Convergence Problem with orthotropic material
name11
Member
I am performing a Tensile test for a thin fabric with Orthotropic properties. I turned on large deflections to get non-linear behaviour & also took around 500 initial substeps & 50 min. substeps but it doesn't converges and nodes gets distorted on the fixed end. The same i performed for Structural Steel and i got the desired result. Can anyone please help why this convergence problem is arising for orthotropic materials & how to get the convergence right?
Comments
@name11
Can you share the Workbench Project Archive .wbpz file? If so, put it in a .zip file and attach it to your reply.
I have attached the required file. Thanks.
@name11
There is a potential mistake when using an Orthotropic material with shell elements that the element coordinate system doesn't align with the Global coordinate system. See this discussion. https://forum.ansys.com/discussion/515/shell-element-with-orthotropic-materials-gives-very-different-results-from-experimental-data#comment-e7d844c9-0cc3-468a-b493-a82b00ea5abb
In your case it happens to have worked out that the element coordinate system aligned with the global coordinate system, but you can't count on that.
I didn't like the values you had for Shear Modulus.
I came up with values that were consistent with the isotropic relationship.
The sheet is 200 mm long x 50 mm wide x 1 mm thick. I see that the solution fails to converge after stretching it about 2.4 mm along the length. The reason is that the sheet will buckle, which means the structure will suddenly change its deformation from just being stretched to going sideways in some manner.
ANSYS has an Eigenvalue Buckling Analysis. If you setup the Static Analysis to pull just 1 mm, where it has no problem converging, then run the Eigenvalue Buckling analysis after that, it will calculate that the critical load factor is 2.8 or 2.8 mm since the applied load was 1 mm.
It is possible, but very challenging, to simulate the post-buckling behavior of a structure.
What is the goal of this analysis? Is 2 mm of stretch (1% strain) sufficient? Why do you need to stretch it to 5 mm? Is the post-buckled state important to see?
Attached is an ANSYS 19.0
Thanks for the Help. Post buckled exact state is not needed and i think 1% strain is enough to represent plastic behaviour.
I did the eigen value Buckling analysis, one with previous properties and the other what you suggested, but in neither of the cases i could get the critical load factor as 2.8.
@name11
In the Eigenvalue Buckling analysis, under Analysis Settings, change Include Negative Load Multiplier to No. Otherwise it is telling you the compressive buckling Load multiplier.
The values below are from the F5 system solved in ANSYS 2020 R1
Thanks for your Help Sir. Is it possible to attain such result in Ansys by keeping large deflections On?
@name11 You can perform the Static Structural analysis with Large Deflection On. The eigenvalue buckling is a linear analysis. The best way to use this is to increase or decrease the load in static structural until the Load Multiplier comes close to 1.0
I mean, is at least 4% strain achievable? As you've mentioned before it's difficult as the sheet starts to buckle after 2.8 mm and hence convergence problem.
@name11
Static Structural can simulate post-buckling behavior in many cases. I don't know if 4% is achievable in your case.
Hello Sir, I am finding this warning every time i am trying to solve ''One or more remote boundary conditions is scoped to a large number of elements which can adversly affect solver performance. Consider using the pinball setting to reduce the number of elements included in the solver''.
I tried using pinball for contact but not getting it. I am attaching my geometry and boundary conditions.
@name11
Don't worry about this warning. You want all the elements on that face to be included.