How can I perform a parametric analysis through PyMechanical?

MSensale

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

MSensale

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)