diff --git a/.github/workflows/ci_cd.yml b/.github/workflows/ci_cd.yml
index 2bdfc0d1..8465584b 100644
--- a/.github/workflows/ci_cd.yml
+++ b/.github/workflows/ci_cd.yml
@@ -47,7 +47,7 @@ jobs:
     runs-on: public-ubuntu-latest-8-cores
     timeout-minutes: 60
     container:
-      image: ghcr.io/ansys/mechanical:25.2.0
+      image: ghcr.io/ansys/mechanical:26.1.0
       options: --entrypoint /bin/bash
     needs: [style, doc-style]
 
@@ -86,7 +86,7 @@ jobs:
           SPHINXOPTS: '-j auto -W --keep-going'
         run: |
           . /env/bin/activate
-          xvfb-run make -C doc linkcheck
+          xvfb-run mechanical-env make -C doc linkcheck
 
       - name: Upload HTML Documentation
         uses: actions/upload-artifact@v4
@@ -95,6 +95,13 @@ jobs:
           path: doc/_build/html
           retention-days: 7
 
+      - name: Upload examples
+        uses: actions/upload-artifact@v4
+        with:
+          name: examples-out
+          path: examples/02_technology_showcase
+          retention-days: 7
+
   doc-deploy:
     name: Documentation deploy
     runs-on: ubuntu-latest
diff --git a/.github/workflows/ci_cd_nightly.yml b/.github/workflows/ci_cd_nightly.yml
index fb8f3b0a..b5fd64cf 100644
--- a/.github/workflows/ci_cd_nightly.yml
+++ b/.github/workflows/ci_cd_nightly.yml
@@ -111,6 +111,13 @@ jobs:
           path: doc/_build/html
           retention-days: 7
 
+      - name: Upload example output
+        uses: actions/upload-artifact@v4
+        with:
+          name: examples
+          path: examples/02_technology_showcase
+          retention-days: 7
+
   build-failure:
     name: Teams notify on failure
     if: failure()
diff --git a/.pre-commit-config.yaml b/.pre-commit-config.yaml
index 336e3b0f..d3194b6a 100644
--- a/.pre-commit-config.yaml
+++ b/.pre-commit-config.yaml
@@ -9,7 +9,7 @@ repos:
   rev: 1.20.0
   hooks:
   - id: blacken-docs
-    additional_dependencies: [black==23.12.1]
+    additional_dependencies: [black==25.1.0]
 
 - repo: https://github.com/pycqa/isort
   rev: 7.0.0
@@ -44,4 +44,4 @@ repos:
   hooks:
   - id: add-license-headers
     args:
-    - --start_year=2023
\ No newline at end of file
+    - --start_year=2023
diff --git a/examples/02_technology_showcase/prestressed_modal_cyclic_symmetry_analysis.py b/examples/02_technology_showcase/prestressed_modal_cyclic_symmetry_analysis.py
new file mode 100644
index 00000000..01200a16
--- /dev/null
+++ b/examples/02_technology_showcase/prestressed_modal_cyclic_symmetry_analysis.py
@@ -0,0 +1,714 @@
+# Copyright (C) 2023 - 2025 ANSYS, Inc. and/or its affiliates.
+# SPDX-License-Identifier: MIT
+#
+#
+# Permission is hereby granted, free of charge, to any person obtaining a copy
+# of this software and associated documentation files (the "Software"), to deal
+# in the Software without restriction, including without limitation the rights
+# to use, copy, modify, merge, publish, distribute, sublicense, and/or sell
+# copies of the Software, and to permit persons to whom the Software is
+# furnished to do so, subject to the following conditions:
+#
+# The above copyright notice and this permission notice shall be included in all
+# copies or substantial portions of the Software.
+#
+# THE SOFTWARE IS PROVIDED "AS IS", WITHOUT WARRANTY OF ANY KIND, EXPRESS OR
+# IMPLIED, INCLUDING BUT NOT LIMITED TO THE WARRANTIES OF MERCHANTABILITY,
+# FITNESS FOR A PARTICULAR PURPOSE AND NONINFRINGEMENT. IN NO EVENT SHALL THE
+# AUTHORS OR COPYRIGHT HOLDERS BE LIABLE FOR ANY CLAIM, DAMAGES OR OTHER
+# LIABILITY, WHETHER IN AN ACTION OF CONTRACT, TORT OR OTHERWISE, ARISING FROM,
+# OUT OF OR IN CONNECTION WITH THE SOFTWARE OR THE USE OR OTHER DEALINGS IN THE
+# SOFTWARE.
