General Mechanical

General Mechanical

Element choice for incompressible material

    • shubham14
      Subscriber

      I am trying to change the mesh option to introduce hybrid element in my mesh for large deformation, but i am not getting any such options in ansys. Can anyone help me how and from where to put hybrid element in mesh if it is available in ansys.


       


      Thanks 


      Shubham 

    • peteroznewman
      Subscriber

      Hybrid meshing is for fluid flow CFD models. It doesn't apply to Structural Mechanics models.


       

    • shubham14
      Subscriber

      Hi Peter,


      Thanks for your response, i want to add hybrid element in my mesh, not Hybrid meshing. 


      Regards,


      Shubham

    • peteroznewman
      Subscriber

      What do you mean by hybrid element? 
      What two things are mixed together in this hybrid element? 
      Do you mean an element that can compute stress and fluid pressure and temperature all at once? 

    • shubham14
      Subscriber

      Hi Peter,


      can i do this thing in ansys workbench and from where i will get the option for Hybrid elements.


       


    • peteroznewman
      Subscriber

      I doubt the text above was from ANSYS, since they don't use the term hybrid for elements that have a hydrostatic pressure DOF. Here is an excerpt from the ANSYS Help for the element that works with incompressible materials.


      SOLID285 Element Description


      SOLID285 element is a low-order 3-D, 4-node mixed u-P element. The element has a linear displacement and hydrostatic pressure behavior. The element is suitable for modeling irregular meshes (such as those generated by various CAD/CAM systems) and general materials (including incompressible materials).


      The element is defined by four nodes having four degrees of freedom at each node: three translations in the nodal x, y, and z directions, and one hydrostatic pressure (HDSP)

    • shubham14
      Subscriber

      Hi Peter,


      Thanks a lot


      This is really gonna helpful for me, can you please guide me how will I get this option in Ansys workbench mesh setting to change element type that will be suitable for incompressible material.

    • peteroznewman
      Subscriber

      First note that SOLID285 is a linear element, therefore you need a linear mesh. Click on Mesh in the outline and in the details window, set Element Order to Linear.


      Second, note that SOLID285 is a Tetrahedral element, therefore you need a tetrahedral mesh. Click on Mesh and insert a Mesh Control on the body and use the Method Tetrahedrons. You can use Patch Conforming or Patch Independent.


      Expand the Geometry branch in the outline and click on the first Solid body in the list, then click on Insert Commands button to insert a command object below that body. In the Command editing window, type the following command:


           ET,matid,SOLID285


      Note that if you have a multibody part, you have to put this command object under each body individually. But that is as simple as a drag and drop.


      Under Analysis Settings, change Large Deflection to On.


      In Engineering Data, create a Hyperelastic material model, or use Neoprene Rubber for a quick try out.


      Apply supports and loads and Solve. All the regular methods of obtaining convergence apply.


      After the solver finishes, you can search Solution Output for the word SOLID285 to confirm that you are using this element.


         *** ELEMENT RESULT CALCULATION TIMES
           TYPE    NUMBER   ENAME      TOTAL CP  AVE CP

              1       175  SOLID285      0.000   0.000000

      Please edit the Title of this discussion to Element choice for incompressible material since Hybrid is not a word that applies in ANSYS.


      Regards,
      Peter


      ANSYS 19.2 archive is attached.


      If this answers your question, please click Is Solution below this post to close the discussion, or ask a follow-up question.

    • shubham14
      Subscriber

      Hello Peter, 


      Thank you so much for guidance, my model is 2D so which type of element i can apply for incompressible material because for 2d case i am getting triangular and quadrilateral mesh. 

    • peteroznewman
      Subscriber

      PLANE182 for linear elements or PLANE183 for quadratic elements support Hyperelasticity material models. I think these are default elements without using a Command object.


       

Viewing 9 reply threads
  • You must be logged in to reply to this topic.