Items covered in this section: • Default with SolidWorks • Pre-Template set up work • SolidWorks Templates & Settings we are going to cover: Part Assembly Drawing − Sheet format − BOM − Revision Block • Tools Options • Property Tab Builder (Newer Feature Still working on Templates)
Default with SolidWorks • By default when SW opens - NOVICE is set • The template that opens is what the default is set to, if no default is set then it defaults to the “Templates” that were created upon install. • Should already be set. If not just click on the icon shown.
Default with SolidWorks• TEMPLATES: This is set when you open SolidWorks the first time, there are a few generic selections as a standard. The Custom Templates have already been created and can be found in the following location: • L:VAULTDPT Templates• Click on the Advanced button in the lower Left corner if it has not already been selected.• If it has been selected you should see what is in the image on the right (below).
Pre-Template set up work Metadata - Sometimes referred to as custom properties or attributes, these are typically the attributes used to identify information in documents. − Part Number - Customer ID − Description - Weight − Material - Program − Finish - Material Size − Drawn By / Date - Surface Treatment − Check By / Date - Reference Drawing − Approved By / Date - Blank Number − ANY INFORMATION THAT WILL BE USED IN BOM, DRAWINGS ETC… Define location for all templates to be saved − PDM System? We will be migrating into a PDM System in the near future. Hopes are that most of the required information for the PDM System will already be in the Parts/Drawings − Network Shared Location: L:VAULT − Who is the Admin? − At present I am the Admin. However, I will be teaching everyone how to use the Admin tools and the system as a cross over function.
SolidWorks Templates Types:• Part Templates (*.prtdot)• Assembly Templates (*.asmdot)• Custom Property File (properties.txt)• Drawing Templates (*.drwdot)• Drawing Sheet Format (*.slddrt) Revision Block (*. sldrevtbt) Bill Of Materials (*. Sldbomtbt)• Others for reference:
Part Templates Contain:PART TEMPLATE • Part Templates drive all custom properties in drawings • Part Templates have standards built into them• Open SW Part OPEN SW PART DEFINE SAVE AS TO OPTIONS SHARED DOCUMENT LOCATION PROPERTIES SET DEFINE ORIENTATION METADATA “ISO” Part Number = File Name $PRP:"SW-File Name"
ASSEMBLY TEMPLATE Part Templates Contain: • Part Templates drive all custom properties in drawings• Open SW Assy • Part Templates have standards built into them OPEN SW ASSEMBLY DEFINE SAVE AS TO OPTIONS SHARED DOCUMENT LOCATION PROPERTIES SET DEFINE ORIENTATION METADATA “ISO” Part Number = File Name $PRP:"SW-File Name"
DRAWING TEMPLATE• Drawings have MORE options and settings then Part and Assembly templates.• Components of a drawing: Drawing Templates (*.drwdot) Drawing Sheet Format (*.slddrt) Revision Block (*. sldrevtbt) Bill Of Materials (*. Sldbomtbt)
DRAWING TEMPLATE• Drawing Templates (*.drwdot) • This contains document specific found in “Tools, Options, Document Properties” • Fonts • Dimension standards and styles • Line fonts • Predefined views, etc… • You can save the Revision Template!
DRAWING TEMPLATE• Drawing Sheet Format (*.slddrt) • The geometry and notes that make up the drawings title block. • This also contains the anchors for the BOM, Revision Table etc. • SLDDRT file is setup for a particular paper size, unlike a template which can be for any size. • When a format is used in a drawing, all the fonts and other settings get updated with the current document settings.
