Part II: Building Intelligence into Your Parts
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. n
- 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. - Right-click anywhere in the FeatureManager and select Roll To End.
- 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. - 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. - 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. - 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. - 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. - 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. - Dimension the center of the large circle to the edges of the model.
- 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. - 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. - 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.