+
+""".. _ref_example_td_013:
+
+Centrifugal Impeller Analysis Using Cyclic Symmetry and Linear Perturbation
+---------------------------------------------------------------------------
+
+The impeller blade assembly in this example is a subsystem of a gas turbine
+engine used in aerospace applications. The model consists of a shroud and
+an impeller blade assembly with a sector angle of 27.692 degrees. The full
+model is composed of 13 primary blades and splitters located at a distance
+of 1 mm from the rigid wall at the start of the analysis.
+
+Coverage:
+Modal, perturbed prestressed modal with linear and nonlinear base static
+solution, full-harmonic are performed on the cyclic-sector model.
+Cyclic symmetry is applied.
+Pressure, rotational velocity and thermal boundary condition are applied.
+
+"""
+
+## %%
+# Import the necessary libraries
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+from pathlib import Path
+from typing import TYPE_CHECKING
+
+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
+
+if TYPE_CHECKING:
+    import Ansys
+
+# %%
+# Initialize the embedded application
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+app = App(globals=globals())
+print(app)
+
+# set the number of cores to use for the solve process
+
+# config = app.ExtAPI.Application.SolveConfigurations["My Computer"]
+# config.SolveProcessSettings.MaxNumberOfCores = 1
+
+# %%
+# Create functions to set camera and display images
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+# Set the path for the output files (images, gifs, mechdat)
+output_path = Path.cwd() / "out"
+
+
+def display_image(
+    image_path: str,
+    pyplot_figsize_coordinates: tuple = (16, 9),
+    plot_xticks: list = [],
+    plot_yticks: list = [],
+    plot_axis: str = "off",
+) -> None:
+    """Display the image with the specified parameters.
+
+    Parameters
+    ----------
+    image_path : str
+        The path to the image file to display.
+    pyplot_figsize_coordinates : tuple
+        The size of the figure in inches (width, height).
+    plot_xticks : list
+        The x-ticks to display on the plot.
+    plot_yticks : list
+        The y-ticks to display on the plot.
+    plot_axis : str
+        The axis visibility setting ('on' or 'off').
+    """
+    # Set the figure size based on the coordinates specified
+    plt.figure(figsize=pyplot_figsize_coordinates)
+    # Read the image from the file into an array
+    image_path = str(output_path / image_path)
+    plt.imshow(mpimg.imread(image_path))
+    # Get or set the current tick locations and labels of the x-axis
+    plt.xticks(plot_xticks)
+    # Get or set the current tick locations and labels of the y-axis
+    plt.yticks(plot_yticks)
+    # Turn off the axis
+    plt.axis(plot_axis)
+    # Display the figure
+    plt.show()
+
+
+# %%
+# Configure graphics for image export
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+# Define the graphics and camera
+graphics = app.Graphics
+camera = graphics.Camera
+
+# Set the camera orientation to the isometric view and set the camera to fit the model
+camera.SetSpecificViewOrientation(ViewOrientationType.Iso)
+camera.SetFit()
+
+# Set the image export format and settings
+image_export_format = GraphicsImageExportFormat.PNG
+settings_720p = Ansys.Mechanical.Graphics.GraphicsImageExportSettings()
+settings_720p.Resolution = (
+    Ansys.Mechanical.DataModel.Enums.GraphicsResolutionType.EnhancedResolution
+)
+settings_720p.Background = Ansys.Mechanical.DataModel.Enums.GraphicsBackgroundType.White
+settings_720p.Width = 1280
+settings_720p.Height = 720
+settings_720p.CurrentGraphicsDisplay = False
+
+# %%
+# Download and Import CDB File
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Download the CDB file from the specified URL
+# and save it to a temporary directory.
+# The CDB file is then imported into the Ansys Mechanical model
+# using the Model Import API.