DRAWING TEMPLATE• Revision Block (*. sldrevtbt)• Can be saved to the Drawing Templates (*.drwdot) • RMB on drag handle for save option
DRAWING TEMPLATE• Bill Of Materials (*. Sldbomtbt) There must be a SW Document ( Part or Assy) on the drawing A drawing can contain a table-based Bill of Materials or an Excel-based Bill of Materials, but not both. We will be using the SW Table-Based BOM – RMB to save. SW Help - Drawings and Detailing > Tables
TOOLS OPTIONS• Bringing it all together• Options or Tools > Options and select File Locations• Specify folders to search for different types of document.• Folders are searched in the order in which they are listed • DOCUMENT TEMPLATES • BOM TEMPLATES • CUSTOM PROPERTY FILE • REVISION TABLE TEMPLATES • SHEET FORMATS • CREATE TABS AS NEEDED
TOOLS OPTIONS• Default Templates Options• Options or Tools > Options and select Default Templates• Specify the folder and template file for automatically created parts, assemblies, and drawings. For example, when you import a file from another application or create a derived part, the default template is used for the new document.
PROPERTY TAB BUILDER• Property Tab Builder is a stand-alone utility you use to create a customized interface for entering properties into SolidWorks files.• Why ? Create standard metadata for users to access.• The tabs you create with Property Tab Builder appear in the SolidWorks interface on the Custom Properties tab in the Task Pane.• You create different tab templates for parts, assemblies, and drawings.• Save the tab templates in the location where you store your properties.txt file. .prtprp for parts .asmprp for assemblies .drwprp for drawings• No longer use the properties interface.• Find other – Start, All Programs, SolidWorks 20XX, SolidWorks Tools• Lets set one up for a SW Part - Number, Description, Created by and Date
PROPERTY TAB BUILDER• Dynamic with the properties, drop down menu for selection.
PROPERTY TAB BUILDER• By default it the Part option is selected.
PROPERTY TAB BUILDER• Select the group box• Change Caption Name to a functionally name : SW World 2011• Choose whether it is a expanded or collapsed box.
PROPERTY TAB BUILDER• Choose which type of element you would like to add to the Tab Template • Use group boxes to group related elements. You can place multiple group boxes at the page level. You cannot place group boxes inside other group boxes. You place all other elements inside group boxes. • Text boxes accept free-form text, dates, or Yes/No values. • List boxes present users with a list of predefined text values. You can populate the list by typing values or importing them from a text file, Excel spreadsheet, or Access database. • Number boxes accept numeric values. • Check boxes toggle between two predefined values. You can control which other elements are available in each state. • Radio buttons allow selection of one of two or three predefined values. You can control which other elements are available in each state.
PROPERTY TAB BUILDER• Lets add the first property for CREATED BY • Title of block • Metadata property • Where the information comes from • Custom or configuration specific
PROPERTY TAB BUILDER• Add the other properties• Use the help file• PTB is easy to use
Dauphin Precision ToolSolidworks Design ConsiderationsCreating SolidWorks Parts
START WITH A PLAN: Prepare a strategy that establishes desirable characteristics of good models Functionality Predictability Build intelligence into your part that is mindful of dimensioning schemes and manufacturing Performance Stability processes Think as far forward as possible. Don‟t be afraid to Accuracy Changeability experiment and change course when you encounter obstacles
MAKE USE OF THE ORIGINWith the origin placed at a meaningfullocation you may be able to use thedefault planes for assembly mating.This allows you to edit or suppress partfeatures without affecting the assembly.Thoughtful placement of the origin allowsyou to make the most of symmetry.It is very useful to control the orientation and the position of the part using the origin.As you create the part consider if there is a logical orientation of the geometry thatwill help you organize and control the design? Does the orientation of the partaccurately communicate the design intent? Can six standard views be created intheir correct orientation?Locating the origin at a meaningful location will allow you to dimension additionalfeatures off the default planes. Convenient placement of the origin also allows you totake advantage of symmetry.
CONSIDER SYMMETRYBuilding parts symmetrically about the origincan significantly reduce modeling time.Mirroring features is typically easier thanmirroring sketch entities.Mirroring bodies is quicker and more reliablethan mirroring features.By creating geometry symmetrically aroundthe origin can significantly reduce modelingtime, more importantly it is easier to modifythe part later. Mirroring bodies is faster thanmirroring features, dynamic mirroring is auseful tool when sketching. You can alsoaccomplish symmetry by using Circularpatterns.
