General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Extract joint probes with scripting API

    • Cheyenne Hua
      Subscriber

      I have a model with some joints (bushings to ground). I have several analyses in this model, in each analysis I have some joint probes that are telling me the joint force.  I want to print the joint forces to a text file using scripting.  First I was trying to just print the joint forces to the shell.  I found this example to base my code on: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/act_script/act_script_examples_evaluate_spring_reaction_forces.html 

      EXAMPLE: 

      # Get access to solver data
      analysis = Model.Analyses[0]
      solver_data = analysis.Solution.SolverData
      
      # Get access to result reader
      with analysis.GetResultsData() as reader:
          spring_results = reader.GetResult("SPRING")
          # Get a list of all springs
          springs = Model.Connections.GetChildren(DataModelObjectCategory.Spring, False)
      
          for spring in springs:
              print(spring.Name)
      
              spring_data = solver_data.GetObjectData(spring)
              element_id = spring_data.ElementId
      
              fForce = spring_results.GetElementValues(element_id)
              print(fForce[0])

      But it's for springs.  Trying to change it to work for bushing joints, I don't know what to put here: reader.GetResult("SPRING")  I tried "reader.GetResult("JOINT") but that does not compile.  It does run if I keep it as "SPRING" but the results are nonsense.  Please help! I could not find any documentation on the GetResult function.

      Here is my code so far:

      # Get access to solver data
      analysis = Model.Analyses[0]
      solver_data = analysis.Solution.SolverData
      # Get access to result reader
      with analysis.GetResultsData() as reader:
          joint_results = reader.GetResult("SPRING")
          # Get a list of all joints
          joints = Model.Connections.GetChildren(DataModelObjectCategory.Joint, True)
          for joint in joints:
              print(joint.Name)
              joint_data = solver_data.GetObjectData(joint)
              element_id = joint_data.ElementId
              print(element_id)
              fForce = joint_results.GetElementValues(element_id)
              print(fForce[0])

      I am using 2022 R1

    • mjmiddle
      Ansys Employee

      You can show all available solution quantities using:

      reader.ResultNames

      A bushing can be chosen as MPC or bushing formulation. The MPC type produces MPC184 element and the bushing formulation produces a COMBI250 element.

      For MPC type, you'll get these solution quantities from the bushing:

      'BOLT', 'BOLTTOOL', 'BOLT_MPC184', 'CONTAREA', 'CONTDEBOND', 'CONTFNODE', 'CONTHNODE', 'CONTPNUM', 'ELEMENTAL_REAL', 'JF', 'JFL', 'JM', 'JML', 'JOINT_ACC', 'JOINT_DOMG', 'JOINT_OMG', 'JOINT_ROT', 'JOINT_U', 'JOINT_VEL', 'JR', 'JU', 'M', 'R', 'REULER'

      Use "JF" to report the joint forces on the bushing:

      jf = reader.GetResult("JF")

      You can report the component types with jf.Components which returns ['X', 'Y', 'Z'].

      When you use jf.GetElementValues(element_id), the values will be in global coordinate system. You can compare to a joint probe set to "Total Force" except this will report in the joint reference coordinate system.

Viewing 1 reply thread
  • The topic ‘Extract joint probes with scripting API’ is closed to new replies.