+# The CDB file is a pre-existing model file that contains
+# the geometry and mesh information for the analysis.
+# Define the model
+
+geometry_path = download_file("cyclic_sector_model.cdb", "pymechanical", "embedding")
+model = app.Model
+
+# Add the geometry import to the geometry import group
+geometry_import_group = model.GeometryImportGroup
+geometry_import = geometry_import_group.AddModelImport()
+geometry_import.ModelImportSourceFilePath = geometry_path
+geometry_import.UnitSystemTypeForImport = ModelImportUnitSystemType.UnitSystemMetricNMM
+print(geometry_import.UnitSystemTypeForImport)
+geometry_import.Import()
+
+# Visualize the model in 3D
+app.plot()
+
+# %%
+# Store all main tree nodes as variables
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Store the main tree nodes of the Ansys Mechanical model
+# in variables for easy access.
+# The variables include the model, geometry, mesh,
+# named selections, connections, and coordinate systems.
+
+GEOM = ExtAPI.DataModel.Project.Model.Geometry
+MSH = ExtAPI.DataModel.Project.Model.Mesh
+NS_GRP = ExtAPI.DataModel.Project.Model.NamedSelections
+CONN_GRP = ExtAPI.DataModel.Project.Model.Connections
+CS_GRP = ExtAPI.DataModel.Project.Model.CoordinateSystems
+
+# %%
+# Define and Select NMM Units System
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Define the unit system for the model as Standard NMM (Newton, millimeter).
+# This unit system is commonly used in engineering applications
+# and is suitable for the analysis being performed.
+
+ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMM
+
+# %%
+# Materials Assignment
+# ~~~~~~~~~~~~~~~~~~~~~
+# Assign materials to the geometry components of the model.
+# The materials are defined in the Ansys Mechanical
+# database and are assigned to the geometry components based on their names.
+
+blade1 = GEOM.Children[1]
+blade1.Material = "Structural Steel"
+blade2 = GEOM.Children[2]
+blade2.Material = "Structural Steel"
+
+# %%
+# Coordinate System Definition
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Define a local coordinate system (LCS) for the model.
+
+LCS1 = CS_GRP.AddCoordinateSystem()
+LCS1.CoordinateSystemType = CoordinateSystemTypeEnum.Cylindrical
+LCS1.OriginX = Quantity("0 [mm]")
+LCS1.OriginY = Quantity("0 [mm]")
+LCS1.OriginZ = Quantity("0 [mm]")
+LCS1.SecondaryAxisDefineBy = CoordinateSystemAlignmentType.GlobalZ
+
+# %%
+# Add Named Selections
+# ~~~~~~~~~~~~~~~~~~~~~
+# The named selections are used to specify the locations
+# where loads and boundary conditions will be applied during the analysis.
+
+NS_LOW = NS_GRP.AddNamedSelection()
+NS_LOW.Name = "NS_LOW"
+NS_LOW.ScopingMethod = GeometryDefineByType.Worksheet
+
+GEN_CRT = NS_LOW.GenerationCriteria
+CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT1.Active = True
+CRT1.Action = SelectionActionType.Add
+CRT1.EntityType = SelectionType.GeoFace
+CRT1.Criterion = SelectionCriterionType.Size
+CRT1.Operator = SelectionOperatorType.Equal
+CRT1.Value = Quantity("607.35 [mm^2]")
+GEN_CRT.Add(CRT1)
+
+CRT2 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT2.Active = True
+CRT2.Action = SelectionActionType.Filter
+CRT2.EntityType = SelectionType.GeoFace
+CRT2.Criterion = SelectionCriterionType.LocationZ
+CRT2.Operator = SelectionOperatorType.Equal
+CRT2.Value = Quantity("46.544 [mm]")
+GEN_CRT.Add(CRT2)
+
+CRT3 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT3.Active = True
+CRT3.Action = SelectionActionType.Add
+CRT3.EntityType = SelectionType.GeoFace
+CRT3.Criterion = SelectionCriterionType.Size
+CRT3.Operator = SelectionOperatorType.Equal
+CRT3.Value = Quantity("997.65 [mm^2]")
+GEN_CRT.Add(CRT3)
+
+CRT4 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT4.Active = True
+CRT4.Action = SelectionActionType.Filter