DEFINE WHAT IS IMPORTANT Think through your design intent and use the appropriate relationships to ensure that functionality is upheld. This will communicate your strategy to others while making changes easier to apply. As you constrain geometry consider how the part is used and think how to define the features that are important. If engineering drawings require a different dimensioning scheme you can add them as reference.
CREATE FEATURES IN LOGICAL SEQUENCETop down – start with the smallestmass that will contain the entirepart then subtract material Sketch Based FeaturesBottom up – begin with a coreshape then create additionalfeatures Applied FeaturesFillets can be sketched or applied Applied Features shouldfeatures – though there are appear towards the Bottomlimitations to sketch fillets of the Feature Manager Apply Drafts before Fillets Apply Fillets before Shells
LIMIT THE SCOPE OF FEATURESSeparate features allow you to simplifypart representation by suppressing anycombination of featuresSeveral simple sketches are easier tomanage than one complex sketchWhen you‟re creating a model it is goodpractice to break the part down intoseparate features. Sometimes we try tocombine too many details into onefeature, producing an “all or nothing”scenario. Separate features permit you toedit, suppress, or delete any combinationof features. This ability allows you tosimplify the part representation; useful forspeeding up assemblies or simulations.
GUIDE LINES FOR SKETCHESFor most cases use fully defined sketchesGenerally it is good practice to use fully definedsketches and to keep your sketches simple.Keep sketches simple due to the fact that complexsketches are more difficult to understand or modify.Use construction geometry to get the desireddimensioning scheme. Sometimes it will benecessary to create centerlines or constructiongeometry to get the dimensions that can be„Marked for Drawing‟.Be sure to understand sketch relationshipsTo ensure stability and predictability it is veryimportant for you to understand the graphicalfeedback and the relationships you are creating insketches. It is useful to rotate the part to be sureyou are selecting the correct entities; also you cansketch without automatically inferring referencesby pressing down the Ctrl key.
CAREFULLY CHOOSE REFERENCES Choose references that allow the geometry to move with intent as changes are made Create only enough references that allow the model to follow design intent Select references that won‟t disappear by relating to sketches rather than edges As often as possible reference default datum planes
DON‟T ADD FEATURES WHEN YOU CAN EDITRollback and insert features – or editexisting features. Especially importanton parts with complex geometry or alarge feature count.Insert features close to the parentgeometry.This practice keeps features in alogical sequence and reduce rebuildtime while working.One of the advantages of a featurebased CAD system is that you canreturn to any point in the history of thegeometry creation and make edits.It is important to get comfortable rollingback your model.
SURFACES AS CONSTRUCTION GEOMETRY CAD users tend to think surfacing makes models more complicated when in fact, the opposite can be true. This technique of mixing surfaces with solid features is known as hybrid modeling.
PRINCIPLES OF PARAMETRIC MODELING• When confronted with a design problem, engineers are faced with a methodological choice: analytical study or CAD and simulation• The power and speed of designing in SolidWorks® has led many to invest their time (sometimes exclusively) in CAD and simulation• Skipping the analytical methods can result in a loss of fundamental design insight and suboptimal parameterization• The intent of parametric modeling theory is to integrate analytical methods directly into the CAD and simulation environment and thereby give the designer maximal insight, efficiency, and power• An integrated approach to parametric design that combines analytical engineering sciences directly into CAD and further uses simulation for design optimization• Advantages The resulting integrated parametric designs are elegant, efficient, economical, optimized, and easily adapt to change• Key concept A parametric model is the solution to a design problem
ESSENTIAL COMPONENTS OFPARAMETRIC MODELING THEORY• Understand problem at hand List design constraints and assign nomenclature Draw freehand sketches as needed to describe the problem List relevant physics (e.g. geometry, materials, statics, dynamics, thermal)• Specify design intent Determine design problem Determine key parameters that will drive design Determine which parameters will be computed or optimized• Build parametric model with analytical methods• Confirm and adjust model with simulation
Dauphin Precision Tool Solidworks FeaturesCreating SolidWorks Parts
STANDARD FEATURES TO BE USEDRevolves add or remove material by revolving one or more profiles around a centerline. You can create revolvedboss/bases, revolved cuts, or revolved surfaces. The revolve feature can be a solid, a thin feature, or a surface.To create a revolve feature, use the following guidelines:1. Create a sketch that contains one or more profiles and a centerline, line, or edge to use as the axis around which the feature revolves (As shown below).2. Click one of the following Revolve Tools:
