CHAPTER TE RI AL Introducing SolidWorks I MA n SolidWorks, you build 3D parts from a series of simple 2D sketches and features such as extrude, revolve, fillets, cuts, and holes, among others. You can then create 2D drawings from the 3D parts and assemblies. TE D This chapter will familiarize you with some of the tools available to make the transition to SolidWorks, and with some of the basic facts and concepts that you need to know to get the most out of the software.
Part I: Introducing SolidWorks Basics compatible with OpenGL. Hardware changes too rapidly for me to give specific recommendations here, but generally, nVidia brand boards in the Quadro line are acceptable, as are AMD/ATI brand boards in the FirePro line. You should expect to pay $100 to $500 for a serviceable low- to mid-range video card. Cards that are marketed as game cards, such as the Radeon or GeForce, have known limitations and do not work well with SolidWorks.
Chapter 1: Introducing SolidWorks SolidWorks 2011 also creates a folder in the My Documents folder called GaBi which appears to only have empty folders, but you should not remove it. Also in My Documents are two folders called SolidWorks Downloads and SolidWorks Visual Studio Tools for Applications. Both of these should also remain where they are. The SolidWorks Downloads folder is a good place to look for items that are downloaded automatically from the Background Downloader or the SWIM.
Part I: Introducing SolidWorks Basics FIGURE 1.2 The Welcome to SolidWorks screen Using Quick Tips The Quick Tips setting enables balloons with tips to help you get started with several tasks. For example, the first Quick Tip you see may be the one shown in Figure 1.3. When you begin to create your first document in SolidWorks, a Quick Tip helps guide you on your way. FIGURE 1.3 The SolidWorks Document Quick Tip As you continue working, Quick Tips displays a box, shown in Figure 1.
Chapter 1: Introducing SolidWorks FIGURE 1.4 The main Quick Tip window FIGURE 1.5 Turning Quick Tips on or off Creating a new document To start a new SolidWorks document, click the New icon in the title bar of the SolidWorks application. With standard functions such as creating a new document, SolidWorks works just like a Microsoft Office application, and the icons even look the same.
Part I: Introducing SolidWorks Basics One of the most common questions new users ask is how they can change the default so that new documents come up with a certain type of units every time. Units in new documents are set within the templates. To create a part with inch units, use a template with inch units. You can have as many templates as you want, and can have a different template for each type of units you might use.
Chapter 1: Introducing SolidWorks FIGURE 1.8 The Getting Started option on the SolidWorks Resources tab of the Task Manager The terminology SolidWorks has used over the past several releases has changed and may seem confusing to some of you. In 2007, SolidWorks changed the name Online User’s Guide to SolidWorks Help. This is a help file on the local computer; it is not online in that it is not on the Internet. In 2010, the SolidWorks Web Help option was added to the Help menu.
Part I: Introducing SolidWorks Basics in the first place. This SolidWorks Bible fills in the gaps in information about the standard version of the software. Checking out the Tip of the Day The SolidWorks Tip of the Day is displayed at the bottom of the SolidWorks Resources tab in the Task Pane. Cycling through a few of the tips or using them to quiz coworkers can be a useful skills-building exercise.
Chapter 1: Introducing SolidWorks Templates and Formats Description .sldbombt BOM template (table-based) .sldtbt General table template .slddrt Drawing sheet format .sldholtbt Hole table template .sldrevtbt Revision table template .sldwldtbt Weldment cutlist template .xls BOM template (Excel-based) Library Files Description .sldblk Blocks .sldlfp Library part file Styles Description .sldgtolfvt Geometric tolerance style .sldsffvt Surface finish style .
Part I: Introducing SolidWorks Basics Best Practice It is especially important to have copies of these files in a location other than the default installation folder when you are doing complex implementations that include templates of various types of tables or customized symbol files. Uninstalling SolidWorks or installing a new version will wipe out all your hard work. Choose Tools ➪ Options ➪ File Location to save these files in separate library folders on the local hard drive or on a network location.
Chapter 1: Introducing SolidWorks FIGURE 1.9 The Novice and Advanced interfaces for the New SolidWorks Document dialog box Depending on your needs, it might be reasonable to have templates for metric and inch part and assembly, templates for steel and aluminum, and templates for sheet metal parts and for weldments, if you design these types of parts. If your firm has different customers with different requirements, you might consider using separate templates for each customer.
