General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Pre-Integrated shell in Ansys-LS-Dyna

    • Rico Hubert
      Subscriber

      Hello,

       

      I want to perform an explicit forming simulation with an orthotropic continuum shell. Due to specific bending characteristics derived from measurement I would like to input section paramters within a pre-integrated shell model. However, I did not find any possibility to define a pre-integrated shell element via LS-Dyna keywords. I found the solutions for static structural in the workbench using an APDL-Code, but I require an explicit solver. As far as I know, orthotropic material models are not included in explicit dynamics, as far as I can see.

      Is there a way to implement a pre-integrated shell model in either LS-Dyna or explicit Dynamics?

      Kind regards

    • Andreas Koutras
      Ansys Employee

      Hello Rico,

      Please see if the following helps. Thanks.

      Mat_117 is a resultant shell formulation and no stresses are computed. As
      per the materials manual's note:
      
      1. This material does not support specification of a material angle for each 
      through-thickness integration point of a shell.
      
      2. The objective of this resultant formulation is to provide a fast and cheap
      approximation for the composite material behavior without having to to
      integrate thru' the many layers of material layers. Therefore, ALL the
      resultant formulated materials 116, 117, 118, 130, 139, 166, 170 are default to
      1 thru' thickness integration point.
      • Rico Hubert
        Subscriber

        Hello,

        thank you very much for your reply. Sorry to answer this late. The described material model is exactly what I need, however, I am not sure if it is supported by ANSYS-LS-DYNA. The *MAT choices in the engineering data section do not list it and the user manual does not name it as well. Is it however possible to implement it with a keyword snippet directly in mechanical? If so, is there an example on the code structure to correctly implement stiffness-matrix values?

        Thanks again!

        Greetings

    • Andreas Koutras
      Ansys Employee

      Hello Rico,

      You can use Ansys Composite PrepPost (ACP) to calculate the stiffness matrix of the laminate. ACP is included with a Mechanical Enterprise license.

      https://forum.ansys.com/forums/reply/278708/

      • Rico Hubert
        Subscriber

        Hello,

        thanks again for replying. I know about ACP, however, I want to simulate fabric draping with a fabric that has a rather high bending stiffness. Since the material is dry and not homogenous, I want to include bending properties that are independant of the membrane stiffness, which is commonly done by using a pre-integrated shell, as far as I've read. I can input all stiffness values manually, as I gained the values from experiment. I would know how to CODE a preintegrated shell *GENS within Structural, however, they are not included in Explicit Dynamics, meaning I need the LS-DYNA extension which however works on LS-DYNA Keywords. Basically all I would need is the MAT_117 but I am not sure if this is included in LS-DYNA within the ANSYS workbench.
        Thanks again!
        Greetings

    • Erik Kostson
      Ansys Employee

       

       

       

      Hi

      You said:

      ”Basically all I would need is the MAT_117 but I am not sure if this is included in LS-DYNA within the ANSYS workbench.”

       

      This material is or at least should be included in the LS-Dyna system in Workbench (I do not see why it should not) – you just need to define a Keyword Snippet (LS-DYNA) under the relevant part in geometry tree (in the keyword snippet one needs to define the MAT117 material card (C11,etc….)).

      See here for an example on a Keyword Snippet (LS-DYNA) MAT definition:
      https://forum.ansys.com/forums/topic/import-ls-dyna-mat24-material-card-in-ansys-workbench-and-switch-on-non-linear-properties/

      All the best

      Erik

       

       

       

Viewing 3 reply threads
  • You must be logged in to reply to this topic.