Cyclic Symmetry Analysis

In this example, using the support files, you will perform a Thermal Stress analysis using Cyclic Symmetry or Pre-Meshed Cyclic Region 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 Ansys DesignModeler and python files.

Cyclic_Symmetry.agdb
Cyclic_Symmetry.py

These files are available here.

Procedure

Open Workbench and insert a Transient Thermal system into the Project Schematic.
Drag and drop an Static Structural system onto the Solution cell of the thermal analysis so that the systems are linked as shown.
Right-click the Geometry cell of the thermal system and select Properties.
Enable the Named Selections check box under the Basic Geometry Options category.
Right-click the Geometry cell of the thermal system and select Import Geometry > Browse and then navigate to the proper folder location and select Cyclic_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 Cyclic_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
NAMED_SELECTIONS = Model.NamedSelections

PARTS = GEOM.GetChildren(DataModelObjectCategory.Part,False)
for part in PARTS:
    bodies = part.GetChildren(DataModelObjectCategory.Body, False)
    for body in bodies:
        if body.Name == "Solid":
            SOLID_BODY = body
        if body.Name == "SurfaceBody":
            SHELL_BODY = body

TRANS_THERM = DataModel.Project.Model.Analyses[0]
ANALYSIS_SETTINGS1 = TRANS_THERM.AnalysisSettings
TRANS_THERM_SOLUTION = TRANS_THERM.Solution
STAT_STRUC = DataModel.Project.Model.Analyses[1]
ANALYSIS_SETTINGS2 = STAT_STRUC.AnalysisSettings
STAT_STRUC_SOLUTION = STAT_STRUC.Solution

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

#Scenario 3: Set isometric view and zoom to fit
cam = Graphics.Camera
cam.SetSpecificViewOrientation(ViewOrientationType.Iso)
cam.SetFit()

#Scenario 4: Store Named Selections for applying Symmetry and to setup Thermal Stress analysis
tot_child_NS_GRP = NAMED_SELECTIONS.Children.Count
for i in range(0, tot_child_NS_GRP, 1):
	ns = NAMED_SELECTIONS.Children[i].Name
	if(ns=='Low_Face'):
		LOW_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='High_Face'):
		HIGH_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Pressure_Face'):
		LOAD_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Fixed_Face'):
		FIXED_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Front_Face'):
		FRONT_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Back_Face'):
		BACK_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Edges1'):
		EDGES1 = NAMED_SELECTIONS.Children[i]
	if(ns=='Edges2'):
		EDGES2 = NAMED_SELECTIONS.Children[i]
	if(ns=='Edges3'):
		EDGES3 = NAMED_SELECTIONS.Children[i]
	if(ns=='Low_Edge'):
		LOW_EDGE = NAMED_SELECTIONS.Children[i]
	if(ns=='High_Edge'):
		HIGH_EDGE = NAMED_SELECTIONS.Children[i]
	if(ns=='Shell_Face'):
		SHELL_FACE = NAMED_SELECTIONS.Children[i]
	if(ns=='Solid_Body'):
		SOLID_BODY = NAMED_SELECTIONS.Children[i]
	if(ns=='Shell_Body'):
		SHELL_BODY = NAMED_SELECTIONS.Children[i]

#Scenario 5: Insert Coordinate System for applying Cyclic Symmetry
COORDINATE_SYSTEM = COORDINATE_SYSTEMS.AddCoordinateSystem()
COORDINATE_SYSTEM.OriginX = Quantity("0 [mm]")
COORDINATE_SYSTEM.OriginY = Quantity("0 [mm]")
COORDINATE_SYSTEM.OriginZ = Quantity("0 [mm]")
COORDINATE_SYSTEM.PrimaryAxis=CoordinateSystemAxisType.PositiveZAxis
COORDINATE_SYSTEM.CoordinateSystemType=CoordinateSystemTypeEnum.Cylindrical

#Scenario 6: Insert Cyclic Symmetry using local Coordinate System
SYMMETRY=MODEL.AddSymmetry()
# Insert Cyclic Symmetry scoped to Solid faces
SYMMETRY_REGION1=SYMMETRY.AddCyclicRegion()
SYMMETRY_REGION1.CoordinateSystem=COORDINATE_SYSTEM
# Select Low and High Boundary with proper Coordinate System
SYMMETRY_REGION1.LowBoundaryLocation=LOW_FACE
SYMMETRY_REGION1.HighBoundaryLocation=HIGH_FACE

#Scenario 7: Define mesh controls and generate mesh
MESH.Activate()
# Error Limits Standard Mechanical
MESH.ShapeChecking=False

FACE_MESHING = MESH.AddFaceMeshing()
FACE_MESHING.Location =  SHELL_FACE
FACE_MESHING.Suppressed=True

MESH_SIZE01 = MESH.AddSizing()
MESH_SIZE01.Location = EDGES1
MESH_SIZE01.Type = SizingType.NumberOfDivisions
MESH_SIZE01.NumberOfDivisions = 9
MESH_SIZE01.Behavior=SizingBehavior.Hard
MESH_SIZE01.Suppressed=True

MATCH_CONTROL01=MESH.AddMatchControl()
MATCH_CONTROL01.LowGeometrySelection=LOW_FACE
MATCH_CONTROL01.HighGeometrySelection=HIGH_FACE
MATCH_CONTROL01.HighCoordinateSystem=COORDINATE_SYSTEM
MATCH_CONTROL01.Suppressed=True