STANDARD FEATURES TO BE USED3. In the Property Manager set the options.4. Click
STANDARD FEATURES TO BE USEDExtrude- Adds or removes material byExtruding one or more profiles through yourPart. You can create Extrude boss/bases, orExtrude cuts. The Extrude feature can be asolid, or a thin feature.To create a Extrude feature, use the followingguidelines
STANDARD FEATURES TO BE USED 1 2 31. Create the sketch Select the Right Plane (or the Plane that runs through Centerline of Part) While the Right Plane is selected click on the Sketch Tab then the Sketch Icon Sketch the profile using Sketch Lines and Construction Lines as required (shown above)
STANDARD FEATURES TO BE USED 1 22. Create the Extrude Once Sketch is complete Click the Featured tab and select Extrude Cut ( while still in Sketch) On the Left the Extrude Properties Manager pops up (shown next slide) Continued next slide……
STANDARD FEATURES TO BE USED 4 1 2 33. Create the Extrude Continued……… In the Extrude Properties Manager in the Direction 1 section select the scroll down and select Mid Plane (as shown) Also in Direction 1 section set the depth/width of the Extrude Cut Feature In the Configurations section select This Configuration (This Feature should be in the Turning Configuration) Then click the
STANDARD FEATURES TO BE USED 1 3 2 4 51. Create a Wrap Feature The use of this Feature allows you to create a specific Helix Angle With SolidWorks you only need to input two dimension values when the sketch is set up as shown above Either input in Length of Cut & Helix Angle Or input Lead and Helix Angle Select the top plane. With Top Plane selected click Sketch tab and start New Sketch Sketch a Construction Line through the Center of Part Then select the Line tool and Sketch the Triangle as shown above When Sketch is complete select Features Tab and select Wrap Continued on next slide…….
STANDARD FEATURES TO BE USED 1 3 22. Create a Wrap Feature continued……. With Feature Selected click on Deboss Then click the Face to apply the Feature You will also need to set a depth to create the feature After everything is set click
STANDARD FEATURES TO BE USED 1 3 2 5 3. Create a 3D Sketch Path – • This shows the Wrap Feature we just set up that will be used to create the 3D Sketch • Select the curve edge that is on the top surface as shown • Once the curve is selected click on the Sketch Tab, Then click the scroll down next to Sketch Icon and click 3D Sketch • Now in the 3D Sketch and the Curve edge is still 4 selected, in the Sketch Tab click on Convert Entities this will create a 3D spline of the selected edge • That 3D Spline will be used as the path for the Helix
STANDARD FEATURES TO BE USED1. Create the Profile Sketch 1 Select the Face you want to start the Sketch on While the Face is selected click on 3 the Sketch Tab then the Sketch Icon For this Profile we will use existing Geometry. Click on the edges you want to use; Then select Convert Entities (shown Right and Below) Still in the Sketch now select the Line tool and sketch lines to close the profile as shown (in blue Right) When Sketch is finished click 2
STANDARD FEATURES TO BE USEDCreate a special Reference Plane The ability to add additional Reference Plans gives you control over your Features You can set Planes where you need them and in the orientation you want them This adds leverage and control in your design
STANDARD FEATURES TO BE USED > 2 11. Create a special Reference Plane Select a Point/Line/Face on the the current geometry Then click on Insert > Reference Geometry > Plane This will now open the Plane Property Manager Continued………
STANDARD FEATURES TO BE USED1 1 32 22. Create a special Reference Plane Continued……. Once the Plane Property Manager opens the Point/Vertex you selected is already set as First Reference You need to set the Second Reference which will be the edge of the existing curve (shown purple above) Once those two References are set you will see the Blue Transparent Plane (as shown above) Click the Continued next slide……
STANDARD FEATURES TO BE USED 2 1 3 33. Create a special Reference Plane Continued……… Now that the base plane is in place we can now set up the Reference Planes needed to create the Plane required for the Profile Path Sketch With the first plane selected follow the same direction we used to Insert the previous Plane Insert > Reference Geometry > Plane You will need a Vertical line (as shown above) to be used as the Second Reference Once these References are set you can click
STANDARD FEATURES TO BE USED 1 2 14. Create a special Reference Plane Continued……… Just as with the last Plane; with previous Plane selected go to Insert > Reference Geometry > Plane This will again open the Plane Property Manager The selected Plane will already be set as First Reference. We will be setting this new Plane at a distance so select that icon and set a distance that makes the Plane as near Tangent to the existing curve as possible (as shown above) Once this is set click the
STANDARD FEATURES TO BE USED 2 15. Create the Path Sketch Select the last new Reference Plane created and with it selected open a new Sketch Add a Radius that sweeps from just in front of the Profile Sketch Plane/Face to beyond the OD of the Part so that when the Swept-Cut is applied it comes off the Part. Once Sketch is complete click Continued next slide……..
