I would like to get the shape/geometry of the result of a structural simulation I ran.
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:
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)
If the result is not a single solid, change "Tolerance" to User Defined.
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.
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
Does AIM have a method to get the deformed geometry back to SpaceClaim?
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.
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.
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.
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.
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
Now that FE-modeler is phased out (in 19.1 and newer), what is the substituting procedure (besides exporting to .stl)?
It's been relabelled as "External Model", so try that.
Both External Model and Mechanical Model are not attaching with Mechanical APDL.
I've been trying the procedure to obtain the solid model. But I am not understanding the step 5. Where I am supposed to get that input file?
This post has the text for the input file. Just rename it with a .inp file extension.
As "FE modeller" is not available in Ansys latest version, this thread's procedure is not applicable for latest version ansys workbench. "External Model and Mechanical Model" are not working according to this procedure. Can you provide instruction using latest version? Is it possible?
Can this single part in step 5 be an assembled part? some parts together? then how should the input be modified?
Have you also linked Engineering Data?
Edit: don't need that, and it works fine here.
Instead of dragging the mechanical model on top of the static structural, drag and drop it first as a stand-alone module BESIDE static structural (dont link it yet) Once you are done, take the solution cell from the static structural and join it with the mechanical model's Model. This should then work.
rajansanand, this discussion is about how to convert a deformed mesh into geometry.You are asking a different question, how to deform a mesh to use as the imperfection for a buckling analysis.Please open a New Discussion for this question, or do a search on the site to look for an answer.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.