Symmetric Symmetry Analysis

In this example, using the support files, you will perform a Static Structural analysis using Symmetric Symmetry and execute a sequence of python journal commands that will define and solve the analysis.

This example begins in the Mechanical application. It requires you to download the following files.

Symmetric_Symmetry.agdb
Symmetric_Symmetry.xml
Symmetric_Symmetry.py

These files are available here.

Procedure

Open Workbench and insert a Static Structural system into the Project Schematic.
Double-click the Engineering Data cell to open the workspace.
Select File > Import Engineering Data, navigate to the proper folder location and select Symmetric_Symmetry.xml.
Return to the Project tab.
Right-click the Geometry cell and select Properties.
Enable the Named Selections check box under the Basic Geometry Options category.
Right-click the Geometry cell and select Import Geometry > Browse and then navigate to the proper folder location and select Symmetric_Symmetry.agdb.
Open Mechanical: right-click the Model cell and select Edit.
Select the Automation tab and select the Scripting option to open the Mechanical Scripting pane.
Select the Open Script option ( ) from the Editor toolbar. Navigate to the proper folder location and select Symmetric_Symmetry.py.
Select the Run Script option ( ) from the Editor toolbar.

Scripts Illustrated

In this example, the python file automatically performs the following actions:

#Scenario 1: Store main Tree Object items
MODEL = Model
GEOM = MODEL.Geometry
COORDINATE_SYSTEMS = Model.CoordinateSystems
MESH = Model.Mesh

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

#Scenario 2: Set Display Unit System
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS

#Scenario 3: Insert Worksheet based Named Selections for applying Symmetric Symmetry and to setup Static Structural analysis
# Create Named Selection for applying Symmetric Symmetry
FIRSTNS = DataModel.Project.Model.AddNamedSelection()
FIRSTNS.ScopingMethod=GeometryDefineByType.Worksheet
FIRSTNS.Name = "SELECTION2"
GEN_CRT1 = FIRSTNS.GenerationCriteria
CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
CRT1.Active=True
CRT1.Action=SelectionActionType.Add
CRT1.EntityType=SelectionType.GeoFace
CRT1.Criterion=SelectionCriterionType.LocationY
CRT1.Operator=SelectionOperatorType.Equal
CRT1.Value=Quantity('0 [m]')
GEN_CRT1.Add(CRT1)
FIRSTNS.Activate()
FIRSTNS.Generate()

# Create Named Selection for applying Fixed Support
NAMED_SELCTIONS = DataModel.Project.Model.NamedSelections
FIRSTNS.Duplicate()
SECONDNS=NAMED_SELCTIONS.Children[1]
SECONDNS.Name = "SELECTION3"
GEN_CRT2 = SECONDNS.GenerationCriteria
CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
CRT1.Active=True
GEN_CRT2[0].Criterion=SelectionCriterionType.LocationX
GEN_CRT2[0].Value=Quantity('-7.5 [m]')
SECONDNS.Activate()
SECONDNS.Generate()

# Create Named Selection for applying Pressure
SECONDNS.Duplicate()
THIRDNS=NAMED_SELCTIONS.Children[2]
THIRDNS.Name = "SELECTION4"
GEN_CRT3 = THIRDNS.GenerationCriteria
CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
CRT1.Active=True
GEN_CRT3[0].Value=Quantity('7.5 [m]')
THIRDNS.Activate()
THIRDNS.Generate()

#Scenario 4: Assign proper material to body")
PART1.Activate()
PART1.Assignment="T5"

#Scenario 5: Insert Coordinate System for applying Symmetric Symmetry
COORDINATE_SYSTEM = COORDINATE_SYSTEMS.AddCoordinateSystem()
COORDINATE_SYSTEM.OriginZ = Quantity("0.1 [m]")
COORDINATE_SYSTEM.AddTransformation(TransformationType.Offset,CoordinateSystemAxisType.PositiveZAxis)
COORDINATE_SYSTEM.SetTransformationValue(1,0.4)
COORDINATE_SYSTEM.AddTransformation(TransformationType.Rotation,CoordinateSystemAxisType.PositiveXAxis)
COORDINATE_SYSTEM.SetTransformationValue(2,90)

#Scenario 6: Insert Symmetric Symmetry using local Coordinate System
SYMMETRY=MODEL.AddSymmetry()
# Insert Symmetric Symmetry using Pre-selection
SELECTION=ExtAPI.SelectionManager.AddSelection(FIRSTNS)
SELECTION2=ExtAPI.SelectionManager.CurrentSelection
SYMMETRY_REGION=SYMMETRY.AddSymmetryRegion()
SYMMETRY_REGION.Type=SymmetryRegionType.Symmetric
SYMMETRY_REGION.CoordinateSystem=COORDINATE_SYSTEM
SYMMETRY_REGION.SymmetryNormal=SymmetryNormalType.ZAxis
# Clear Selection for inserting new objects with default scoping
CLRSEL = ExtAPI.SelectionManager.ClearSelection()

#Scenario 7: Define global mesh size and generate mesh
MESH.Activate()
MESH.ElementSize = Quantity('0.5 [m]')
MESH.GenerateMesh()

#Scenario 8: Define load and boundary conditions in Static Structural analysis
# Add Fixed Support
FIX_SUPPORT = STAT_STRUC.AddFixedSupport()
FIX_SUPPORT.Location = SECONDNS

# Add Pressure
PRESSURE = STAT_STRUC.AddPressure()
PRESSURE.Location = THIRDNS
PRESSURE.AppliedBy=LoadAppliedBy.SurfaceEffect
PRESSURE.Magnitude.Output.SetDiscreteValue(0,Quantity("-100 [Pa]"))

#Scenario 9: Add results in Static Structural analysis
STAT_STRUC_SOLUTION.Activate()
TOTAL_DEFORMATION = STAT_STRUC_SOLUTION.AddTotalDeformation()
NORMAL_STRESS = STAT_STRUC_SOLUTION.AddNormalStress()

#Scenario 10: Solve and review Results
STAT_STRUC_SOLUTION.Activate()
STAT_STRUC.Solve(True)

#Total Deformation Result
TOTAL_DEF_MIN = TOTAL_DEFORMATION.Minimum.Value
TOTAL_DEF_MAX = TOTAL_DEFORMATION.Maximum.Value

#Normal Stress Result
NORMAL_STRESS_MIN = NORMAL_STRESS.Minimum.Value
NORMAL_STRESS_MAX = NORMAL_STRESS.Maximum.Value

Summary

This example demonstrates how scripting in Mechanical can be used to automate your actions.