[kandelabr]

Hello!
I'm trying to calculate NPSH of a centrifugal pump but my interPhaseChangeDyMFoam simulation doesn't obey mass conservation. It also keeps minimum p_rgh very close to 0 (which is measured not true) and maximum p_rgh oscillates around set fixedValue by ~300%.
I guess it's a boundary condition issue.

What I have:
U:

• Inlet: flowRateInletVelocity
• Outlet: inletOutlet

p_rgh:

• Inlet: fixedFluxPressure*
• Outlet: fixedValue
• Walls: fixedFluxPressure

I use dynamicMesh for impeller rotation.

There are no tutorials or anything I could find for proper BC for such cases. Am I missing something?

Thank you in advance!

[kandelabr]

OK so after a ton of wrestling with the setup I found the problem.
I copied boundary conditions from the propeller tutorial.

The problem (as I can explain it at the moment) was that in the initial few timesteps pressures went berserk and induced cavitation which (at least in my specific geometry) then caused even more cavitation to occur which again did not help with convergence or anything at all.

I solved the issue by ramping up flow velocities and mesh rotation*:

0.orig/U:

suction_inlet
{
    type flowRateInletVelocity;
    volumetricFlowRate** table (
        (0 1e-9)
        (0.001 1e-9)
        (0.002 0.05)
        (100 0.05)
    );
    value uniform (0 0 0);
}

constant/dynamicMeshDict:

origin (0 0 0);
axis (1 0 0);
omega table (
    (0 0)
    (0.001 0)
    (0.002 628)
    (100 628)
);

Now I get results closer to what's physically possible - at least p_rgh is positive

Hope this is of any use to anybod.

EDIT:
** after some additional wrestling I discovered the main source of the problem: flowRateInlet must not be volumetric! In case pressure drops near the inlet (for whatever reasons, mainly numerical) flowrates change unphysically. So, set massFlowRate.
* with current setup, ramping up anything is not needed anymore.

Good luck!