Extrusion failure do to 3D sketch flaw...

[NateFarringer]

Attached is a part I am having more of a headache with than anticipated. I intend to turn this into an iPart down the road, so I have setup the constraints to be easily adjustable by controlling everything with user parameters. The issue I am running into seems to be with the 3D sketch in the lofts on either end. If I make a change to the overall length in 1-inch increments, all is well and I can do that all day. If I try to make any larger changes, most often times the "Fully Constrained" 3D sketches flip directions and cause the extrude between to fail. I cannot find a better way to constrain the 3D sketch on the mirrored loft, and it really shouldn't be failing with how it's currently setup. Changing other things will also randomly cause things to fail, but this is the most easily reproducible method.

Obviously, maybe I overlooked something, as I don't work with 3D sketches on a daily basis so any input/advice would be greatly appreciated.

[johnsonshiue]

Hi! I think I have seen this behavior before. It is because the given constraint may lead to two solutions. Could you tell me the exact steps to see the flipping behavior?

Many thanks!

[NateFarringer]

That is correct, there are technically two solutions from what I can gather. However, because the sketch is fully constrained, it does not allow for me to further constrain it so only one solution is acceptable. I have reworked the constraints MANY MANY times with different methods to try and resolve it successfully, but none seem to work as good as what I currently have attached.

To see the behavior of it flipping, you just need to change the overall length of the part in the "User Parameters" drastically, say by 10". However, if you change it by only 1" incrementally, it seems to solve properly.

Basically, the ends need to have a completely smooth transition into the center section, which I have done using splines that run tangent along the top and side profiles and connected to the circular sections in a perpendicular fashion. 

Hopefully you can draw enough intent from that!

[johnsonshiue]

Hi! I see the issue now. It is indeed related to how the 3D splines are constrained. I need to figure out why it behaves this way.

Many thanks!

[johnsonshiue · Accepted solution]

Hi! I think this has something to do with lack of negative sketch dimension values. In general, sketch dimensions always have to be positive. The one exception is the dimension between a 3D point and a workplane. To stablize the solution, I created 4 more offset workplanes. Then dimension the CV points to those planes. Now, you can preserve the spline even when the overall length changes. Please take a look at attached part.

Many thanks!

[NateFarringer]

That seems to have done the trick! Thank you very much, I will keep this in mind for future reference!