.. DO NOT EDIT.
.. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY.
.. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE:
.. "examples/basic/example_09_tracemapping.py"
.. LINE NUMBERS ARE GIVEN BELOW.

.. only:: html

    .. note::
        :class: sphx-glr-download-link-note

        :ref:`Go to the end <sphx_glr_download_examples_basic_example_09_tracemapping.py>`
        to download the full example code.

.. rst-class:: sphx-glr-example-title

.. _sphx_glr_examples_basic_example_09_tracemapping.py:

.. _ref_example_09:

Trace Mapping Example
---------------------

Using the provided file, this example demonstrates how to
import trace map data into a static structural analysis of
a new Mechanical session and execute a sequence of
Python scripting commands to mesh the model and export an image.

.. GENERATED FROM PYTHON SOURCE LINES 13-15

Import necessary libraries
~~~~~~~~~~~~~~~~~~~~~~~~~~

.. GENERATED FROM PYTHON SOURCE LINES 15-23

.. code-block:: Python


    import os

    from ansys.mechanical.core import launch_mechanical
    from ansys.mechanical.core.examples import download_file
    from matplotlib import image as mpimg
    from matplotlib import pyplot as plt








.. GENERATED FROM PYTHON SOURCE LINES 24-29

Launch mechanical
~~~~~~~~~~~~~~~~~
Launch a new Mechanical session in batch, setting ``cleanup_on_exit`` to
``False``. To close this Mechanical session when finished, this example
must call  the ``mechanical.exit()`` method.

.. GENERATED FROM PYTHON SOURCE LINES 29-34

.. code-block:: Python


    mechanical = launch_mechanical(batch=True, cleanup_on_exit=False)
    print(mechanical)






.. rst-class:: sphx-glr-script-out

 .. code-block:: none

    Ansys Mechanical [Ansys Mechanical Enterprise]
    Product Version:242
    Software build date: 06/03/2024 09:35:09





.. GENERATED FROM PYTHON SOURCE LINES 35-38

Download the required files
~~~~~~~~~~~~~~~~~~~~~~~~~~~
Download files and print path

.. GENERATED FROM PYTHON SOURCE LINES 38-69

.. code-block:: Python


    all_input_files = {
        "geometry_file_name": "example_09_pcb.agdb",
        "def_file": "example_09_edb.def",
        "copper_alloy_material_file": "example_09_mat_copper_alloy.xml",
        "fr4_material_file": "example_09_mat_fr4.xml",
    }

    project_directory = mechanical.project_directory
    print(f"project directory = {project_directory}")

    for file_type, file_name in all_input_files.items():
        file_path = download_file(file_name, "pymechanical", "00_basic")

        print(f"Downloaded the {file_type} to: {file_path}")

        # Upload the file to the project directory.
        mechanical.upload(file_name=file_path, file_location_destination=project_directory)

        # Build the path relative to project directory.
        base_name = os.path.basename(file_path)
        combined_path = os.path.join(project_directory, base_name)
        part_file_path = combined_path.replace("\\", "\\\\")
        mechanical.run_python_script(f"{file_type} = '{part_file_path}'")
        result = mechanical.run_python_script(f"{file_type}")
        print(f"path of {file_type} on server: {result}")


    png_image_name = "myplot.png"
    mechanical.run_python_script(f"image_name='{png_image_name}'")





.. rst-class:: sphx-glr-script-out

 .. code-block:: none

    project directory = /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/
    Downloaded the geometry_file_name to: /home/runner/.local/share/ansys_mechanical_core/examples/example_09_pcb.agdb

    Uploading example_09_pcb.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.:   0%|          | 0.00/2.27M [00:00<?, ?B/s]
    Uploading example_09_pcb.agdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.: 100%|██████████| 2.27M/2.27M [00:00<00:00, 241MB/s]
    path of geometry_file_name on server: /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/example_09_pcb.agdb
    Downloaded the def_file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_09_edb.def

    Uploading example_09_edb.def to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.:   0%|          | 0.00/1.31M [00:00<?, ?B/s]
    Uploading example_09_edb.def to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.: 100%|██████████| 1.31M/1.31M [00:00<00:00, 613MB/s]
    path of def_file on server: /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/example_09_edb.def
    Downloaded the copper_alloy_material_file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_09_mat_copper_alloy.xml

    Uploading example_09_mat_copper_alloy.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.:   0%|          | 0.00/18.1k [00:00<?, ?B/s]
    Uploading example_09_mat_copper_alloy.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.: 100%|██████████| 18.1k/18.1k [00:00<00:00, 57.9MB/s]
    path of copper_alloy_material_file on server: /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/example_09_mat_copper_alloy.xml
    Downloaded the fr4_material_file to: /home/runner/.local/share/ansys_mechanical_core/examples/example_09_mat_fr4.xml

    Uploading example_09_mat_fr4.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.:   0%|          | 0.00/15.6k [00:00<?, ?B/s]
    Uploading example_09_mat_fr4.xml to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/.: 100%|██████████| 15.6k/15.6k [00:00<00:00, 57.0MB/s]
    path of fr4_material_file on server: /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/example_09_mat_fr4.xml

    ''



.. GENERATED FROM PYTHON SOURCE LINES 70-74

Run the script
~~~~~~~~~~~~~~
Run the Mechanical script to attach the geometry and set up and solve the
analysis.