MATCH_CONTROL02=MESH.AddMatchControl()
MATCH_CONTROL02.LowGeometrySelection=LOW_EDGE
MATCH_CONTROL02.HighGeometrySelection=HIGH_EDGE
MATCH_CONTROL02.HighCoordinateSystem=COORDINATE_SYSTEM
MATCH_CONTROL02.Suppressed=True

MESH.GenerateMesh()

#Scenario 8: Setup Transient Thermal analysis
ANALYSIS_SETTINGS1.SetStepEndTime(1, Quantity("10 [sec]"))

TEMPERATURE01 = TRANS_THERM.AddTemperature()
TEMPERATURE01.Location = FIXED_FACE
TEMPERATURE01.Magnitude.Output.DiscreteValues=[Quantity('5[C]')]

TEMPERATURE02 = TRANS_THERM.AddTemperature()
TEMPERATURE02.Location = SHELL_FACE
TEMPERATURE02.Magnitude.Output.DiscreteValues=[Quantity('30[C]')]

#Scenario 9: Define load and boundary conditions in Thermal Stress analysis
STAT_STRUC.Activate()
TOT_CHILD_STAT_STRUC = STAT_STRUC.Children.Count
for i in range(0, TOT_CHILD_STAT_STRUC, 1):
	ns = STAT_STRUC.Children[i].Name
	if(ns=='Imported Load (A6) '):
		IMPORTED_LOAD_GRP = STAT_STRUC.Children[i]

IMPORTED_BODY_TEMP01=IMPORTED_LOAD_GRP.Children[0]
IMPORTED_BODY_TEMP01.Location=SOLID_BODY

IMPORTED_BODY_TEMP02=IMPORTED_LOAD_GRP.AddImportedBodyTemperature()
IMPORTED_BODY_TEMP02.Location=SHELL_BODY

# Add Fixed Support
FIXED_SUPPORT = STAT_STRUC.AddFixedSupport()
FIXED_SUPPORT.Location = FIXED_FACE

# Add Pressure
PRESSURE = STAT_STRUC.AddPressure()
PRESSURE.Location = LOAD_FACE
PRESSURE.AppliedBy=LoadAppliedBy.SurfaceEffect
PRESSURE.DefineBy=LoadDefineBy.Components
PRESSURE.XComponent.Output.DiscreteValues = [Quantity("2 [MPa]")]

#Scenario 10: Add results in Transient Thermal analysis
TRANS_THERM_SOLUTION.Activate()

TEMPERATURE01_RST = TRANS_THERM_SOLUTION.AddTemperature()

#Scenario 11: Add results in Thermal Stress analysis
STAT_STRUC_SOLUTION.Activate()
# Insert Deformation results
TOTAL_DEFORMATION = STAT_STRUC_SOLUTION.AddTotalDeformation()
# Insert Equivalent Stress result
EQUIVALENT_STRESS = STAT_STRUC_SOLUTION.AddEquivalentStress()

#Scenario 12: Solve and review Results using Cyclic Symmetry
TRANS_THERM_SOLUTION.Activate()
TRANS_THERM_SOLUTION.Solve(True)

#Temperature Result
TEMPERATURE_RST_MIN = TEMPERATURE01_RST.Minimum.Value
TEMPERATURE_RST_MAX = TEMPERATURE01_RST.Maximum.Value

STAT_STRUC_SOLUTION.Activate()
STAT_STRUC_SOLUTION.Solve(True)

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

#Equivalent Stress Result
EQV_STRESS_MIN = EQUIVALENT_STRESS.Minimum.Value
EQV_STRESS_MAX = EQUIVALENT_STRESS.Maximum.Value

#Scenario 13: Suppress Cyclic Symmetry and insert Pre-Meshed Cyclic Region using local Coordinate System
SYMMETRY_REGION1.Suppressed=True

SYMMETRY_REGION2=SYMMETRY.AddPreMeshedCyclicRegion()
SYMMETRY_REGION2.CoordinateSystem=COORDINATE_SYSTEM
# Select Low and High Boundary with proper Coordinate System
SYMMETRY_REGION2.LowBoundaryLocation=LOW_FACE
SYMMETRY_REGION2.HighBoundaryLocation=HIGH_FACE
SYMMETRY_REGION2.NumberOfSectors=4

#Scenario 14: Activate few mesh controls to get mapping mesh and generate mesh
MESH.Activate()
#Activate few mesh controls to get mapped meshed on low and high faces
FACE_MESHING.Suppressed=False
MESH_SIZE01.Suppressed=False
MATCH_CONTROL01.Suppressed=False
MATCH_CONTROL02.Suppressed=False

MESH.GenerateMesh()

#Scenario 15: Solve and review Results using Pre-Meshed Cyclic Region
TRANS_THERM_SOLUTION.Activate()
TRANS_THERM_SOLUTION.Solve(True)

#Temperature Result
TEMPERATURE2_RST_MIN = TEMPERATURE01_RST.Minimum.Value
TEMPERATURE2_RST_MAX = TEMPERATURE01_RST.Maximum.Value

STAT_STRUC_SOLUTION.Activate()
STAT_STRUC_SOLUTION.Solve(True)

#Deformation Result
TOTAL_DEF2_MIN = TOTAL_DEFORMATION.Minimum.Value
TOTAL_DEF2_MAX = TOTAL_DEFORMATION.Maximum.Value

#Equivalent Stress Result
EQV_STRESS2_MIN = EQUIVALENT_STRESS.Minimum.Value
EQV_STRESS2_MAX = EQUIVALENT_STRESS.Maximum.Value

Summary

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