TAGGED: apdl-commands, mechanical, membrane, structural, workbench
February 7, 2021 at 9:25 pmA_SarafrazSubscriber
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
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
it ends in the same error. What should I do?February 8, 2021 at 6:51 am1shanAnsys EmployeenCould you try turning the Large deflection option (under solver controls) to ON and check if the error persists. Also check out this discussion https://forum.ansys.com/discussion/7042/connection-between-shell-element-and-link-element. You could also try using a plane strain formulation in workbench. Please follow this discussion https://forum.ansys.com/discussion/21217/2d-element-type-in-workbench.nRegards,nIshannFebruary 8, 2021 at 11:05 amA_SarafrazSubscriberHell 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.nFebruary 8, 2021 at 12:55 pmErik KostsonAnsys EmployeeSee if this discussion helps :nnSee if this discussion helps :nnnFebruary 8, 2021 at 3:22 pmA_SarafrazSubscriberMany Thanks nHowever, no, it did not help.nFebruary 9, 2021 at 6:14 am1shanAnsys EmployeenShell 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.nFebruary 10, 2021 at 3:18 pmA_SarafrazSubscriberYou 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,nAlinFebruary 10, 2021 at 5:05 pmErik KostsonAnsys EmployeeIt 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 bestnnEriknFebruary 11, 2021 at 8:48 amA_SarafrazSubscriberDear 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,nAlinFebruary 11, 2021 at 11:24 amErik KostsonAnsys EmployeeThat is great to hear .nnAll the bestnnEriknViewing 9 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.