Angle • Tangency • Radius/Diameter • Symmetry (multi-select the elements on the both side and then select the centerline) Remark: To discontinue the command, click the icon again. You can also create constraints with other sketches and 3D elements out of the sketch To show or hide all geometrical constraints on the screen, select “View / Sketch Relations” A- 9Version 1- May07 Written by Dickson Sham
  10. 10. Solidworks 2006 Fundamentals Sketch Color and Diagnostic 1. Blue: Under-constrained 2. Black: Fixed/Fully constrained Case1 3. Red: Over-constrained Case2 Only case 1 & 2 are allowable. For Size dimensions case 3, you must fix the error and location before quitting the sketch mode, dimensions otherwise a warning message will have been fully pop-out and you cannot continue defined until the error is fixed. Case3 One dimension is redundant A- 10Version 1- May07 Written by Dickson Sham
  11. 11. Solidworks 2006 Fundamentals Sketch View Orientation • By default, the screen is parallel to the sketch support. • To making constraints between the sketch geometry and the 3D element, you may need to rotate the model into a 3D view. • To return the default orientation, press “space” key on the keyboard to activate the menu of orientation, and then select “Normal to” (the viewpoint normal to the sketch plane) We can create a distance constraint between the circle centre and the solid edge A- 11Version 1- May07 Written by Dickson Sham
  12. 12. Solidworks 2006 Fundamentals Solids Solid Modeling Feature-Based Solid Modeling Sketch Extrude Hole Fillet If deleting Hole, If deleting Fillet, If deleting Extrude, Parent and Children Relation we get: we get: we get: A- 12Version 1- May07 Written by Dickson Sham
  13. 13. Solidworks 2006 Fundamentals Solids Limit Type Types of limit are : B C A E A E B C D surface E F G H A plane surface Solid (body) F G H A- 13 Extrude in both directionsVersion 1- May07 Written by Dickson Sham
  14. 14. Solidworks 2006 Fundamentals Solids Extrude A. Extruded Boss/Base (material added by extruding a sketch) B. Extruded Cut (material removed by extruding a sketch) A B By default, extrusion start from the sketch; but it can also start from the offset direction from the sketch Define the depth by different modes, e.g. dimension, up to next, through all, up to surface You can define the extrusion direction by selecting a datum plane, a line, a planar surface, and a straight solid edge. Extrude in opposite direction Define wall thickness (optional) Define the region for A- 14 “Crossed “ profileVersion 1- May07 Written by Dickson Sham
  15. 15. Solidworks 2006 Fundamentals Solids Revolve A. Revolved Boss/Base (material added by rotating a sketch) B. Revolved Cut (material removed by rotating a sketch) A B Centerline LINE You can change the mode to Two-Direction or Mid- plane You need to draw another straight line along the centerline so that the profile is closed A- 15Version 1- May07 Written by Dickson Sham
  16. 16. Solidworks 2006 Fundamentals Solids Sweep A. Swept Boss/Base (material added by sweeping a profile along a path) B. Cut-Sweep (material removed by sweeping a profile along a path) A B Profile Control - Follow Path keeping the angle value between the sketch plane used for the profile and the tangent of the path - Keep Normal Constant Path Sweeping the profile while the profile‟s normal is Profile unchanged A- 16Version 1- May07 Written by Dickson Sham
  17. 17. Solidworks 2006 Fundamentals Solids Loft A. Lofted Boss/ Base (material added by sweeping one or more planar section curves along one or more guide curves B. Cut- Loft (material removed in the same way) A B You can drag to change the closing point Section 1 (blue point) Make the loft tangent to the Section 2 connecting faces on start/ finish ends - You can use an additional guide curve to control sweeping path If sections do not have the same number of vertices, “ratio coupling” Section 3 will be used by default A- 17Version 1- May07 Written by Dickson Sham
  18. 18. Solidworks 2006 Fundamentals Solids Hole A. Simple Hole (circular material removed from the existing solid); B. Hole Wizard Several types of holes are available: Simple, Tapered, Counterbored, Countersinked, Pipetap) Click here to define the position of the hole Recall the dimensions for standard screws Define the depth of the hole You can add “Dimensional” relations between the hole A- 18 center and the solid edgesVersion 1- May07 Written by Dickson Sham
