[Far]

Please refer to following link (specially Page # 9 and Fig. #10). Do you think quality is acceptable for the high quality CFD simulation? I am not saying it is wrong, but I am interested to find out mathematical reasoning (from CFD point of view in terms of accuracy, convergence etc) behind this. As it will help me to create the less dense mesh on the body of the wings with large length to chord ratio.


http://www.pointwise.com/T-Rex/Pointwise_T-Rex.pdf

[cnsidero]

Far,

Generally speaking, solution accuracy, regardless of mesh type, is a function of the chosen solver numerical methods. In my review of the literature concerning tet element quality, a commonly used metric is the maximum included dihedral angle. As max included angle increases, tri/tet quality decreases. You will notice that anisotropic tris/tets from Pointwise have max included angles generally < 90. So by the max angle metric they are of high quality.

Continuing, there is one additional metric to consider. The deviation angle between the face normal and the vector connecting the cell centers on each side of the face. If you have a hard time understanding this, simply draw a picture of a long, narrow rectangle and split at two opposing corners to give you two aniso tris. First draw the normal vector of the long hypotenuse - this is the face vector. Second find the cell center of each triangle and draw a line connecting the two. The angle between them is that deviation angle.

Large deviation angles commonly causes issues for cell-centered, finite volume based CFD solvers - the method used by many of the popular commercial codes. The reason being is that when one wants to compute the fluxes on a face - a necessary procedure for finite volume method - you need to compute face information by interpolating the adjacent cell center information. In particular, when you need the gradient at the face center, the simplest way is to compute the gradient along the adjacent cell centers vector. This is where deviation angle comes into play. As the adjacent cell center vector deviates from the face normal (direction of the gradient at face center), the interpolated gradient direction is clearly not aligned and likely not representative of the face normal gradient. Hence, error and solution stiffness start coming into play.

Now you can attempt to rectify this by interpolating the gradient from the cell-center to the face-center a little more intelligently. It's called the non-orthogonal correction to the gradient. There's various ways to do it, it's best to dig around in the literature if you're interested. In addition, the correction is usually added explicitly, ie. to the RHS of the linear system, meaning it can make solution convergence more difficult.

Where I've seen these meshes used most successfully is with vertex-centered finite volume or finite element based solvers. It seems the numerics lend themselves better to stretched tet meshes and the solver writers are trying to consider them during algorithm development.

Most finite volume based solvers (cell centered or vertex centered) and users would still prefer to stay away from stretched tet meshes, partly because of the unknown behavior they might incur but most simply because they contain lot more cells. Pointwise addresses this by allowing the combination of anisotropic tets into prisms***. For every three neighboring anisotropic tet you can make one prism. Ideally, if the mesh was initially 100% aniostropic tets and every triplet could be combined you would get a two thirds (67%) reduction in cell count. First, no mesh has 100% aniostropic tets and second not every anisotropic tet can be recombined. In practice, Pointwise's aniostropic combination algorithm typically reduces the cell count between 55-60% and I've seen it higher sometimes. This procedure gives you the desired prisms in the boundary layer while significantly reducing the cell count. The aniso tet combination method in Pointwise can combine ansio tets into prisms anywhere in the boundary layer - it doesn't require each prism layer to be complete before moving to the next one. This is how it achieves such high combination percentages.

-Chris

*** The anisotropic combination algorithm is invoked during CAE export. Solvers that support mixed-element meshes (Fluent, OpenFOAM, CGNS, etc) will have a check box that says "Combine Anistropic Tetraheda" option during exporting the mesh to the solvers format. The Pointwise message window will report the combination stats after export.

[Far]

Thankyou Chris for very detailed and informative reply covering meshing from solver point of view. It is simply great.

Once again thankyou. Have a nice day.

[Hybrid]

Thanks Chris for such an expert opinion.

Will you help me, how to improve quality of unstructured meshes in Pointwise? I face skewness angle about 1.0 and hardly achieve prisms.

How to make prisms?

[Far]

Do you need hybrid mesh?

You can get prisms using extrude option