+CRT4.EntityType = SelectionType.GeoFace
+CRT4.Criterion = SelectionCriterionType.LocationZ
+CRT4.Operator = SelectionOperatorType.GreaterThan
+CRT4.Value = Quantity("21 [mm]")
+GEN_CRT.Add(CRT4)
+NS_LOW.Activate()
+NS_LOW.Generate()
+
+NS_HIGH = NS_GRP.AddNamedSelection()
+NS_HIGH.Name = "NS_LOW"
+NS_HIGH.ScopingMethod = GeometryDefineByType.Worksheet
+
+GEN_CRT = NS_HIGH.GenerationCriteria
+CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT1.Active = True
+CRT1.Action = SelectionActionType.Add
+CRT1.EntityType = SelectionType.GeoFace
+CRT1.Criterion = SelectionCriterionType.Size
+CRT1.Operator = SelectionOperatorType.Equal
+CRT1.Value = Quantity("607.35 [mm^2]")
+GEN_CRT.Add(CRT1)
+
+CRT2 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT2.Active = True
+CRT2.Action = SelectionActionType.Filter
+CRT2.EntityType = SelectionType.GeoFace
+CRT2.Criterion = SelectionCriterionType.LocationZ
+CRT2.Operator = SelectionOperatorType.Equal
+CRT2.Value = Quantity("24.348 [mm]")
+GEN_CRT.Add(CRT2)
+
+CRT3 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT3.Active = True
+CRT3.Action = SelectionActionType.Add
+CRT3.EntityType = SelectionType.GeoFace
+CRT3.Criterion = SelectionCriterionType.Size
+CRT3.Operator = SelectionOperatorType.Equal
+CRT3.Value = Quantity("997.65 [mm^2]")
+GEN_CRT.Add(CRT3)
+
+CRT4 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT4.Active = True
+CRT4.Action = SelectionActionType.Filter
+CRT4.EntityType = SelectionType.GeoFace
+CRT4.Criterion = SelectionCriterionType.LocationX
+CRT4.Operator = SelectionOperatorType.GreaterThan
+CRT4.Value = Quantity("13 [mm]")
+GEN_CRT.Add(CRT4)
+NS_HIGH.Activate()
+NS_HIGH.Generate()
+
+NS_PRES = NS_GRP.AddNamedSelection()
+NS_PRES.Name = "NS_PRES"
+NS_PRES.ScopingMethod = GeometryDefineByType.Worksheet
+
+GEN_CRT = NS_PRES.GenerationCriteria
+CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT1.Active = True
+CRT1.Action = SelectionActionType.Add
+CRT1.EntityType = SelectionType.GeoFace
+CRT1.Criterion = SelectionCriterionType.Size
+CRT1.Operator = SelectionOperatorType.Equal
+CRT1.Value = Quantity("2423.7 [mm^2]")
+GEN_CRT.Add(CRT1)
+
+CRT2 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT2.Active = True
+CRT2.Action = SelectionActionType.Add
+CRT2.EntityType = SelectionType.GeoFace
+CRT2.Criterion = SelectionCriterionType.Size
+CRT2.Operator = SelectionOperatorType.Equal
+CRT2.Value = Quantity("101.11 [mm^2]")
+GEN_CRT.Add(CRT2)
+NS_PRES.Activate()
+NS_PRES.Generate()
+
+NS_BODIES = NS_GRP.AddNamedSelection()
+NS_BODIES.Name = "NS_BODIES"
+NS_BODIES.ScopingMethod = GeometryDefineByType.Worksheet
+
+GEN_CRT = NS_BODIES.GenerationCriteria
+CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT1.Active = True
+CRT1.Action = SelectionActionType.Add
+CRT1.EntityType = SelectionType.GeoBody
+CRT1.Criterion = SelectionCriterionType.Size
+CRT1.Operator = SelectionOperatorType.GreaterThan
+CRT1.Value = Quantity("1 [mm^3]")
+GEN_CRT.Add(CRT1)
+NS_BODIES.Activate()
+NS_BODIES.Generate()
+
+NS_RESP_VERTEX = NS_GRP.AddNamedSelection()
+NS_RESP_VERTEX.Name = "NS_RESP_VERTEX"
+NS_RESP_VERTEX.ScopingMethod = GeometryDefineByType.Worksheet
+
+GEN_CRT = NS_RESP_VERTEX.GenerationCriteria
+CRT1 = Ansys.ACT.Automation.Mechanical.NamedSelectionCriterion()
+CRT1.Active = True
+CRT1.Action = SelectionActionType.Add
+CRT1.EntityType = SelectionType.GeoVertex
+CRT1.Criterion = SelectionCriterionType.LocationX
+CRT1.Operator = SelectionOperatorType.Equal
+CRT1.Value = Quantity("96.3 [mm]")
+GEN_CRT.Add(CRT1)
+NS_RESP_VERTEX.Activate()
+NS_RESP_VERTEX.Generate()
+
+# %%
+# Add and Define Premeshed Cyclic Region
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Add a symmetry region to the model to define the
+# cyclic symmetry boundary conditions.