  19. 19. Solidworks 2006 Fundamentals Solids Fillets Fillet (creating a curved face of a constant or variable radius that is tangent to, and that joins, two faces.) Click to select Constant Variable Face to the edge All round Radius Radius face The tangent edges are also highlighted by the system,Tangent Propagation: a fillet is according toapplied to the selected edge and all “Tangentedges tangent to the selected edge Propagation” Without With Setback Setback A- 19Version 1- May07 Written by Dickson Sham
  20. 20. Solidworks 2006 Fundamentals Solids Chamfer Chamfer (removing & adding a flat section from a selected edge to create a beveled surface between the two original faces common to that edge.) Length1 Angle For Vertex Two Dimensioning Modes for Edges Length2 Length1 A- 20Version 1- May07 Written by Dickson Sham
  21. 21. Solidworks 2006 Fundamentals Solids Draft Draft (adding or removing material depending on the draft angle and the pulling direction) Remark: Neutral plane always Neutral Plane keeps unchanged after a draft Pulling direction is created Top face as neutral plane Case 1 Case 2 Side faces to draft Bottom face as neutral plane A- 21Version 1- May07 Written by Dickson Sham
  22. 22. Solidworks 2006 Fundamentals Solids Other Features Shell (empty a solid while keeping a given thickness on its sides) Face to remove Wall thickness Rib (create a wall by extending an open profile up to limiting faces) Accepted A line with two ends, which are not The rib always touches the solid faces, not matter touching solid faces how the faces are changed / moved. Accepted A- 22Version 1- May07 Written by Dickson Sham
  23. 23. Solidworks 2006 Fundamentals Reference Geometry Reference Geometry Select “insert / Reference Geometry”, then select Reference Select a line and a point Offset the reference plane up to a point Offset by value / Rotate by value Select a curve and a point Select a surface and a point Obtain the axis of a cylindrical surface A- 23Version 1- May07 Written by Dickson Sham
  24. 24. Solidworks 2006 Fundamentals Curves 3D Sketch 3D Sketch (Draw a sketch in 3D space; you don‟t need to create a plane before creating a 3D sketch) Build a 3D Sketch:- •Click “3D Sketch” Icon •Draw a profile (with lines, curves and/or axis) (Remark: if you switch the viewpoint to Front View, the sketch plane will be “Front Plane”; similar for other viewpoints) (Remark: 3D sketch can be a non-planar curve) •Add geometrical constraints (relations) •Add dimensional constraints & modify the values •Click “3D Sketch” icon again to exit This is a 3D sketch A- 24Version 1- May07 Written by Dickson Sham
  25. 25. Solidworks 2006 Fundamentals Curves Projected Curve Sketch onto Face(s) (project a sketch onto a face. The projection can only be along the normal of the sketch) Along the normal Limitations: of the sketch (1) Only planar sketches can be projected (2) You cannot select other projection direction than the normal of the sketch You can project it onto a face of a surface or a solid Sketch onto Sketch (create a curve resulting from the A 3D resultant intersection of the extrusion of two curves. ) Curve The two extruded surfaces will not be created after this command A- 25Version 1- May07 Written by Dickson Sham
  26. 26. Solidworks 2006 Fundamentals Curves Helix Curve Insert / Curve / “Helix/Spiral” Pitch 3 ways to define a helix: 1) Pitch and revolution 2) Height and revolution Height Draw a circle on a 3) Pitch and Height sketch With Taper (optional) Spiral Curve Define Pitch and Revolution Draw a circle on a sketch A- 26Version 1- May07 Written by Dickson Sham
  27. 27. Solidworks 2006 Fundamentals Curves Composite Curve Insert / Curve / “Composite” Simply select the broken curves /edges and click ok to join them as one. (A composite curve is then created, representing this group of curves/edges) Curve through reference points Cannot define Control the direction of point tangency Create a 3D Spline by defining the control points Control point Limitation: Cannot define the direction of tangency at a control point. Control point Control If you need to control the direction, use “3D sketch” point A- 27Version 1- May07 Written by Dickson Sham
