Sean Harvey
Ansys Employee
nThanks for your patience. For the thickness of the ply you right mouse button on Parameters, pick Create Parameter, then in the object you pick the object of interest. Since thickness is set at the fabric object, you pick the fabric in the tree as I have done here. Then in property under object you change to thickness. You can see the bottom of the dialog box reports what is currently set, in this case .01.nnFor the ply angle, you do the same thing, but once you click in object, you scope to a modeling ply and then in the property change to ply angle.nFor the a failure criteria this is the procedure.nIn ACP Post you right mouse button on Parameter and Create Parameter and change the Category to Expression Output. Then in the script you replace the 0.0 to the right of the return value with something like.ndb.active_model.solutions ['Solution 1'].plots['Failure.1'].minmax[1] nYou can see in the image. Make sure what is inside the quotes matches the object names in the tree, so I have Solution 1, you may have Solution 2. etc.nminmax[0] grabs the min, minmax[1] grabs the max.nndb.active_model.solutions ['Solution 1'].plots['Failure.1'].minmax[1]nIf you want Von Mises Stress failure, that only works with isotropic materials as that criteria is not typically used for composites, but if you still want to work with the Von Mises Stress, you can create a user defined stress result (right mouse button on Solution to see that). Then you can add script to compute the user defined result (using the VM stress equation) and follow the above steps to retrieve that as parameter. In the ACP help search for user-defined plots and they give examples of how to work with these results.nYou can also go to engineering data and change the ply type of the material to isotropic and then it will let you use the Von Mises criteria for failure (see the Failure Definitions Object where you can set the criteria), but again, be sure this is what you want as. nHope this helps.nRegards,nSea