STANDARD FEATURES TO BE USED2 3 3 16. Create the Swept-Cut 2 First Select Features Tab and select Swept Cut; This will open the Cut Sweep Property Manager Next you will want to be sure the Profile box is highlighted then select the Profile Sketch Then select the Path box to highlight it then select the Path Sketch Next Go To Options section and click the Orientation scroll Menu and select Follow Path; Leave boxes checked by default then click the
STANDARD FEATURES TO BE USED 2 1 Create a Circular Pattern – 3 • This shows the Swept Cut we just set up as the Feature to Pattern • Then click on the Features Tab, select the scroll down on Linear Pattern to select 3 • Circular Pattern. Once the Circular Pattern Property Manager is open click on View > Temporary Axis select the Axis that is in the Center of the Part and set it for the Rotation Parameter 4 • • Set the angle for your circular pattern Set the number of Instances of the Feature to Pattern • Be sure that the selected Cut Sweep is in the5 • Features to Pattern box Once everything is set the way you need it 6 click the
STANDARD FEATURES TO BE USEDCreate the Lofted-Cut This Feature allows you to make controlled cut Features that otherwise would be difficult if not impossible to complete There are a few additional References that need to be set up in order to use this Feature properly
STANDARD FEATURES TO BE USED 2 5 4 2. Create Second additional Reference Plane Select the First Plane created 3 1 Then click on Insert > Reference Geometry > Plane This will now open the Plane Property Manager This Plane will be set at a Distance (Just beyond the1. Create First additional Reference Plane OD of the part) Select the Top or Right Plane Once Parameters are set click Then click on Insert > Reference Geometry > Plane This will now open the Plane Property Manager For the first Reference Plane you will need to set it at an Angle (360/6 (number of Circular Pattern Instances)) For the Second Reference you will need to click on View > Temporary Axis and select the Axis in the Center of the Part Once Parameters are set click
STANDARD FEATURES TO BE USED 7 3. Create Third additional Reference Plane 6 Select the First Plane created Then click on Insert > Reference Geometry > Plane This will now open the Plane Property Manager This Plane well be set at a Distance (Just beyond the CL of the part) Once Parameters are set click
STANDARD FEATURES TO BE USED4. Create the First Lofted-Cut Profile First Select the Second Reference Plane and while Plane is selected open a New Sketch Now select the Line Icon and sketch Profile as shown above Once Sketch is complete and fully defined click Continue to the next step…….
STANDARD FEATURES TO BE USED5. Create the Second Lofted-Cut Profile First Select the Third Reference Plane and while Plane is selected open a New Sketch Now select the Line Icon and sketch Profile as shown above Once Sketch is complete and fully defined click Continue to the next step…….
