Learning Forum

[mszoke]

Dear All,

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!

Thank you!

Matt

BOUNDARY CONDITIONS:

[peteroznewman]

Hello 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.n

[mszoke]

Hi 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,nMattnnn

[peteroznewman]

Hello 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.n

[mszoke]

Thank 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:nn

[peteroznewman]

Hello 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.n