Skip to main content
M
mlindqvist1-Visitor
1-Visitor
September 7, 2015
Solved

Split surface in Creo for analysis in Ansys?

  • September 7, 2015
  • 6 replies
  • 11168 views

I'm a novice in Ansys and I'm trying to split a surface to apply a load on a portion of that surface. How do I do this in Creo?

Best answer by 346gnu

Mat's

I found  (by accident) that if I enter Ansys whilst in Simulate then the selectable surfaces equivalent to the surface regions appear in Ansys.

6 replies

J
JonathanHodgson13-Aquamarine
13-Aquamarine
September 7, 2015

As far as I'm aware, there's no way to do this 'properly' in the main Creo modeller.  Presumably if you create a surface region within Mechanica (sorry, Simulate) and then mesh it in Simulate to export to Ansys, that will do what you need.

Otherwise, one suggestion I've heard is to create a very small step in the surface to force an edge (you can probably then delete the tiny vertical elements within Ansys and 'merge' the two resulting free edges).

Another technique, depending on the geometry might be convert your model to surfaces and delete either the surface for load attachment, or the surrounding surfaces, and then re-create the missing surface in Ansys (or you could cut/delete surfaces twice and export two sets of surfaces) - but I'm just brainstorming now!

M
mlindqvist1-VisitorAuthor
1-Visitor
September 7, 2015

I just succeeded with a variant of your last suggestion. I have played around with a lot of alternatives, unfortunately I can't remember the exact steps but it went something like this. Open the model in FEM mode. Being in FEM mode, with your surface regions completed, click "Save as" and choose iges as the file type. This is now imported to ansys with the proper split of surfaces... 

    J
    JonathanHodgson13-Aquamarine
    13-Aquamarine
    September 7, 2015

    Nice - that's worth remembering!  Export the IGES (or possibly STEP) from a Mechanica session...

    M
    MauroStefanovic1-Visitor
    1-Visitor
    September 7, 2015

    Cattura.PNG

    Another way is exporting solid model with surfaces patches where you need to load or costraint and use command FACESPLIT in Workbench.

      3
      346gnu13-AquamarineAnswer
      13-Aquamarine
      December 16, 2015

      Mat's

      I found  (by accident) that if I enter Ansys whilst in Simulate then the selectable surfaces equivalent to the surface regions appear in Ansys.

      R
      ronbak1-Visitor
      1-Visitor
      January 11, 2016

      you create a slicing sketch on a plane in designmodeler. usually a large rectangle , create surface from sketch.  Freeze both surfaces.  Slice using surface. Use the plane you created as the tool.  You will now what 3 bodies.  Suppress the cutting plane.  You will have to bond edges in Structural.  I just learned the hard way.  Completely different methodology that Creo.slice.PNG

      3
      346gnu13-Aquamarine
      13-Aquamarine
      January 11, 2016

      That assumes one has a Design Modeller license

      Regards

      M
      mlindqvist1-VisitorAuthor
      1-Visitor
      January 11, 2016

      Yes. I was hoping I could do this with Creo+ANSYS only. We have access to Spaceclaim, but I don't want yet another software to learn.

      R
      ronbak1-Visitor
      1-Visitor
      January 11, 2016

      Ok then. taking my example.  Create two parts.  Top and bottom in creo. assembly them.  bring into ANSYS as surface bodies. bond the edges in structural.  be careful when picking target and contact edges.

      M
      MauroStefanovic1-Visitor
      1-Visitor
      January 11, 2016

      If you have design modeler license, for me simplest way is extrude a sketch with option imprint faces. So this command creates Patches.Cattura.PNG

        M
        mlindqvist1-VisitorAuthor
        1-Visitor
        January 12, 2016

        Nice! I actually helped a company here in Sweden with some training and modeling techniques for exactly this kind of product! But that was all in Creo Simulate so then this was not an issue.

        R
        rsingaram1-Visitor
        1-Visitor
        April 28, 2017

        Hi

        I just came across the same question and got the following procedure worked (that the customer do not have Ansys-Design Modeler  - Direct from Creo).

        So this can be another method to solve this.

        Basically you need to think in terms of surfaces to split and so have to export as iges format first.

        Re-import into Creo back (make sure the options "Solidify" as "off" during import options).

        Insert a profile (corresponding to the area that you want to apply inside Ansys force/pressure later) before imported feature. i.e this feature is before the imported feature in the features tree list. Then it can be accessed by imported feature after this. This profile has to be on the surface going to be split later. So can be directly sketched if the surface is flat or projected if surface is not flat.

        Select the surface (that is to be split) and trim this using the above profile. Use trim surface feature. Make sure select 3rd option of split that keeps both faces.

          Now export as iges file and Ansys should be happy now.


        - Singaram Ravi

        Terms & ConditionsAccessibility statement