Hello,

May I know how to construct "mirror" or "auxillary" cells for the setting of boundary conditions on unstructured grids? How are the variables assigned on such cells? Any suitable references on this subject?

Thanks very much, Chan K I

I use unstructured grids, and I don't know what you mean by mirror or auxillary cells. I never had to use those.

What kind of method do you use? (finite elements, classical finite volumes, Galerkin finite volumes)Since you use the word cell, I beleive it is one kind of finite volume scheme. But if you give more Info, somebody will give you better help.

Hi Sebastian,

I am using an explicit finite-volume scheme for the compressible 2D Euler Equations.

I have come across the setting of zero flux wall boundary conditions using "auxillary" or "phantom" cells which lie outside the wall boundaries. CFD books I've referred to so far describe their use in the context of structured grids.

I'm unsure how this might be extended suitably to unstructured grids.

Thanks very much, Chan KI

Hi.

For cell-centered scheme the solutions on he boundary must be saved.

I think there are two ways to save boundary solutions. The first is to save them on the center of boundary face(edge for 2-D case). The other is that what you want, that is to use ghost cell to save BCs.

The way to extrapolation of the velocity vector and other variables is same as structured mesh solver. The only one which is different from structured solver is how or where to save the boundary solutions. The simplest way to save BCs is just to extend Q array. You have NCELLS of interior cells, and NBFACES of bounday faces, then the size of Q array is Q(NVARIS,NCELLS+NBFACES). For matrix solver you should use the size of NCELLS. The BCs are saved at Q array from NCELLS+1 to NCELLS+NBFACES.

Except that I descrived above there are many ways to implement arrays in the computer program. It depends on your choice.

Good luck.

Jongtae Kim

You said that you used an unstructured grid. Than I expect that your mesh is composed of triangular elements or quadrilateral elements. Furthermore, in order to avoid orthogonality problems, a cell-centered sheme is avoided. Therefore, your unknowns should be located on the mesh vertices and an interpolation functions of an order superior or equal to one is used.

If your unknowns are located on the mesh vertices the variables are unknowns when there is a neumann boundary condition and the control volume for these follow (in parts) your boundary. The neumann boundary condition is then taken into accout when the integral int grad (phi) dot n dS is evaluted. For zero flux, this integral must than be zero.

Hi.

The orthogonality problem is one of very old issues. Nowadays skewness originated from the stretched triangular meshes is avoided by using mixed-element meshes.

Vertex-centered FVM is very attractive in view of memory efficiendy and post-processing. But if rectangular or hexa meshes are used, there is no difference between cell-centered and Vertex-centered FVM. And if linear interpolation function is used in the context of FEM, it is very similar to Vertex-centered FVM. What I want to say is all the things are dependent on your choice. For example, if you have very powerful advancing-front remeshing tool, then FE or Vertex-centered FVM is a good choice for a solver. And if you have cartesian mesh or mixed-element mesh generator, cell-centered FVM is very very good. You can use hanging node adaption and face-based BCS without singular points.

Have nice days Jongtae Kim

I use cell-centered FVM and I don't know much about vertex-centered FVM, so I¡¯m gonna state about cell-centered FVM

Reflecting the interior cells through the boundary gives the fictitious exterior cells which have the same shape with the interior cells. Allocate variables at ghost cells according to the boundary types (wall, inflow, outflow). If the slip condition is applied at the wall boundary, make the density, pressure, and tangential velocity in the ghost cell agree with those values in interior while the normal velocity is the negative value of the interior cell. This simulates zero normal velocity on the wall. If the no-slip condition is applied, make both normal and tangent velocity negative and others agree with those of interior. If turbulence model is used the treatment is different. I don¡¯t know much about it. If the equation is strictly hyperbolic, characteristic theory is used for inflow/outflow boundary conditions. If not, it is not difficult to impose inflow/outflow boundary conditions. For outflow boundary, Neumann condition is applied in general, which imposes the same variable at ghost cell with the values of interior cell.

Regards,

Kang, Seok Koo

Graduate Student, Lab. of Hydraulic Eng., Department of Civil Engineering, Hanyang University, South Korea.

1) I agree with you that orthogonality is not an issue with vertex-centered (or Galerkin) finite volume methods.

2) But the is still issue with cell-centerd finite volume methods (or classical finite volume methods). Since the line to centre of gravity must be orthogonal to the interface between two volumes. If it not the case, the approximation of the flux between these two volumes won't be consistent.