  28. 28. Solidworks 2006 Fundamentals Surfaces Extrude Extrude (create a surface by extruding a profile along a given direction) If the profile is planar, the direction will be its normal by default. But you can change it to other direction. Revolve Revolve (create a surface by revolving a planar profile about an axis) Remark: The axis must be a straight line A- 28Version 1- May07 Written by Dickson Sham
  29. 29. Solidworks 2006 Fundamentals Surfaces Sweep Sweep (create a surface by sweeping out a profile along a path) Profile Options •Profile Orientation •Additional Guide Curves •Start /End Tangency Path Loft Loft (create a surface by sweeping two or more section curves along an automatically computed or user-defined spine. The surface can be made to respect one or more guide curves. ) Options •Additional Guide Curves •Start /End Tangency •Centerline A- 29Version 1- May07 Written by Dickson Sham
  30. 30. Solidworks 2006 Fundamentals Surfaces Offset Offset (create a surface, or a set of surfaces, by offsetting an existing surface, or a set of surfaces) Remark: if Offset value = 0, you can duplicate the selected surface Fill Fill (create a surface to fill the opening among a number of boundary segments) We can specify the desired continuity type between any selected support surfaces and the fill surface (Point or Tangent continuous) The four points must be tangent-continuous A- 30Version 1- May07 Written by Dickson Sham
  31. 31. Solidworks 2006 Fundamentals Surfaces Trim Surface Standard Trim (split a surface by means of a trim tool. The trim tool can be a surface or a sketch) Trim Tool ( always keeps unchanged) Result by “Standard Trim” Original Piece to keep Mutual Trim (trim two or more surfaces) Trim by a sketch Result by “Trim” Pieces to keep A- 31Version 1- May07 Written by Dickson Sham
  32. 32. Solidworks 2006 Fundamentals Surfaces Untrim - Surface UNtrim (patch surface holes and external edges by extending an Surface untrim, select the existing surface along its natural boundaries) face. Under Options, select All edges. All Surface untrim, select edges are extended to both left edges and the their natural boundaries. inner edge. Under Options, select Connect endpoints. OR Knit - Surface Knit (join surfaces as one element) REMARK: If the resultant surface hasn‟t any open ends, the enclosed volume can be The two original surfaces A- 32 transformed into a solid are hidden; a “Knit”Version 1- May07 surface is created Written by Dickson Sham
  33. 33. Solidworks 2006 Fundamentals Surfaces Surface- Fillets Same Fillet (creating a curved face of a constant or variable radius as Solid that is tangent to, and that joins, two surfaces.) Constant Variable Face to All round Radius Radius face Tangent Propagation: a fillet is applied to the selected edge and all edges tangent to the selected edge Without With Setback Setback A- 33Version 1- May07 Written by Dickson Sham
  34. 34. Solidworks 2006 Fundamentals Surfaces Extend (Surface only) Extend the whole Surface / the surface from an edge Click the face The extrapolated surface is joined with the original surface as one Extend by Curvature Trend Click the edge Extend Surface along the tangential direction This will be a A- 34 straight edgeVersion 1- May07 Written by Dickson Sham
  35. 35. Solidworks 2006 Fundamentals Surfaces Draft Analysis Draft Analysis (analyze the draft angle on a surface/ a group of surfaces) STEPS: 1. Select “Tools / Draft Analysis” on the menu bar 2. Select a Direction as “Direction of Pull” 3. Enter a value as A (Angle), e.g 3 deg 4. Click “Calculate” icon If the big surface has no undercut, it should either all Green or all Red. Green: draft > 3deg Yellow: -3deg< draft <3deg Parting Red: draft < -3 deg surface/plane Positive draft Negative draft Direction of Pull A- 35Version 1- May07 Written by Dickson Sham
  36. 36. Solidworks 2006 Fundamentals Solids + Surfaces Cut Solid (with Surface) Cut with Surface (split a solid with a plane or surface ) Thicken Surface Thick Surface (add material to a surface in two opposite directions or in one direction) A- 36Version 1- May07 Written by Dickson Sham
