How to get Young's Modulus for each element in the mesh?

Erik Kostson

How to get Young's Modulus for each element in the mesh using ACT mechanical scripting?

Erik Kostson

Below is one way of doing this:

import materials
elements = ExtAPI.DataModel.MeshDataByName('Global').Elements

for element in elements:
    current_geo_body = element.GetBody()
    current_material=current_geo_body.Material # access material class for this geo bodycurrent_geo_body=body.GetGeoBody() # get GeoData of this current body
    print(current_material.DisplayName)
    current_properties=materials.GetMaterialPropertyByName(current_material,"Elasticity") # list values for Elasticity property
    print("Element nr: " + str(element.Id) + ", Mod.: " + str(current_properties.get("Young's Modulus")[1]))

or if we have a element named selection (main_NS):

import materials

elementids = ExtAPI.DataModel.GetObjectsByName("main_NS")[0].Ids # Element named selection

mesh = ExtAPI.DataModel.AnalysisList[0].MeshData


for el in elementids:
    element=mesh.ElementById(el)
    current_geo_body = element.GetBody()
    current_material=current_geo_body.Material # access material class for this geo bodycurrent_geo_body=body.GetGeoBody() # get GeoData of this current body
    print(current_material.DisplayName)
    current_properties=materials.GetMaterialPropertyByName(current_material,"Elasticity") # list values for Elasticity property
    print("Element nr: " + str(element.Id) + ", Mod.: " + str(current_properties.get("Young's Modulus")[1]))