+# The symmetry region is defined by specifying the
+# low and high boundary locations,the coordinate system,
+# and the number of sectors.
+# The symmetry region allows for the analysis of a smaller
+# portion of the model while accounting for the cyclic
+# nature of the full model.
+model = app.Model
+SYMM = model.AddSymmetry()
+SYMMETRY_REGION = SYMM.AddPreMeshedCyclicRegion()
+SYMMETRY_REGION.LowBoundaryLocation = NS_LOW
+SYMMETRY_REGION.HighBoundaryLocation = NS_HIGH
+SYMMETRY_REGION.CoordinateSystem = LCS1
+SYMMETRY_REGION.NumberOfSectors = 13
+
+# %%
+# Define Analysis
+# ~~~~~~~~~~~~~~~~~~~~
+# The analysis type is set to Modal, which is used to
+# determine the natural frequencies and mode shapes of the system.
+# The analysis is performed in a cyclic symmetry environment,
+# which allows for the analysis of a smaller portion of the
+# model while accounting for the cyclic nature of the full model.
+# The analysis is defined with a maximum of 2 modes to find
+# and a harmonic index range of 0 to 6.
+# The harmonic index is used to specify the frequency range for the analysis.
+# The analysis settings and solution settings are defined for the modal analysis.
+
+MODAL01 = model.AddModalAnalysis()
+
+# Solve first standalone Modal analysis
+ANA_SETTING_MODAL01 = model.Analyses[0].AnalysisSettings
+SOLN_MODAL01 = model.Analyses[0].Solution
+
+ANA_SETTING_MODAL01.MaximumModesToFind = 2
+ANA_SETTING_MODAL01.HarmonicIndexRange = CyclicHarmonicIndex.Manual
+ANA_SETTING_MODAL01.MaximumHarmonicIndex = 6
+
+# %%
+# Insert results
+# ~~~~~~~~~~~~~~~~
+# Insert results for the modal analysis.
+# The results include the total deformation, which is
+# used to visualize the mode shapes of the system.
+# The total deformation is calculated based on the modal analysis results.
+
+TOT_DEF_MODAL01 = SOLN_MODAL01.AddTotalDeformation()
+
+# %%
+# Solve Modal Analysis
+# ~~~~~~~~~~~~~~~~~~~~~
+# Solve the modal analysis to obtain the natural frequencies and mode shapes of the system.
+# The solution is performed for the specified number of modes and harmonic indices.
+# The results are stored in the solution object for further analysis and visualization.
+app.save_as(str(output_path / "before_solve_prestressed.mechdb"), overwrite=True)
+
+SOLN_MODAL01.Solve(True)
+SOLN_MODAL01_SS = SOLN_MODAL01.Status
+
+app.save_as(str(output_path / "after_solve_prestressed.mechdb"), overwrite=True)
+# sphinx_gallery_start_ignore
+assert str(SOLN_MODAL01_SS) == "Done", "Solution status is not 'Done'"
+# sphinx_gallery_end_ignore
+
+H0_FRQ1_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][0]
+H0_FRQ2_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][1]
+H1_FRQ1_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][2]
+H1_FRQ2_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][3]
+H2_FRQ1_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][4]
+H2_FRQ2_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][5]
+H3_FRQ1_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][6]
+H3_FRQ2_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][7]
+H4_FRQ1_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][8]
+H4_FRQ2_MODAL01 = TOT_DEF_MODAL01.TabularData["Frequency"][9]
+
+# %%
+# Add Static Structural Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# The static structural analysis is used to analyze
+# the response of the system under static loading conditions.
