I am starting to use the simcenter for make a study the effects it causes a forming punch in the sheet
metal, this for the purpose of analyzing the reduction of material thickness in forming.
i am using a sol601-106 for this problem,but i´ve enable the Shell THK for can measure this characteristic
in the material,but when the solver finishing, in the results, the Shell thk do not appers.
I using onlye Cquad elements for this problem and 2D elements for reducing time of calculate.
In the file .f06 appers two warnings of contact that say: contact surface compliance not used for contac
group 101 and group 102.
already tried with aument the density mesh, and change with Quad 8,but although the solution ends,
the Shell THK does not appear and in file f06 the warning appears
i leave a two images for explain better this, i hope find the solution a this problem with you all.thanks
Solved! Go to Solution.
Is your model configured as described in Remarks 1&2 of the SHELLTHK case control?
Shell thickness results are output only for large strain analysis, i.e., PARAM,LGSTRN,1. Note that large strain formulation is not available for 8-node shell elements. However, by specifying ELCV=1 in the NXSTRAT entry, 8-node shell elements will be converted to 9-node shell elements which support large strain.
Large strain shell elements require the use of an elastic-plastic material through the MATS1 entry with TYPE=PLASTIC. On the MATS1 entry, either TID must be specified to define a multilinear plastic material, or H and LIMIT1 must be specified to define a bilinear plastic material for the shell elements.
I think part of my mistake was to use LGDISP, the material I'm using is aluminum, a plastic-elastic material, just one question in the large strain analysis, can I use 4-node shell elements ?. But I will make these changes, and I think you are right, and I hope this time it works, thank you very much for your time JimB