Part I: Introducing SolidWorks Basics To create a template, open a document of the appropriate type (part or assembly), and make the settings you want the template to have; for example, units are one of the most common reasons to make a separate template, though any Document Property setting is fair game for a template, from the dimensioning standard used to the image quality settings. You can find these settings through the menus at Tools ➪ Options ➪ Document Properties.
Chapter 1: Introducing SolidWorks FIGURE 1.11 The New SolidWorks Document dialog box FIGURE 1.12 Additional subfolders added to a File Locations path FIGURE 1.13 The tabs associated with the subfolders in New SolidWorks Document dialog box Using default templates Default templates are established at Tools ➪ Options ➪ Default Templates. The default templates must be in one of the paths specified in File Locations. Figure 1.14 shows the Default Templates settings. FIGURE 1.
Part I: Introducing SolidWorks Basics There are two Default Template options: Always use these default document templates and Prompt user to select document template. The Default Template options apply to situations when a template is required by an automatic feature in the software such as an imported part or a mirrored part. In this situation, depending on the option selected, the system automatically uses the default template or the user is prompted to select a template.
Chapter 1: Introducing SolidWorks “Feature-based” modeling means that you build the model by creating 2D sketches and applying processes (features) to create the 3D shape. For example, you can create a simple box by using the Extrude process, and you can create a sphere using the Revolve process. However, you can make a cylinder using either process, by revolving a rectangle or extruding a circle. You start by visualizing the 3D shape, and then apply a 3D process to a 2D sketch to create that shape.
Part I: Introducing SolidWorks Basics TABLE 1.2 Feature Types Sketch Required Sketch Optional No Sketch (Applied Features) Extrude Loft Fillet Revolve Sweep Chamfer Rib Dome Draft Hole Wizard Boundary Shell Wrap Deform Flex In addition to these features, other types of features create reference geometry, such as curves, planes, axes, surface features (Chapter 20); specialty features for techniques like sheet metal (Chapter 21); plastics/mold tools (Chapter 24).
Chapter 1: Introducing SolidWorks FIGURE 1.16 Features used to create a simple part If the order of operations used in the previous part were slightly reordered (by putting the shell and fillet features before Step 6), the resulting part would also look slightly different, as shown in Figure 1.17.
Part I: Introducing SolidWorks Basics FIGURE 1.17 Using a different order of features for the same part Figure 1.18 shows a comparison of the FeatureManager design trees for the two different feature orders. You can reorder features by dragging them up or down the tree. Relationships between features can prevent reordering; for example, the fillets are dependent on the second extruded feature and cannot be reordered before it. This is referred to as a Parent/Child relationship.
Chapter 1: Introducing SolidWorks removing the sleeve inside instead of the hole on top. You can try this for yourself by opening the part indicated previously, dragging the Shell1 feature in the FeatureManager, and dropping it just above the Cut-Extrude1 feature. Note You can only drag one item at a time in the FeatureManager. Therefore, you may drag the shell, and then drag each of two fillets, or you could just drag the cut feature down the tree.
Part I: Introducing SolidWorks Basics You can use 3D sketches for the Hole Wizard, routing, weldments, and complex shape creation, among other applications. Cross-Reference For more information on 3D sketching, please refer to Chapter 6. n For a simple example of working with sketch relations in a 2D sketch, consider the sketch shown in Figure 1.19.
Chapter 1: Introducing SolidWorks Cross-Reference You can read more about the PropertyManager in Chapter 2. n FIGURE 1.21 Dragging an endpoint where lines have relations Next, add a second parallel and a horizontal relation, as shown in Figure 1.22. If you are following along by re-creating the sketch on your computer, you will notice that one line has turned from blue to black. FIGURE 1.22 Horizontal and parallel relations are added. The line colors represent sketch states.
Part I: Introducing SolidWorks Basics l l Brown: Dangling. The relation has lost track of the entity to which it was connected. Pink. The pink sketch status is no longer used. There can be entities with different states within a single sketch. In addition, endpoints of lines can have a different state than the rest of the sketched entity. For example, a line that is sketched horizontally from the origin has a coincident at one endpoint to the origin, and the line itself is horizontal.
