SolidWorks 2011 Parts Bible - Matt Lombard [20]
15. Click the right mouse button (RMB) on the Materials entry in the FeatureManager, and select 1060 Alloy from the list. If it is not there, click Edit Material and find it from the larger list.
16. Choose File⇒Properties, and click the Custom tab.
17. Add a property called Material of type Text. In the Value/Text Expression column, click the down arrow and select Material from the list. Notice that the Evaluated Value shows 1060 Alloy.
18. Add another property called description and give it a default value of Description. At this point, the window should look like Figure 1.27.
Figure 1.27
Setting up Custom Properties
19. Click OK to close the Summary Information window.
20. Change the names of the standard planes by clicking them twice slowly or clicking once and pressing F2. Rename them Front, Top, and Side, respectively.
21. Ctrl+select the three planes from the FeatureManager, click the RMB, and select Show (the eyeglasses icon).
22. From the View menu, make sure that Planes is selected.
23. Click the RMB on the Front plane and select Sketch.
24. Select the Line tool and click and drag anywhere to draw a line.
25. Select the Smart Dimension tool and click the line, then click in the space in the Graphics Window to place the dimension. If you are prompted for a dimension value, press 1 and click the check mark, as shown in Figure 1.28.
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. Once you've done it, every part made from this template that uses an Extrude feature will have an option box for Link to Thickness, which enables you to establish a thickness variable automatically for each part you create. This is typically a sheet metal part feature, but you can use it in all types of parts.
29. Choose File⇒Save As and then select Part Template from the drop-down list. Ensure it is going into your template folder by giving it an appropriate name reflecting the inch units and 1060 material, and then click Save.
30. Edit the material applied to change it from 1060 Alloy to Plain Carbon Steel, and save it as another template with a different name.
31. Change the primary units to millimeters with two places, and save as a third template file.
32. Exit the file.
Tutorial: Using Parametrics in Sketches
What separates parametric CAD tools from simple 2D drawing programs is the intelligence that you can build in to a parametric sketch. In this tutorial, you learn some of the power that parametrics can provide in both structured (using actual dimensions) and unstructured (just dragging the geometry with the mouse) changes.
1. Open a new SolidWorks document by clicking the New toolbar button or by choosing File⇒New.
2. From the list of templates, select a new part template, either inch or millimeter.
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. Click the Circle from the Sketch toolbar (choose Tools⇒Sketch Entities⇒Circle).
7. Sketch a circle centered on the Origin. With the Circle tool activated, click the cursor at the Origin in the graphics area. The Origin is the asterisk at the intersection of the long vertical red arrow and the short horizontal red arrow. After clicking the first point, which represents the center of the circle, move the cursor away