Hi all, I am writing a colloocated FVM code. Only interior elements are solved. How to extrapolate the interior pressure onto the boundary on a unstructure mesh. I found it is critial to the convergece in external flow. thanks in advance

You can extrapolates the pressure or pressure correction from interior to the boundary. Linear extrapolation is used, but one can also linearly extrapolate the gradient...

Thank you Huafei. In structured mesh, the linear extrapolation is of no problem since it is easy to find the third cell through ijk indexing. However, this is not the case in unstructured mesh. I have tried using the adjacent interior cell value as the boundary value directly but it will adversely affect the convergence in external flow. Another possible apporach is to reconstruct the boundary value. But, reconstruction procedure needs the gradient of pressure ( or pressure correction), which is dependent on the boundary pressure that is to be determined!. Any advice ?

Hi Tony,

The answer is: just take the cell-centered gradient in the near boundary cell. You can then use it in the Taylor series expression for the surface value of the pressure (or any other variable). The face value of pressure, Pe, will be the cell-centered value, Pp, plus a scalar product of the cell-centered pressure gradient and the translation vector, Rpe. The translation vector, Rpe, is the difference between the position vectors of the face midpoint and the near-boundary cell midpoint.

regards

DML

Hi DML. The problem is the calculation of the cell-centered gradient in the cell adjacent to the boundary. To calculate the cell-centered gradient there, you have to know the boundary pressure first. So, I think some kind of iterative procedure may be necessary. That is, first let the face value of pressure Pe be the cell-centered value Pp, and then calculate the pressure gradient in the near bondary cell. Finally, apply the pressure gradient to reconstruct the boundary pressure just like what you suggest. Repeat the above steps until the variation of the reconstructed boundary pressure is within the tolerence. Any comments ?

Hi Tony,

Only in the first iteration (outer iteration of the segregated solver is meant) of the very first time step the pressure gradient will be unknown. So it should be initialized to 0.0 and the scalar product with the translation vector will be zero; you will have Pe=Pp. In the subsequent iterations, the gradient of P is available. Use it to reconstruct the face value of P (Pe).

From my experience, to iterate just to calculate the gradient is very questionable. The problem is that if the gradient is unavailable, then it can make sense to iterate to calculate it only if the cell-centered pressures are accurate. Usually, the gradients are calculated once per outer iteration and the cell-centered pressures are only the estimates of the correct pressure field.

It seldom the problem for the pressure, but in general, you may need a limiter to avoid unphysical gradient values.

regards

DML

Hi DML. Thank you very much for your helpful comments. I think the limiter may be the key to my problem. But, to my limited knowledge, the limiter is usually used in inviscid flow. Can you suggest a limiter suitable for viscous flow ?

Tony,

The remark about the limiter for the gradient was related to your original post where you mentioned that the convergence may be the issue.

One should avoid unphysical gradients because in the cell-centered formulation on unstructured meshes the gradients are not only directly used to reconstruct the face value of variables (consider the Rhie and Chow approximation as an example). You may find it helpful to underrelax the gradient of the pressure between the outer iterations. This usually promotes convergence.

For other variables (e.g. temperature, T) a simple limiter can be imposed on the calculated gradient. The limiter requires that the vertex value of T calculated using Tp and gradT should be bounded by the cell-centered values (and the boundary face-values) of the elements (and boundary faces) sharing the vertex.

Hope it helps.

regards

DML

Hi there,

In my case (structured collocated FVM) I tested several type of BC for the pressure on an airfoil. I finally decided that providing a mesh that is orthogonal at the boundary, then the simple dp/dn= 0.0 works fine (meaning that you copy the value at j=2 to j=1). I actually compared the pressure profile to a potential flow solution, and it ws right on. In addition, this approach dp/dn=0.0 (neumann BC) was extremely convinient when solving the pressure poisson equation with a multigrid solver. At that point i don't know if one can actually generate an unstructured mesh with orthogonality at the wall, but if you can, just try this dp/dn=0.0 Sincerely,

Frederic Felten.

Thank you all for your helpful discussions and suggestions

Tony