Dear ALL:

I am using the SIMPLER algorithm to firstly calculate the 2D duct flow. Giving the following BC: 1) Entry of a duct: imposed velocity, pressure unknown. 2) Exit of a duct: velocity unknown (0 neumann boundary condition: pu/pn=0 ), pressure imposed and equal to 0.

Both pressure and pressure correction equations were solved. The pressure correction results are only used to correct velocities. The pressure was diectly solved by the pressure equation.

The result for Stokes flow (no inertia term) is correct. However, with the Reynolds number increases (low only 100), the solution become worse. The calculation still converged, but result is not correct. The solved pressure at inlet is not constant and distorted.

Should I give a pressure BC at inlet? How to deal with pressure at inlet?

Thanks in advance. Jack

Some simple rules when dealing with incompressible flows (then always subsonic...): -whenever you impose the normal velocity, the pressure has to be unknown (free), hence if the velocity is imposed at the inlet pressure must not. -whenever the normal velocity is unknown (such as an outlet), the pressure must be imposed.

Your problem might not be related to the simpler algorithm, -do you use an upwind scheme to stabilize your scheme? -do you use a staggered grid or re-interpolation to make sure the space of approximation for pressure and velocity are different? -your relaxation parameters might not be correct.

regards.

See the following references for treatment of pressure boundary conditions in the SIMPLE algorithm. (1) S. R. Mathur and J. Y. Murthy, Pressure boundary coditions for incompressible flow using unstructured meshes, Numerical Heat Transfer, Part B, Vol. 32, pp. 283-298, 1997, (2) K. M. Kelkar and D. Choudhury, Numerical method for the prediction of incompressible flow and heat transfer in domains with specified pressure boundary conditions, Numerical Heat Transfer, Part B. vol. 38, pp 15-36, 2000.

There are two ways to treat the outlet boundary conditions (1) to specify the pressure at outlet : read above refernces. I think it is not correct to specify the outlet velocities using the Neuman conditions(du/dn=0.) when you use the pressure boundary condition. (2) to correct the outlet velocities to satisfy the overall mass conservation : for example the flow in the channel, during the iteration process, you can calculate alpa=(sum of inlet mass flow rate)/ ( sum of outlet mass flow rate) and then multiply alpa for the oulet velocities such as u(imax,j)=alpa*u(imax,j), and the pressure at the outlet can be obtained from linear extrapolation of that in the adjacent interior nodes.

I hope this helps,

Halim Choi

Thank you very much for your help. If SIMPLE algorithm, the problem should be Ok because the pressure is obtained by pressure correction equation. Pressure can be calculated refert to a reference node where p is set to zero. But, This is SIMPLER, pressure is obtained by pressure equation.

Yes, an upwind scheme is used to stabilize scheme. I use co-located mesh and interpolation like Chow and Chie to make sure the space approximation for pressure and velocity coupling. The relaxation parameters use implicit way in the solution of the algebraic equations. The relaxation parameter is 0.5 for velocities, and 1 for pressure.

regards. Jack

Thanks for Halim Choi's help for this peoblem. I will try to read the mentioned paers.

Best regards, Jack

I would agree with the points Seb Perron recorded in his message. However, I would expect that you have to check the value of Peclet number (convective/diffusion). You might try the power law scheme. For more information about treating the outflow boundary conditions read the two pages (102-103) and pages (129-130) for pressure boundary conditions in Patanker'a book titled" Numerical heat transfer and fluid flow". Best of luck