How to use membrane elements in Workbench

A_SarafrazA_Sarafraz Member Posts: 1

Dear all,

I am a naive user, trying to model a circular pre-strained membrane using Ansys Workbench. I could model the circular membrane using a surface body, then using the static structural and modal analysis to find the effects of external pressure on the fundamental frequency. Everything is fine, but I found that the workbench uses shell181 elements, which, by default, incorporates bending stiffness in the analysis. I want to remove the effects of bending stiffness.

I searched for that, and I found that I can add commands to the model as

ET,matid,181

KEYOPT,matid,1,1

However, then running the model leads to a solver pivot error.

When I also tried to use other shell elements other than the default shell181, like shell41 as

ET,matid,41

it ends in the same error. What should I do?


Best Answers

  • 1shan1shan Posts: 262Ansys Employee
    Accepted Answer

    Hello @A_Sarafraz

    Shell 181 with KEYOPT(1) = 1 has no bending stiffness, a condition that can result in solver and convergence problems. For example if your circular membrane is along xz and the pressure is along the y direction, you would have a moment at the first iteration but no reaction forces (since the element are laid out in the normal plane) and no bending moments (since bending stiffness is zero). This results in a pivot error. You could try adding 2 load steps (under analysis settings), the first one with an in-plain force. Then the second one with the actual pressure and the in-plain force reduced to zero. Also try using a curved membrane (this worked for me) instead of the flat membrane.

    For additional documentation regarding shell181 refer the help documentation SHELL181 (ansys.com)


    Regards,

    Ishan.

  • ekostsonekostson Posts: 219Ansys Employee
    edited February 10 Accepted Answer

    It can be very difficult to get membrane elements to converge, so what we do is:

    2 step solution

    first step apply some initial pre-strain/stress , to build up out of plane stiffness in the membrane (see the post I mentioned above - so using inistate command)

    second, apply the external out of plane loads.


    All the best


    Erik

Answers

Sign In or Register to comment.