Can you change the curve extension to linear or none by any chance? Solves the issue for me & makes it more simple for NX to extrude the curve.
In my opinion, this thing is messing up the curve. This is probably why it fails to extrude it.
I would report this as a PR. I have tried it in NX 12 and it works fine, but in NX 11 with the extension set to natural or circular it fails.
It's really frustrating to know that it only works in NX12. Anyway, thank you for your video!
My workaround is to keep only the extension range in Trim Curve, and then extrude the curve string of the original curve and the extension.
just to nail the issue down... it is not an extrude problem, the problem lies within trim curve.
The function creates a spline as the output geometry, with duplicate start poles, which is a degeneracy - that is why extrude fails. In NX12, trim curve creates an arc. It is simply a bug in NX11, but already fixed in NX12.
When you open the part in NX12, you'll need to renew the existing trim curve feature. Then it works.
So as another workaround for NX11, you can first extend the curve by "curve length" function to cross the bounding curve, and then extrude the curve with the "stop at intersection" option in the selection bar turned on.