+# The analysis is performed in a cyclic symmetry environment,
+# which allows for the analysis of a smaller portion
+# of the model while accounting for the cyclic nature of the full model.
+# The analysis settings and solution settings are defined for the static structural analysis.
+# The analysis is set to be a linear static analysis, which means that the response of the system
+# is assumed to be linear with respect to the applied loads.
+
+STAT_STRUC01 = model.AddStaticStructuralAnalysis()
+ANA_SETTING_STAT_STRUC01 = Model.Analyses[1].AnalysisSettings
+SOLN_STAT_STRUC01 = Model.Analyses[1].Solution
+
+# %%
+# Apply Loads and Boundary Conditions
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Apply pressure, rotational velocity and thermal boundary conditions
+
+PRES_STAT_STRUC01 = STAT_STRUC01.AddPressure()
+PRES_STAT_STRUC01.Location = NS_PRES
+PRES_STAT_STRUC01.Magnitude.Output.DiscreteValues = [Quantity("20 [MPa]")]
+
+ROT_VEL_STAT_STRUC01 = STAT_STRUC01.AddRotationalVelocity()
+ROT_VEL_STAT_STRUC01.DefineBy = LoadDefineBy.Components
+ROT_VEL_STAT_STRUC01.CoordinateSystem = LCS1
+ROT_VEL_STAT_STRUC01.ZComponent.Output.DiscreteValues = [Quantity("3000 [rad sec^-1]")]
+
+THERM_COND_STRUC01 = STAT_STRUC01.AddThermalCondition()
+THERM_COND_STRUC01.Location = NS_BODIES
+THERM_COND_STRUC01.Magnitude.Output.DiscreteValues = [Quantity("50 [C]")]
+
+# %%
+# Add Modal to perform prestress modal analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Setup and solve prestress modal analysis
+# The prestress modal analysis is used to analyze the
+# response of the system under prestressed conditions.
+
+MODAL02 = model.AddModalAnalysis()
+Pre_Stress02 = MODAL02.Children[0]
+Pre_Stress02.PreStressICEnvironment = Model.Analyses[1]
+ANA_SETTING_MODAL02 = Model.Analyses[2].AnalysisSettings
+SOLN_MODAL02 = Model.Analyses[2].Solution
+
+ANA_SETTING_MODAL02.MaximumModesToFind = 2
+ANA_SETTING_MODAL02.HarmonicIndexRange = CyclicHarmonicIndex.Manual
+ANA_SETTING_MODAL02.MaximumHarmonicIndex = 6
+
+# %%
+# Insert results
+# ~~~~~~~~~~~~~~~~
+# Insert results for the prestress modal analysis.
+
+TOT_DEF_MODAL02 = SOLN_MODAL02.AddTotalDeformation()
+
+# %%
+# Solve Prestressed Modal Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Solve the prestress modal analysis to obtain
+# the natural frequencies and mode shapes of the
+# system under prestressed conditions.
+# The solution is performed for the specified number
+# of modes and harmonic indices.
+# The results are stored in the solution object for
+# further analysis and visualization.
+
+SOLN_MODAL02.Solve(True)
+SOLN_MODAL02_SS = SOLN_MODAL02.Status
+# sphinx_gallery_start_ignore
+assert str(SOLN_MODAL02_SS) == "Done", "Solution status is not 'Done'"
+# sphinx_gallery_end_ignore
+
+H0_FRQ1_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][0]
+H0_FRQ2_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][1]
+H1_FRQ1_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][2]
+H1_FRQ2_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][3]
+H2_FRQ1_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][4]
+H2_FRQ2_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][5]
+H3_FRQ1_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][6]
+H3_FRQ2_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][7]
+H4_FRQ1_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][8]
+H4_FRQ2_MODAL02 = TOT_DEF_MODAL02.TabularData["Frequency"][9]
+
+# %%
+# Add Static Structural to perform Non-linear Static Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Setup Non-linear Static Structural Analysis
+# The non-linear static analysis is used to analyze the
+# response of the system under non-linear loading conditions.