.. GENERATED FROM PYTHON SOURCE LINES 74-236

.. code-block:: Python


    output = mechanical.run_python_script(
        """
    import os


    # Imports a geometry file into the active model.

    geometry_import = Model.GeometryImportGroup.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_preferences.NamedSelectionKey = "NS"
    geometry_import.Import(
        geometry_file_name, geometry_import_format, geometry_import_preferences
    )


    print("geometry import : Done ")

    # Insert a Static Structural Analysis

    analysis = Model.AddStaticStructuralAnalysis()
    print(analysis)

    ExtAPI.DataModel.Project.UnitSystem = UserUnitSystemType.StandardNMM

    # Import Materials

    materials = ExtAPI.DataModel.Project.Model.Materials
    materials.Import(copper_alloy_material_file)
    materials.Import(fr4_material_file)


    # create lists of body ids to create named selections later

    board_bodyids = []
    component_bodyids = []
    geo = ExtAPI.DataModel.GeoData
    mesh = ExtAPI.DataModel.Project.Model.Mesh
    for asm in geo.Assemblies:
        for part in asm.Parts:
            for body in part.Bodies:
                if body.Name[:9] != "Component":
                    board_bodyids.append(body.Id)
                else:
                    component_bodyids.append(body.Id)

    # Assign  Materials based on Body Names

    parts = ExtAPI.DataModel.Project.Model.Geometry.Children  # list of parts
    for part in parts:
        for body in part.Children:
            body.Material = "Copper Alloy" if body.Name[:9] == "Component" else "FR-4"


    # Function to create named selection from list of body ids

    def create_named_selection_from_id_list(ns_name, list_of_body_ids):

        selection_manager = ExtAPI.SelectionManager
        selection = ExtAPI.SelectionManager.CreateSelectionInfo(
            SelectionTypeEnum.GeometryEntities
        )
        selection.Ids = list_of_body_ids
        selection_manager.NewSelection(selection)

        model = ExtAPI.DataModel.Project.Model
        named_sel = model.AddNamedSelection()
        named_sel.Name = ns_name
        named_sel.Location = selection
        selection_manager.ClearSelection()


    create_named_selection_from_id_list("board_layers", board_bodyids)
    create_named_selection_from_id_list("components", component_bodyids)

    # make a selection to be used with mesh methods

    selection_manager = ExtAPI.SelectionManager
    selection = ExtAPI.SelectionManager.CreateSelectionInfo(
        SelectionTypeEnum.GeometryEntities
    )
    selection.Ids = board_bodyids
    selection_manager.NewSelection(selection)

    mesh = ExtAPI.DataModel.Project.Model.Mesh

    mesh_method = mesh.AddAutomaticMethod()
    mesh_method.Location = selection
    mesh_method.Method = MethodType.Sweep
    mesh_method.ElementOrder = ElementOrder.Linear
    mesh_method.SweepNumberDivisions = 1

    mesh_sizing = mesh.AddSizing()
    mesh_sizing.ElementSize = Quantity("0.25 [mm]")
    mesh.GenerateMesh()


    # Defining External Data Object  for Importing Trace

    external_data_files = Ansys.Mechanical.ExternalData.ExternalDataFileCollection()
    external_data_files.SaveFilesWithProject = True
    external_data_file = Ansys.Mechanical.ExternalData.ExternalDataFile()
    external_data_files.Add(external_data_file)  # Single File
    external_data_file.Identifier = "edb"
    external_data_file.Description = ""
    external_data_file.IsMainFile = False
    external_data_file.FilePath = def_file
    external_data_file.ImportSettings = (
        Ansys.Mechanical.ExternalData.ImportSettingsFactory.GetSettingsForFormat(
            Ansys.Mechanical.DataModel.MechanicalEnums.ExternalData.ImportFormat.ECAD
        )
    )
    import_settings = external_data_file.ImportSettings
    import_settings.UseDummyNetData = False
    imported_trace_group = Model.Materials.AddImportedTraceExternalData()
    imported_trace_group.ImportExternalDataFiles(external_data_files)

    allImpTraces = ExtAPI.DataModel.GetObjectsByType(
        Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.ImportedTrace
    )

    imp_trace = [
        x for x in allImpTraces if x.Parent.ObjectId == imported_trace_group.ObjectId
    ][0]
    imp_trace.Activate()
    # imp_trace.InternalObject.GeometryDefineBy = 1

