Static Structural Universal Joint Analysis

In this example, using the support files, you will insert a Static Structural analysis object into an undefined Mechanical session and execute a sequence of python journal commands that specify a Joint as Universal, define mesh and boundary and result objects and solve the analysis.

This example begins in the Mechanical application. It requires you to download the following Ansys DesignModeler and python files.

Mechanical_Static_Joint_002_Example.agbd
Mechanical_Static_Joint_002_Example.py

These files are available here.

Procedure

Open Mechanical directly without importing a geometry or specifying an analysis type. This can be done through Start Menu.
From the Analysis drop-down menu of the Insert group on the Home tab, insert a Static Structural system into the tree.
Select the Geometry object and select the Attach Geometry option from the Geometry group on the Geometry Context tab. Navigate to the proper folder location and select Mechanical_Static_Joint_002_Example.agbd.
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 Mechanical_Static_Joint_002_Example.py.
Select the Run Script option ( ) from the Editor toolbar.

Scripts Illustrated

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

#=======================================================================================================================
# 	ACT Mechanical API Example for General Joint as Translational
#   Python Script Scenarios:
#   1. Set up the Unit Systems
#   2. Set up the Tree Object Items
#   3. Define Named Selections
#   4. Define General Joint as Translational
#   5. Define Mesh Settings
#   6. Insert Displacement BC
#   7. Insert Results
#   8. Solve and review the results

# Reference case: None. Created from scratch.
# Reference geometry: ...\DS_Parts\PARA_Parts\LONGBAR.x_t
# Script is created by Rahul B Patil.
#=======================================================================================================================

#Scenario 1 - Set up the Units System

ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS


#Scenario 2 - Set up the Tree Object Items

CONNECTION_GROUP = Model.Connections
MESH = Model.Mesh
STATIC_STRUCTURAL = Model.Analyses[0]
ANALYSIS_SETTINGS = STATIC_STRUCTURAL.Children[0]
STATIC_STRUCTURAL_SOLUTION = STATIC_STRUCTURAL.Solution


#Scenario 3 - Define Named Selections

NS_FIXED_FACE = DataModel.Project.Model.AddNamedSelection()
NS_FIXED_FACE.ScopingMethod=GeometryDefineByType.Worksheet
NS_FIXED_FACE.Name = "NS_FIXED_FACE"
GEN_CRT1 = NS_FIXED_FACE.GenerationCriteria
CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
CRT1.Active=True
CRT1.Action=SelectionActionType.Add
CRT1.EntityType=SelectionType.GeoFace
CRT1.Criterion=SelectionCriterionType.LocationZ
CRT1.Operator=SelectionOperatorType.Equal
CRT1.Value=Quantity('0.00 [m]')
GEN_CRT1.Add(CRT1)
NS_FIXED_FACE.Activate()
NS_FIXED_FACE.Generate()
NS_BC_FACE = DataModel.Project.Model.AddNamedSelection()
NS_BC_FACE.ScopingMethod=GeometryDefineByType.Worksheet
NS_BC_FACE.Name = "NS_BC_FACE"
GEN_CRT1 = NS_BC_FACE.GenerationCriteria
CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
CRT1.Active=True
CRT1.Action=SelectionActionType.Add
CRT1.EntityType=SelectionType.GeoFace
CRT1.Criterion=SelectionCriterionType.LocationZ
CRT1.Operator=SelectionOperatorType.Equal
CRT1.Value=Quantity('20.00 [m]')
GEN_CRT1.Add(CRT1)
NS_BC_FACE.Activate()
NS_BC_FACE.Generate()


#Scenario 4 - Define General Joint as Translational
   	
JOINT_GENERAL = CONNECTION_GROUP.AddJoint()
JOINT_GENERAL.ConnectionType = JointScopingType.BodyToGround
JOINT_GENERAL.Type = JointType.General
JOINT_GENERAL.TranslationZ = FixedOrFree.Free
JOINT_GENERAL.MobileLocation = NS_FIXED_FACE
# The below commands help in setting the rotational dofs
JOINT_GENERAL.Rotations = JointRotationDOFType.FreeAll
JOINT_GENERAL.Rotations = JointRotationDOFType.FixAll


#Scenario 5 - Define Mesh Settings

MESH.ElementSize = Quantity("0.25 [m]")
MESH.GenerateMesh()


#Scenario 6 - Insert Displacement BC

DISPLACEMENT_BC = STATIC_STRUCTURAL.AddDisplacement()
DISPLACEMENT_BC.Location = NS_BC_FACE
DISPLACEMENT_BC.ZComponent.Output.DiscreteValues = [Quantity("0.01 [m]")]


#Scenario 7 - Insert Results

DIRECTIONAL_DEFORMATION = STATIC_STRUCTURAL_SOLUTION.AddDirectionalDeformation()	
DIRECTIONAL_DEFORMATION.NormalOrientation = NormalOrientationType.ZAxis

JOINT_PROBE_RELATIVE_DISPLACEMENT = STATIC_STRUCTURAL_SOLUTION.AddJointProbe()
JOINT_PROBE_RELATIVE_DISPLACEMENT.BoundaryConditionSelection = JOINT_GENERAL
JOINT_PROBE_RELATIVE_DISPLACEMENT.ResultType = ProbeResultType.DeformationProbe
JOINT_PROBE_RELATIVE_DISPLACEMENT.ResultSelection = ProbeDisplayFilter.ZAxis


#Scenario 8 - Solve and review the results

STATIC_STRUCTURAL_SOLUTION.Solve(True)

DIRECTIONAL_DEFORMATION_MAX = DIRECTIONAL_DEFORMATION.Maximum.Value
DIRECTIONAL_DEFORMATION_MIN = DIRECTIONAL_DEFORMATION.Minimum.Value
JOINT_PROBE_RELATIVE_DISPLACEMENT_MAX = JOINT_PROBE_RELATIVE_DISPLACEMENT.MaximumZAxis.Value
JOINT_PROBE_RELATIVE_DISPLACEMENT_MIN = JOINT_PROBE_RELATIVE_DISPLACEMENT.MinimumZAxis.Value

Summary

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