Unable to deform

[stephlouv]

Dear All,

I have a problem using deformable part.

I'am designing an arrow, cut in a sheetmetal, used to indicate the flow direction on our product.
Most of the time it is screwed on cylindrical face.

In my part they are two solid.
A flat one, for drawing purpose.
And a curved one, made by wrapping contour curved on a cylindrical sheet, a divide face, and a thicken sheet on it.
These two bodies are sharing the "Thickness" expression (self explanatory)
And the curved one, need the user input the wrapping diameter value.

When i'am creating the deformable, i'am selecting all features, select the two expressions. Done.

When i'am trying to deform, I get this :
"Unable to deform as one or more member feature have failed during update".

And info windows show me this :
============================================================
Information listing created by : a4847
Date : 1/04/2014 09:13:54
Current work part : 00-5125-0181-0000-00/1
Node name : niv-w7-ddsjb25j
============================================================

************************************************************

Update Warning and Failure Report

************************************************************

------------------------------------------------------------
00-5125-0181-0000-00/1
------------------------------------------------------------
Thicken(19) Error: No face selected.

What I dont understand is if i'am changing the same parameters in the model, everything is fine.
Any idea ?

Thank you

Stéphane

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

We would actually need to see the part and the part where it's used before we could make any suggestions.

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.

 

[stephlouv]

I'am under NX 8.0.3.4

Here is the part file.
I spoke about sheet metal, but the part doesn't use any NX sheet metal feature.

Add it in any asm, try to deform, the problem occur.

http://files.engineering.com/getfil...2c2-9480-d02448f09b63&file=00_1196_0002_A.prt

Thank you

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

This appears to be beyond the scope of what Deformable Parts was designed to do.

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.

 

[SvenBom]

Did it work in previous releases of NX?
I've had a similar problem with NX Sheet Metal model. First, I have modeled a simple NX Sheet Metal part. Then, I have divided this one body into 3 bodies using Extrude/Subtract command. After that, I have defined a deformable part. The deformation worked in actual part. But, if this part was placed into assembly, it didn't work. I received exactly the same error as you are getting.

This procedure worked in NX7.5 (don't remember wich qrm). But it didn't worked in NX8.5 (don't now about NX8). So, the problem was reported to GTAC.
Two days ago, the third maintenance pack for NX8.5.3 was released. And now, it works again. So it was a problem with NX version.

Maybe you have the same problem with NX8. Maybe, your part was perfect in NX7.5, but something has changed with NX8. And therefore, deformable part doesn't work anymore. Well, this is just my guessing, since I don't have NX8 installed.

To better understand, how my model was created, I have attached the test model. It is created in NX8.5.3 mp03. This kind of model didn't work in any other version of NX8.5. I have also attached the image of the part, so that you can at least see the part, if you can not open it.

 

[JohnRBaker]

No, what the OP is trying to do is not possible using the Deformable Part. You can create the Deformable Part feature OK in the Master Part file, but when you attempt to place in an Assembly there is no way that you can link it the proper geometry based on the functions being performed, such as Wrap Curve, Trim Face and Thicken Sheet.

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.

 

[SvenBom]

I have just created a new assembly with the part from stephlouv. And it works. I have changed the thickness from 0.0625 to 0,02. And the wrapping diameter was changed from 180/25.4 to 1. And the part has deformed in the assembly according to those two parameters.
I did this in NX8.5.3mp03.

 

[stephlouv]

Never give up !
Never surrender !

Check this one.
Even if it's more "complex" than my first design, 14 features instead of 9 !
It's working as deformable.

Ha ! Je me marre !

"My english is bad ? That's why i'am french."

 

[stephlouv]

I tested the first design on a NX9.0.0.19
It is working.

Looks if the problem coming from NX8.0.3.4

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

OK, I guess I made an assumption about the idea that the 'arrow' was supposed to conform to a model already in the assembly. I was looking too hard at making it more elegant than it was intended to be. My bad

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.