SolidWorks 2011 Parts Bible - Matt Lombard [184]
Note
The Fit Spline feature fits a spline to a set of sketch entities within the specified tolerance. It can be a useful tool for smoothing out sketch geometry.
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.
9. 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.
10. 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 reference and the outer end of the Fit Spline that you have just created as the second reference. Click OK to accept the new plane. This is illustrated in Figure 12.38.
Figure 12.38
Creating a new plane
12. Drag the Rollback bar down between Sketch3 and Loft1. If it goes beyond Loft1, then you need to navigate back to this position again.
12. Right-click Sketch3 and select Edit Sketch Plane. Select the newly created Plane1 from the Flyout FeatureManager, and click OK to accept the change.
13. 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 12.39. Do not exit the sketch.
14. One of the goals of these edits is to smooth out the part. Remember that the Deviation Analysis told you that the edges created between the lines and arcs in Sketch3 were not very tangent. For this reason, it would be a good idea to replace the lines and arcs in Sketch3 with another Fit Spline.
Right-click one of the solid sketch entities in Sketch3, and click Select Chain.
Figure 12.39
Sketch3 in its new location
15. Create another Fit Spline using the same technique as in Step 8. Exit the sketch.
16. Drag the Rollback bar down one feature so that it is below the Loft. Notice that the Loft feature has failed. If you hold the cursor over the feature icon, the tooltip confirms this by displaying the message, “The Loft Feature Failed to Complete.”
17. Edit the Loft feature. Expand the Centerline Parameters panel if it is not already expanded, and delete the Spiral from the selection box. In its place, select the Spiral Fit Spline.
18. If the loft does not preview, check to ensure that the Show Preview option is selected in the Options panel, at the bottom.
19. If it still does not preview, right-click in the graphics window and select Show All Connectors. Position the blue dots on the connector so that it looks like Figure 12.40.
20. Click OK to accept the loft. The loft should be much smoother now than it was before. In addition, the spiral feature should no longer be under the loft; it should now be the first item in the design tree.
21. Drag the Rollback bar down to just before the Shell feature. Notice that Fillet5 has failed. Move the mouse over Fillet5. The tool tip tells you that it is missing some references. Edit Fillet5 and select edges in order to create fillets, as shown in Figure 12.41.
Figure 12.40
Positioning the connectors
Figure 12.41
Repairing Fillet5
22. Right-click in the design tree and select Roll To End. This causes the FeatureManager to become unrolled all the way to the end.
23. The outlet of the involute is now longer than it should be. This is because the original extrude was never deleted from the end. Right-click the Extrude1 feature and select Parent/Child. The feature needs to be deleted, but you need to know what is going to be deleted with it.
24. The Shell is listed as