# pressure Poisson equation in fractinoal step metho

 Register Blogs Members List Search Today's Posts Mark Forums Read October 7, 2000, 00:25 pressure Poisson equation in fractinoal step metho #1 Rui Guest   Posts: n/a Hi, all: I was mixed by one problem for some time and wonder if there is someone can cast some light on my head. I am solving the flow in a straight channel, the driving force is body force. The pressure at the both ends is zero (expose to air). There are two cases: 1. Body is parallel with the straight channel; 2. Body force has component both norm and parallel to the straight channel. My NS solver is the unsteady state, fractional step solver. Of perticular importantce, my boundary condition for the pressure Poisson equation is: a. zero at entrance and exit b. zero Neumann at bondary The solver gives reasonable result for the first body force case,but for the second case where there is force towards the wall, the calculation is totally off: the velocity is no longer parallel to the wall, and some streamlines intersect with the wall. I think there must be something wrong with my boundary condition for pressure. I have tried: 1. Change the B.C of pressure to full-Neumann(except a single point), but the solution blow up even after the first step. I guess there must be some people in this community have encountered the samiliar problem (basically this is a case where strong body force dominates the solution, this should be the case for turbo-machine simulation), and wonder if you can offer a hand. In all: 1. Is fraction step solver good for this kind of simulation? 2. what is the proper B.C for pressure. Thanks. Rui  October 8, 2000, 13:30 Re: pressure Poisson equation in fractinoal step m #2 Chidu Guest   Posts: n/a I would say in the case where the body force is not along the flow direction the pressure field is not obvious. It would be better to put a Dirichlet condition on the pressure at the exit and a Neumann condition at the inlet. Infact this is the way to do it in both the cases. regards, chidu...  October 8, 2000, 15:35 Re: pressure Poisson equation in fractinoal step m #3 Rui Guest   Posts: n/a Hi, I have tried this, but it does not cure the problem, my thinking is that: The poission equ is: Laplace(P)=f(x,y) for case of body foce not parllel to flow direction. if 3 Neumann and 1 dirchlet applied, then the solution of it would be P=g(x,y), and dp/dx is not zero. Starting from u=v=0 and a body force of F(y)=F1*i+F2*j, then: for the first step, u*=F1*dt+0 v*=F2*dt+0, note we have du*/dx=0 here; for the second step, based on the above, we have dp/dx not equal to 0; for the thrid step, u=u*+dp/dx*dt, then du/dx is not zero, thus dv/dy is not zero from continuity equation, thus it is imaginable to have v not equal to 0 in velocity field, thus the streamline intersect with wall. What really need is that the pressure solution will make a dp/dx=0 and dp/dy=-F2/dt so that in the third step the v velocity generated in the first step will be killed to be zero. But how? rui  October 8, 2000, 20:04 Re: pressure Poisson equation in fractinoal step m #4 Jongtae Kim Guest   Posts: n/a Hi, there. Is your code based on colocated method? If then, there is a possibiloty for that kind of nonphysical solution near boundaries. This is because of incorrect pressure gradient calculated. I recommand you to solve a problem which is a cavity flow with buoyancy force. Two side walls are adiabatic or symmetric, and top wall is high Temperature and bottom wall has lower temperature. The exact solution is no velocities everywhere. If your solution is exact, I am wrong. But if you have velocities at the wall very very larger than others, you should find a way to solve that terrible problem. That kind of problem was already issued in some papers.  October 8, 2000, 21:57 Re: pressure Poisson equation in fractinoal step m #5 Sebastien Perron Guest   Posts: n/a I use a fractional step solver, and never had such problems. But I know, in some particuliar cases you can have problems. 1) If you do a complete splitting of the operators (i.e. remove the pressure gradient from the momentum equations) the solution can be highly dependant on the velocity and time step (even for stationary cases) if you use an implicit scheme. But if you use an explicit scheme for the convective terms and a implicit scheme for the diffusive terms, you will get far better results. But, if you do a complete splitting of the operators, the boundary conditions for the velocity have to be changed. (Look for the work from Kim and Moin). 2) Your boundary conditions could be incorrect. Usually, the boundary conditions for the correction of pressure is such that at the end of the time step the normal velocity at the wall will agree with the boundary conditions for velocity. As an exemple: -d(delta p)/dn=(1/delta t)(vb-vn) vb= normal velocity imposed at the boundary (usually zero for a wall) vn=normal velocity at time t=n+1/2. (the one that as to be corrected. Good luck  October 9, 2000, 00:14 Re: pressure Poisson equation in fractinoal step m #6 Rui Guest   Posts: n/a hi, thanks for the response. My method is something like colocated method (I am not using FDM, FVM so, I am not very sure what would be it proper name). I would look into the thing you suggested. But I think the possibility is not large. I will try. thanks.  October 15, 2000, 04:57 Re: pressure Poisson equation in fractinoal step m #7 Tony Guest   Posts: n/a The original NS eq¡¯s (not including free-surface problems) do not require a pressure BC except for a reference pressure datum. Applying Green¡¯s identity to the pressure Poisson eq due to time splitting (or projection), the boundary integral can be converted to only contain the velocity components at the mid timestep (n+1/2) (if Crank-Nicolson for time). It will vanish at solid boundaries no matter it is slip or nonslip. At the exit or entrance, use the velocity updated. So, there is really not need to bother yourself on the so-called pressure BC, since it is not there. Thread Tools Search this Thread Show Printable Version Email this Page Search this Thread: Advanced Search Display Modes Linear Mode Switch to Hybrid Mode Switch to Threaded 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 Off Pingbacks are On Refbacks are On Forum Rules Similar Threads Thread Thread Starter Forum Replies Last Post Allan Main CFD Forum 13 January 14, 2013 12:49 renyun0511 OpenFOAM Running, Solving & CFD 0 November 10, 2010 01:47 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 MÃ¡rcio Main CFD Forum 0 January 24, 2007 05:22 chandra Main CFD Forum 9 May 5, 2005 06:01

All times are GMT -4. The time now is 08:52.