Documentation

In this article, we will discuss a schematic methodology that is recommended to be followed in designing a C-section structured body-fitted high-orthogonal mesh with quadratic elements. This is implemented using the blockMesh technique in OpenFOAM. The study case, that will be used to explain the procedure for required mesh, is mirrored cambered foils at a high angle of attack, as shown in figure 1. The foil has a chord, , separated with the mirrored one with a distance, , and each one of them is tilted from the free-stream velocity, , with angle of attach, .

Part I: Preliminary design of the mesh, by doing a simple sketch.

1.

Define the main vertices that defines the boundary surfaces of the computational domain.

• Add at least 3 points (red ones in figure 2) at any quarter circle.
• Add at least 6 points (blue ones in figure 2) at the foil body.
• Add points (green ones in figure 2) along any symmetric lines.
• Add points (purple ones in figure 2) that bound the bodies on the domain edges.
• Add points (brown ones in figure 2) on long straight lines.
• Add points (Grey ones in figure 2) on corners.

2.

Define the secondary vertices that defines the interior blocks of the computational domain. Plot straight lines to design blocks with 4 edges, defining new vertices. These vertices are defined when two plots or more intersect in a point. The following design has 35 points.

Part II: Preliminary building of the mesh using blockMesh.

1.

Add the vortices to the blockMeshDict with the help of the sketch that you made before. Assuming the x-direction is along the horizontal flow direction and the y-direction is the transverse direction. Then, the -direction is the outward direction along the span of wing.

• Starting with the negative z-plane, give a name to the vertices in the following format, name nv# , where n is an abbreviation of negative plane and v is an abbreviation of vertex. Fill the vertices from the bottom left corner point and moves to the right until the row is finished. Then move up to the higher row starting from the left side again. Further, you may add spaces to align the start of each component, as this would help in the review process if there were mistakes. Remember the numbering in OpenFOAM starts with 0.
• After finishing the vertices of the negative -plane, copy and past them. Then, start to remove the negative sign in the -plane to make the positive one and change the naming from nv# to pv#.

2.

Construct the blocks with the help of the sketch that you made before. Start with the bottom left corner one and move to the right finishing the row. Then, move to the second row starting from the left side again. Start building the block from the same relatively vertices and moves along the local -direction of the block then the -direction, following the main picture of blocking. Further, you may add spaces to align the start of each vertex, as this would help in the review process if there were mistakes. In this level, use a single division in all directions and a simple grading of 1. In addition, you may add a comment of the number of the block, as this would help in the review process if there were mistakes.

3.

Leave the edges blank, as there is no need to stress about the arcs or the curved edges in the domain in this step of building the mesh. All edges will be straight lines, and this would help in the review process if there were mistakes.

4.

Fill faces of the domain’s boundaries with the help of the sketch that you made before. Further, you may add spaces to align the start of each vertex, as this would help in the review process if there were mistakes.

5.

Run the command blockMesh on the console window and open the Paraview of the case to see the wireframe of the domain.

6.

Increase the number of divisions to (20 20 1) in , respectively.

7.

Add the arcs and polylines one by one. Start with exterior edges then do the interior ones. At each edit, check the change by repeating step (5) in Part II.

8.

Apply the clustering on the blocks using simple grading and edge grading. You may use the OpenFoam User Guide Greenshields (2022) and equations to calculate the number of divisions in each direction.

blockMesh calculates the cell sizes using a geometric progression to generate a non-uniform mesh. Along a length , if cells are requested with a ration of between the last and first cells, the size of the smallest cell, , is given by:

(1)

where is the ratio between one cell size and the next which is given by:

(2)

(3)

9.

Finally, it is important to check and visualize the quality of the designed mesh. This is done by running the checkMesh command after generating the mesh. Then, visualize the mesh quality using Paraview.

The suggested options for checkMesh command are shown in the following line:

The mesh quality parameters, such as skewness, aspect ratio, orthogonality, and so on, and topology quality parameters are explained in details in wolfdynamics.com (2017). The standard limiting values for mesh quality with checkMesh can be found in the file primitiveMeshCheck.C, located in the directory:
$WM_PROJECT_DIR/src/OpenFOAM/meshes/primitiveMesh/primitiveMeshCheck. The standard values, that can be changed by the user, are defined as:

Even if the results from the meshCheck were okay, it is highly recommended to follow the suggested following values by SimScale (2022) and CFDSupport (2022) to avoid low-quality meshes, because they will almost always result in numerical inaccuracies, causing the simulations to fail or produce misleading results.

The mesh quality of the built mesh for the problem of reflected airfoils are shown in the figures 9-12.

The mesh quality results meet the recommended values, expect for the aspect ratio. The aspect ratio can be improved by increasing the number of divisions, which will increase the computational time. Otherwise, the convergence speed will significantly decrease with the high aspect ratio, but likely it is not fatal for the solver stability. Thus, the next steps to be done are the mesh independent analysis and validation study.

The article provided a schematic procedure to construct a structured mesh over simple geometries using blockMesh in OpenFOAM. Further, the article test the procedure over a two-reflected-airfoils problem. The results of proposed procedure showed a good mesh quality, which was analyzed by meshCheck in OpenFOAM. A future work of constructing a similar procedure for the complex geometries using snappyHexMesh in OpenFOAM will be conducted.

This article was firstly uploaded on Linked-In among the CFD and OpenFOAM community. The post can be found here. They discussed the article and provided suggestions for improvement.

The author thanks each of the Ocean TAMU professors Björn Windén, Mirjam Fürth, and Sharath Girimaji, for their technical support and invitation to write this article for the CFD users community for the Ocean Engineering department at Texas A&M University, ocean-cfd.engr.tamu.edu.