Part II: Building Intelligence into Your Parts
Caution
Do not exit the Fit Spline by pressing the Enter key as you do with other commands, because it simply exits you
out of the command without creating a spline. n- Right-click on spline and select the Curvature Comb. Notice how the comb is affected
by the transition from the spiral to the straight line. - Exit the sketch, and create a new plane. Choose Insert ➪ Reference Geometry ➪ Plane
from the menus. Select the Right plane from the Flyout FeatureManager as the first refer-
ence and the outer end of the Fit Spline that you have just created as the second refer-
ence. Click OK to accept the new plane. This is illustrated in Figure 11.27.
FIGURE 11.27
Creating a new plane- Drag the Rollback bar down between Sketch3 and Loft1. If it goes beyond Loft1, then
you need to navigate back to this position again. - Right-click Sketch3 and select Edit Sketch Plane. Select the newly created Plane1 from
the Flyout FeatureManager, and click OK to accept the change. - Notice that the loft profile has moved to a place where it does not belong. This is
because the sketch has a Pierce constraint to the spiral, and there are multiple places
where the spiral pierces the sketch plane.
Edit Sketch3 and delete the Pierce constraint on the sketch point in the middle of the
construction line. Create a Coincident relation between the sketch point and the outer
end of the Fit Spline, as shown in Figure 11.28. Do not exit the sketch.