Hi there,

(1)-i'm seeking informations and references on how to implement non-orthogonal boundary conditions for complex geometries using the finite volume method. (2)-I'm also interested on how the pressure at the wall has to be set ?

Thanks in advance for your help. Sincerely,

Frederic Felten

Take a look at the paper by Zang, Koseff, Street in JCP. I am not exactly sure about the year, it is either 1994 or 1995. The paper is on non-staggered implementation of a fractional step method. But, strictly speaking, it is a mixed (staggered/non-staggered) method. It uses cell-centered cartesian velocities and face-centered contravariant fluxes. The latter variables are used to conserve mass much like in the standard staggered schemes. So the pressure boundary conditions should be generic enough.

some further details about your general FV approach would be useful to evaluate the problem.

Structured/unstructured grid. Cell centered /cell vertex method ? Upwind/central differencing?

And: Euler or Navier stokes ?

Frank

Here is the overall picture: Unsteady Navier-Stokes, finite volume, curvilinear, second order(central difference), structured mesh, collocated arrangement for the cartesian velocities, and the fluxes are contravariant on the faces. A fractional step method is used (I have to solve a pressure poisson equation) and the time marching is implemented using a 3rd order runge-kutta.

So far my pressure solver give me back a divergence free field after correction, but only for the interior points. I'm experiencing some problems(non divergence free field at the wall) when the mesh at the wall is not exactly orthogonal. If you have experienced a similar problem or have some info that could help me solve this, please feel free to post a message.

Sincerely,

Frederic Felten.

Just to be sure:

Do you mean "collocated" or "colocated"?

i mean collocated as in non-staggered.

Sincerely,

Frederic felten

Except for the 3rd order runge-kutta integration scheme, you seem to be doing exactly what Zang et al. have done in their JCP paper that I had mentioned in my earlier posting. Let me know if you have a problem locating this paper.

i found this paper, and i'm looking at the BC for pressure. About doing the same thing, well it's not true since they are using a QUICK scheme, then not respecting the exact energy conservation by introducing dissipation. With the 2nd order central differencing, one respects exactly the energy conservation for the inviscid terms (check JCP 143, pp 90-124, 1998. by Morinishi, Lund, Vasilyev and Moin). Another thing that is different, i do not transform from physical space to computational space, solving everything directly in physical space (except for the viscous terms where the transformation is necessary).

Thanks for your help,

Sincerely,

Frederic Felten

What you describe is "co"+"location", in which the variables for a cell are located at a common point.

"collocation" refers to (I think) interpolation technicques using families of functions. I'm sure one of the resident mathematicians will provide details. For an example, see the SIAM J. on Numerical Analysis, v. 34, #6, pp. 2274-2287, 1997. "Spline Collocation Differentiation Matrices," by Russell and Sun.

I forgot for a minute there that your primary interest is in DNS/LES.

The QUICK scheme is used in this paper just for computing the predicted values of the contravariant fluxes from the predicted cell centered velocities. You can replace this with a symmetric interpolation scheme. The method will not develop checker board type oscillations since the corrected values of the cell-centered velocities and face-centered fluxes are updated indendently (using the cell-centered pressure gradients and the face-centered pressure gradients respectively).

The type of approach described above has been adopted recently by Mittal et al. You can download the JCP paper from Prof. Mittal website at UF, Gainesville. In this paper, they use cell-centered velocities and face-centered fluxes (although on cartesian meshes). There is no upwinding (i.e. QUICK type interpolations) anywhere and yet the method is free from checker board type oscillations.

I understand that the way you compute contra-variant fluxes could be different from the way Zang et al. compute them. But once they are computed, your Poisson equation for pressure and the boundary conditions perhaps are of the same form as in their paper. i.e. Area integral of intermediate contravariant flux = Area integral of the pressure gradient (computed at face centers). So the solution of Poisson equation may be obtained in exactly the same way even if the rest of the solver is different.

I use a cell-centered finite volume scheme on unstructered grids. I don't use a staggered grid approach (the velocity is re-interpolated on the volume interfaces, this is similar to the Rie Chow scheme). The continuity equation is solved via a projection-2 scheme. My BC's could be similars to those you need. If you are interested, I could send you a paper that will be presented at CFD2001 (University of Waterloo, Canada) at the end of May.

Regards.

Thanks for your offer sebastien. If you coul send me this paper i'd be delighted.

Sincerely,

Frederic Felten feltenf@hotmail.com

hi frederic,

i think there are several ways to attack your problem. I used differnt types of boundary conditions for non-orthogonal curvatures, and the easiest way for me was to use the compatibility relations (meauzé, fourmeux, fatsis etc. all from ONERA france) The basic idea is: The euler equations are time-hyperbolic, that means there are real eigen values, that means the assambled jacobien matrix could be diagonalized for every direction n=(nx, ny, nz). In general the euler-equations are substitued by a normalized charistic set of variables. The new equation is pretty similiar to the euler ones.

d/dt W + n (nabla) W =0

and this gives you at the and all the variables that you need at the border... If your are more interested please let me now.

bernd halleluja from switzerland

On the other hand you could if your border is a haerd one, like a airfoil etc. than you could also use the pressure normal equations, which means you should make a projetion of the physical values from the flow field to the border by respecting the geometries. Normally people are making an extrapolation first or second order of the density (rho) and the velocities (x,v) (respect the geometries by using co- and contra variant velocities) from these values, you could determine the pressure gradient on the profile and from that the pressure value itself. It is phyiscal motivated approach, i prefore the mathmatical on with the compatibility relations.

Last point: For what kind of mach-number do you want to use your boundary conditions? Subsonic, transonic, hypersonic...

thanx and good luck, bernd

Thank you very much for your help bernd. i now have plenty of informations to work with.

Sincerely,

Frederic felten