Chapter 1: Introducing SolidWorks Best Practice It is considered best practice to fully define all sketches. However, there are times when this is not practical. When you create freeform shapes, generally by using splines, these shapes cannot easily be fully defined, and even if they are fully defined, the extra dimensions are usually meaningless, because it is impractical to dimension splines on manufacturing drawings. n FIGURE 1.
Part I: Introducing SolidWorks Basics Editing Design Intent One of the most prominent aspects of design in general is change. I have often heard it said that you may design something once, but you will change it a dozen times. This concept carries over into solid modeling work. Design Intent is sometimes thought of as a static concept that controls changing geometry. However, this is not always the way things are.
Chapter 1: Introducing SolidWorks FIGURE 1.26 The Display/Delete Relations PropertyManager enables you to repair broken relations. Cross-Reference You can read more about repairing dangling entities in Chapter 12. n Using suppressed sketch relations Suppressing a sketch relation means that the relation is turned off and not used to compute the position of sketch entities. Suppressed relations are generally used in conjunction with configurations.
Part I: Introducing SolidWorks Basics of this is that you do not edit a SolidWorks drawing by simply moving lines on the drawing; you must change the model, which causes all drawing views of the part or assembly to update correctly. Other associative links include using inserted parts (also called base or derived parts), where one part is inserted as the first feature in another part. This might be the case when you build a casting.
Chapter 1: Introducing SolidWorks 9. Change the unit system to IPS, inches with three decimal places, using millimeters as the dual units with two decimal places. Set angular units to Degrees with one decimal place. 10. Change to the Grid/Snap page. 11. Turn off Display grid. 12. Change to the Image Quality page. 13. Move two-thirds of the way to the right, so it is closer to High. Make sure the Save tessellation with part document option is selected. 14.
Part I: Introducing SolidWorks Basics FIGURE 1.28 Drawing a line and applying a dimension 26. Press Esc to exit the Dimension tool and click the RMB on the displayed dimension and select Link Value. 27. Type thickness in the Name box, and click OK. 28. Press Ctrl+B (rebuild) to exit the sketch, select the sketch from the FeatureManager, and press Delete on the keyboard. Note You do the exercise of creating the sketch and deleting it only to get the link value “thickness” entered into the template.
Chapter 1: Introducing SolidWorks 3. Press the Spacebar on the keyboard to open the View Orientation dialog box, and double-click the Front view. 4. Right-click the Front plane in the FeatureManager, or whatever the first plane listed is, and select Sketch. 5. Click the View menu, and make sure the Sketch Relations item is depressed. This shows small icons on the screen to indicate when parametric relations are created between sketch entities. 6.
Part I: Introducing SolidWorks Basics 9. Activate the 3 pt Corner Rectangle. To find it through a menu, choose Tools ➪ Sketch Entities ➪ 3pt Corner Rectangle. 10. Click the first point inside the circle, click the second point outside the circle, and click the third point such that one end of the rectangle is completely inside the circle. Use Figure 1.30 as a reference. Avoid making any two points vertical or horizontal from one another.
Chapter 1: Introducing SolidWorks FIGURE 1.31 Creating a midpoint relation between a centerline and a line FIGURE 1.32 Making the rectangle symmetric about the centerline 13. Drag one of the corners of the rectangle from inside the circle and drop it on the circumference of the circle itself. The point here is that you want the corner of the circle to be right on the circle always. A coincident relation is created by the drag-and-drop action.
Part I: Introducing SolidWorks Basics line, the vertical dimension, or the dimension aligned with the angle of the line. When the dimension is aligned with the angle, as shown in Figure 1.33, click the RMB. This locks in that orientation and enables you to select a location for the dimension without affecting its orientation. Click to place the dimension. If the dimension does not automatically give you the opportunity to change the dimension, double-click the dimension and change it to 0.5 inch or 12 mm.
Chapter 1: Introducing SolidWorks FIGURE 1.34 Creating an angle dimension FIGURE 1.35 Using arrows or scroll wheel to change dimension values Summary While product development is about design, it is even more about change. You design something once, but you may modify it endlessly (or it may seem that way sometimes). Similarly, SolidWorks is about design, but it really enables change.
