[giof]

Hello everyone
I am new to Prostar.

I am trying to do a stationary mass flow simulation using these settings:
Stagnation Inlet: Pstag = 0.000E+00 for inlet
Pressure boundary Constant static pressure: P =-6.300E+03 for outlet.
SOLUTION PROCEDURE SIMPLE
RESIDUAL TOLERANCE 1.00E-03
FLUID FLOW TURBULENT INCOMPRESSIBLE
TURBULENCE MODEL HIGH RE K-EPS MODEL
REFERENCE PRESSURE PREF = 1.000E+05 Pa

The problem is simple because I know only pressure for inlet and outlet.

The solution diverges.
I also tried PISO solution algorithm but the solution diverges.
I did the same simulation using CCM and the solution does not diverges(the result is ok!)
I tried to change in prostar the inlet boundary using pressure boundary and it works but the results is not what I expect.

Using stagnation inlet in prostar there are master processor reported warnings in file star.info
Warning 020: The center of cell adjacent to boundary is outside the cell, 220768 or cell is concave



Can you help me?

Thanks in advance

[Blanco]

Are you using the same mesh between CCM+ and Star-Cd?
The warning you get is not so serious, anyway I would check mesh quality on the inlet boundary (you have some concave cells there).

Try to modify underelaxation factors for pressure and velocity, then note that a pressure-pressure boundary is not the best setup from a numerical perspective, if I remember well this is written also in the user-guide. Double check your simulation setup.

If your setup is really correct, then at last you can try to start with a small pressure difference between inlet and outlet, solve for it, then use the result to start a new simulation changing only the pressure difference (going to your desired value). This could help but I'm pretty sure this would work by changing only the underelax factors.

Regards,

Andrea

[giof]

Hi Andrea,
Thank you for your answer,

Yes, I am using the same mesh between CCM+ and Star-Cd.

I tried to change underelax factor using PISO solution algorithm but there is this error:
Error076 negative densities found at more than 100 cells.
I used underelax factor=0.5, 0.7, 1.

I did the same simulation(stagnation inlet/pressure outlet) using CCM and the result is ok.

Can it be a mesh problem?

Regards,

Gio

[Blanco]

Ok, the negative densities error means that something is wrong somewhere in the setup. I know that 2 pressure boundaries destabilize the sim from the numerical point of view, however if CCM+ can manage to give you a solution, also Star should be able to do it. This even if the mesh is not so good (in any case I would double check the mesh. Remember that you can see "where" you get negative densities...)

I would put down underelax factor for pressure to 0,1, 0,5 for velocity, to stabilize as much as possible the numerics. Then I would check boundary conditions and initial conditions: are boundary conditions very different compared to initial conditions? If yes, this could cause instability in the run-up of the sim (and hence negative densities). You could use a better initialization or a varying boundary conditions to start the sim.

The other option is to proceed with the other method I suggested (do a first run with reduced pressure difference between inlet and outlet, modify boundary cond., restart).

Good luck!

Andrea

[giof]

I partially solved the problem:

If I use SIMPLE solution algorithm and compressible flow changing also fluid initialization, it works.

If I try to run solver using the same setup but incompressible flow, it not works(Error012).

PISO solution gives Error076.

I'll try your suggestions and tell you, thank you very much!