+STAT_STRUC02 = model.AddStaticStructuralAnalysis()
+ANA_SETTING_STAT_STRUC02 = Model.Analyses[3].AnalysisSettings
+SOLN_STAT_STRUC02 = Model.Analyses[3].Solution
+
+# %%
+# Turn on large deflection option
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# This option is required for the non-linear static
+# analysis to account for large displacements and rotations.
+
+ANA_SETTING_STAT_STRUC02.LargeDeflection = True
+
+# %%
+# Apply Loads and Boundary Conditions
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Apply pressure, rotational velocity and thermal boundary conditions
+
+PRES_STAT_STRUC02 = STAT_STRUC02.AddPressure()
+PRES_STAT_STRUC02.Location = NS_PRES
+PRES_STAT_STRUC02.Magnitude.Output.DiscreteValues = [Quantity("20 [MPa]")]
+
+ROT_VEL_STAT_STRUC02 = STAT_STRUC02.AddRotationalVelocity()
+ROT_VEL_STAT_STRUC02.DefineBy = LoadDefineBy.Components
+ROT_VEL_STAT_STRUC02.CoordinateSystem = LCS1
+ROT_VEL_STAT_STRUC02.ZComponent.Output.DiscreteValues = [Quantity("6000 [rad sec^-1]")]
+
+THERM_COND_STRUC02 = STAT_STRUC02.AddThermalCondition()
+THERM_COND_STRUC02.Location = NS_BODIES
+THERM_COND_STRUC02.Magnitude.Output.DiscreteValues = [Quantity("50 [C]")]
+
+# %%
+# Add modal to perform prestress modal analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Setup and solve modal with prestress from non-linear static analysis
+
+MODAL03 = model.AddModalAnalysis()
+Pre_Stress03 = MODAL03.Children[0]
+Pre_Stress03.PreStressICEnvironment = Model.Analyses[3]
+ANA_SETTING_MODAL03 = Model.Analyses[4].AnalysisSettings
+SOLN_MODAL03 = Model.Analyses[4].Solution
+
+ANA_SETTING_MODAL03.MaximumModesToFind = 2
+ANA_SETTING_MODAL03.HarmonicIndexRange = CyclicHarmonicIndex.Manual
+ANA_SETTING_MODAL03.MaximumHarmonicIndex = 6
+
+# %%
+# Insert results
+# ~~~~~~~~~~~~~~~~
+# Insert results for the prestress modal analysis.
+# The results include the total deformation, which is used to
+# visualize the mode shapes of the system.
+
+TOT_DEF_MODAL03 = SOLN_MODAL03.AddTotalDeformation()
+
+# %%
+# Solve Prestressed Modal Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Solve the prestress modal analysis to obtain the natural
+# frequencies and mode shapes of the system under prestressed conditions.
+# The solution is performed for the specified number of modes and harmonic indices.
+# The results are stored in the solution object for further analysis and visualization.
+
+SOLN_MODAL03.Solve(True)
+SOLN_MODAL03_SS = SOLN_MODAL03.Status
+# sphinx_gallery_start_ignore
+assert str(SOLN_MODAL03_SS) == "Done", "Solution status is not 'Done'"
+# sphinx_gallery_end_ignore
+
+H0_FRQ1_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][0]
+H0_FRQ2_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][1]
+H1_FRQ1_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][2]
+H1_FRQ2_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][3]
+H2_FRQ1_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][4]
+H2_FRQ2_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][5]
+H3_FRQ1_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][6]
+H3_FRQ2_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][7]
+H4_FRQ1_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][8]
+H4_FRQ2_MODAL03 = TOT_DEF_MODAL03.TabularData["Frequency"][9]
+
+# %%
+# Add Harmonic Response Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Setup and Solve Standalone FULL Harmonic Analysis
+# The harmonic response analysis is used to analyze the
+# response of the system under harmonic loading conditions.
