Note

Go to the end to download the full example code.

Modal acoustics analysis#

This example demonstrate modal acoustic analysis that involves modeling both a structure and the surrounding fluid to analyze frequencies and standing wave patterns within the structure. This type of analysis is essential for applications such as Sonar, concert hall design, noise reduction in various settings, audio speaker design, and geophysical exploration.

Mechanical enables you to model pure acoustic problems and fluid-structure interaction (FSI) problems.A coupled acoustic analysis accounts for FSI. An uncoupled acoustic analysis simulates the fluid only and ignores any fluid-structure interaction.

Import necessary libraries#

import os

from PIL import Image
from ansys.mechanical.core import App
from ansys.mechanical.core.examples import delete_downloads, download_file
from matplotlib import image as mpimg
from matplotlib import pyplot as plt
from matplotlib.animation import FuncAnimation

Embed mechanical and set global variables

app = App()
app.update_globals(globals())
print(app)

cwd = os.path.join(os.getcwd(), "out")


def display_image(image_name):
    plt.figure(figsize=(16, 9))
    plt.imshow(mpimg.imread(os.path.join(cwd, image_name)))
    plt.xticks([])
    plt.yticks([])
    plt.axis("off")
    plt.show()

Ansys Mechanical [Ansys Mechanical Enterprise]
Product Version:251
Software build date: 11/27/2024 09:34:44

Configure graphics for image export#

Graphics.Camera.SetSpecificViewOrientation(ViewOrientationType.Iso)
image_export_format = GraphicsImageExportFormat.PNG
settings_720p = Ansys.Mechanical.Graphics.GraphicsImageExportSettings()
settings_720p.Resolution = GraphicsResolutionType.EnhancedResolution
settings_720p.Background = GraphicsBackgroundType.White
settings_720p.Width = 1280
settings_720p.Height = 720
settings_720p.CurrentGraphicsDisplay = False

Download geometry and materials files#

geometry_path = download_file("sloshing_geometry.agdb", "pymechanical", "embedding")
mat_path = download_file("Water_material_explicit.xml", "pymechanical", "embedding")

Import the geometry#

geometry_import_group = Model.GeometryImportGroup
geometry_import = geometry_import_group.AddGeometryImport()
geometry_import_format = (
    Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.Format.Automatic
)
geometry_import_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
geometry_import_preferences.ProcessNamedSelections = True
geometry_import.Import(
    geometry_path, geometry_import_format, geometry_import_preferences
)

Graphics.Camera.SetFit()
Graphics.ExportImage(
    os.path.join(cwd, "geometry.png"), image_export_format, settings_720p
)
display_image("geometry.png")

Store all variables necessary for analysis#

GEOM = Model.Geometry
MESH = Model.Mesh
NS = Model.NamedSelections
CONN = Model.Connections
MAT = Model.Materials

Import material setup analysis#

Model.AddModalAcousticAnalysis()
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardMKS
MAT.Import(mat_path)
print("Material Import Done !")

Material Import Done !

Get all required named selections and assign materials#

acst_bodies = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Acoustic_bodies"
][0]
struct_bodies = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Structural_bodies"
][0]
top_bodies = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "top_bodies"
][0]
cont_bodies = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "container_bodies"
][0]
cont_V1 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_V1"
][0]
cont_V2 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_V2"
][0]
cont_V3 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_V3"
][0]
cont_face1 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_face1"
][0]
cont_face2 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_face2"
][0]
cont_face3 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_face3"
][0]
cont_face4 = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Cont_face4"
][0]
free_faces = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "Free_faces"
][0]
fsi_faces = [
    i
    for i in NS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True)
    if i.Name == "FSI_faces"
][0]

solid1 = [
    i
    for i in GEOM.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True)
    if i.Name == "Solid1"
][0]
solid2 = [
    i
    for i in GEOM.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True)
    if i.Name == "Solid2"
][0]
solid3 = [
    i
    for i in GEOM.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True)
    if i.Name == "Solid3"
][0]
solid4 = [
    i
    for i in GEOM.GetChildren[Ansys.ACT.Automation.Mechanical.Body](True)
    if i.Name == "Solid4"
][0]

Assign material water to acoustic parts

solid1.Material = "WATER"
solid2.Material = "WATER"
solid3.Material = "WATER"
solid4.Material = "WATER"

Mesh#

MESH.ElementOrder = ElementOrder.Quadratic

method1 = MESH.AddAutomaticMethod()
method1.Location = acst_bodies
method1.Method = MethodType.AllTriAllTet

method2 = MESH.AddAutomaticMethod()
method2.Location = top_bodies
method2.Method = MethodType.Automatic

# Add mesh sizing

sizing1 = MESH.AddSizing()
sizing1.Location = top_bodies
sizing1.ElementSize = Quantity("0.2 [m]")
sizing1.Behavior = SizingBehavior.Hard