    NSall = ExtAPI.DataModel.Project.Model.NamedSelections.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    ns_object = [i for i in NSall if i.Name == "board_layers"][0]
    imp_trace.Location = ns_object
    imp_trace.PropertyByName("PROPID_ExternalData").InternalValue = 1


    layers = imp_trace.Layers
    num_layers = layers.Count
    for layer in layers:
        layer["Trace Material"] = "Copper Alloy"
    vias = imp_trace.Vias
    num_vias = vias.Count
    for via in vias:
        via["Plating Material"] = "Copper Alloy"
    imp_trace.Import()


    # Exporting trace map snapshot to a png file

    Graphics.Camera.SetFit()
    set2d = Ansys.Mechanical.Graphics.GraphicsImageExportSettings()
    set2d.CurrentGraphicsDisplay = False
    mechdir = ExtAPI.DataModel.AnalysisList[0].WorkingDir
    png_file_path = os.path.join(mechdir, image_name)
    Graphics.ExportImage(png_file_path, GraphicsImageExportFormat.PNG, set2d)

    """
    )








.. GENERATED FROM PYTHON SOURCE LINES 237-241

Initialize the variable needed for the image directory
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Set the ``image_dir`` for later use.
Make the variable compatible for Windows, Linux, and Docker containers.

.. GENERATED FROM PYTHON SOURCE LINES 241-246

.. code-block:: Python


    mechanical.run_python_script(f"image_dir=ExtAPI.DataModel.AnalysisList[0].WorkingDir")
    result_image_dir_server = mechanical.run_python_script(f"image_dir")
    print(f"Images are stored on the server at: {result_image_dir_server}")





.. rst-class:: sphx-glr-script-out

 .. code-block:: none

    Images are stored on the server at: /tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/StaticStructural/




.. GENERATED FROM PYTHON SOURCE LINES 247-251

Download the image and plot
~~~~~~~~~~~~~~~~~~~~~~~~~~~
Download one image file from the server to the current working directory and plot
using matplotlib

.. GENERATED FROM PYTHON SOURCE LINES 251-280

.. code-block:: Python



    def get_image_path(image_name):
        return os.path.join(result_image_dir_server, image_name)


    def display_image(path):
        print(f"Printing {path} using matplotlib")
        image1 = mpimg.imread(path)
        plt.figure(figsize=(15, 15))
        plt.axis("off")
        plt.imshow(image1)
        plt.show()


    image_path_server = get_image_path(png_image_name)

    if image_path_server != "":
        current_working_directory = os.getcwd()

        local_file_path_list = mechanical.download(
            image_path_server, target_dir=current_working_directory
        )
        image_local_path = local_file_path_list[0]
        print(f"Local image path : {image_local_path}")

        display_image(image_local_path)





.. image-sg:: /examples/basic/images/sphx_glr_example_09_tracemapping_001.png
   :alt: example 09 tracemapping
   :srcset: /examples/basic/images/sphx_glr_example_09_tracemapping_001.png
   :class: sphx-glr-single-img


.. rst-class:: sphx-glr-script-out

 .. code-block:: none


    Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/StaticStructural/myplot.png to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/myplot.png:   0%|          | 0.00/36.4k [00:00<?, ?B/s]
    Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech8C1A/Project_Mech_Files/StaticStructural/myplot.png to /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/myplot.png: 100%|██████████| 36.4k/36.4k [00:00<00:00, 188MB/s]
    Local image path : /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/myplot.png
    Printing /home/runner/work/pymechanical-examples/pymechanical-examples/examples/basic/myplot.png using matplotlib




.. GENERATED FROM PYTHON SOURCE LINES 281-284

Close mechanical
~~~~~~~~~~~~~~~~
Close the mechanical instance.

.. GENERATED FROM PYTHON SOURCE LINES 284-288

.. code-block:: Python


    print("Closing mechanical...")
    mechanical.exit()
    print("Mechanical closed!")




.. rst-class:: sphx-glr-script-out

 .. code-block:: none

    Closing mechanical...
    Mechanical closed!





.. rst-class:: sphx-glr-timing

   **Total running time of the script:** (1 minutes 5.719 seconds)


.. _sphx_glr_download_examples_basic_example_09_tracemapping.py:

.. only:: html

  .. container:: sphx-glr-footer sphx-glr-footer-example

    .. container:: sphx-glr-download sphx-glr-download-jupyter

      :download:`Download Jupyter notebook: example_09_tracemapping.ipynb <example_09_tracemapping.ipynb>`

    .. container:: sphx-glr-download sphx-glr-download-python

      :download:`Download Python source code: example_09_tracemapping.py <example_09_tracemapping.py>`

    .. container:: sphx-glr-download sphx-glr-download-zip

      :download:`Download zipped: example_09_tracemapping.zip <example_09_tracemapping.zip>`


.. only:: html

 .. rst-class:: sphx-glr-signature

    `Gallery generated by Sphinx-Gallery <https://sphinx-gallery.github.io>`_