SolidWorks 2011 Parts Bible - Matt Lombard [99]
10. Edit the sketch (see Figure 6.22). If you show the Sketch Relation icons again, the errors will be easier to identify. When you use Display/Delete Relations (Tools⇒Relations⇒Display/Delete Relations), the first two Coincident relations appear to be dangling. Clicking the relation in the Relations panel of the Display/Delete Relations PropertyManager shows that one point was coincident to a line and the other point was coincident to a point.
11. Click the name of the dangling entity in the Entities panel of the PropertyManager; then click the vertex indicated in Figure 6.18 in the Replace box at the bottom. When you have fixed the errors, exit the sketch and confirm that the flag is no longer on Sketch2.
An easier way to repair the dangling relation is to click on the dangling sketch point once. It will turn red. Next, drag the point onto an entity that you want to reattach the relation to.
12. Exit the sketch.
13. Drag the rollback bar to just before CutExtrude1. Edit 3DSketch1. This sketch is overdefined. If the Sketch Relations are not selected at this point, then select them again.
Tip
Because selecting and deselecting the display of the sketch relations in the graphics window is a task that you will perform many times, this is a good opportunity to set up a hotkey for this function. As a reminder, to set up a hotkey, choose Tools⇒Customize⇒Keyboard, and in the Search box type relations. In the Shortcut column for this command, select a hotkey to use.
14. Double-click any of the relation icons; the Display/Delete Relations PropertyManager appears. Notice that one of the sketch relations is a Fixed relation. Delete the Fixed relation, and exit the sketch.
15. Right-click anywhere in the FeatureManager and select Roll To End.
16. Click CutExtrude1 in the FeatureManager so that you can see it in the graphics window and then click a blank space to deselect the feature.
Figure 6.22
Fixing dangling errors
17. Ctrl+drag any face of the cut feature, and drop it onto another flat face. The Ctrl+drag function copies the feature and the sketch, but the external dimensions and relations become detached. This will only work if Instant3D is unselected.
18. Click Dangle in response to the prompt. This means that you will have to reattach some dangling dimensions rather than re-creating them. Edit the newly created sketch, which now has an error on it.
19. Two of the dimensions that went to external edges now have the olive dangling color. Select one of the dimensions; a red handle appears. Drag the red handle and attach it to a model edge. Do this for both dimensions. The dimensions update to reflect their new locations. Exit the sketch and verify that the error flag has disappeared.
20. Expand CutExtrude1, and select Sketch5 under it. Ctrl+select a flat face on the model other than the one that Sketch5 is on. In the menu, choose Insert⇒Derived Sketch. You are now in a sketch editing the derived sketch.
21. The sketch is blue, and so you should be able to resize it, right? No, it doesn't work that way for derived sketches. You can test this by dragging the large circle; it only repositions the entire sketch as a unit.
22. Dimension the center of the large circle to the edges of the model.
23. Drag the smaller circle, and notice that it swivels around the larger circle. Create an angle dimension between the construction line between the circle centers and one of the model edges. Notice that the sketch is now fully defined.
24. Exit the sketch, and look at the name of the derived sketch in the FeatureManager. The term derived appears after the name, and the sketch appears as fully defined.
25. Right-click the sketch and select Underive Sketch. Notice that the sketch is now underdefined. The Underive command removes the associative link between the two sketches.
Tutorial: Controlling Pictures, Text, Colors, and Styles
This tutorial guides you through some of the miscellaneous functions in sketches, and shows you what they are used for and how they are