# Add mesh sizing

sizing2 = MESH.AddSizing()
sizing2.Location = acst_bodies
sizing2.ElementSize = Quantity("0.2 [m]")
sizing2.Behavior = SizingBehavior.Hard

# Add mesh method

method3 = MESH.AddAutomaticMethod()
method3.Location = cont_bodies
method3.Method = MethodType.Sweep
method3.SourceTargetSelection = 4

MESH.GenerateMesh()

Graphics.ExportImage(os.path.join(cwd, "mesh.png"), image_export_format, settings_720p)
display_image("mesh.png")

Insert contacts#

Contact 1

CONN_GROUP = CONN.AddConnectionGroup()
CONT1 = CONN_GROUP.AddContactRegion()
CONT1.SourceLocation = cont_V1
CONT1.TargetLocation = cont_face1
CONT1.ContactFormulation = ContactFormulation.MPC
CONT1.Behavior = ContactBehavior.Asymmetric
CONT1.PinballRegion = ContactPinballType.Radius
CONT1.PinballRadius = Quantity("0.25 [m]")

Contact 2

CONT2 = CONN_GROUP.AddContactRegion()
CONT2.SourceLocation = cont_V2
CONT2.TargetLocation = cont_face2
CONT2.ContactFormulation = ContactFormulation.MPC
CONT2.Behavior = ContactBehavior.Asymmetric
CONT2.PinballRegion = ContactPinballType.Radius
CONT2.PinballRadius = Quantity("0.25 [m]")

Contact 3

CONT3 = CONN_GROUP.AddContactRegion()
CONT3.SourceLocation = cont_V3
CONT3.TargetLocation = cont_face3
CONT3.ContactFormulation = ContactFormulation.MPC
CONT3.Behavior = ContactBehavior.Asymmetric
CONT3.PinballRegion = ContactPinballType.Radius
CONT3.PinballRadius = Quantity("0.25 [m]")

Contact 3

sel_manager = ExtAPI.SelectionManager
cnv4 = DataModel.GeoData.Assemblies[0].Parts[1].Bodies[0].Vertices[3]
cont_V4 = sel_manager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
cont_V4.Entities = [cnv4]

Contact 4

CONT4 = CONN_GROUP.AddContactRegion()
CONT4.TargetLocation = cont_face4
CONT4.SourceLocation = cont_V4
CONT4.ContactFormulation = ContactFormulation.MPC
CONT4.Behavior = ContactBehavior.Asymmetric
CONT4.PinballRegion = ContactPinballType.Radius
CONT4.PinballRadius = Quantity("0.25 [m]")

Fully define Modal Multiphysics region with two physics regions

MODAL_ACST = DataModel.Project.Model.Analyses[0]
ACOUST_REG = MODAL_ACST.Children[2]
ACOUST_REG.Location = acst_bodies


STRUCT_REG = MODAL_ACST.AddPhysicsRegion()
STRUCT_REG.Structural = True
STRUCT_REG.RenameBasedOnDefinition()
STRUCT_REG.Location = struct_bodies

Analysis settings#

ANALYSIS_SETTINGS = MODAL_ACST.Children[1]
ANALYSIS_SETTINGS.MaximumModesToFind = 12
ANALYSIS_SETTINGS.SearchRangeMinimum = Quantity("0.1 [Hz]")
ANALYSIS_SETTINGS.SolverType = SolverType.Unsymmetric
ANALYSIS_SETTINGS.GeneralMiscellaneous = True
ANALYSIS_SETTINGS.CalculateReactions = True

Boundary conditions and load#

Free surface

FREE_SF = MODAL_ACST.AddAcousticFreeSurface()
FREE_SF.Location = free_faces

Solid fluid interface

FSI_OBJ = MODAL_ACST.AddFluidSolidInterface()
FSI_OBJ.Location = fsi_faces

Gravity

ACCELERATION = MODAL_ACST.AddAcceleration()
ACCELERATION.DefineBy = LoadDefineBy.Components
ACCELERATION.YComponent.Output.DiscreteValues = [Quantity("9.81 [m sec^-1 sec^-1]")]

Fixed Support

fv1 = DataModel.GeoData.Assemblies[0].Parts[1].Bodies[0].Vertices[0]
fv2 = DataModel.GeoData.Assemblies[0].Parts[1].Bodies[1].Vertices[0]
fv3 = DataModel.GeoData.Assemblies[0].Parts[1].Bodies[2].Vertices[0]
fv4 = DataModel.GeoData.Assemblies[0].Parts[1].Bodies[3].Vertices[0]

fvert = sel_manager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
fvert.Entities = [fv1, fv2, fv3, fv4]
FIXED_SUPPORT = MODAL_ACST.AddFixedSupport()
FIXED_SUPPORT.Location = fvert

