Learning Forum

[name11]

[peteroznewman]

nCan you share the Workbench Project Archive .wbpz file? If so, put it in a .zip file and attach it to your reply.n

[name11]

I have attached the required file. Thanks.nn

[peteroznewman]

nThere 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. /forum/discussion/515/shell-element-with-orthotropic-materials-gives-very-different-results-from-experimental-data#comment-e7d844c9-0cc3-468a-b493-a82b00ea5abbnIn 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. nI didn't like the values you had for Shear Modulus.nI came up with values that were consistent with the isotropic relationship.nThe 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.nANSYS 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.nIt is possible, but very challenging, to simulate the post-buckling behavior of a structure.nWhat 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?nAttached is an ANSYS 19.0nn

[name11]

Thanks for the Help. Post buckled exact state is not needed and i think 1% strain is enough to represent plastic behaviour.nI 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.nnn

[peteroznewman]

nIn the Eigenvalue Buckling analysis, under Analysis Settings, change Include Negative Load Multiplier to No. Otherwise it is telling you the compressive buckling Load multiplier.nThe values below are from the F5 system solved in ANSYS 2020 R1nn

[name11]

Thanks for your Help Sir. Is it possible to attain such result in Ansys by keeping large deflections On?n

[peteroznewman]

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 1.0n

[name11]

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.n

[peteroznewman]

nStatic Structural can simulate post-buckling behavior in many cases. I don't know if 4% is achievable in your case.n

[name11]

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''.nI tried using pinball for contact but not getting it. I am attaching my geometry and boundary conditions.nn

[peteroznewman]

nDon't worry about this warning. You want all the elements on that face to be included.n