How to create a named selection of nodes which have equivalent stress above a certain limit?

Rohith Patchigolla

I have an equivalent stress result in Mechanical. I want to create a nodal named selection which has nodes corresponding to equivalent stress above a certain value

Rohith Patchigolla

Here is a simple script (tested in 2021R2). Please try pasting this script in Mechanical Scripting Console after solving the model. This should create a new Nodal named selection with the corresponding nodes.

#Inputs
#Stress Limit in MPa
strLimitMPa = 10
#Use the name of the Equivalent Stress object in the tree (try to have a unique name for the result objects)
stress_Object_Name = "Equivalent Stress 1"

#Remainig Code
strLimit = strLimitMPa*1e6
eqvStr = DataModel.GetObjectsByName(stress_Object_Name)[0]
plt = eqvStr.PlotData
scopedNodes = plt["Node"]
scopedResults = plt["Values"]

# Get indices of elements in scopedResults  that are greater than certain stress value
indices = [i for i, value in enumerate(scopedResults) if value > strLimit]

# Filter scopedNodes list based on the indices
filtered_scopedNodes = [scopedNodes[i] for i in indices]

nodeSel = ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.MeshNodes)
nodeSel.Ids = filtered_scopedNodes

NsObj = DataModel.GetObjectsByType(DataModelObjectCategory.NamedSelections)
if len(NsObj) == 0:
    newNodalNS = Model.AddNamedSelection()
else:
    newNodalNS = Model.NamedSelections.AddNamedSelection()
newNodalNS.Location = nodeSel
newNodalNS.Name = "NodesAboveLimit_" + str(strLimitMPa) + "_MPa_" + eqvStr.Name
Tree.Refresh()

Pernelle Marone-Hitz

Also see this post which does a similar operation, but for total deformation: https://discuss.ansys.com/discussion/2431/filter-elements-with-deformation-above-a-value-and-change-their-material-properties