Remote & Embedding Example

This code, which uses the same example, first demonstrates how to use a remote session and then demonstrates how to use an embedding instance.

Remote Session

Download required files

Download the required files. Print the file paths for the geometry file and script file.

import os

from ansys.mechanical.core import launch_mechanical
from ansys.mechanical.core.examples import download_file

geometry_path = download_file("Valve.pmdb", "pymechanical", "embedding")
print(f"Downloaded the geometry file to: {geometry_path}")

script_file_path = download_file("remote_script.py", "pymechanical", "embedding")
print(f"Downloaded the script file to: {script_file_path}")

Downloaded the geometry file to: /github/home/.local/share/ansys_mechanical_core/examples/Valve.pmdb
Downloaded the script file to: /github/home/.local/share/ansys_mechanical_core/examples/remote_script.py

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.

import os

from ansys.mechanical.core import launch_mechanical

# Launch mechanical
mechanical = launch_mechanical(batch=True, loglevel="DEBUG")
print(mechanical)

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

Initialize variable for workflow

Set the part_file_path variable on the server for later use. Make this variable compatible for Windows, Linux, and Docker containers.

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

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

# Build the path relative to project directory.
base_name = os.path.basename(geometry_path)
combined_path = os.path.join(project_directory, base_name)
part_file_path = combined_path.replace("\\", "\\\\")
mechanical.run_python_script(f"part_file_path='{part_file_path}'")

# Verify the path
result = mechanical.run_python_script("part_file_path")
print(f"part_file_path on server: {result}")

project directory = /tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/

Uploading Valve.pmdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/.:   0%|          | 0.00/774k [00:00<?, ?B/s]
Uploading Valve.pmdb to dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/.: 100%|██████████| 774k/774k [00:00<00:00, 285MB/s]
part_file_path on server: /tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/Valve.pmdb

Run mechanical automation script

Run remote_script.py in the mechanical remote session.

mechanical.run_python_script_from_file(script_file_path)

''

Get list of generated files

list_files = mechanical.list_files()
for file in list_files:
    print(file)

/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file.mechdb
/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/.mech_lock
/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/MatML.xml
/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERep.xml
/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/ds.dat
/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERepOutput.xml

Write the file contents to console

def write_file_contents_to_console(path, number_lines=-1):
    count = 1
    with open(path, "rt") as file:
        for line in file:
            if number_lines == -1 or count <= number_lines:
                print(line, end="")
                count = count + 1
            else:
                break

Download files back to local working directory

dest_dir = "download"
dest_dir = os.path.join(os.getcwd(), dest_dir)
for file in list_files:
    downloaded = mechanical.download(file, target_dir=dest_dir)
    if file.endswith(".out"):
        print("contents of ", downloaded, " : ")
        write_file_contents_to_console(downloaded[0], number_lines=-1)

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file.mechdb to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/file.mechdb:   0%|          | 0.00/7.06M [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file.mechdb to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/file.mechdb: 100%|██████████| 7.06M/7.06M [00:00<00:00, 207MB/s]

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/.mech_lock to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/.mech_lock:   0%|          | 0.00/17.0 [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/.mech_lock to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/.mech_lock: 100%|██████████| 17.0/17.0 [00:00<00:00, 50.9kB/s]

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/MatML.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/MatML.xml:   0%|          | 0.00/23.3k [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/MatML.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/MatML.xml: 100%|██████████| 23.3k/23.3k [00:00<00:00, 31.8MB/s]

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERep.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/CAERep.xml:   0%|          | 0.00/28.1k [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERep.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/CAERep.xml: 100%|██████████| 28.1k/28.1k [00:00<00:00, 64.1MB/s]

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/ds.dat to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/ds.dat:   0%|          | 0.00/4.85M [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/ds.dat to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/ds.dat: 100%|██████████| 4.85M/4.85M [00:00<00:00, 292MB/s]

Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERepOutput.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/CAERepOutput.xml:   0%|          | 0.00/862 [00:00<?, ?B/s]
Downloading dns:///127.0.0.1:10000:/tmp/ANSYS.root.1/AnsysMech4174/Project_Mech_Files/file_Mech_Files/StaticStructural/CAERepOutput.xml to /__w/pymechanical/pymechanical/examples/embedding_n_remote/download/CAERepOutput.xml: 100%|██████████| 862/862 [00:00<00:00, 2.71MB/s]

Exit remote session

Close the Mechanical instance.

mechanical.exit()

Embedded Instance

Download the geometry file

Download Valve.pmdb.

import os

import ansys.mechanical.core as mech
from ansys.mechanical.core.examples import download_file

geometry_path = download_file("Valve.pmdb", "pymechanical", "embedding")
print(f"Downloaded the geometry file to: {geometry_path}")

Downloaded the geometry file to: /github/home/.local/share/ansys_mechanical_core/examples/Valve.pmdb

Embed Mechanical and set global variables

Find the mechanical installation path & version. Open an embedded instance of Mechanical and set global variables.

