# Pressure at the surfaces of a cell

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 January 5, 2001, 17:14 Pressure at the surfaces of a cell #1 Gao Guest   Posts: n/a Hello All: I was writing a 2D NS code with defining U, V, P at the cell centre.I tried different ways to interpolate the Pressure at the surfaces of the cells to avoid the decoupling problem, but still couldn't work it out now (convergence problem). I would be very grateful to Anyone who can give me a hint on how to define the Pressure at the cell surfaces? Thanks and Best regards!

 January 7, 2001, 16:23 Colocated Craziness #2 Answer Man Guest   Posts: n/a If you are talking about SIMPLE then.. are you using Rhie-Chow for velocity interpolation... With this I think the pressure is just a linear interpolation. I would suggest reading Computational Methods for Fluid Dynamics. by Ferziger and Peric. In the back of the book they give reference to a cite with free code using Finite Volume with a colocated grid arrangement (2d or 3d)...etc..etc.. This would probably answer all your questions

 January 7, 2001, 18:49 Re: Colocated Craziness #3 Gao Guest   Posts: n/a Tiffiny: Thank so much for your knowledge and great help. I was thinking only to interpolate the pressure values at the faces using momentum equation coefficients described by Rhie & Chow in "Numerical study of the turbulent flow past an airfoil with trailing edge separation", while the U and V at the faces still uses central differencing. Based on your experinece,what do you think about this method? I understand that you suggest using Rhie-Chow for velocity interpolation, while the pressure uses linear interpolation (like central differencing). Is my understanding correct? Looking forward to your suggestions! Once again, thanks!

 January 8, 2001, 12:40 Re: Pressure at the surfaces of a cell #4 kalyan Guest   Posts: n/a I am guessing that you interpolate the pressure to the cell faces and compute the pressure gradient at the center using these (face) values. If you use symmetric interpolation, the pressure and velocity would indeed decouple. So you need some kind of a biased interpolation (upwinding of some sort). However, it is better to interpolate the predicted velocities to the cell faces (from cell centered) values using non-symmetric interpolations and then used these to compute the source term for the pressure. i.e. Laplacian (p) = Divergence (v*) Both Laplacian and Divergence operators can be symmetric. v* are face values of the predicted (intermediate) which are obtained using non-symmetric (upwind) interpolation from cell centers. All other operators in other equation can be symmetric and the method would be stable. A 1995 JCP paper by Zang, Street et al. may offer more help. The paper is non-staggered fractional step method although I do not recollect the exact title.

 January 8, 2001, 13:26 Re: Pressure at the surfaces of a cell #5 John C. Chien Guest   Posts: n/a (1). I like your question, because it does raised the fundamental question about the development of numerical schemes in CFD. (2). It seems to me that after so many years of CFD development, there is still no systematic and easy to understand approach to follow in developing numerical schemes which actually work. (3). My feeling is: more research is needed to seek out the fundamental principle of method development, so that it can be used to develop good numerical schemes for use in CFD. (4). What I am trying to say is: we need to know what is the right way to develop a good numerical scheme to solve the CFD equations. Without that, CFD will be based on someone's method instead of more fundamental mathematical and physical principles. (5). If you are not getting the converged solution, then is it possible to know "why", so that we can take the right approach? (by the way, I don't have the solution yet. But I am getting the feeling that the foundation of CFD is rather soft. Any time when it rains, we are going to have mud slide, and the house will be destroyed)

 January 8, 2001, 15:14 Linear Loony-Toon #6 Answer Man Guest   Posts: n/a Check out this reference. It talks about the momentum interpolation scheme for velocity... S. Majumdar. 1988. Role of Underrelaxation in momentum interpolation for calculation of flow with non-staggered grids. Numerical Heat transfer. Vol.13. pp. 125-132

 January 8, 2001, 20:58 Re: Colocated Craziness #7 Ha Lim Choi Guest   Posts: n/a I just wondering why you do not get the converged solution. There are two velocity components when one use the cell-centered, nonstaggered grid method; the cell-centered velocity and the cell face velocity. The momentum equations are first solved at the cell-centered locations using the pressure terms evaluated through the linear interpolation (central difference). Then, the cell face velocity components (usually mass flux instead of velocity components) are obtained through the interpolation of momentum equations for neighbouring cell-centered velocity components (Rhie and Chow interpolation scheme, momentum interpolation method). Using the momentum equations for cell-face velocity components, we derive the velocity correction equations for the cell-face velocity components, and there by the pressure correction equation. After solving the pressure correction equation, we correct the cell-face velocity components, and the cell-centered velocity components are also corrected using the linear interpolation of pressure correction field. These procedures are not well explained in Rhie and Chow paper. Many authors refined the Rhie and Chow scheme and I want to recommend to read following papers. The nonstaggered, momentum interpolation method is well established for a long time ago even for the unstructured grid situation and commonly employed in the most of commercial codes, such as FLUENT, CFX, STAR-CD, CFD-ACE, etc. (1)T. F. Miller and F. W. Schmidt, "Use of a pressure-weighted interpolation method for solution of the incompressible Navier-Stokes equations on a nonstaggered grid system, Numerical Heat Transfer, Vol. 14, pp. 213-233, 1988. (2)W. Rodi, S. Majumdar and B. Schonung, "Finite -volume Method for two-dimensional incompressible flows with complex boundareies", Computer Methods in Applied Mechanics and Engineering, Vol. 75, pp. 369-392, 1989. (3)S. K Choi, H. Y. Nam and M. Cho,"Use of the momentum interpolation method for numerical solution of incompressible flows in complex geometries; choosing cell face velocities", Numerical Heat Transfer, Part B, Vol. 23, pp. 21-41, 1993. (4)M. Peric, "A finite-volume methods for the prediction of three-dimensional fluid flow in complex ducts, Ph.D thesis, University of London, 1985. (5)M. Thomadakis and M. Leschziner, "A pressure-correction method for the solution of incompressible viscous flows on unstructured grids", Int. J. Numer. Methods Fluids. Vol. 22, pp. 581-601, 1996. (6) S. R. Mathur and J. Y. Murthy, "A pressure based method for unstructured meshes", Numerical Heat Transfer, Part B, Vol. 31, pp. 195-215, 1997. I hope it helps Ha Lim Choi

 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 harshad OpenFOAM Running, Solving & CFD 1 September 30, 2010 04:43 MASOUD FLUENT 3 September 16, 2010 17:50 ibuki FLUENT 0 January 5, 2010 08:37 paka OpenFOAM 15 July 21, 2008 05:03 mimě Siemens 1 June 17, 2002 08:29

All times are GMT -4. The time now is 01:56.

 Contact Us - CFD Online - Privacy Statement - Top