Tutorial: Editing and Copying in soliworks

This tutorial guides you through some common sketch relation editing scenarios and using some of the Copy, Move, and Derive tools. Follow these steps to learn about editing and copying sketches:

  1. . Open the part named Chapter6 Tutorial1.sldprt from the CD-ROM. This part has several error flags on sketches. In cases where there are many errors, it is best to roll the part back and go through the errors one by one.
  2. . Drag the rollback bar from just after the last fillet feature to just after Extrude3. If Extrude3 is expanded so that you can see Sketch3 under it, then drop the rollback bar to after Sketch3. If a warning message appears, telling you that Sketch3 will be temporarily unabsorbed, then select Cancel and try the rollback again. Figure 6.15 shows before and after views for the rollback.
  3. . Edit Sketch3 and deselect the Sketch Relations display (View ➪ Sketch Relations). Relations with errors will still be displayed. Click Display/Delete Relations on the toolbar (the Eyeglasses tool), and set it to All in This Sketch. Notice that all the relations conflict, but only one is unsolvable: the Equal Radius relation. This appears to be a mistake because the two arcs cannot be equal.
  4. . Delete the Equal Radius relation. Select the relation in red and click the Delete button in the PropertyManager. (You can also press the Delete key on the keyboard.) The sketch is still not fixed.

Tutorial-Editing-and-Copying-in-soliworksRollback bar

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Rollback cursor                 Model in rolled back state

FIGURE 6.15 Rolling the part back to Extrude3

5. Click the green check mark icon to close the Display/Delete Relations PropertyManager.

6. Right-click the graphics window and select SketchXpert; then click Diagnose.

7. Using the double arrows in the Results panel, toggle through the available solutions. All the solutions except one remove sketch relations. Accept the one solution that removes the dimension. This is shown in Figure 6.16.The sketch no longer shows errors in the graphics window, but it still does in the FeatureManager.

8. Close the sketch. Notice that the error flag does not disappear until the sketch has been repaired and closed.

9. Use the rollback bar to roll forward to after Extrude2 and Sketch2. Figure 6.17 shows the tool tip message that appears if you place the cursor over the feature with the error. With time, you will begin to recognize the error messages by a single keyword or even by the shape of the message text. This message tells you that there is a dangling relation — a relation that has lost one of the entities.

10. Edit the sketch (see Figure 6.18). 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.

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FIGURE 6.16 Using the SketchXpert to resolve an overdefined sketch

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FIGURE 6.17 A tool tip gives a description of the error

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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.

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.

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