# how to extrapolate the presssure onto boundary

 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 10, 2002, 22:45 how to extrapolate the presssure onto boundary #1 Tony Guest   Posts: n/a 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

 September 10, 2002, 23:34 Re: how to extrapolate the presssure onto boundary #2 Huafei,liu Guest   Posts: n/a 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...

 September 11, 2002, 01:44 Re: how to extrapolate the presssure onto boundary #3 Tony Guest   Posts: n/a 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 ?

 September 11, 2002, 09:08 Re: how to extrapolate the presssure onto boundary #4 D.M. Lipinski Guest   Posts: n/a 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

 September 11, 2002, 21:35 Re: how to extrapolate the presssure onto boundary #5 Tony Guest   Posts: n/a 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 ?

 September 12, 2002, 03:02 Re: how to extrapolate the presssure onto boundary #6 D.M. Lipinski Guest   Posts: n/a 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

 September 12, 2002, 05:17 Re: how to extrapolate the presssure onto boundary #7 Tony Guest   Posts: n/a 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 ?

 September 12, 2002, 06:28 Re: how to extrapolate the presssure onto boundary #8 D.M. Lipinski Guest   Posts: n/a 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

 September 12, 2002, 11:48 Re: how to extrapolate the presssure onto boundary #9 frederic felten Guest   Posts: n/a 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.

 September 15, 2002, 22:05 Re: how to extrapolate the presssure onto boundary #10 Tony Guest   Posts: n/a Thank you all for your helpful discussions and suggestions Tony

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Attesz CFX 7 January 5, 2013 04:32 hdj CFX 1 November 27, 2005 08:15 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15 Mark CFX 6 November 15, 2004 16:55 Jan Ramboer Main CFD Forum 11 August 16, 1999 08:59

All times are GMT -4. The time now is 14:48.