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

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

Add Static Analysis

Add static analysis to the Model.

analysis = Model.AddStaticStructuralAnalysis()

Import geometry

geometry_file = geometry_path
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.Import(geometry_file, geometry_import_format, geometry_import_preferences)

Assign material

matAssignment = Model.Materials.AddMaterialAssignment()
tempSel = ExtAPI.SelectionManager.CreateSelectionInfo(
    Ansys.ACT.Interfaces.Common.SelectionTypeEnum.GeometryEntities
)
bodies = [
    body
    for body in ExtAPI.DataModel.Project.Model.Geometry.GetChildren(
        Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Body, True
    )
]
geobodies = [body.GetGeoBody() for body in bodies]
ids = System.Collections.Generic.List[System.Int32]()
[ids.Add(item.Id) for item in geobodies]
tempSel.Ids = ids
matAssignment.Location = tempSel
matAssignment.Material = "Structural Steel"

Define mesh settings

mesh = Model.Mesh
mesh.ElementSize = Quantity("25 [mm]")
mesh.GenerateMesh()

Define boundary conditions

fixedSupport = analysis.AddFixedSupport()
fixedSupport.Location = ExtAPI.DataModel.GetObjectsByName("NSFixedSupportFaces")[0]

frictionlessSupport = analysis.AddFrictionlessSupport()
frictionlessSupport.Location = ExtAPI.DataModel.GetObjectsByName("NSFrictionlessSupportFaces")[0]

pressure = analysis.AddPressure()
pressure.Location = ExtAPI.DataModel.GetObjectsByName("NSInsideFaces")[0]

inputs_quantities = [Quantity("0 [s]"), Quantity("1 [s]")]
output_quantities = [Quantity("0 [Pa]"), Quantity("15 [MPa]")]

inputs_quantities_2 = System.Collections.Generic.List[Ansys.Core.Units.Quantity]()
[inputs_quantities_2.Add(item) for item in inputs_quantities]

output_quantities_2 = System.Collections.Generic.List[Ansys.Core.Units.Quantity]()
[output_quantities_2.Add(item) for item in output_quantities]

pressure.Magnitude.Inputs[0].DiscreteValues = inputs_quantities_2
pressure.Magnitude.Output.DiscreteValues = output_quantities_2

Solve model

Model.Solve()

Add results

solution = analysis.Solution
solution.AddTotalDeformation()
solution.AddEquivalentStress()
solution.EvaluateAllResults()

Save model

project_directory = ExtAPI.DataModel.Project.ProjectDirectory
print(f"project directory = {project_directory}")
ExtAPI.DataModel.Project.SaveAs(os.path.join(project_directory, "file.mechdb"))

project directory = /tmp/ANSYS.root.1/AnsysMech0E91/Project_Mech_Files/

Export result values to a text file

fileExtension = r".txt"
results = solution.GetChildren(
    Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Result, True
)

for result in results:
    fileName = str(result.Name)
    print(f"filename: {fileName}")
    path = os.path.join(project_directory, fileName + fileExtension)
    print(path)
    result.ExportToTextFile(f"{path}")
    print("Exported Text file Contents", path)
    try:
        write_file_contents_to_console(path, number_lines=20)
    except:
        print(os.listdir(project_directory))

app.close()

filename: Total Deformation
/tmp/ANSYS.root.1/AnsysMech0E91/Project_Mech_Files/Total Deformation.txt
Exported Text file Contents /tmp/ANSYS.root.1/AnsysMech0E91/Project_Mech_Files/Total Deformation.txt
['file_Mech_Files', 'file.mechdb']
filename: Equivalent Stress
/tmp/ANSYS.root.1/AnsysMech0E91/Project_Mech_Files/Equivalent Stress.txt
Exported Text file Contents /tmp/ANSYS.root.1/AnsysMech0E91/Project_Mech_Files/Equivalent Stress.txt
['file_Mech_Files', 'file.mechdb']