Unable to Create a Section

[Jashe]

I have attached a screen shot of the Update Error I am getting when I try to create a section. I've been seeing this more and more. Can anybody tell me whats going on here? And hopefully how to resolve it?

 

[NutAce]

It will be difficult to determine the exact reason for this error without example data.

Try Fully loading your data (to resolve any Wavelinks or inter-part expressions which need to be updated).
If that doesn't help move your section line anchor to another suitable position. Sometimes a minimal difference in position helps to solve the issue.


Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Toost]

Click the "Show detailed information", it often gives information on where to look.
Does your model contain imported geometry ?
If so, Use the Examine geometry function, select w a rectangle around everything and examine.
Is the section line tangent to complex geometry ?
( a plane, (the section cut), touching a sphere gives a point as contact. This did produce this message in older NX versions.
If that section plane is tangent to complex geometry , it will/might give this message.)
Try as Ronald say move the section line slightly.

Regards,
Tomas

 

[Jashe]

I've went through and found the component that is creating the error. When I delete it and update, the section appears. These components are all Parasolids. I wish I could send the whole file but it's proprietary. I've attached a zip with the part file & drawing with the problem components if anyone wants to see if they can figure this one out ( I hope somebody can, I can't just be leaving components out of the views).

FYI, ignore the title block. It's just the generic one they give us.

 

[cowski]

In the model file, bodies 5, 10, and 19 have geometry errors (consistency errors, face self-intersection, etc). When the errors are fixed, there is a good chance the section view will work normally. When you run examine geometry, a solid part must pass all the body checks and the face self-intersection check. If it does not, errors may appear in downstream operations (drafting views, tool path generation, CAE meshing, etc).

ALWAYS use examine geometry and fix major errors on your parts before releasing them for further use.

www.nxjournaling.com

 

[Jashe]

Thank you all. The geometry was sent to us from the supplier I believe so we didn't have the live model to work with.

 

[cowski]

When working with imported geometry, I suggest running examine geometry right after the import and using heal geometry and/or optimize face as necessary. Sometimes using a different neutral format (parasolid vs. STEP or vice-versa) will reduce such issues. The synchronous commands can be used to fix up minor errors. In extreme cases, it might be necessary to ask the originator to make a few changes before exporting.

www.nxjournaling.com

 

[Toost]

Since these solids are imported into NX ( ?) , non-parametric.
You can use the File- export- heal geometry option.
It will export the solids into a new file and clean / Heal / repair , if possible, the solids.
( note the file name and the directory where the healed file becomes saved.)
You can then re-import that part into the model file, delete the original solids and update the drawing.


Regards,
Tomas

 

[Jashe]

Thanks Toost, that worked out perfectly.