deformed parts moving in an assembly 4

[sam5a1]

OK, here's something I haven't seen before. I hope someone can tell me why this is happening so I can fix it.
I have a deformable part that is used in 4 places in the same assembly. The parts were made deformed in the assembly after they were all added and constrained. I also tried making the parts deformable before adding to the assembly then deforming them when they were added. Every combination end in the same results. When they are deformed, they move to the original location they came into the assembly at. They override all the dimensions and new dimensions don't have any effect on them. This includes using the Fix and Bond constraints. I have included a picture of the assembly using only the parts. One is before the deform, and all had fixed constraints, and the other is after the deform. As you can see, they have moved and there is no way to make them move to a different location after they are deformed. Any ideas what is causing this?

 

[sam5a1]

Sorry, hit the send button too soon

NX 7.5.4.3
Teamcenter 8.3.2
Dell T3600 Precision

 

[JohnRBaker]

We'll need more than a picture to see what might be happening.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[sam5a1]

what do you want? just the parts or the entire assembly?

 

[JohnRBaker]

If everything zipped-up is not too large, then yes, everything that's relevant.

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.

 

[sam5a1]

Here's the 2 assemblies, one before deforming the part and one after deforming the part.

 

[JohnRBaker]

OK, here are my parts. I suspect that the problem was the Sheet Metal feature. I created my model using normal solid modeling and it seems to work fine.

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.

 

[sam5a1]

After using yours and doing modifications and alterations to try to zero in on the issue, it appears that the sheet metal is the culprit. So far it appears that the contour flange function and re-bend make the most trouble. Another oddity with the contour flange is that is you deform the part before adding it to the assembly, the parts stay where they are placed.

Since I need the flat pattern for this part, I may have to get creative and WAVE link a body into the modeling space of the drawing,convert that to sheet metal and get the flat pattern from there. This is going to take some tinkering and testing to overcome this flaw. Does this behavior still exist in versions 8.5 or 9?

Thanks for your time and effort John,



Scott

 

[JohnRBaker]

Just opening your 'Before Deformation' assembly in NX 9.0 and then deforming them does NOT seem to have improved the behavior any.

However, to really be definitive, I would have to start from scratch creating new NX 9.0 parts using the Sheetmetal Contour Flange function, particularly if the problem was with the SheetMetal features to start with.

Your best bet might be to contact GTAC and have them provide the parts to development where they can determine what is exactly happening and they will be in a better position to know if something has been done or not, and if not, then we now have something that development can work with to fix the problem in a future release 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.

 

[sam5a1]

I agree completely and have started down that path. It just seems that this behavior is something that GTAC would want to know about.

 

[Millimeter]

Hi sam5a1.
And yes, Deformable Parts show odd behavior in NX 8.5
We don't use the sheet metal application, however many times perfectly restrained already deformed parts, suddenly jumps in space when we tried to change the value of deformation.
As a workaround we switched to Reference Sets.

 

[Millimeter]

By the way, in our case we can't contact GTAC at will, because we are only allowed to "upset" the management when the nature of the problem is critical or unsolvable.

 

[SvenBom]

Deformable part in NX8.5 had one critical problem. Deformable parts, created in NX7.5 or older were suddenly unusable in NX8.5. When placed in the assembly, you could not change the deformation. You could change deformation parameters, if you open just this part. But when placed in the assebmly, it didn't work.
But this problem was fixed in NX8.5.3 with mp03.

 

[sam5a1]

Thanks Millimeter and SvenBom for your input. Knowing the problem that NX8.5 had with NX7.5 deform parts and the mp03 fix is great. We're looking at going to 8.5 or 9 and having this knowledge before hand is very valuable.
Millimeter, I was debating if alt reps would be better to "simulate" the deform parts. Alt reps make it easy to pick predefined sizes but have extra baggage. Have to look into ref sets further.
Sorry to hear you can't contact GTAC when needed. If your management could only understand that one or 2 emails (> 5 minutes of your time) or 1 phone call (> 10 minutes) could save hours+ of your time trying to find a workaround. I hope they let you use the knowledge base GTAC has. It has a vast amount of knowledge stored there.

 

[JohnRBaker]

OK, I found a way to "have your cake and eat it too".

What I did was I took my Deformed part and after creating the Deform Feature I converted it to a Sheet Metal model, which can now be flattened and/or Flat Pattern drawings created from it. I've attached a new set of part files with these changes. Note that the Deform part has both the formed model for placement into your Assembly and a Flat-Solid which can be used to manufacture the blanks for what I assume to be something like a 'leaf' spring. And when you open the assembly they can still be deformed as desired without any unexpected behavior.

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.

 

[sam5a1]

Thanks John, that would seem to be the best, cleanest work around to the problem. I was a bit surprised that it let you convert it to sheetmetal after the deform. I guess that isn't considered as adding a feature.
I filled an IR yesterday with GTAC. The behavior was show to be the same in versions 7.5, 8 8.5 and 9 so it was converted to a PR, status 2.

 

[NutAce]

Hi John, Sam...

We noticed the same behavior (Deformable parts moving to their inserted position after deforming in Assembly)
In our case the issue was that we used (in the deformable part) an ABS CSYS instead of a Dynamic CSYS as a reference.

I know this happened in NX7.5. I haven't checked in NX8.5 though.


Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.3 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5
HP EliteBook 8570W Intel(R) Core(TM) I7-3740QM CPU @ 2.70GHz, 16Gb Win7 64B

 

[sam5a1]

Thanks Ronald, that is not something I had thought about. I shall look in to it.


Scott

 

[sam5a1]

After submitting to GTAC and digging into what was causing this behavior, it turned out that Ronald was 100% correct about the ABS CSYS except that we created our parts with the first CSYS as an ABS CSYS. After changing this to Dynamic CSYS, the deformed parts moved back to the position they were constrained to. A very easy work around.

This behavior was noted by GTAC to occur in all versions: 7.5, 8, 8.5 and 9. The other thing they found was that, while this occurred sporadically with non-sheet metal parts, it almost always occurred with sheet metal parts.

Just wanted to let everyone know what the resolution was.

 

[Millimeter]

Thank you so much sam5a1 and Ronald for the info.