MODAL_ACST.Activate()
Graphics.ExportImage(
    os.path.join(cwd, "geometry.png"), image_export_format, settings_720p
)
display_image("geometry.png")

Add results#

Add 10 modes

soln = Model.Analyses[0].Solution
TOT_DEF1 = soln.AddTotalDeformation()
TOT_DEF2 = soln.AddTotalDeformation()
TOT_DEF2.Mode = 2
TOT_DEF3 = soln.AddTotalDeformation()
TOT_DEF3.Mode = 3
TOT_DEF4 = soln.AddTotalDeformation()
TOT_DEF4.Mode = 4
TOT_DEF5 = soln.AddTotalDeformation()
TOT_DEF5.Mode = 5
TOT_DEF6 = soln.AddTotalDeformation()
TOT_DEF6.Mode = 6
TOT_DEF7 = soln.AddTotalDeformation()
TOT_DEF7.Mode = 7
TOT_DEF8 = soln.AddTotalDeformation()
TOT_DEF8.Mode = 8
TOT_DEF9 = soln.AddTotalDeformation()
TOT_DEF9.Mode = 9
TOT_DEF10 = soln.AddTotalDeformation()
TOT_DEF10.Mode = 10

Add acoustic pressure

ACOUST_PRES_RES = soln.AddAcousticPressureResult()

Add force reaction scoped to fixed Support

FORCE_REACT1 = soln.AddForceReaction()
FORCE_REACT1.BoundaryConditionSelection = FIXED_SUPPORT

Solve#

soln.Solve(True)

Messages#

Messages = ExtAPI.Application.Messages
if Messages:
    for message in Messages:
        print(f"[{message.Severity}] {message.DisplayString}")
else:
    print("No [Info]/[Warning]/[Error] Messages")

[Warning] The license manager is delayed in its response. The latest requests were answered after 21 seconds.
[Warning] The application requires the use of OpenGL version 4.3. The detected version 3.1 Mesa 21.2.6 does not meet this requirement. This discrepancy may produce graphical display issues for certain features. Furthermore, future versions of Mechanical may not support systems that do not meet this requirement.

Results#

Total deformation - mode 1

Tree.Activate([TOT_DEF1])
Graphics.Camera.SetFit()
Graphics.ExportImage(
    os.path.join(cwd, "totaldeformation1.png"), image_export_format, settings_720p
)
display_image("totaldeformation1.png")

Acoustic pressure

Tree.Activate([ACOUST_PRES_RES])
Graphics.ExportImage(
    os.path.join(cwd, "acoustic_pressure.png"), image_export_format, settings_720p
)
display_image("acoustic_pressure.png")

Display all modal frequency, force reaction and acoustic pressure values

FREQ1 = TOT_DEF1.ReportedFrequency.Value
FREQ2 = TOT_DEF2.ReportedFrequency.Value
FREQ3 = TOT_DEF3.ReportedFrequency.Value
FREQ4 = TOT_DEF4.ReportedFrequency.Value
FREQ5 = TOT_DEF5.ReportedFrequency.Value
FREQ6 = TOT_DEF6.ReportedFrequency.Value
FREQ7 = TOT_DEF7.ReportedFrequency.Value
FREQ8 = TOT_DEF8.ReportedFrequency.Value
FREQ9 = TOT_DEF9.ReportedFrequency.Value
FREQ10 = TOT_DEF10.ReportedFrequency.Value

PRMAX = ACOUST_PRES_RES.Maximum.Value
PRMIN = ACOUST_PRES_RES.Minimum.Value

FRC1_X = FORCE_REACT1.XAxis.Value
FRC1_Z = FORCE_REACT1.ZAxis.Value

print("Modal Acoustic Results")
print("----------------------")
print("Frequency for mode 1 : ", FREQ1)
print("Frequency for mode 2 : ", FREQ2)
print("Frequency for mode 3 : ", FREQ3)
print("Frequency for mode 4 : ", FREQ4)
print("Frequency for mode 5 : ", FREQ5)
print("Frequency for mode 6 : ", FREQ6)
print("Frequency for mode 7 : ", FREQ7)
print("Frequency for mode 8 : ", FREQ8)
print("Frequency for mode 9 : ", FREQ9)
print("Frequency for mode 10 : ", FREQ10)
print("Acoustic pressure minimum : ", PRMIN)
print("Acoustic pressure Maximum : ", PRMAX)
print("Force reaction x-axis : ", FRC1_X)
print("Force reaction z-axis : ", FRC1_Z)

