Learning Forum

[Cheyenne Hua]

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]

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.