Modal Acoustic Analysis

In this example, using the attached files, you will insert a Modal 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.

Mechanical_Modal_Acoustics_013_Geometry.agdb
Mechanical_Modal_Acoustics_013_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 Modal 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 Mechanical_Modal_Acoustics_013_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_Modal_Acoustics_013_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 Define main Tree node objects
GEOMETRY = Model.Geometry
MESH = Model.Mesh
NS_GRP = Model.NamedSelections

#Scenario 2 Store Named selections as variables
NS_OUTER_FACE = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Acoustic_outer_face'][0]
NS_FSI_FACE = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'FSI_Face'][0]
NS_ACOUSTIC_BODY = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Acoustic_body'][0]
NS_SOLID_BODY = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Solid_body'][0]
NS_SOLID_FACE1 = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Solid_face1'][0]
NS_ACST_FACE1 = [i for i in NS_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Acst_face1'][0]

#Scenario 3 Assign Water to Acoustic parts 
GEOM_WATER = [i for i in GEOMETRY.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True) if i.Name == 'Water'][0]

GEOM_WATER.Material = 'Water Liquid'

#Scenario 4 Insert and setup mesh controls
MESH.ElementOrder = ElementOrder.Quadratic

FACE_MESH1 = MESH.AddFaceMeshing()
FACE_MESH1.Location = NS_SOLID_FACE1

FACE_MESH2 = MESH.AddFaceMeshing()
FACE_MESH2.Location = NS_ACST_FACE1

MESH_SIZE1 = MESH.AddSizing()
MESH_SIZE1.Location = NS_SOLID_BODY
MESH_SIZE1.ElementSize = Quantity('0.125 [in]')

MESH_SIZE2 = MESH.AddSizing()
MESH_SIZE2.Location = NS_ACOUSTIC_BODY
MESH_SIZE2.ElementSize = Quantity('5 [in]')

#Scenario 5 Define Physics Regions
MODAL_ACOUSTIC = Model.Analyses[0]

ANALYSIS_SETTINGS = Model.Analyses[0].AnalysisSettings
ANALYSIS_SETTINGS.IgnoreAcousticDamping = True

ACOUSTIC_REGION = MODAL_ACOUSTIC.Children[2]
ACOUSTIC_REGION.Location = NS_ACOUSTIC_BODY
ACOUSTIC_REGION.Acoustics = True

STRUCTURAL_REGION = MODAL_ACOUSTIC.AddPhysicsRegion()
STRUCTURAL_REGION.Location = NS_SOLID_BODY
STRUCTURAL_REGION.Structural = True

#Scenario 6 Insert Acoustic Pressure and FSI
ACOUSTIC_PRESSURE = MODAL_ACOUSTIC.AddAcousticPressure()
ACOUSTIC_PRESSURE.Location = NS_OUTER_FACE
ACOUSTIC_PRESSURE.Magnitude = Quantity('0.000001 [psi]')

FLUID_SOLID_INTERFACE = MODAL_ACOUSTIC.AddFluidSolidInterface()
FLUID_SOLID_INTERFACE.Location = NS_FSI_FACE

#Scenario 7 Insert results Total Deformation and Acoustic Pressure
SOLUTION = MODAL_ACOUSTIC.Solution
TOTAL_DEFORMATION_1 = SOLUTION.AddTotalDeformation()

ACOUSTIC_PRESSURE_RESULT_1 = SOLUTION.AddAcousticPressureResult()
ACOUSTIC_PRESSURE_RESULT_1.Location = NS_ACOUSTIC_BODY

ACOUSTIC_PRESSURE_RESULT_2 = SOLUTION.AddAcousticPressureResult()
ACOUSTIC_PRESSURE_RESULT_2.SetNumber = 2

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

#Frequency for particular mode from details view
FREQ1 = TOTAL_DEFORMATION_1.ReportedFrequency.Value

#Frequency for all modes from tabular data
FREQ1 = TOTAL_DEFORMATION_1.TabularData["Frequency"][0]
FREQ2 = TOTAL_DEFORMATION_1.TabularData["Frequency"][1]
FREQ3 = TOTAL_DEFORMATION_1.TabularData["Frequency"][2]
FREQ4 = TOTAL_DEFORMATION_1.TabularData["Frequency"][3]
FREQ5 = TOTAL_DEFORMATION_1.TabularData["Frequency"][4]
FREQ6 = TOTAL_DEFORMATION_1.TabularData["Frequency"][5]


PRESSURE_MAX = ACOUSTIC_PRESSURE_RESULT_1.Maximum.Value
PRESSURE_MIN = ACOUSTIC_PRESSURE_RESULT_1.Minimum.Value

Summary

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