Create CFD Case

The creation of a CFD case can be started activating the Create CFD Case green button. A dialog window opens as illustrated below:

PGEMCFDCaseSrfaceMesh

It requests a Case name definition for the CFD case. Initially, only the Surface Mesh entry on the left side menu is active as STL structures are requested to create a CFD case.

Surface Mesh

There are two possibilities to provide STL structures for modeling:

From a STL file enabling the Load STL from file radio button. Once the file is selected the menu on the left side becomes active allowing further settings. In addition, definition for the mesh type is available in the selection of Mesh was created in.
Create mesh from the selected structures of the currently displayed model. To this end, the Generate STL from selected structure radio button has to be enabled. Consequently, the following settings are available:

Smoothing (FWHM)	It is a Gaussian filter and allows smoothing the data before creating the STL structure. The default value corresponds to the pixel size in the data.
Segmentation Threshold	All pixels with the value above the threshold are included in the segment. When the Optimal checkbox is enabled the threshold will be calculated automatically such that the volume of selected data is conserved.
Reduction	If enabled, allows creating simplified mesh based on data simplification. The defaults value is 2 and is representing the smallest value to be defined. Initially, the program will use this number and multiply the pixel size of the data with this value. Finally, the mesh will be generated on the new data. It is a faster procedure and the results will consist in mesh being less precise. Please note that if only this checkbox is enabled the generated files will be bigger and change in topography of the mesh will occur.
Decimation	Allows simplifying mesh. Please note that in this case the simplification procedure is done after the mesh is created. It is a slow procedure which generates smaller files. Decimation only changes the number of STL nodes, particularly the vertices of the surface mesh. However, no change in the mesh geometry occurs, preserving thus the mesh topology.
Generate	The activation of this button starts the mesh calculation. Upon completion a dialog opens showing the 3D preview of the mesh and allowing the definition of the Full bounding box as illustrated below: The manipulation of the bounding box allows setting cutting planes. The result would be a surface mesh consisting of the "original" body and flat surfaces on the cutting planes that are just adjacent to the "original" body mesh. The flat surfaces are useful to define the boundary conditions. Confirm with OK to return to the Create CFD Case interface. Consequently, the menu on the left hand side is becoming active. Note that for the CFD modeling only a small part of the selected element should be enclosed within the box.

Volume Mesh

Once the surface mesh is created the user can proceed with the creation of the volume mesh.

The Volume Mesh interface is organized in two main sections:

BlockMesh parameters: the name is representing the OpenFOAM application responsible for the part of generating volume mesh. It allows creating cuboid structures filled with block cells. Inside it, the surface mesh will placed, and the block cells which are inside the cuboid will be initial volume mesh cells. These block cells are representing the starting point on which the final volume mesh will be build. Please note that the final volume mesh doesn’t have cuboidal cells.
SnappyHexMesh parameters: is the name of the application that sculpts the volume mesh. The volume cells are no longer blocks: they are snapped to the surface.

PGEMCFDVolumeMesh

The Volume Mesh setting parameters are summarized in the table below:

Bounding box	Is representing the cube that has to enclose the whole surface mesh. Its coordinates are defined by the X, Y, Z values in the Min and Max fields. In general these values are filled in automatically immediately after the surface mesh is generated in the Surface Mesh menu entry. It represents the bounding box used to create the cutting plane. Its size can be adjusted activating the Adjust bounding box button. Please note that if the surfer mesh is loaded from an external STL file, the Adjust bounding box is grayed out. Therefore the user has to know the location of the bounding box and needs to introduce manually the coordinates. The Cell size determines the number of cells in each direction: X, Y, Z. This parameter is essential for further volume mesh development. The smaller the cells size, the more cells of volume mesh and more elements will have to be solved.
Point in mesh location	Is representing any point inside the surface mesh. This point is used only to determine whether "sculpting" of the volume mesh should take place inside or rather outside the surface mesh. Please note that Adjust point in mesh is grayed out when the surfer mesh is loaded from an external STL file.
Surface refinement level	Allows refining the mesh in the neighborhood of particular surfaces. Please note that this procedure affects the volume nearby. If enabled, the Min and Max level need to be specified. When a value of 1 is set there will be no refinement calculation. In case the values are different, the refinement will be applied nearby the whole surface. Additionally, particular surfaces can be selected: segment or cutting planes.
Volume refinement	Allows defining how many times the volume mesh inside the whole volume will be refined. If the check box is enabled, there are three Modes for the refinement procedure: Inside: the number in the Level field indicates how many times the cells will be divided Outside: the number in the Level field indicates how many times the cells will be divided Distance: allows specifying many distances from the surface. The advantage consists in the fact that each distance can have a different level. For example cells can be divided 6 times for the first two mm of volume mesh, counting from the surface, then 4 times for next two mm and 2 times for the next two mm. To this purpose the number of Steps needs to be set to 3. For each step the corresponding Distance and Level need to be specified: - step 1: distance 2 and level 6, - step 2: distance 4 and level 4, - step 3: distance 6 and level 2. It is important that levels are ordered starting from the nearest one.

Boundary Conditions

Boundary conditions for two physical variables can be defined for each surface belonging to the surface mesh: pressure and velocity.

PGEMCFDBoundaryConditions

The settings available in this interface are:

Field type	Allows selection of a scalar or vector type.
Internal field	If uniform entry is selected means that all cells of the volume mesh will have the same value. When non-uniform is selected, a file needs to be provided using the Load button.
Boundary field	Allows determining boundary conditions on the boundary: walls and cutting planes. Three options are available: zero gradient, fixed value (can be uniform or not), surface normal fixed value: is representing the vector value normal to the surface, including the outside points and excluding the inside points.
[scalar]	Is an integer value and need to be specified in the dedicated field.
Unit	Allows defining the specific unit for the P(pressure) and U(velocity) respectively

Solution Controls

PGEMCFDSolutionControls

The following settings are available:

Write interval	Allows defining how often the OpenFOAM solver should write down the results.
End Time	Allows defining the iteration number of the solver. The number is representing the iteration for the steady state simulations.
Calculate WSS	Allows calculating the wall share stress for the particular iteration number specified in the at time field.

The easiest way to store all the settings done for the project is using the Save button below the left side menu. All the information will be saved in a .cfdCase file which can be easily retrieved using the Load button.

Finally, to send the CFD case to the OpenFoam interface activate the Send Case button.

In This Section

Management of the OpenFoam Remote Cases