Hex Meshing

Mesh Geometry option allows to set the geometry as a mesh boundary. The geometry along with the boundaries of the base mesh should form a closed surface. The meshing algorithm uses this geometry to cut a mesh and conform its shape to it. Two additional options are available:

Boundary Layer feature is an optional meshing stage used to better resolve the flow in the viscous layer near the walls. At this stage, the mesh is shrunk and additional mesh layers are inflated to increase mesh density near the boundary.

Boundary Layer option is available for meshed geometry (Mesh Geometry has to be enabled). The following options allow to specify the sizing of the boundary layer:

Create Cell Zone is an optional meshing feature used to mark sub-volume of the mesh. This option is only visible when Mesh Geometry is enabled. Instead of using this geometry to remove cells, cells will remain inside this geometry (similarly to Create Baffle). The mesh cells will adapt to the geometry surface, but the mesh boundary will not be created in the geometry location. All the cells located inside the geometry will be marked as a Cell Zone and the cell zone will derive name from the geometry.

It is possible to create a cell zone the meshing by extracting cells from an existing mesh. However, defining the cell zone during meshing allows adapting cells to the cell zone geometry.

Refine Geometry uses the geometry to mark a volume refinement. Mesh density inside the geometry can be increased by multiple times relative to the base mesh (higher refinement level). Outside the geometry the mesh is smoothly coarsen by decreasing refinement level. The refinement transition region size (and thus the total cell count) can be controlled by using Cells between Levels option under Meshing Settings panel.

The following options are available for the Refine Geometry tool:

It is possible to apply the same meshing properties to multiple geometries. For this purpose use the Copy Meshing Properties button. All meshing settings will be copied from the source to the destination geometries.

To copy meshing properties follow these steps:

The Copy Properties panel will appear to the left.

The Box base mesh is a simple and most commonly used for creating general 3D meshes. Box type has a cuboid shape where the edges are parallel to the global coordinate system axes. The Box base mesh type is selected by default. Depending on which type is selected the suitable parameters will be shown below.

The Cylinder base mesh is typically used for axis-symmetric geometries such as rotors or impellers. Topologically cylinder consists of five boxes connected in such a way that the mesh can have a cylindrical shape with good cells quality.

While selecting the base mesh type the suitable parameters will be shown below. These parameters are characteristic dimensions of the selected shape.

The Plate base mesh is used for generating 2D meshes. It is essentially a two-dimensional version of Box placed in an X-Y plane. All geometries in SimFlow are 3D, and thus the geometry must be located in the way it will cut through the Plate plane. SimFlow only operates on 3D meshes, and despite the Plate will be used for 2D simulation the mesh will still remain 3D. The mesh will be one cell wide in the Z direction. To enforce 2D flow a special Empty boundary condition type will be assigned to the front and back of the Plate mesh (boundaries for the Z direction). User have freedom to choose appropriate boundary conditions to the sides (X min/max and Y min/max edges).

While selecting the base mesh type the suitable parameters will be shown below. These parameters are characteristic dimensions of the selected shape.

The Wedge base mesh is used to create 2D axis-symmetric meshes. It is essentially a section of a Cylinder placed in an X-Y plane.

The mesh consists of one cell in the third dimension in which the fluid dynamics equations will not be solved. This base mesh type will automatically take care of preparing appropriate boundaries for the Z-direction. Special Wedge boundary conditions are automatically assigned to both sides of the computational domain to enforce 2D axis-symmetric flow.

Usually, the mesh is created inside a geometry defining a single volume. However, in certain situations, multiple separate regions can be used. A typical example would be a simulation of a flow where part of the domain is a porous region. The porous region in this case would be another volume unconnected to the whole fluid domain. Another example can be a Conjugate Heat Transfer (CHT) simulation. In this case often the fluid domain is defined by the separate geometry per each region - fluid and solid. For those situations, the simplest option is to create a Multi-Zone Mesh.

When you enable Multi-Zone Mesh a list of Material Points will be displayed. There you can add multiple material points. Each material point should have a name that will be used to create a cell zone named after that material point. If a material point is named none, the mesh will be assigned to default region and will not be put into any cell zone. Each of the material points should be located in a separate, unconnected region of the geometry.

Note, the multi-zone mesh removes walls between zones but adapts cells to match wall location. Generated mesh will consist of a single mesh region and multiple cell zones representing separate volumes. This feature is useful for the conjugate heat transfer simulation. All the subregions can be created in a single meshing step instead of meshing each region separately. Having multiple cell zones allows to convert the mesh into multiple subregions - appropriate boundaries between cell zones will be created and by default coupled with its neighbour located in second subregion. To create a subregions from the cell zones use the Cell Zones to Regions option from the MESH panel.

In the CPU tab you can set the number of processors used for meshing. Serial (1 processor) is set as default. If you have a multi-core processor, you can use the parallel option to perform meshing in parallel. Meshing in parallel is performed by decomposing mesh into multiple subdomains and then meshing each subdomain using own processor.

Settings tab contains additional global meshing options. The most commonly used parameters are visible under the Settings tab, while a more advanced options can be accessed from Advanced Meshing Options.

The meshing process can be split into three stages: Base , Mesh and Layers. Meshing Stages define which of the stages should be performed. Each stage can be performed separately or some stages can be omitted. The following options are available:

If the meshing process takes a long time, it is comfortable to set the notification after the meshing process is finished. To activate this option check Notify me when meshing is finished and type your e-mail address. You will receive a notification when the mesh will be ready.

Mesh button starts the meshing process. Depending on the mesh settings and hardware, the mesh generation can take from a few seconds to even a few hours.

If you are generated mesh more than once, for example, you decided to increase mesh density, the Restore Previous Mesh will become active. By clicking this button you will replace the current mesh with the previous one. You can think about this option as a one-level undo.