Learning Forum

[A_Sarafraz]

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?

[1shan]

nCould you try turning the Large deflection option (under solver controls) to ON and check if the error persists. Also check out this discussion /forum/discussion/7042/connection-between-shell-element-and-link-element. You could also try using a plane strain formulation in workbench. Please follow this discussion /forum/discussion/21217/2d-element-type-in-workbench.nRegards,nIshann

[A_Sarafraz]

Hell nThanks for the answer. The large deformations are on. The error is still there. I intend to do it by membrane elements and not a 2D plane strain formulation. It shows the following error:nI used XZ-plane for drawing my circular membrane; thus, Y-direction is the transverse displacement direction. I checked node 599, and it is in the middle of the domain and not on the boundary. Do you have any suggestions?nAs my thickness is shallow, I expect no difference between shell and membrane analysis, but I want to see it in my results.n

[Erik Kostson]

See if this discussion helps :nnSee if this discussion helps :nnn

[A_Sarafraz]

Many Thanks nHowever, no, it did not help.n

[1shan]

nShell 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.nFor additional documentation regarding shell181 refer the help documentation SHELL181 (ansys.com)nnRegards,nIshan.n

[A_Sarafraz]

You are right. Having a slightly curved initial configuration solved the pivot error problem. However, then I have a diveverged solution problem. To be honest, I meanwhile used Comsol and solved my problem by checking the difference between membrane analysis and shell analysis and both of them were the same as Ansys shell analysis. Thus, I just stopped simulating membrane using Ansys workbench.nBests,nAlin

[Erik Kostson]

It can be very difficult to get membrane elements to converge, so what we do is:n2 step solutionnfirst 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)nsecond, apply the external out of plane loads.nnAll the bestnnErikn

[A_Sarafraz]

Dear nIt solved the problem. Although I have solved my own problem using Comsol, it is really nice to learn Ansys. I am now eager to learn APDL as well and its commands.nBest regards,nAlin

[Erik Kostson]

That is great to hear .nnAll the bestnnErikn