Using mechanical scripting, how can we define composite failure criteria and composite failure results (using Composite Failure Tool inside mechanical)?
Below is an example (max strain failure):
# Create a new Composite Failure Criteria object composite_failure_criteria = Model.AddCompositeFailureCriteria() # Activate the Max Strain Failure Criterion composite_failure_criteria.MaximumStrain.Active = True #composite_failure_criteria.Puck.Active = True # for Puck fai. # Modify the Max Strain Failure Criterion settings composite_failure_criteria.MaximumStrain.EvaluateMaterialThreeDirectionFailure = True composite_failure_criteria.MaximumStrain.MaterialOneDirectionFailureWeightingFactor = 1.5 composite_failure_criteria.MaximumStrain.TensileLimitMaterialOneDirection = 0.01 #composite_failure_criteria.Puck.MatrixTensionFailureWeightingFactor = 1.2 # for Puck solution = Model.Analyses[0].Solution composite_failure_tool = solution.AddCompositeFailureTool() composite_failure_tool.Properties[3].InternalValue=2 composite_failure_tool.Properties[4].InternalValue=composite_failure_criteria.ObjectId composite_failure_result = composite_failure_tool.AddInverseReserveFactor()
For more info on all related methods and properties see here:
https://ansyshelp.ansys.com/public/account/secured?returnurl=/Views/Secured/corp/v251/en/act_ref/Ansys_ACT_Automation_Mechanical_Results_CompositeFailureResults.html
