Deformable part in sheet metal

[BradFromPurdue]

I am trying to create a sheet metal part that is formed with an overbend which relaxes once it gets welded into an assembly. I have defined my deformable part with the bend angle of my Contour Flange as the input. When I go to deform the component (or add the component) in my assembly, it previews correctly, but I get a "Modeler error: object is not of type expected" error which causes the update to fail. Is Deformable Part just not set up to handle Sheet Metal parts, or am I doing something wrong? Any other suggestions for a work around?

NX 7.5.5.4

 

[JohnRBaker]

I had NO problems whatsoever using NX 7.5.5.4 to create a Deformable Feature containing a Sheet Metal Contour Flange and then editing it after I had added it to an Assembly.

Could you provide a sample part file with the Deformable Feature already defined? If not, could you at least provide a picture of what you're attempting, indicating which parameters you are trying to control once the Deformable Feature has been added to an assembly?


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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[CAD2015]

Yes,
Could you provide a sample part file with the Deformable Feature already defined? If not, could you at least provide a picture of what you're attempting, indicating which parameters you are trying to control once the Deformable Feature has been added to an assembly?


MZ7DYJ

 

[BradFromPurdue]

Thank you for your help, I must be doing something wrong.
[ol 1]

[li]This is the sketch for my base contour flange. The dimension I want to deform is p36, currently set to 87.5°[/li]

[li]This is the complete part. The Body in my Part Navigator is a migrated solid from an older CAD system - it is suppressed with no children, totally separate from the sheet metal.[/li]

[li]For the deformation I chose Tools/Define Deformable Part.../(default name) Next/(all features except Body) Next/[/li]

[li](p36 expression, with options of 87.5 and 90 - but I couldn't get this to work even if I left Expression Rules on None) Next[/li]

[li] (no references required) Next/(review summary) Finish[/li]

[li]When I go to my assembly, right-click the part and choose Deform.../Create. Note both of my options show up correctly. I chose 90 this time, but the same thing happens if I leave it at 87.5[/li]

[li]This is the error I get. Notice that the deformed part (on the left) is previewing with the 90° angle.[/li]

[li]When I click through all the errors, my part returns to its default (87.5°) state.[/li]
[/ol]

 

[kapmnit123]

Hi Brad,
You may consider using a sheet metal feature (cutout)to do the pockets (i assume you used Extrude to do the pockets).
Since it is not a good practice to mix Sheet metal and modeling commands so you can also try using "CONVERT TO SHEET METAL" just before making it a deformable part..This will at least make it a true sheet metal component.
Let us know if this helps.
Best Regards
Kapil Sharma

 

[CAD2015]

Brad,
Can you send the NX file?
It'll be a lot better!

MZ7DYJ

 

[BradFromPurdue]

Thanks again for the help guys!

Kapil - against my preference as well, my company has set a best-practice standard to use Extrude instead of Normal Cutout. I forget why - we're fairly new to the NX world and I think it was a matter of preference. I thought Extude was (also) a Sheet Metal command, so there was no need to convert to sheet metal. Besides, isn't Deform a Modeling command anyway? I went ahead and Converted to Sheet Metal and redid my deformation - still got the same error.

MZ - I've never exported a .PRT from Team Center. Please see my attachment - hope it works!

 

[JohnRBaker]

OK, I don't know exactly what is causing the problem but I suspect that it has something to do with the fact that this part appears to have started out in life as an I-deas part which was migrated to NX (the hints are in the text of the error message).

So I first deleted the dumb body (which I assume was from I-deas). Still didn't work. Then I removed the holes. Still no joy. So I tried running Part Cleanup a couple of times and I finally managed to get past the big error message but then I hit a 'Memory Access Violation'. I then tried repeating this in NX 8.5 with the modified and cleaned-up part and while the 'Memory Access Violation' error was gone I now got some errors about the features data not properly updating and the Deformed Component still failed.

So I decided to just start from scratch and create your part over again using some of what you did but using the 'Normal Cutout' instead of the Extrude/Subtract. I also performed the additional instances inside the sketch for the 'Normal Cutout' (makes for a cleaner model while retaining the ability to edit all the parameters for the cutouts). Now this model works just fine, so the problem was NOT the fact that it was a Sheet Metal model (I think we had already settled that issue earlier) but rather it appears to have been some legacy data left over from the I-deas to NX migration, however that was accomplished.

So give the attached model a try and see if this is what you were trying to accomplish. Also note how I constructed the 'holes' using the multiple loop sketch for the Normal Cutout as this is a 'better' approach to use, despite what your co-workers might think.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[BradFromPurdue]

Aha! Thanks so much John. You are exactly right - the part was migrated from I-deas, and deleting it didn't help me either. I will make a go of it from scratch - at least there was nothing wrong with my Deform steps.

For what it's worth, I prefer the sketch patterning tools as well. However, my company felt the ability of assemblies to recognize instance patterning (for fasteners, etc.) in NX 7.5 with Pattern Face trumped the cleaner model tree. You've given me some good arguments to bring up - thanks again!

 

[SDETERS]

With all of this being said was there a IR reported to GTAC about this issue?

 

[JohnRBaker]

Note that starting with NX 8.0 we introduced a new 'instancing' tool for features, 'Pattern Feature', which replaces completely the old feature array tools (but the Pattern Face functionality is unchanged, at least for now). The only limitation of the NX 8.0 implementation was that this functionality was not available when working with Sheet Metal features such as 'Normal Cutouts'. However, that limitation has been removed with the release of NX 8.5 so if I had remodeled your part with the current release of NX I would have still used the 'Normal Cutout' but I would have used the new 'Pattern Feature' function to create the additional 'holes'. And the good news is that these new 'Pattern Features' are recognized by Assembly modeling when creating Component Arrays (for fasteners, etc.).

And since you've mentioned that you like the NX 7.5 sketch patterning tools, well this was our first effort at using a new 'patterning service' which will be the architectural basis for all future 'patterning' requirements in NX. The first of these new 'pattern' implementations was the NX 8.0 Pattern Feature functionality. Therefore it should look very familiar to you when you do upgrade to the latest version of NX.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.