  37. 37. Solidworks 2006 Fundamentals Transformation (Solid/ Surface) Pattern /Mirror Features to Pattern - Select “Hole1” & “Fillet1” on the tree Bodies to Pattern Faces to Pattern - Select the solid body - Select all faces of the hole Instance to skip - Select the bad instance to skip A- 37 3 instances skippedVersion 1- May07 Written by Dickson Sham
  38. 38. Solidworks 2006 Fundamentals Transformation (Solid/ Surface) Translate, Rotate, Mirror, Scale Select Insert/Features/ “Move/Copy”, then select “Translate” or “Rotate” These commands are also valid for surfaces Rotate Translate Select Insert/Features/ “Pattern/Mirror”, then select “Mirror” Select Insert/Features/ “Scale” Mirror Uniform Scale X-Y-Z Individual A- 38 ScaleVersion 1- May07 Written by Dickson Sham
  39. 39. Solidworks 2006 Fundamentals Solids + Surfaces Face - Replace Face - Replace (a Boolean operation combining a surface with a body. This capability adds or removes material by modifying the surface of the solid.) The solid face is Add a surface replaced; Material on top Original Solid is added inside the cover surface Face - Move Face – Move (offset, translate, and rotate faces and features directly on solid or surface models. ) Offset Translate Rotate Original Boss The radius of the The radius of the curved face increases curved face remains A- 39 the same.Version 1- May07 Written by Dickson Sham
  40. 40. Solidworks 2006 Fundamentals Assembly Assembly Design An assembly stores a collection of components (parts or sub assemblies). The file extension is .sldasm. Main Assembly Part Sub-assembly Parts belonging to “Sub-assembly” Constraints among the parts of sub-assembly Constraints between the part (base) and the sub-assembly A- 40Version 1- May07 Written by Dickson Sham
  41. 41. Solidworks 2006 Fundamentals Assembly Create a New Assembly Create a New Assembly by: - Select File /New / Assembly Insert existing components Click “Insert Component” icon Select the file of the component Then press “Enter” key to complete (the component will be “fixed” at the assembly origin) Or Click on an empty space in the geometry area (the component will be placed at that location but it is still free-to-move) A- 41Version 1- May07 Written by Dickson Sham
  42. 42. Solidworks 2006 Fundamentals Assembly Move components Upper Assembly is activated Component being moved Remark: (1)You can only move the components of the active assembly (2) To activate an assembly, right-click on itThe base is deactivated and then select “Edit Assembly” Instant Simulation Their axes are coincided Drag the bucket by mouse The base is fixed A- 42Version 1- May07 Written by Dickson Sham
  43. 43. Solidworks 2006 Fundamentals Assembly Constraints between components Click the icon “Mate” to define the constraints between two components To align the axis onto another axis, select the corresponding circular faces and then use “concentric” mate A- 43Version 1- May07 Written by Dickson Sham
  44. 44. Solidworks 2006 Fundamentals Assembly Interference check Click “Interference Detection” icon Click “Calculate” icon Check the result on the list Press “Esc” key on the keyboard to exit Interference result The overlapped portion is highlighted A- 44Version 1- May07 Written by Dickson Sham
  45. 45. Solidworks 2006 Fundamentals 2D Drawing Part /Assembly Drawings We can create a 2D drawing from a part It is unidirectional arrow; 3D can change 2D, but not vice versa or an assembly. They have the parent- and-child relationship; 3D model is the parent and the drawing is his child. If the 3D model is changed, the drawing will be changed automatically. The file extension of Solidworks drawings is *.slddrw, no matter it is a part drawing or an assembly drawing. Same as the assembly file, the drawing file cannot be opened properly if the system cannot locate the part/assembly file. Wherever when we open the drawing file, the system will try to locate the parent part/assembly file to update all the views. A- 45Version 1- May07 Written by Dickson Sham
