How do I get deformed geometry

  • 1.8K Views
  • Last Post 24 May 2018
mingyao.ding@ansys.com posted this 06 March 2017

I would like to get the shape/geometry of the result of a structural simulation I ran.

Order By: Standard | Newest | Votes
peteroznewman posted this 22 October 2017

There are two approaches to get the deformed geometry out of a Static Structural solution into a CAD program: a two step process and a fifteen step process. Thanks to SimuTech group for teaching me this method.

FOR VIEWING OUTSIDE FACES ONLY

In Mechanical: Insert a total displacement for a selected body into the solution, then right click on it and export an stl file.  

In CAD:  import the stl file. Some CAD systems don't handle imported stl files very well. New versions are getting better at that. See the next approach.

 

TO CREATE A SOLID BODY (more useful in CAD programs)

Here are the steps to export a Parasolid file:

In Mechanical:

 

  1. Create a Named Selection named "top" that contains the part you want to export.
  2. Analysis Settings set to Save APDL db
    def1
     
  3. Drop a Mechanical APDL component onto the Static Structural Solution 
    def2
  4. Right click on Analysis row of Mechanical APDL system on project page and select "Add Input File" 
  5. Select attached input file upgeom.inp (this is setup to select a single part in your model).
  6. Drop an FE Modeler component onto the Mechanical APDL Analysis
  7. Update the Static structural solution, Mechanical APDL Analysis, and FE modeler. 
    If the Static structural solution was done before step 1 above, clear generated data first.

Open FE Modeler

8. Right click on "Geometry Synthesis" and select "Insert>>Initial Geometry"

9. Right click on "Initial Geometry" and select "convert to parasolid"

10. Drop a DesignModeler (Geometry) Component onto FE modeler Model cell

11. Update FE modeler and DM

Start DM (double click on Geometry field)

  1. Add a  Body Operation, "Type" set to Sew, setting the "Create Solids?" to Yes

 

If the result is not a single solid, change "Tolerance" to User Defined.

def3

13. In DM open Tools>>Options then go to:

DesignModeler>>Geometry>>Export Options>>Parasolid Export Version and select 24.0 for NX8

 


14. Export Parasolid file. 

 

15. In CAD system import Parasolid file.

peteroznewman posted this 22 October 2017

This site won't allow a file with an inp extension to be attached, so below is the contents of upgeom.inp which is attached as upgeom.txt

resume

/prep7

cmsel,s,top

esln,r

upgeom,1.0,1,last,file,rst

cdwrite,db

finish

Attached Files

peteroznewman posted this 31 October 2017

Does AIM have a method to get the deformed geometry back to SpaceClaim?

CakeOrDeath posted this 22 May 2018

Hi,

Great walkthrough! However, I seem to experience a problem when converting to a parasolid. Even though my initial geometry turns out OK, all faces, vertices, etc are detected correctly, when I convert to parasolid it doesn't detect any of the geometry correctly. I'm just trying the process out with a deformed beam so I wouldn't have thought it was too complicated to handle.

Any advice?

peteroznewman posted this 22 May 2018

Please attach your workbench archive .wpbz file and let's take a look. Also say what version of ANSYS you are using.

You would think ANSYS would build-in a useful output in a simple way, such as right mouse click > Export Deformed Geometry.

CakeOrDeath posted this 22 May 2018

Hi,

Thanks very much! Hopefully I have created the .wpbz file correctly, but if there are any issues then please let me know.

I'm using ANSYS version 17.1.

 Indeed! Clearly there is a need for people to use the deformed geometries in CAD software or for further analysis in other software packages, so you think it would an easier process.

 

Attached Files

peteroznewman posted this 23 May 2018

Hi,

By carefully following the directions, I was able to get a deformed Parasolid in the end, but I had to try twice. The first time I didn't get good surfaces so I went back and changed the Mechanical Units to mm then it worked.

Attached is an ANSYS 17.1 archive.

Attached Files

CakeOrDeath posted this 24 May 2018

Hi,

Thank you so much for all your help! I changed the units and that seemed to fix everything.

I knew it would be some setting that I didn't have quite right that was holding me back

 

 

Close