Harmonic Acoustic Analysis

In this example, using the attached files, you will insert a Harmonic Acoustic analysis system 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.

Harmonic_Acoustics_Example.agdb
Harmonic_Acoustics_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 Harmonic Acoustics 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 Harmonic_Acoustics_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 Harmonic_Acoustics_Example.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 all main tree nodes as variables
GEOMETRY = Model.Geometry
MESH = Model.Mesh
NAMED_SELECTIONS = Model.NamedSelections
CONNECTIONS = Model.Connections


#Scenario 2 Suppress unneeded bodies and assign material
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS

SPEAKER_BOX = [i for i in GEOMETRY.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True) if i.Name == 'speaker-box assy'][0]
PLATE = [i for i in GEOMETRY.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True) if i.Name == 'plate'][0]
FEA_DOMAIN = [i for i in GEOMETRY.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True) if i.Name == 'FEA_Domain'][0]
PML_REGION = [i for i in GEOMETRY.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True) if i.Name == 'PML_Region'][0]

SPEAKER_BOX.Suppressed = 1
PLATE.Suppressed = 1

FEA_DOMAIN.Material = "Air"
PML_REGION.Material= "Air"

#Scenario 3 Store Named selections as variable
FEA_BODY = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'FEA_Body'][0]
PML_BODY = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'PML_Body'][0]
MASS_SOURCE_FACE = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Mass_Source_face'][0]
PRESSURE_FACES = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'PRESSURE_FACES'][0]

#Scenario 4 Add mesh sizing and method
SIZING1 = MESH.AddSizing()
SIZING1.Location = FEA_BODY
SIZING1.ElementSize =Quantity('0.01 [m]')

SIZING2 = MESH.AddSizing()
SIZING2.Location = PML_BODY
SIZING2.ElementSize =Quantity('0.01 [m]')

MESH_METHOD1 = MESH.AddAutomaticMethod()
MESH_METHOD1.Location = FEA_BODY.Location

MESH_METHOD1.Method =MethodType.HexDominant


MESH_METHOD2 = MESH.AddAutomaticMethod()
MESH_METHOD2.Location = PML_BODY.Location

MESH_METHOD2.Method =MethodType.HexDominant

#Scenario 5 Insert automatic node merge
MESH_EDIT = Model.AddMeshEdit()
NODE_MERGE_GROUP = MESH_EDIT.AddNodeMergeGroup()
NODE_MERGE_GROUP.ToleranceValue = Quantity('0.001 [m]')
MESH_EDIT.Generate()

#Scenario 6 Setup Harmonic Acoustics and defined Acoustic and PML regions
ANALYSIS_SETTINGS = Model.Analyses[0].AnalysisSettings
ANALYSIS_SETTINGS.RangeMaximum = Quantity('3000 [Hz]')
ANALYSIS_SETTINGS.SolutionIntervals = 1
ANALYSIS_SETTINGS.CalculateVelocity = True
ANALYSIS_SETTINGS.CalculateEnergy = True
ANALYSIS_SETTINGS.GeneralMiscellaneous = True
ANALYSIS_SETTINGS.FarFieldRadiationSurface =FarFieldRadiationSurfaceType.Manual

HARMONIC_ACOUSTICS = Model.Analyses[0]
ACOUSTIC_REGION1 = HARMONIC_ACOUSTICS.Children[2]
ACOUSTIC_REGION1.Location = FEA_BODY

ACOUSTIC_REGION2 = HARMONIC_ACOUSTICS.AddPhysicsRegion()
ACOUSTIC_REGION2.Location = PML_BODY
ACOUSTIC_REGION2.Acoustics = True
ACOUSTIC_REGION2.ArtificiallyMatchedLayers = ArtificiallyMatchedLayers.PML

MASS_SOURCE = HARMONIC_ACOUSTICS.AddAcousticMassSource()
MASS_SOURCE.Location = MASS_SOURCE_FACE
MASS_SOURCE.Magnitude.Output.DiscreteValues = [Quantity('0.01 [kg m-2 s-1]')]

ACOUST_PRESSURE = HARMONIC_ACOUSTICS.AddAcousticPressure()
ACOUST_PRESSURE.Location = PRESSURE_FACES

FARFFIELD_RAD_SURFACE = HARMONIC_ACOUSTICS.CreateAutomaticFarFieldRadiationSurfaces()

#Scenario 7 Insert Acoustic results and solve
SOLUTION = Model.Analyses[0].Solution

ACOUSTIC_PRESSURE_RESULT = SOLUTION.AddAcousticPressureResult()
ACOUSTIC_PRESSURE_RESULT.Location = FEA_BODY

SOUND_PRESSURE_LEVEL = SOLUTION.AddAcousticSoundPressureLevel()
SOUND_PRESSURE_LEVEL.Location = FEA_BODY

FAR_FIELD_SPL = SOLUTION.AddAcousticFarFieldSPL()
FAR_FIELD_SPL.SphereRadius = Quantity('1 [m]')
FAR_FIELD_SPL.ThetaAngleEnd = Quantity('90 [deg]')
FAR_FIELD_SPL.ThetaAngleNoOfDivisions = 90

FAR_FIELD_AWEIGHTED_SPL = SOLUTION.AddAcousticFarFieldAWeightedSPL()
FAR_FIELD_AWEIGHTED_SPL.SphereRadius = Quantity('1 [m]')
FAR_FIELD_AWEIGHTED_SPL.ThetaAngleEnd = Quantity('90 [deg]')
FAR_FIELD_AWEIGHTED_SPL.ThetaAngleNoOfDivisions = 90

#Scenario 8 Solve and store results
SOLUTION.Solve(True)

PRESSURE_MAX = ACOUSTIC_PRESSURE_RESULT.Minimum.Value
PRESSURE_MIN = ACOUSTIC_PRESSURE_RESULT.Maximum.Value

SPL_MIN = SOUND_PRESSURE_LEVEL.Minimum.Value
SPL_MAX = SOUND_PRESSURE_LEVEL.Maximum.Value

FF_SPL_MIN = FAR_FIELD_SPL.Minimum.Value
FF_SPL_MAX = FAR_FIELD_SPL.Maximum.Value

FF_A_SPL_MIN = FAR_FIELD_AWEIGHTED_SPL.Minimum.Value
FF_A_SPL_MAX = FAR_FIELD_AWEIGHTED_SPL.Maximum.Value

Summary

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