+
+HARM_RESP01 = model.AddHarmonicResponseAnalysis()
+ANA_SETTING_HARM_RESP01 = Model.Analyses[5].AnalysisSettings
+SOLN_HARM_RESP01 = Model.Analyses[5].Solution
+
+# %%
+# Specify the frequency range for the harmonic response analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+ANA_SETTING_HARM_RESP01.RangeMinimum = Quantity("1200 [Hz]")
+ANA_SETTING_HARM_RESP01.RangeMaximum = Quantity("5500 [Hz]")
+ANA_SETTING_HARM_RESP01.SolutionIntervals = 10
+
+# %%
+# Specify Full Harmonic Response Analysis Method
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# The full harmonic response analysis method is used to
+# analyze the response of the system under harmonic loading conditions.
+# The method is specified as Full, which means that the analysis
+# will consider the full frequency range specified above.
+
+ANA_SETTING_HARM_RESP01.SolutionMethod = HarmonicMethod.Full
+
+# %%
+# Apply Structural Damping Coefficient
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Structural damping coefficient is used to account for
+# energy dissipation in the material during dynamic loading.
+
+ANA_SETTING_HARM_RESP01.StructuralDampingCoefficient = 0.02
+
+# %%
+# Apply Loads and Boundary Conditions
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Apply Pressure
+
+PRES_HARM_RESP01 = HARM_RESP01.AddPressure()
+PRES_HARM_RESP01.Location = NS_PRES
+PRES_HARM_RESP01.Magnitude.Output.DiscreteValues = [Quantity("20 [MPa]")]
+
+# %%
+# Insert results
+# ~~~~~~~~~~~~~~~
+# Insert results for the harmonic response analysis.
+# The results include the total deformation, which is used to visualize
+# the response of the system under harmonic loading conditions.
+# The total deformation is calculated based on the harmonic response analysis..
+# The results are stored in the solution object for further analysis and visualization.
+
+FRQ_RES_DEF_HARM_RESP01 = SOLN_HARM_RESP01.AddDeformationFrequencyResponse()
+FRQ_RES_DEF_HARM_RESP01.Location = NS_RESP_VERTEX
+FRQ_RES_DEF_HARM_RESP01.NormalOrientation = NormalOrientationType.YAxis
+
+SOLN_HARM_RESP01.Activate()
+TOT_DEF4_1 = SOLN_HARM_RESP01.AddTotalDeformation()
+TOT_DEF4_1.Frequency = Quantity(3000, "Hz")
+TOT_DEF4_1.Amplitude = True
+TOT_DEF4_1.Name = "Total Deformation"
+TOT_DEF4_1.CreateParameter("Maximum")
+
+SOLN_HARM_RESP01.Activate()
+TOT_DEF4_2 = SOLN_HARM_RESP01.AddTotalDeformation()
+TOT_DEF4_2.Frequency = Quantity(2500, "Hz")
+TOT_DEF4_2.Amplitude = True
+TOT_DEF4_2.Name = "Total Deformation 2"
+TOT_DEF4_2.CreateParameter("Maximum")
+
+# %%
+# Solve Full Harmonic Response Analysis
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+# Solve the full harmonic response analysis to obtain the frequency response of the system.
+
+SOLN_HARM_RESP01.Solve(True)
+SOLN_HARM_RESP01_SS = SOLN_HARM_RESP01.Status
+# sphinx_gallery_start_ignore
+assert str(SOLN_HARM_RESP01_SS) == "Done", "Solution status is not 'Done'"
+# sphinx_gallery_end_ignore
+
+# %%
+# Post-process results
+# ~~~~~~~~~~~~~~~~~~~~~~~~
+# Activate the results and set the view to isometric
+
+TOT_DEF4_1.Activate()
+camera.SetFit()
+camera.SetFit()
+graphics.ExportImage(
+    str(output_path / "deform_frequency_response.png"),
+    image_export_format,
+    settings_720p,
+)
+display_image("deform_frequency_response.png")
+
+app.save_as(str(output_path / "final.mechdb"), overwrite=True)
+
+
+# Close the app
+app.close()
+
+# delete example file
+delete_downloads()