Rigid Dynamics: General Analysis

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 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.

Mechanical_RBD_Geometry.agdb
Mechanical_RBD_Script.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_Geometry.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_Script.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 - Set up the Tree Object Items

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

# Scenario 2 - Define Named Selections

ns_sphere_surface = DataModel.GetObjectsByName("NS_sphere_surface")[0]
ns_concave_surface = DataModel.GetObjectsByName("NS_concave_surface")[0] 
ns_fixed_surface = DataModel.GetObjectsByName("NS_fixed_surface")[0]

# Scenario 3 - Define Fixed Joint
   	
fixed_joint = connections.AddJoint()
fixed_joint.ConnectionType = JointScopingType.BodyToGround
fixed_joint.Type = JointType.Fixed
fixed_joint.MobileLocation = ns_fixed_surface

# Scenario 4 - Define Contact

contact = connections.AddContactRegion()
contact.SourceLocation = ns_sphere_surface
contact.TargetLocation = ns_concave_surface
contact.RestitutionFactor = 0

# Scenario 5 - Define Mesh Settings

mesh.Resolution = 4
mesh.ElementSize = Quantity("0.005 [m]")
mesh.GenerateMesh()

# Scenario 6 - Define Analysis Settings

analysis_settings.NumberOfSteps = 1
analysis_settings.SetStepEndTime(1, Quantity("0.5 [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("0.05 [s]"))

# Scenario 7 - Insert Standard Earth Gravity

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

# Scenario 8 - Insert Results

total_deformation = solution.AddTotalDeformation()

joint_probe_total_moment = solution.AddJointProbe()
joint_probe_total_moment.BoundaryConditionSelection = fixed_joint
joint_probe_total_moment.ResultType = ProbeResultType.MomentReaction
joint_probe_total_moment.ResultSelection = ProbeDisplayFilter.XAxis	

# Scenario 9 - Set up Unit System

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

# Scenario 10 - Solve and Define the Results

solution.Solve(True)

maximum_total_deformation = total_deformation.Maximum.Value
minimum_total_deformation = total_deformation.Minimum.Value
maximum_of_maximum_total_deformation = total_deformation.MaximumOfMaximumOverTime.Value
minimum_of_minimum_total_deformation = total_deformation.MaximumOfMaximumOverTime.Value
maximum_x_total_moment = joint_probe_total_moment.MaximumXAxis.Value
minimum_x_total_moment = joint_probe_total_moment.MinimumXAxis.Value

Summary

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