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fail to extrude a trim curve

Valued Contributor
Valued Contributor

Simple job fails. Help would be appreciated.

 

ScreenClip.pngFig.1 In SKETCH_000, the left arc is used as the boundary to extend the right arc.ScreenClip [1].pngFig.2 Trim Curce extends the right arc.ScreenClip [3].pngFig.3 The original right arc can be extruded as usual.ScreenClip [4].pngFig.4 The extended curve fails to be extruded!

 

12 REPLIES

Re: fail to extrude a trim curve

Valued Contributor
Valued Contributor

The curvature combs of the orginal arc and the extended arc have some weird difference.

 

ScreenClip [5].pngFig.5 The original arc.     ScreenClip [6].pngFig.6 The extened arc.

Re: fail to extrude a trim curve

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

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.

 

Regards

Paras

Paras Raina
Sr. Application Engineer | Solid Edge ST10 | NX 11
MSC Systems Pvt. Ltd. (India)

Re: fail to extrude a trim curve

Siemens Legend Siemens Legend
Siemens Legend

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.

 

Regards

 

Paul

Re: fail to extrude a trim curve

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

@Paul_BevanAfter all the MP's (NX 11 is on MP4 as of now), I can't believe this to be some kind of bug.

Paras Raina
Sr. Application Engineer | Solid Edge ST10 | NX 11
MSC Systems Pvt. Ltd. (India)

Re: fail to extrude a trim curve

Valued Contributor
Valued Contributor

Hi, @Paul_Bevan, thank you for checking it!

Re: fail to extrude a trim curve

Siemens Legend Siemens Legend
Siemens Legend
It looks like it is unfortunately

Re: fail to extrude a trim curve

Siemens Legend Siemens Legend
Siemens Legend

(view in My Videos)

Re: fail to extrude a trim curve

Valued Contributor
Valued Contributor

Hi, @Paul_Bevan

 

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.

 

ScreenClip.png

 

ScreenClip [1].png

 

ScreenClip [2].png

 

Re: fail to extrude a trim curve

Siemens Legend Siemens Legend
Siemens Legend

Hi,

 

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.

 

Johannes