Learning Forum

[Diane]

Hello,

I am working on a 2D static structural model with non-linear hyperelastic materials and large deformations are enabled. I am applying a large negative pressure as shown below over 80 substeps.

[Ashish Khemka]

Hi Diane,nnYou can interrupt the run when you want. Also, you can create restart points and can restart the analysis when needed.nnRegards,nAshish Khemkann

[peteroznewman]

nWouldn't it be better if the solution did not fail with highly distorted elements? I see an hourglass mode has developed in the mesh. This is a well known defect. You should take measures to prevent that. One measure is to implement mixed u-P element formulation. That is turned on by using keyopt(6)=1. Have you done that?n

[Diane]

Thank you for your responses! nArrayYou're right, it would be much better if I can avoid the error. nI just added the keyopt(6)=1 command as you suggested for the bodies of my model that represent soft tissues (hyper-elastic materials). I am not very familiar with changing the element formulation. If I understood well, what I am doing is just changing the way the strain is being calculated by ANSYS? Will this impact the outputs I already obtained before adding the keyopt command? I also read that keyopt(6)=1 is usually used for SOLID272 elements but my model's elements are 2D plane strain, is that okay? nImplementing the mixed u-P element formulation prevented the solution from failing in some cases but not in others. I am still getting highly distorted elements as shown in the screenshot below. nNot that the there is a No separation contact between the 2 bodies at the boundaries of which the failed mesh element shows. nThank you again for your consistent support. Your replies are always extremely useful!nBest regards, nDiane n

[peteroznewman]

nKeyop(6)=1 is available to enable mixed u-P element formulation for 2D 4-node quad elements such as PLANE182.nhttps://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_elem/Hlp_E_PLANE182.htmln Since you said the suggestion helped, then I assume you were successful at adding this keyop. You can check in the Solution Output that this keyop is being used. Go look for those lines in the output.nMixed u-P formulation adds an extra degree of freedom to keep track of pressure separate from deformation. Without that, the pressure is calculated from the deformations, which is more difficult to converge on. The results should be similar either way.nHere is another idea, hourglass mode is a defect that is only possible with quad elements, triangle elements can't have this defect. So you could remesh all the hyperelastic bodies with an All Triangles mesh control. Try set the Global Element Order to Quadratic.n

[Diane]

nAlright, I understand now, thank you!nI looks like I wasn't successful in adding this keyop after all because I cannot find it in the Solver Output. What I did was inserted a command to the surfaces that had hyperelastic material assignment as shown below. Is this the correct way of doing it? n

[peteroznewman]

nYes, but you also have to select Geometry in the outline and set Element Control to Manual, otherwise it will override the setting you made above.n