Meshing

Generate stirred tank reactor mesh

Generate a blockMeshDict with

inp=bird/meshing/stirred_tank_mesh_templates/base_tank/tank_par.yaml
out=bird/meshing/stirred_tank_case_templates/base/system/blockMeshDict

python applications/write_stirred_tank_mesh.py -i $inp -o $out

Then activate openFOAM environment and mesh with

blockMesh -dict system/blockMeshDict
stitchMesh -perfect -overwrite inside_to_hub inside_to_hub_copy
stitchMesh -perfect -overwrite hub_to_rotor hub_to_rotor_copy
transformPoints "rotate=((0 0 1)(0 1 0))"

Visualize mesh in Paraview

Related tutorial

• tutorial_cases/stirred_tank

Block cylindrical meshing

Generates system/blockMeshDict

root=`pwd`
caseFolder=bird/meshing/block_cyl_cases_templates/case
mesh_temp=bird/meshing/block_cyl_mesh_templates/sideSparger

python applications/write_block_cyl_mesh.py -i $mesh_temp/input.json -t $mesh_temp/topology.json -o $caseFolder/system

Then, activate the openFOAM environment and construct the mesh with

cd $caseFolder
blockMesh
transformPoints "scale=(0.001 0.001 0.001)"
transformPoints "rotate=((0 0 1) (0 1 0))"
cd $root

Visualize the mesh in Paraview

How to change the dimensions or mesh refinement?

The geometry and the mesh size are controlled by the input file input.json. The input file can also be in .yaml format. The parser will decide the file format based on its extension. See bird/meshing/block_cyl_mesh_templates/baseColumn/ for an example of .yaml

How to change the arrangement of concentric cylinders?

The block topology is controlled by topology.json We recommend always working with a schematic as shown below

The purple blocks are walls (not meshed) and the white blocks are fluid blocks (meshed). The symmetry axis is indicated as a dashed line

In topology.json, the purple blocks are defined as

"Walls": {
                "Support": [
                            {"R": 0, "L": 3},
                            {"R": 1, "L": 3}
                           ],
                "Sparger": [
                            {"R": 0, "L": 2},
                            {"R": 1, "L": 2},
                            {"R": 2, "L": 2}
                           ]
        }

How to change boundaries?

Boundaries are defined with three types, top, bottom and lateral

For example, if one wants to create a boundary called wall_sparger, shown below as the red lines

one can define the boundary as follows in topology.json

"Boundary": {
                "wall_sparger":[
                           {"type": "bottom", "Rmin": 2, "Rmax": 2, "Lmin": 2, "Lmax": 3},
                           {"type": "top", "Rmin": 0, "Rmax": 0, "Lmin": 1, "Lmax": 2},
                           {"type": "top", "Rmin": 1, "Rmax": 1, "Lmin": 1, "Lmax": 2},
                           {"type": "top", "Rmin": 2, "Rmax": 2, "Lmin": 1, "Lmax": 2}
                         ],

For lateral boundaries (called inlet in this example), and shown below as the red line

one can define the boundary as follows in topology.json

"Boundary": {
                "inlet": [
                           {"type": "lateral", "Rmin": 2, "Rmax": 3, "Lmin": 2, "Lmax": 2}
                         ],

Related tutorials

• tutorial_cases/side_sparger

• tutorial_cases/bubble_column_20L

Block rectangular meshing

Generates system/blockMeshDict

root=`pwd`
caseFolder=bird/meshing/block_rect_cases_templates/case
mesh_temp=bird/meshing/block_rect_mesh_templates/loopReactor

python applications/write_block_rect_mesh.py -i $mesh_temp/input.json -o $caseFolder/system

Then, activate openFOAM environment and construct the mesh with

cd $caseFolder
blockMesh
cd $root

Visualize the mesh in Paraview

How to change the block rectangular geometry?

The geometry of the block cylindrical mesh is defined within a 3D domain (X,Y,Z). The blocks that represent the fluid domain are a subset of a block rectangular background domain. The fluid blocks are defined using the geometry corners. For the mesh shown above, the geometry corners are the red blocks shown below

The corners are defined in input.json

"Geometry": {
        "Fluids": [
                [ [0,0,0], [9,0,0], [9,0,4], [0,0,4] ],
                [ [0,1,4], [0,4,4], [0,4,0], [0,1,0] ]
        ]
}

Related tutorials

• tutorial_cases/loop_reactor_mixing

• tutorial_cases/loop_reactor_reacting

Generate STL patch mesh

Boundaries may be specified with the surfaceToPatch utility in OpenFOAM, based on STL files that can be generated with

python applications/write_stl_patch.py -v

The verbose flag (-v) generates a plot of the stl mesh (as shown below)

How to change the set of shapes in the boundary patch?

Edit the json files that are read when generating the mesh. In the case tutorial_cases/loop_reactor_mixing, the boundary condition inlets consists of 3 discs

{
    "inlets": [
        {"type": "circle", "centx": 5.0, "centy": 0.0, "centz": 0.5, "radius": 0.4, "normal_dir": 1,"nelements": 50},
        {"type": "circle", "centx": 2.5, "centy": 0.0, "centz": 0.5, "radius": 0.4, "normal_dir": 1,"nelements": 50},
        {"type": "circle", "centx": 7.5, "centy": 0.0, "centz": 0.5, "radius": 0.4, "normal_dir": 1,"nelements": 50}
    ],
}

What if the STL patches overlap?

If STL patches are defined such that there is an overlap between patches, the final patch will be the union of the overlapping patches. In case of an overlap, the final patch will be therefore smaller than without an overlap. An example of this behavior is shown below for a U-loop reactor.

In this case, the inlet (highlighted in red) contain 2 circular spargers. On the left, the two spargers contain an overlap and on the right they are disjoint. The inlet patch surface area is 13% smaller on the left than the right, but both simulations successfully run.

Related tutorials

• tutorial_cases/loop_reactor_mixing

• tutorial_cases/loop_reactor_reacting

• tutorial_cases/bubble_column_20L