STANDARD FEATURES TO BE USED 5 2 36. Create the Lofted-Cut Path 1 First Select the Edge of the existing Geometry as shown Once Edge is selected click on Sketch Tab, then click scroll down next to the Sketch Icon and click 3D sketch Now in the 3D Sketch with the edge still selected click on Convert Entities 4 Select the new Converted Entity and in the Sketch Properties Manager on the Left check the box that says „For Construction‟ Still in the 3D Sketch click the Line Icon and Sketch a new 3D line. You want to be sure this new line extends beyond the Second and Third Reference Planes Once the line is complete select the Line and Control + click the Construction Line The Relations Property Manager opens. Here you want to make the lines Collinear Once this is set click
STANDARD FEATURES TO BE USED 1 3 5 4 1 25. Create the Lofted-Cut Select the First Profile Sketch and Control + Select the Second Profile Sketch With these two Sketches selected click the Features Tab and click Lofted Cut Icon This will open the Lofted Cut Property Manager (shown above Left) The two Selected Sketches are in the Profiles box Now highlight the Guide Curves box (may have to hit the scroll down on the right to expand window) and select the 3D sketch for the Path/Guide Curve Once everything is selected click
STANDARD FEATURES TO BE USEDCreate the Helix This Feature allows you to create a controlled Helix Feature There are a few pieces of additional References that need to be set up in order to use this Feature properly
STANDARD FEATURES TO BE USEDSelect Face then open New SketchThen click Covert Entities Select the Sketch you just created Then click Insert > Curves > Helix/Spiral Set the Properties Manager Once set click
STANDARD FEATURES TO BE USED Sketch Profile for Helix Diameter must be larger Sketch Horizontal line to be Then OD of body used as the Path for the Swept Surface Sketch Vertical line to be used as the Profile for the Swept Surface Create the Helix Select the First sketch (circle) Click Insert > Curves > Helix/Spiral Set parameters in Property Manager When set click the
STANDARD FEATURES TO BE USED 1 2 3 Create Swept Surface – • Once Sketches are complete you can select the Surfaces Tab and then the Swept Surface Icon • The Property Manager will open. In the Profile and Path section highlight the Profile box and select the Second sketch line; highlight the Path box and select the Third sketch line; In the Guide Curves section select the Helix • When everything is set select the
STANDARD FEATURES TO BE USEDWith „Mark for Drawings‟You can specify that dimensionsmarked for drawings be insertedautomatically into new drawingviews. Go to Tools > Options andin the Document Properties tab,click Detailing. Select Dimensionsmarked for drawing under Autoinsert on view creation.Dimensions marked for drawing toadd dimensions to models, withoutduplicates in multiple viewsThe dimensions are indicated in thepart sketches as Mark for drawing. This should have already been set when the template was created. If it is not just click the check box. Even though it may be set it is always good practice to get familiar with the various locations for settings.
STANDARD FEATURES TO BE USED Open/Edit Sketch and select Dimensions You want to be marked 1 When over a Dimension Right 2 Mouse Button Click to open the Pop-up window shown Then select „Mark for Drawing‟ 3 When Dimensions are „Marked for Drawing‟ they change to black to signify that they have been marked
DRAWING TEMPLATELinking Metadata to the drawing:$PRPSHEET:”Property Name”$PRPSHEET:”Description”Metadata from the Model (Part or Assembly on the drawing) Properties of Top level SW Part or Assembly
DRAWING TEMPLATE • There are two levels to a SolidWorks Drawing• Edit sheet format – You are here only to set up, you should not be in this on every drawing.• Edit sheet – This is where all of you work is to be done… Note you can not select the items on the Sheet format like “Description”
CREATE LINKED NOTES• You can link note text in the Drawing Sheet or Drawing Sheet Format to Document Properties. Link note to a Drawing View − Double click the view to lock the View Focus. This will insure that the note follows the view if the view is moved. Link note to a Document Property. − Set up a Custom Property at the part file − Choose the option “Model in view specified in sheet properties”
DRAWING TEMPLATE• Metadata coming from the Part Custom Properties to the drawing and feeding the Linked Notes.
DRAWING TEMPLATE• Metadata coming from the Part to the drawing and feeding the TEXT.• $PRPSHEET:"Description“• $PRPSHEET:”Property Name”• Metadata from the Model (Part or Assembly on the drawing) Driven by the custom properties of the Part