  46. 46. Solidworks 2006 Fundamentals 2D Drawing Create Views To create a 2D drawing:- •Select “File/New…” on the menu •Click “Drawing” and then OK •Select a template, e.g. A-4 Landscape •Click “Browse”, the select a part /assembly file •Then Select “Single View” or “Multiple Views” (Single view – create views one by one and we can see the preview; Multiple Views – create many views at one time by highlighting the view icons below) •If you want to scale down the view to fit it onto the paper, you can use “Custom size”. But generally, we prefer using a bigger paper to making the model views smaller. To change the properties of the 2D drawing:- •Right-click on the paper and then select “Properties” •We can now change the paper size and also change the projection method. (By default, First Angle projection is used. First Angle projection is commonly used in China, but Third angle projection is used in United states and Taiwan.) •(Remark: After the projection method is changed, all existing views will be updated correspondingly) A- 46Version 1- May07 Written by Dickson Sham
  47. 47. Solidworks 2006 Fundamentals 2D Drawing Create Views To remove all tangent edges on a view: To add or remove curves on a view: -Right-Click on the view (For dependent curves, projected from 3D) -Select Tangent Edge/ Tangent Edges Removed -We can only hide the curve that we don‟t want to see. We cannot delete it. -To hide the curve, right-click on the view and then select “Hide edge” then select the curve (For independent curves, created on the view) - Simply select and delete it. To show hidden edges on a view: To create a section view: •Single Click on the view -Double-click the parent view •Select “Hidden Lines Visible” -Select “ insert/ Drawing View / Section” on the menu bar on the pop-up window on the left -Pick two points to define the mirror line A- 47Version 1- May07 Written by Dickson Sham
  48. 48. Solidworks 2006 Fundamentals 2D Drawing Dimensioning To Create Dimensions on a view:- •Click “Smart Dimension” icon •Select an entity / entities to dimension •Remark: Type of dimension (distance, length, angle, diameter) is automatically selected •To add a tolerance, select the dimension and then change the type of tolerance, e.g. LIMIT or Symmetric LIMIT Symmetric •To add a text before or after the dimension, type in the text before or after <DIM> To change the dimension properties of the sheet:- •Select “Tools /Options” on the menu bar •Select “Document Properties” •Select “Detailing / Dimensions” •Change the arrow style to “closed filled” •Select “Precision…” to increase/decrease the number of decimal places •Select “Detailing /Arrows” to change the arrow size •Select “Detailing / Annotation Fonts/ Dimension” to change the dimension font size A- 48Version 1- May07 Written by Dickson Sham
  49. 49. Solidworks 2006 Fundamentals 2D Drawing Editing Title Block To edit Title Block:- -Double-click “Sheet Format 1‟ on the tree (All the views will become invisible, and you can now select, add or delete any lines on the title block) -After editing, double-click “Sheet Format1” again to exit To add a text onto Title Block:- •Double-click “Sheet Format 1‟ on the tree to activate •Click “Note” icon •Type in the text •(You can change the text properties by the toolbar “Formatting”) •Click ok to complete •Drag the text to the desired position •Double-click “Sheet Format 1” on the tree again to exit A- 49Version 1- May07 Written by Dickson Sham
  50. 50. Solidworks 2006 Fundamentals Parameters Equations and Design Tables To Define an Equation to control parameter(s):- (Use a simple box as an example) • Height (30) = Length(80) - Width (50) • Define “Length” and “Width” as the driving parameters, “Height” as the driven parameter. • Select “Tools /Equations” on the menu bar • Click “Add..” • Double-click the feature to show all related parameters • Select the driven parameter • Type „‟=“ • Select a driving parameter, then type “-” • Select the other driving parameter, then click ok • (The equation is added. Now the parameter “Height” is driven by “Length” and “Width” To Create a Design Table to control parameter(s):- • Select “Insert/ Design Table” on the menu bar • Select “Blank” as source; Select “Block model edits that would update the design table”; Deselect the below three options • Click ok to create • Double-Click on the feature “Extrude1” to show all related parameters • Double-Click the parameters to add them into the design table • Add anther rows of values for these parameters • Click on empty space to complete • Select a configuration under “Configuration Manager” A- 50 - END-Version 1- May07 Written by Dickson Sham