Mesh generation

This example shows how to generate a mesh from a CAD model. The CAD model is imported from a file, and the mesh is generated using the Ansys PRIME API.

import os
from pathlib import Path

from ansys.meshing import prime
from ansys.meshing.prime.graphics import Graphics

Parameters for the script

The following parameters are used to control the script execution. You can modify these parameters to suit your needs.

GRAPHICS_BOOL = False  # Set to True to display the graphics
OUTPUT_DIR = Path(Path(__file__).parent, "outputs")  # Output directory

Start a PRIME session

Start a PRIME session and get the model from the client.

prime_client = prime.launch_prime(timeout=120)
print(prime_client)

# Get the model from the client
model = prime_client.model

<ansys.meshing.prime.internals.client.Client object at 0x7f8e04304c80>

Load the CAD file

Load the CAD file from the previous example. The file is loaded into the model, and the part is extracted. The part is then summarized to get the details of the part.

# Load the FMD file
modeling_file = Path(OUTPUT_DIR, "modeling_demo.fmd")
file_io = prime.FileIO(model)
file_io.import_cad(
    file_name=modeling_file,
    params=prime.ImportCadParams(
        model=model,
    ),
)

# Review the part
part = model.get_part_by_name("modelingdemo")
part_summary_res = part.get_summary(prime.PartSummaryParams(model, print_mesh=False))
print(part_summary_res)

if GRAPHICS_BOOL:
    display = Graphics(model=model)
    display()

Static Scene

Interactive Scene

message :
Part Name: modelingdemo
Part ID: 2
    32 Topo Edges
    14 Topo Faces
    1 Topo Volumes

    0 Edge Zones
        Edge Zone Name(s) : []
    0 Face Zones
        Face Zone Name(s) : []
    1 Volume Zones
        Volume Zone Name(s) : [design_body]

    0 Label(s)
        Names: []

    Bounding box (-40 -50 0)
                 (40 50 10)
n_topo_edges :  32
n_topo_faces :  14
n_topo_volumes :  1
n_edge_zonelets :  0
n_face_zonelets :  0
n_cell_zonelets :  0
n_edge_zones :  0
n_face_zones :  0
n_volume_zones :  1
n_labels :  0
n_nodes :  0
n_faces :  0
n_cells :  0
n_tri_faces :  0
n_poly_faces :  0
n_quad_faces :  0
n_tet_cells :  0
n_pyra_cells :  0
n_prism_cells :  0
n_poly_cells :  0
n_hex_cells :  0
n_unmeshed_topo_faces :  0
/opt/hostedtoolcache/Python/3.12.7/x64/lib/python3.12/site-packages/pyvista/core/pointset.py:1365: PyVistaDeprecationWarning: The current behavior of `pv.PolyData.n_faces` has been deprecated.
                Use `pv.PolyData.n_cells` or `pv.PolyData.n_faces_strict` instead.
                See the documentation in '`pv.PolyData.n_faces` for more information.
  warnings.warn(

Mesh generation

The mesh is generated using the Ansys PRIME API. The mesh is generated using the following steps:

1. Initialize the connection tolerance and other parameters.

2. Scaffold the part.

3. Mesh the surfaces.

4. Write the mesh to a file.

# Initialize the connection tolerance and other parameters --
#
# Target element size
element_size = 0.5

# Initialize the parameters
params = prime.ScaffolderParams(
    model,
    absolute_dist_tol=0.1 * element_size,
    intersection_control_mask=prime.IntersectionMask.FACEFACEANDEDGEEDGE,
    constant_mesh_size=element_size,
)

# Get existing topoface or topoedge IDs
faces = part.get_topo_faces()
beams = []

scaffold_res = prime.Scaffolder(model, part.id).scaffold_topo_faces_and_beams(
    topo_faces=faces, topo_beams=beams, params=params
)
print(scaffold_res)

n_incomplete_topo_faces :  0
error_code :  0

Surface meshing

The surface mesh is generated using the previous element size and the topological faces of the part.

surfer_params = prime.SurferParams(
    model=model,
    size_field_type=prime.SizeFieldType.CONSTANT,
    constant_size=element_size,
    generate_quads=True,
)

surfer_result = prime.Surfer(model).mesh_topo_faces(part.id, topo_faces=faces, params=surfer_params)

# Display the mesh
if GRAPHICS_BOOL:
    display = Graphics(model=model)
    display()

Static Scene

Interactive Scene

Export the mesh

The mesh is exported to a CDB file. The CDB file can be used to create a MAPDL case.

mapdl_cdb = Path(OUTPUT_DIR, "modeling_demo.cdb")
file_io.export_mapdl_cdb(mapdl_cdb, params=prime.ExportMapdlCdbParams(model))
assert os.path.exists(mapdl_cdb)
print(f"MAPDL case exported at {mapdl_cdb}")

This get_abaqus_simulation_data is a beta API. The behavior and implementation may change in future.
MAPDL case exported at /home/runner/work/pyansys-workflows/pyansys-workflows/geometry-mesh/outputs/modeling_demo.cdb

Close the PRIME session

Close the PRIME session to release the resources. This is important to prevent memory leaks.

prime_client.exit()