Offset Spline

[Anonymous]

I have a problem with the attached part which is not updating correctly. There is "sketch3" which contains a spline. Sketch4 contains two offsets of the projected spline from Sketch3. When I change dimensions on Sketch3 Inventor tells me that there are open loops in Sketch4.

[johnsonshiue]

Hi! This has something to do with the offset spline and the way Sketch 4 was constrained. Here is a simple workflow to make it work. Before you edit Sketch3, edit Sketch4 first. Remove the horizontal constraints from the two short sketch segments. The offset cures of the projected splines in Sketch4 may no longer fulfill the horizontal constraints. This is because offset curve by definition is a curve going in normal direction of the source curve at a given distance. Unless the end points on the source curve have their normal direction pointing to horizontal direction, the end points of offset curves will not stay in the horizontal direction. The change in direction leads to constraint errors.

Many thanks!

[Anonymous]

Hi, Johnson thanks for the answer. However I still get the problem. I removed the horizontal constraints from the two line segments (and the center points), but when I change for example d418 to 700mm it does not update the extrusion5 correctly. What changed is that now it does not show me any erros on sketch4 itself but does not update correctly the extrusion. When I try to edit the extrusion it shows me "no valid loops" as an error message.

[johnsonshiue · Accepted solution]

Hi! This is a very interesting case. The way the geometry association was established is a bit brittle. First, the projected edges belong to two different solid bodies. Second, the offset curves can change direction. Instead of managing the change at sketch level, I use offset surface to manage at body level. Please see attached part. It does need a bit more work but. It is generally doable. Try changing the dimensions in Sketch3, you will notice that the model will update without an issue. Please let me know if you have any question.

Many thanks!

[Anonymous]

Wow, great solution. Thank you!

My idea was not to project the two edges of the solid bodies because this really got mixed up worse. So I projected the (uniterrupted) spline directly from sketch3, but did not work either.

Seems to be generally much more resistant to changes on surface/body level. Will have this in mind for the future. Thanks again.