Cancel
Showing results for 
Search instead for 
Did you mean: 

Exporting deformed body

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hi All,

 

Can anyone explain me how to export the deformed body once done with the solving. And I don't want to export it as .jt format since it generates only facet body as it not of any use.

I wan to export the deformed elements or cad model so that later i should be able to import it back into NX and do some other simulation on that deformed body.

If we can export only elemnts also it will help me.

 

Thanks in advance

Amit Nandi
Application Engineer, DesignTech Systems Ltd.
5 REPLIES

Re: Exporting deformed body

Siemens Phenom Siemens Phenom
Siemens Phenom
  1. With the FEM part as the displayed part, generate a post processing display of displacement results
  2. Use Identify. Select all of the nodes that you want to update coordinates
  3. Pick 'Create Field' icon on the Identify dialog
  4. Set Independent Domain to Node ID and Dependent Domain to Cartesian and pick OK to created the field in the FEM part.
  5. Open the Node Translate command
  6. Set Method to By Field
  7. Select the nodes to translate
  8. Select the field created in Step 4.

This will apply the displacement field created from results to the node locations. The result will be a "deformed" mesh.

Re: Exporting deformed body

Valued Contributor
Valued Contributor

JimB,

 

Can the Field that is created in Step 3 be used to create a static loading condition in a non-linear contact simulation? 

Re: Exporting deformed body

Siemens Phenom Siemens Phenom
Siemens Phenom

Not that field exactly (because the independent domain is Node ID), but a similar concept.

 

  1. Create the field from Identify in the SIM part with a Cartesian independent domain.
  2. Create an Enforced Displacement constraint in your solution. Specify Type as "Translational Components - Field". You can then reference the field created from Identify to create the constraints. Since the Independent domain is Cartesian, the meshes doe not have to match. The displacements from the original model will be interpolated onto the selected entities in the target model.

 

Search for breakout modeling in the Advanced Simulation online help for more information

 

https://docs.plm.automation.siemens.com/tdoc/nx/10/nx_help/#searchSmiley Tongueage=1;rpp=10;query=breakout

 

Re: Exporting deformed body

Experimenter
Experimenter

Thanks a lot Jim. This solution helped me in first attempt. Smiley Happy

Re: Exporting deformed body

Siemens Valued Contributor Siemens Valued Contributor
Siemens Valued Contributor

If you are interested to change the original CAD geometry (and not just the discretized body geometry), you might want to consider “Global Deformation”. "Global Deformation" changes the original CAD geometry based on discrete deformation results from a FEM analysis.

 

For example, you could use "Global Deformation" to adapt an "as designed" engine fan blade in its hot state to the unwound cold state when the engine is not operating. This representation of the form may be important if it is the state in which the part is manufactured or repaired.

 

You find the “Global Deformation” command in “Modeling”.

 

Martin

Global CAE Portfolio Development