Plot OpenFOAM data#

import pyvista
from pyvista import examples

This example uses data from a lid-driven cavity flow. It is recommended to use pyvista.POpenFOAMReader for reading OpenFOAM files for more control over reading data.

This example will only run correctly in versions of vtk>=9.1.0. The names of the patch arrays and resulting keys in the read mesh will be different in prior versions.

filename = examples.download_cavity(load=False)
reader = pyvista.POpenFOAMReader(filename)

OpenFOAM datasets include multiple sub-datasets including the internal mesh and patches, typically boundaries. This can be inspected before reading the data.

print(f"All patch names: {reader.patch_array_names}")
print(f"All patch status: {reader.all_patch_arrays_status}")
All patch names: ['internalMesh', 'patch/movingWall', 'patch/fixedWalls', 'patch/frontAndBack']
All patch status: {'internalMesh': True, 'patch/movingWall': True, 'patch/fixedWalls': True, 'patch/frontAndBack': True}

This data is represented as a pyvista.MultiBlock object. The internal mesh will be located in the top-level MultiBlock mesh.

mesh = reader.read()
print(f"Mesh patches: {mesh.keys()}")
internal_mesh = mesh["internalMesh"]  # or internal_mesh = mesh[0]
Mesh patches: ['internalMesh', 'boundary']

In this case the internal mesh is a pyvista.UnstructuredGrid.

print(internal_mesh)
UnstructuredGrid (0x7f8663608e20)
  N Cells:      400
  N Points:     882
  X Bounds:     0.000e+00, 1.000e-01
  Y Bounds:     0.000e+00, 1.000e-01
  Z Bounds:     0.000e+00, 1.000e-02
  N Arrays:     4

Additional Patch meshes are nested inside another MultiBlock mesh. The name of the sub-level MultiBlock mesh depends on the vtk version.

boundaries = mesh["boundary"]
print(boundaries)
print(f"Boundaries patches: {boundaries.keys()}")
print(boundaries["movingWall"])
MultiBlock (0x7f8663608f40)
  N Blocks:     3
  X Bounds:     0.000, 0.100
  Y Bounds:     0.000, 0.100
  Z Bounds:     0.000, 0.010

Boundaries patches: ['movingWall', 'fixedWalls', 'frontAndBack']
PolyData (0x7f8663608d00)
  N Cells:      20
  N Points:     42
  N Strips:     0
  X Bounds:     0.000e+00, 1.000e-01
  Y Bounds:     1.000e-01, 1.000e-01
  Z Bounds:     0.000e+00, 1.000e-02
  N Arrays:     4

The default in OpenFOAMReader is to translate the existing cell data to point data. Therefore, the cell data arrays are duplicated in point data.

print("Cell Data:")
print(internal_mesh.cell_data)
print("\nPoint Data:")
print(internal_mesh.point_data)
Cell Data:
pyvista DataSetAttributes
Association     : CELL
Active Scalars  : p
Active Vectors  : U
Active Texture  : None
Active Normals  : None
Contains arrays :
    U                       float32    (400, 3)             VECTORS
    p                       float32    (400,)               SCALARS

Point Data:
pyvista DataSetAttributes
Association     : POINT
Active Scalars  : p
Active Vectors  : U
Active Texture  : None
Active Normals  : None
Contains arrays :
    U                       float32    (882, 3)             VECTORS
    p                       float32    (882,)               SCALARS

This behavior can be turned off if only cell data is required.

reader.cell_to_point_creation = False
internal_mesh = reader.read()["internalMesh"]
print("Cell Data:")
print(internal_mesh.cell_data)
print("\nPoint Data:")
print(internal_mesh.point_data)
Cell Data:
pyvista DataSetAttributes
Association     : CELL
Active Scalars  : p
Active Vectors  : U
Active Texture  : None
Active Normals  : None
Contains arrays :
    U                       float32    (400, 3)             VECTORS
    p                       float32    (400,)               SCALARS

Point Data:
pyvista DataSetAttributes
Association     : POINT
Active Scalars  : None
Active Vectors  : None
Active Texture  : None
Active Normals  : None
Contains arrays : None

Now we will read in all the data at the last time point.

print(f"Available Time Values: {reader.time_values}")
reader.set_active_time_value(2.5)
reader.cell_to_point_creation = True  # Need point data for streamlines
mesh = reader.read()
internal_mesh = mesh["internalMesh"]
boundaries = mesh["boundary"]
Available Time Values: [0.0, 0.5, 1.0, 1.5, 2.0, 2.5]

This OpenFOAM simulation is in 3D with only 1 cell in the z-direction. First, the solution is sliced in the center of the z-direction. pyvista.DataSetFilters.streamlines_evenly_spaced_2D() requires the data to lie in the z=0 plane. So, after the domain sliced, it is translated to z=0.

def slice_z_center(mesh):
    """Slice mesh through center in z normal direction, move to z=0."""
    slice_mesh = mesh.slice(normal='z')
    slice_mesh.translate((0, 0, -slice_mesh.center[-1]), inplace=True)
    return slice_mesh


slice_internal_mesh = slice_z_center(internal_mesh)
slice_boundaries = pyvista.MultiBlock(
    {key: slice_z_center(boundaries[key]) for key in boundaries.keys()}
)

Streamlines are generated using the point data “U”.

streamlines = slice_internal_mesh.streamlines_evenly_spaced_2D(
    vectors='U',
    start_position=(0.05, 0.05, 0),
    separating_distance=1,
    separating_distance_ratio=0.1,
)

Plot streamlines colored by velocity magnitude. Additionally, the moving and fixed wall boundaries are plotted.

plotter = pyvista.Plotter()
plotter.add_mesh(slice_boundaries["movingWall"], color='red', line_width=3)
plotter.add_mesh(slice_boundaries["fixedWalls"], color='black', line_width=3)
plotter.add_mesh(streamlines.tube(radius=0.0005), scalars="U")
plotter.view_xy()
plotter.enable_parallel_projection()
plotter.show()
openfoam example

Total running time of the script: ( 0 minutes 0.151 seconds)

Gallery generated by Sphinx-Gallery