General Mechanical

General Mechanical

Modelling of Sandwich Panel (CEINTF operation)

    • kreggy
      Subscriber

      Good day. I am relatively new in FEM modelling altogether, so I would gladly appreciate your help here.

      I am trying to model a sandwich panel, where an EPS foam is sandwiched by two concrete faces. The concrete face is supported by a steel mesh grid at its mid-thickness, where the two steel mesh are connected by diagonal steel wires embedding through the concrete and EPS. A rigid steel beam at the top of the panel is placed to maintain constant deformation at the top nodes of the panel.

    • Sheldon Imaoka
      Ansys Employee

      To reference nodes or elements that are present in Mechanical (not created by APDL), you would use Named Selections.
      Named Selections of bodies (line or solid bodies) become element components (see "CM" command), which you can select or reference in commands.
      Named Selections of vertices, edges, or surfaces become nodal components that you can also reference in commands.
      I hope this may help you get started.
      Regards Sheldon

    • kreggy
      Subscriber

      With regards to your suggestion, I am thinking of using one of the two APDL commands below, together with the CEINTF operation. Do you think that the code is correct to achieve my objective (to join their nodes such that they deform together), or is there anything I need to change?
      Also, I saw on another forum answer that I can use the Share Typology function in SpaceClaim instead to achieve this. Do you have any thoughts about this?
      I really appreciate your help in my concern. Thank you.
      CODE 1:
      /PREP7
      CMSEL,S,NS_SteelRebars,ELEM
      NSLE,S
      CMSEL,S,NS_ConcreteFace,ELEM
      CMSEL,A,NS_EPSFoam,ELEM
      NSLE,A
      CMSEL,S,NS_SteelBeam,ELEM
      CEINTF,0.1
      ALLSEL,ALL
      /SOLU
      OUTRES,ALL,ALL

      CODE 2:
      /PREP7
      CMSEL,S,NS_SteelRebars,ELEM
      CMSEL,A,NS_ConcreteFace,ELEM
      CMSEL,A,NS_EPSFoam,ELEM
      CMSEL,A,NS_SteelBeam,ELEM
      ALLSEL,BELOW,ELEM
      CEINTF,0.1
      ALLSEL,ALL
      /SOLU
      OUTRES,ALL,ALL
    • Sheldon Imaoka
      Ansys Employee

      I am not able to download your project, but looking at your APDL code, the first set of commands looks correct. You want to select nodes of one side with elements of the other side that you want to connect with constraint equations (CEINTF).
      I reread your post, and just to take a step back - why are you using CEINTF? Is it because of a YouTube video you saw? If, in that video, the elements were created by APDL, then CEINTF may be needed, but if you are creating all the geometry in SpaceClaim and Mechanical, using Contact is better. You can use a Remote Point if you want to make an entire location (such as the rigid steel beam you mentioned) act in a rigid fashion to control movement. In this way, you shouldn't need to use APDL and CEINTF to connect the parts together but just use contact instead.
      Regards Sheldon

    • kreggy
      Subscriber
      Yes, I did create the elements using SpaceClaim but I did insert an APDL command for SOLID65 (since it is an archived element). I also defined the contacts between the solid elements with the properties "No Separation" and "MPC." If this is the case, does this mean that I can opt not to use the CEINTF command? And do I also need to create a contact between the steel bars (link) and the solid elements?
      I really appreciate your help in my problem. Thank you.
    • Sheldon Imaoka
      Ansys Employee

      Please correct me if I'm wrong, but I think that your "Commands (APDL)" object is just switching the element type to SOLID65 - it's not actually generating elements (E, EN command), correct? If so, you can just use contact regions to connect parts together and not use CEINTF.
      If you want your steel bars and solid elements to interact, they should have contact defined.
      Regards Sheldon


Viewing 5 reply threads
  • You must be logged in to reply to this topic.