Run blockMesh and checkMesh from Python¶

Build a mesh from system/blockMeshDict with pybFoam.meshing.generate_blockmesh() and inspect it with pybFoam.meshing.checkMesh(). Both are direct bindings of the OpenFOAM utilities — the returned fvMesh is a regular mesh that can be used immediately for field access, sampling, or further checks.

Prerequisite: OpenFOAM v2312+ sourced; pybFoam installed.

Prepare a working case¶

pybFoam.clone_example() copies the named example into a tmp directory so the baseline under examples/ stays pristine.

from pybFoam import Time, argList, clone_example, dictionary
from pybFoam.meshing import checkMesh, generate_blockmesh

case = clone_example("case")
print(f"working case: {case}")

working case: /tmp/pybfoam_q4adtry1/case

Generate the mesh¶

time = Time(argList([str(case), "-case", str(case)]))
mesh = generate_blockmesh(time, dictionary.read(str(case / "system" / "blockMeshDict")))

print(f"nCells  = {mesh.nCells()}")
print(f"nFaces  = {mesh.nFaces()}")
print(f"nPoints = {mesh.nPoints()}")

nCells  = 2268
nFaces  = 9176
nPoints = 4746

Inspect mesh quality¶

checkMesh returns a structured dict with mesh_stats, cell_types, topology, geometry, quality, passed, failed, and total_errors. Select the flags you want — here we run the topology + geometry checks.

result = checkMesh(
    mesh,
    check_topology=True,
    all_topology=True,
    all_geometry=True,
    check_quality=False,
)

print(f"passed       = {result['passed']}")
print(f"total_errors = {result['total_errors']}")
print(f"hex cells    = {result['cell_types'].get('hexahedra', 0)}")
print(f"max non-orth = {result['geometry']['max_non_orthogonality']:.3f}")

passed       = True
total_errors = 0
hex cells    = 2268
max non-orth = 0.000

Patch breakdown¶

Iterate mesh.boundary() (the fvBoundaryMesh) to see what patches the mesh actually has — useful when verifying that the boundary section of blockMeshDict came through as expected.

boundary = mesh.boundary()
patches = []
for i in range(len(boundary)):
    patch = boundary[i]
    name = str(patch.name())
    size = patch.size()
    patches.append((name, size))
    print(f"{name:<16s} faces={size}")

leftWall         faces=50
rightWall        faces=50
lowerWall        faces=62
atmosphere       faces=46
defaultFaces     faces=0

Plot the patch face counts¶

A simple matplotlib bar chart confirms the mesh has the patches the user expects. A missing or zero-face patch shows up immediately.

import matplotlib.pyplot as plt

names = [p[0] for p in patches]
sizes = [p[1] for p in patches]

fig, ax = plt.subplots(figsize=(6, 3))
ax.bar(names, sizes, color="steelblue")
ax.set_ylabel("number of faces")
ax.set_title(f"Boundary patches ({mesh.nCells()} internal cells)")
for i, n in enumerate(sizes):
    ax.text(i, n, f"{n}", ha="center", va="bottom", fontsize=9)
fig.tight_layout()
plt.show()