Rigid Dynamics: Flexible Part Specification

In this example, using the support files, you will insert a Rigid Dynamics analysis object into an undefined Mechanical session and execute a sequence of python journal commands that defines an analysis, with a focus on flexible part definition, and solves the analysis.

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

Mechanical_RBD_Flexible_Part_Example.agdb
Mechanical_RBD_Flexible_Part_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 Rigid Dynamics 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_RBD_Flexible_Part_Example.agdb.
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_RBD_Flexible_Part_Example.py.
Select the Run Script option ( ) from the Editor toolbar.

Scripts Illustrated

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

# Section 1 - Set up the Tree Object Items

geometry = Model.Geometry
connections = Model.Connections
transient_rbd = Model.Analyses[0]
analysis_settings = transient_rbd.Children[0]
solution = transient_rbd.Solution

# Section 2 - Define the Named Selections

ns_face1 = DataModel.GetObjectsByName("NS_FACE1")[0]
ns_face2 = DataModel.GetObjectsByName("NS_FACE2")[0]
ns_cms1 = DataModel.GetObjectsByName("NS_CMS1")[0]

# Section 3 - Define the Flexible Cms1 Part and Suppress Solid

cms1 = geometry.Children[0].Children[0]
solid = geometry.Children[1].Children[0]
cms1.StiffnessBehavior = StiffnessBehavior.Flexible
solid.Suppressed = True

# Section 4 - Set up the General Revolute Joint

general_revolute_joint = connections.AddJoint()
general_revolute_joint.ConnectionType=JointScopingType.BodyToGround
general_revolute_joint.Type = JointType.General
general_revolute_joint.MobileLocation = ns_face1
general_revolute_joint.Rotations = JointRotationDOFType.FreeX

# Section 5 - Set up the General Joint with 6 DOF
	
general_all_free = connections.AddJoint()
general_all_free.ConnectionType=JointScopingType.BodyToGround
general_all_free.Type = JointType.General
general_all_free.TranslationX=FixedOrFree.Free
general_all_free.TranslationY=FixedOrFree.Free
general_all_free.TranslationZ=FixedOrFree.Free
general_all_free.Rotations=JointRotationDOFType.FreeAll
general_all_free.MobileLocation = ns_face2

# Section 6 - Generate Condensed Geometries

condensed_geometry = Model.AddCondensedGeometry()
condensed_part = condensed_geometry.AddCondensedPart()
condensed_part.GeometrySelection = ns_cms1
condensed_part.NumberOfModes = 10
condensed_part.DetectCondensedPartInterface()
condensed_part.GenerateCondensedParts()

# Section 7 - Define the Analysis Settings

analysis_settings.SetStepEndTime( 1, Quantity("0.5 [s]"))
analysis_settings.SetAutomaticTimeStepping( 1, AutomaticTimeStepping.On)
analysis_settings.SetInitialTimeStep( 1, Quantity("1e-4[s]")) 
analysis_settings.SetMinimumTimeStep( 1, Quantity("1e-7[s]"))
analysis_settings.SetMaximumTimeStep( 1, Quantity("1e-3[s]"))
analysis_settings.SetStoreResultAt( 1,TimePointsOptions.EquallySpacedPoints)
analysis_settings.SetStoreResultAtValue( 1,200)

# Section 8 - Insert Standard Earth Gravity

gravity = transient_rbd.AddEarthGravity()
gravity.Direction=GravityOrientationType.PositiveYAxis

# Section 9 - Define the Expansion Settings

expansion_settings = solution.Children[1]
expansion_settings.Activate()
expansion_settings_state = expansion_settings.GetExpansionState( condensed_part)
expansion_settings_state.Stress = True
expansion_settings_state.Displacement = True
expansion_settings.SetExpansionState( condensed_part, expansion_settings_state)
	
# Section 10 - Insert the Condensed Part Results 

total_deformation = solution.AddTotalDeformation()

joint_probe_deformation = solution.AddJointProbe()
joint_probe_deformation.BoundaryConditionSelection = general_all_free
joint_probe_deformation.ResultType = ProbeResultType.DeformationProbe
	
equivalent_stress = solution.AddEquivalentStress()

middle_principal_strain = solution.AddMiddlePrincipalElasticStrain()

# Section 11 - Set up the Unit Systems

ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS
ExtAPI.Application.ActiveAngleUnit = AngleUnitType.Radian
ExtAPI.Application.ActiveAngularVelocityUnit=AngularVelocityUnitType.RadianPerSecond

# Section 12 - Solve the System and Define the Condensed Part Results

solution.Solve(True)

total_deformation_maximum = total_deformation.Maximum.Value
equivalent_stress_maximum = equivalent_stress.Maximum.Value
middle_principal_stress_maximum = middle_principal_strain.Maximum.Value

Summary

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