OpenFOAM is FVM. Like FDM and FEM, FVM has its strengths and weaknesses. Some of these arise from where the nodes are positioned on the elements and how the equations are linked from one node and cell to the surrounding ones. No method is perfect for all cases. One of the problems you get into with a staggered grid FDM or the FVM used in OpenFOAM is the pressure ambiguity you're describing. This ultimately gets back to the difference in order between the continuity equation and the momentum equations (Navier-Stokes). You can get this Ebook for free on 12/16, 12/24, 1/1, or 1/9 https://www.amazon.com/dp/B082FPFN1M (see second half of Chapter 3)

Dear Bing Han,

actually, pressure driven flows are possible in OpenFOAM. You need a stable set of boundary conditions. The following are the BCs that I used for p_rgh and U to get a pressure driven flow running.

p_rgh inlet: prghTotalPressure

p_rgh outlet: prghPressure

p_rgh walls: fixedFluxPressure

(If you don't use p_rgh, you can also try totalPressure (inlet) and fixedValue (outlet))

U inlet: pressureInletOutletVelocity

U outlet: inletOutlet

U walls: noSlip

Please let me know, if the BCs helped to solve your problem.

Thank you so much for the explanation! Dr. Dudley J Benton. I roughly understand the meaning, I am also extremely grateful for your recommendation that absolutely is what I need to learn! Nevertheless, I think somehow Fluent and Star-ccm+ are embedded some algorithms to make the pressure-driven-flow equations be solved more stably than OpenFOAM does. I am curious about their difference in the way they handle pressure driven flows. I hope I could find the answer from your recommendation soon! Thanks again for your time!

Hello, Mr. Sebastian Borrmann!

I really appreciate your answer that is what I need at the moment! In my calculation, the model consists of one pressure inlet and two pressure outlets, and I used k-epsilon model by simpleFoam solver because of the nearly incompressible steady flow.

I first tried your 2nd suggestion -- "totalPressure (inlet) and fixedValue (outlet)", which moved forward for tens or hundreds of iterations before diverged every time, although I adjusted the p, U, k, epsilon, and nut many times. It is so unstable in my case.

For your first suggestion, I think it is an ideal pressure setting, but I got an error like:

"request for volScalarField rho from objectRegistry region0 failed"

I am not sure where to set the rho for it. Sorry that I am a newbie on OpenFoam. May be the prghTotalPressure or prghPressure are not suitable for simpleFoam solver? I attached my whole file as well, looking forward to your reply, thank you in advance!

I have tried many combinations of BC setting, including total pressure, fixed pressure, etc. As Mr. Sebastian Borrmann suggested, if the BCs were reasonably and stably set, the steady flow could be achieved even if both inlet and outlet were set by fixed pressures that is highly expected.

However, the solver tends to behavior unstably if fixedPressure is applied to both inlet and outlet, especially in a limited tube where the flow cannot develop completely. I am still working on this issue, if anyone has any idea, please feel free to leave a comment.

That is because you cannot have a fixed value of pressure in an outlet where velocity varies. That is a basic fluid mechanics principle where if velocity is somehow not homogeneus on a certain surface pressure will vary in order to mantain total pressure. You necesarily have to use total pressure boundary conditions where pO is the sum of both static pressure and dynamic pressure (i.e.: 0.5*rho*V^2).

The correct boundary condition for every pressure driven patch is totalPressure for the p specification and pressureInletOutletVelocity for the U specification. This has always worked for me. prgh conditions should only be used if your case considers gravity. In such case the pressure boundary condition will be corrected with the hydrostatic pressure.