How do I get deformed geometry

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

«1

Comments

  • peteroznewmanpeteroznewman Member
    edited 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.

  • peteroznewmanpeteroznewman Member
    edited 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

  • peteroznewmanpeteroznewman Member
    edited October 2017

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

  • CakeOrDeathCakeOrDeath Member
    edited 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?

  • peteroznewmanpeteroznewman Member
    edited 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.

  • CakeOrDeathCakeOrDeath Member
    edited 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.

     

  • peteroznewmanpeteroznewman Member
    edited 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.

  • CakeOrDeathCakeOrDeath Member
    edited 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

     

     

  • earvinlloydearvinlloyd Member
    edited January 2019

    Hi,

    Now that FE-modeler is phased out (in 19.1 and newer), what is the substituting procedure (besides exporting to .stl)?

  • RobRob UKForum Coordinator
    edited January 2019

    It's been relabelled as "External Model", so try that. 

  • lordofthethingslordofthethings The ShireMember
    edited April 2019

    Both External Model and Mechanical Model are not attaching with Mechanical APDL.

  • NRafaelNRafael PortugalMember
    edited May 2019

    Hello,

    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?

     

  • peteroznewmanpeteroznewman Member
    edited June 2019

    This post has the text for the input file. Just rename it with a .inp file extension.

  • lincs2k9lincs2k9 Member
    edited October 2019

    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? 

  • mehdimechanicmehdimechanic Member
    edited October 2019

    Can this single part in step 5 be an assembled part? some parts together? then how should the input be modified? 

  • lordofthethingslordofthethings The ShireMember
    edited November 2019

    For newer versions of Ansys that do not have a "Finite Element Modeler"

    1. Run the simulation to get deformed geometry :

    2. Connect the solution part of the static structural to a new instance of "Mechanical Model", update the tolerance if necessary, and check the following options in the properties of the Mechanical Model. Update both the systems.

     

    3. Finally, bring a new instance of the "Geometry" system and connect the model to it. 

    4. Open the Geometry module in DM (Not Spaceclaim), generate it, and then File --> Export --> (STEP format). Wait until the conversion is over. Now you have the solid model ready!

     

  • RobRob UKForum Coordinator
    edited November 2019

    Have you also linked Engineering Data? 

    Edit: don't need that, and it works fine here. 

  • lordofthethingslordofthethings The ShireMember
    edited November 2019

    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.

  • rajansanandrajansanand Member
    edited November 2019
    But...how to provide a fixed amount of imperfection (my model has to be given a fixed amount of imperfection by multiplying a value to the deflected shape i got in eigen value buckling analysis)
  • peteroznewmanpeteroznewman Member
    edited November 2019

    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.

Sign In or Register to comment.