February 13, 2021 at 10:34 pmmszokeSubscriber
I am trying to simulate a simple pressure loading of a thin membrane (Kevlar).
After some digging (I am a newbie to Mechanical!) I found that SHELL181 element with KEYOPT(1)=1 (membrane) is what I will need.
After setting no displacement (ux=0,uy=0,uz=0) at the corner vertices of a 1m x 1m plate and applying a 1MPa pressure over the surface, I am getting 0 displacements and 0 stresses. Something is weird and I am sure I am missing something but after spending 2 days on this very simple problem, I cannot figure out what I am doing wrong?! please see my settings below.
Your help is very much appreciated!
BOUNDARY CONDITIONS:February 14, 2021 at 12:22 ampeteroznewmanSubscriberHello Matt nClick on the Displacement and reply with an image of the Details. Maybe you picked the face and not on the vertex.nUnder Analysis Settings you need to turn on Large Deflection. You should also turn on Auto Time Stepping.nWhy did you choose 1 MPa for the pressure? That is over 10 atmospheres, which is a ridiculously high value to apply to one side of a panel. If you convert that to a force on the 1m x 1m, it is 1 million Newtons or 225,000 lbf.nFebruary 14, 2021 at 1:03 ammszokeSubscriberHi ArrayThank you for the quick response!!! Thank you for your time!nPlease find the screenshots below. nAbout the pressure load. Yes, 1MPa is huge, I started with 100 Pa but that gives me the same 0 results. I also tried 1 Pa, but got the same output. nIf I turn on Large Deflection (that would be the geometrical nonlinearity & stress-stiffening effect if I understand correctly) then I get a Pivot Error message (see below).nThe Auto Time Stepping was on program controlled. I turned it to On but that didn't help. nI found a similar issue on another thread:nhttps://forum.ansys.com/discussion/24276/how-to-use-membrane-elements-in-workbenchNot sure what would be the best solution to approach this problem... It sounds so simple mechanically yet so difficult to solve numerically!nnBest,nMattnnnFebruary 14, 2021 at 1:48 ampeteroznewmanSubscriberHello Matt nTo make a problem that has no problem converging, suppress the Command object that changes the element stiffness to Membrane only. When there is no bending stiffness, that is a special case and makes the problem harder to converge.nChange the Displacement from the 4 Vertices to 4 edges.nChange the Initial Substeps to 100nChange the pressure to 1e-8 MPanSee if that solves. Once you see it solve, you can make changes one at a time to see if it continues to converge.nFebruary 15, 2021 at 1:24 ammszokeSubscriberThank you for the constructive comments! They helped tremendously!nIndeed, having the default KEYOPT(1)=0 option, the problem is solved much faster because the SHELL181 elements have bending resistance. In reality, this is not the case for my application (thin tensioned cloth loaded with uniform pressure distribution). nChanging the initial substeps and the BC helped a lot!nI added one more item under the Geometry Commands, where I pre-tensioned the membrane shells numerically - see screenshot below.nThe INISTATE command does the trick and the solution immediately starts to converge! nYou can use both stress (default) or strain preload (the latter must be set first). nI hope others will find this helpful, too!nnBest,nMattnThe actual problem I was trying to solve:nnFebruary 15, 2021 at 10:35 ampeteroznewmanSubscriberHello Matt, nGlad to hear you have it solved.nI was going to suggest INISTATE in my previous post, but I wanted to first see you get a solution.nThat is definitely what is needed to use Membrane only stiffness.nViewing 5 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.