Rigid Dynamics: Contact 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 contact, 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_Contact_Example.agdb
Mechanical_RBD_Contact_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_Contact_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_Contact_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

connections = Model.Connections
transient_rbd = Model.Analyses[0]
analysis_settings = transient_rbd.Children[0]
mesh = Model.Mesh
solution = transient_rbd.Solution

# Section 2 - Define the Named Selections

ns_torus_surface = DataModel.GetObjectsByName("NS_torus_surface")[0]
ns_cone_surface = DataModel.GetObjectsByName("NS_cone_surface")[0]
ns_fixed_surface = DataModel.GetObjectsByName("NS_fixed_surface")[0]

# Section 3 - Define the Contact

contact = connections.AddContactRegion()
contact.SourceLocation = ns_torus_surface
contact.TargetLocation = ns_cone_surface
contact.ContactType = ContactType.Frictionless
contact.PinballRegion = ContactPinballType.ProgramControlled
contact.RestitutionFactor = 0.5
contact.RBDContactDetection = DSRBDContactDetection.kCDGeometryBased

# Section 4 - Define the Fixed Joint

fixed_joint = connections.AddJoint()
fixed_joint.ConnectionType=JointScopingType.BodyToGround
fixed_joint.Type = JointType.Fixed
fixed_joint.MobileLocation = ns_fixed_surface

# Section 5 - Define the Mesh

mesh.PhysicsPreference = MeshPhysicsPreferenceType.Mechanical
mesh.ElementOrder=ElementOrder.Quadratic
mesh.ElementSize = Quantity("0.005 [m]")
mesh.Resolution = 4
mesh.GenerateMesh()
	
# Section 6 - Insert Standard Earth Gravity
 
gravity = transient_rbd.AddEarthGravity()
gravity.Direction=GravityOrientationType.NegativeZAxis

# Section 7 - Define the Analysis Settings

analysis_settings.SetStepEndTime( 1, Quantity("0.4 [s]"))
analysis_settings.SetAutomaticTimeStepping(1,AutomaticTimeStepping.On)
analysis_settings.SetInitialTimeStep(1,Quantity("0.0001 [s]"))
analysis_settings.SetMinimumTimeStep(1,Quantity("0.0000001 [s]"))
analysis_settings.SetMaximumTimeStep(1,Quantity("0.01 [s]"))

# Section 8 - Define the Contact Results

total_contact_force_reaction = solution.AddForceReaction()
total_contact_force_reaction.LocationMethod=LocationDefinitionMethod.ContactRegion
total_contact_force_reaction.ContactRegionSelection = contact
total_contact_force_reaction.ContactForce=ContactForceType.Total

tangent_contact_force_reaction = solution.AddForceReaction()
tangent_contact_force_reaction.LocationMethod=LocationDefinitionMethod.ContactRegion
tangent_contact_force_reaction.ContactRegionSelection = contact
tangent_contact_force_reaction.ContactForce=ContactForceType.Tangent

normal_contact_force_reaction = solution.AddForceReaction()
normal_contact_force_reaction.LocationMethod=LocationDefinitionMethod.ContactRegion
normal_contact_force_reaction.ContactRegionSelection = contact
normal_contact_force_reaction.ContactForce=ContactForceType.Normal

# Section 9 - Set up the Unit Systems

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

# Section 10 - Solve the System and Define the Contact Results

solution.Solve(True) 

total_contact_force_reaction_z = total_contact_force_reaction.ZAxis.Value
total_contact_force_reaction_maximum_z = total_contact_force_reaction.MaximumZAxis.Value
tangent_contact_force_reaction_maximum_total = total_contact_force_reaction.MaximumTotal.Value
normal_contact_force_reaction_maximum_total = normal_contact_force_reaction.MaximumTotal.Value
normal_contact_force_reaction_minimum_z = normal_contact_force_reaction.MinimumZAxis.Value

# Section 11 - Insert and Evaluate the Energy Probe Results

energy_probe = solution.AddEnergyProbe()
solution.EvaluateAllResults()

maximum_potential_energy = energy_probe.MaximumPotentialEnergy.Value
maximum_kinetic_energy = energy_probe.MaximumKineticEnergy.Value
maximum_total_energy = energy_probe.MaximumTotalEnergy.Value
maximum_external_energy = energy_probe.MaximumExternalEnergy.Value

Summary

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