How can I perform a parametric analysis through PyMechanical?

Options
MSensale
MSensale Member, Employee Posts: 4
Ansys Employee First Comment Solution Developer Community of Practice Member
edited November 2023 in Structures

Here is an example code to perform a parametric analysis through PyMechanical with parameters that are not parametrized by Mechanical itself.

Comments

  • MSensale
    MSensale Member, Employee Posts: 4
    Ansys Employee First Comment Solution Developer Community of Practice Member
    edited September 2023
    Options

    Here is the code :

    from ansys.mechanical.core import launch_mechanical
    from pathlib import Path
    
    ###############################################################################
    # Launch Mechanical
    # ~~~~~~~~~~~~~~~~~
    # Launch a new Mechanical session in batch, setting ``cleanup_on_exit`` to
    # ``False``. To close this Mechanical session when finished, this example
    # must call  the ``mechanical.exit()`` method.
    
    mechanical = launch_mechanical(batch=False, cleanup_on_exit=False)
    print(mechanical)
    
    ###############################################################################
    # Define parameters
    # ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
    P1 = [0.001, 0.005, 0.01, 0.05, 0.1] # Maximum Time Step
    
    P2 = [3, 2.5, 2, 1.5, 1, 0.5, 0.25]  # Face Sizing and Face Sizing 2
    
    P3 = ["Linear"] #Element order
    P4 = ["PurePenalty"] #Contact formulation
    P5 = ["NodalNormalToTarget", "NodalProjectedNormalFromContact", "NodalDualShapeFunctionProjection"] # Detection Method
    
    names = ['Max Time Step', 'Sizing', 'Order', 'Formulation', 'Detection']
    parameters = [P1,P2,P3,P4,P5]
    param = dict(zip(names, parameters))
    
    for key, value in param.items():
    
        length = (len(value))
        for j in range(0, length):
            print(value[j])
    
            ###################################################################################
            # Open the Mechanical model
            # ~~~~~~~~~~~~~~~~~~
            # Run the Mechanical script to attach the geometry and set up and solve the
            # analysis.
    
            file = r"D:\\Data\\project1\\SYS-99.mechdb"
            command = f'ExtAPI.DataModel.Project.Open("{file}")'
    
            # RUN LINES TO PERFORM PRELIMINARY OPERATIONS
            # ~~~~~~~~~~~~~~~~~~
            mechanical.run_python_script(command)
    
            command = """
    import json
    
    #Scenario 1: Store main Tree Object items
    MODEL = Model
    GEOM = MODEL.Geometry
    COORDINATE_SYSTEMS = Model.CoordinateSystems
    MESH = Model.Mesh
    NAMED_SELECTIONS = Model.NamedSelections
    CONNECTIONS = Model.Connections
    
    PARTS = GEOM.GetChildren(DataModelObjectCategory.Part,False)
    for part in PARTS:
        bodies = part.GetChildren(DataModelObjectCategory.Body, False)
        for body in bodies:
            if body.Name == "Part 1":
                PART1 = body
    
    STAT_STRUC = DataModel.Project.Model.Analyses[0]
    ANALYSIS_SETTINGS = STAT_STRUC.AnalysisSettings
    STAT_STRUC_SOLUTION = STAT_STRUC.Solution"""
            output = mechanical.run_python_script(command)
            print(output)
    
            # CHANGE THE PARAMETER
            # ~~~~~~~~~~~~~~~~~~
            if key == 'Max Time Step':
                command = """
    ANALYSIS_SETTINGS.Activate()
    ANALYSIS_SETTINGS.CurrentStepNumber=2
    ANALYSIS_SETTINGS.MaximumTimeStep=Quantity("{0:.3f} [sec]")
                """.format(value[j])
            if key == 'Sizing':
                command = """
    MESH.Children[1].ElementSize = Quantity({0:.1f}, "m")
    MESH.Children[2].ElementSize = Quantity({0:.1f}, "m")""".format(value[j])
            if key == 'Order':
                command = """
    MESH.ElementOrder = ElementOrder.{0:s}""".format(value[j])
            if key == 'Formulation':
                command = """
    CONNECTIONS.Children[0].Children[0].ContactFormulation = ContactFormulation.{0:s}
    CONNECTIONS.Children[0].Children[1].ContactFormulation = ContactFormulation.{0:s}""".format(value[j])
            if key == 'Detection':
                command = """
    CONNECTIONS.Children[0].Children[0].DetectionMethod = ContactDetectionPoint.{0:s}
    CONNECTIONS.Children[0].Children[1].DetectionMethod = ContactDetectionPoint.{0:s}""".format(value[j])
            print(command)
    
            output = mechanical.run_python_script(command)
            print(output)
    
            # UPDATE MESH AND SOLVE
            # ~~~~~~~~~~~~~~~~~~
            command = """
    # Solve Static Analysis
    MESH.GenerateMesh()
    STAT_STRUC = Model.Analyses[0]
    STAT_STRUC.Solution.Solve(True)"""
    
            output = mechanical.run_python_script(command)
            print(output)