Modal Acoustic Results
----------------------
Frequency for mode 1 :  0.46078132766548147
Frequency for mode 2 :  0.4627077354571064
Frequency for mode 3 :  0.6177437587816744
Frequency for mode 4 :  0.6199129375042773
Frequency for mode 5 :  0.6921247123992701
Frequency for mode 6 :  0.7249771259477809
Frequency for mode 7 :  0.7285506780217891
Frequency for mode 8 :  0.8115363751415202
Frequency for mode 9 :  0.8133203759958677
Frequency for mode 10 :  0.8139363245321334
Acoustic pressure minimum :  -1.4709837436676025
Acoustic pressure Maximum :  1.4751087427139282
Force reaction x-axis :  12.112502798586448
Force reaction z-axis :  0.2570330082169942

Total deformation animation for mode 10

animation_export_format = (
    Ansys.Mechanical.DataModel.Enums.GraphicsAnimationExportFormat.GIF
)
settings_720p = Ansys.Mechanical.Graphics.AnimationExportSettings()
settings_720p.Width = 1280
settings_720p.Height = 720

TOT_DEF10.ExportAnimation(
    os.path.join(cwd, "deformation_10.gif"), animation_export_format, settings_720p
)
gif = Image.open(os.path.join(cwd, "deformation_10.gif"))
fig, ax = plt.subplots(figsize=(16, 9))
ax.axis("off")
img = ax.imshow(gif.convert("RGBA"))


def update(frame):
    gif.seek(frame)
    img.set_array(gif.convert("RGBA"))
    return [img]


ani = FuncAnimation(
    fig, update, frames=range(gif.n_frames), interval=100, repeat=True, blit=True
)
plt.show()

Project tree#

app.print_tree()

├── Project
|  ├── Model
|  |  ├── Geometry Imports (✓)
|  |  |  ├── Geometry Import (✓)
|  |  ├── Geometry (✓)
|  |  |  ├── Part
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid1
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid2
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid3
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid4
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  |  ├── Solid
|  |  |  ├── Part 2
|  |  |  |  ├── Line Body
|  |  |  |  ├── Line Body
|  |  |  |  ├── Line Body
|  |  |  |  ├── Line Body
|  |  |  |  ├── Line Body
|  |  ├── Materials (✓)
|  |  |  ├── Structural Steel (✓)
|  |  |  ├── Air (✓)
|  |  |  ├── WATER (✓)
|  |  ├── Cross Sections (✓)
|  |  |  ├── Circular1 (✓)
|  |  ├── Coordinate Systems (✓)
|  |  |  ├── Global Coordinate System (✓)
|  |  ├── Remote Points (✓)
|  |  ├── Connections (✓)
|  |  |  ├── Connection Group (✓)
|  |  |  |  ├── Contact Region (✓)
|  |  |  |  ├── Contact Region 2 (✓)
|  |  |  |  ├── Contact Region 3 (✓)
|  |  |  |  ├── Contact Region 4 (✓)
|  |  ├── Mesh Workflows (✓)
|  |  ├── Mesh (✓)
|  |  |  ├── Patch Conforming Method (✓)
|  |  |  ├── Automatic Method (✓)
|  |  |  ├── Body Sizing (✓)
|  |  |  ├── Body Sizing 2 (✓)
|  |  |  ├── Sweep Method (✓)
|  |  ├── Named Selections
|  |  |  ├── Acoustic_bodies (✓)
|  |  |  ├── Structural_bodies (✓)
|  |  |  ├── Line_bodies (✓)
|  |  |  ├── Free_faces (✓)
|  |  |  ├── FSI_faces (✓)
|  |  |  ├── top_bodies (✓)
|  |  |  ├── container_bodies (✓)
|  |  |  ├── Cont_V1 (✓)
|  |  |  ├── Cont_V2 (✓)
|  |  |  ├── Cont_V3 (✓)
|  |  |  ├── Cont_face1 (✓)
|  |  |  ├── Cont_face2 (✓)
|  |  |  ├── Cont_face3 (✓)
|  |  |  ├── Cont_face4 (✓)
|  |  ├── Modal Acoustics (✓)
|  |  |  ├── Pre-Stress (None) (✓)
|  |  |  ├── Analysis Settings (✓)
|  |  |  ├── Acoustics Region (✓)
|  |  |  ├── Structural Region (✓)
|  |  |  ├── Acceleration (✓)
|  |  |  ├── Free Surface (✓)
|  |  |  ├── Fluid Solid Interface (✓)
|  |  |  ├── Fixed Support (✓)
|  |  |  ├── Solution (✓)
|  |  |  |  ├── Solution Information (✓)
|  |  |  |  ├── Total Deformation (✓)
|  |  |  |  ├── Total Deformation 2 (✓)
|  |  |  |  ├── Total Deformation 3 (✓)
|  |  |  |  ├── Total Deformation 4 (✓)
... truncating after 80 lines

Cleanup#

Save project

app.save(os.path.join(cwd, "modal_acoustics.mechdat"))
app.new()

Delete example file

delete_downloads()

True

Total running time of the script: (0 minutes 52.435 seconds)

Gallery generated by Sphinx-Gallery