SolidWorks 2011 Parts Bible - Matt Lombard [60]
10. Use the Centerpoint Rectangle to create a rectangle centered around the temporary axis of the large cylindrical face. Make sure that the centerpoint, which is the first click you make, picks up a coincident automatic relation with the temporary axis. Make sure the second click to place the corner of the rectangle does not pick up any automatic relations.
You can tell if any relations have been applied if you go to the View menu and activate Sketch Relations. Make sure the centerpoint has a coincident relation and that none of the corners has any relations.
Note
The temporary axis is not on the same plane as the sketch plane, so if the view is not normal to the sketch plane, picking up an automatic relation between the centerpoint of the rectangle and the temporary axis will be difficult.
11. Use the Smart Dimension tool to apply dimensions, as shown in Figure 3.50. Note that the 3.450-inch dimension goes to the part origin on the left. You can select this from either the graphics window or the FeatureManager.
Best Practice
It is best practice to dimension or create sketch relations to items that have the fewest other relations. You should try to use the part origin and standard planes when possible. Dimensioning to reference geometry is better than dimensioning to model edges, although this is not always possible. Experienced users will immediately recognize the need for removing layers of references to prevent restrictive parent-child relations and broken or dangling relations. For beginning users, after you have some experience with making changes to models where relations have been applied carelessly, being more selective with sketch and dimension references will look more attractive to you.
Figure 3.50
Dimensioning the new sketch
12. Click the Extrude toolbar button on the Features tab of the CommandManager. Rotate the model (by dragging with the mouse wheel depressed) slightly so you can see the side of the extrusion preview, as shown in Figure 3.51.
Figure 3.51
Creating the extrusion from the new sketch
You may have to adjust the direction of the extrude using the icon with the arrows just below the Direction1 heading in the Boss-Extrude PropertyManager.
13. Use the Up To Next end condition, which makes the sketch go up to the next solid that it encounters.
14. Use the View menu to turn off the display of Axes, Temporary Axes and Planes.
Summary
Sketching in SolidWorks is something that you will do almost every time you open the software. A lot of automated functions are available that can enable you to do much of the work for you. You also have a lot of control to make changes manually. Remember that the best way to create most sketches is to use automatic relations when you can, sketch the approximate shape that you want to make, and then either drag it to pick up automatic relations, add dimensions, or add relations manually. Remember that you can use the left-click context toolbar to speed up adding relations manually.
The options for creating intelligent relationships that establish your Design Intent, as well as SolidWorks's capabilities in laying out mechanisms, is only limited by your imagination. The more familiar you become with the tools in your toolbox, the more of a craftsman you can become with this software.
Reference geometry is an essential part of creating and controlling relationships in any parametric model. Reference geometry is usually more stable than solid geometry, so sketch relations and dimensions should use reference geometry as references when possible.
Chapter 4: Creating Simple Parts and Drawings
In This Chapter
Establishing design intent
Building a simple part
Making a simple drawing tutorial
Good modeling practice is based on robust