Hi all,

I am performing CFX 5.5.1-simulations on a chamber with one inlet (pressure boundary) and two outlets (both pressure boundaries). During the simulation the average pressure in the chamber is decreasing ...., keeps on decreasing ...., the outlets are biulding walls for 100% ...., only mass enters through the inlet ..., and still the overall pressure is decreasing. I am loosing mass.... Where does it go? Any explanation?

The inflow through the inlet goes over a restriction where Mach=1, so it can be seen as a sort of mass flow boundary. The mach number in the chamber runs up to 4.

Any help is appreciated, Pascale

What is the initial pressure field? What are the values used at the three inlet/outlets?

The initial pressure is 1000 Pa which is the reference pressure. At the inlet and outlets the relative static pressure is set to 0 Pa. After redistribution of the gas, the pressure near the inlet should drop to around -800 Pa (200 Pa absolute pressure). Near the outlets the pressure should increase to around 1000 Pa (2000 Pa absolute pressure).

Thanks for responding, Pacale.

Hi Pascale,

The problem seems to be the initial guess. Try restarting the run with a Local timescale factor of 2 or below, and slowly wean the solution by increasing this factor and finally with a physical timescale. Hope this helps

cfddoctor

Hi Pascale,

Am I missing something? You have specified the same pressure for the inlet and the outlet (zero relative), but you eventually expect ther pressure near the inlet to drop to 200 [Pa] and near the outlet to increase to 2000 [Pa]?

Regards, Robin

Hi Robin,

It is some kind of rotating piece of equipment. Low pressure in the centre, high pressure at the far ends.

Pascale

Perhaps you could be more specific about the pressures. Did you specify a total pressure at your inlet or a static pressure? As for the pressures you expect to see, are these total or static.

Also, If you expect to see a pressure rise across the system, why is this not reflected in your boundary conditions?

Robin

Hi Robin and cfddoctor,

The pressures specified are static pressures. The inflow and outflows go over restrictions. All restrictions have a high inlet pressure and a low outlet pressure. Mach = 1 is supposed to apply for all.

Of course, in the domain the pressure cannot rise spontaneously from inlet to outlet. However, i cannot elaborate on the physical process...

I will continue with the local time scales factors. Is there a way to let it rise automatically?

Pascale

Hi Pascale,

I don't recommend going to a local timestep factor. I think the problem has more to do with your boundary conditions.

A pressure specified inlet is not recommended as it does not define the momentum fully. I recommend specifying the total pressure at your inlet. This should give you much better behavior.

If it is a rotating problem, you timestep should be ~1/Omega, where Omega is the rotation rate in radians per second. You may want to start with a smaller value, but I do not recommend going smaller than .01/Omega. A good timestep to start would be .1/Omega.

You initial guess should also be reasonable. A rough estimate of velocity, pointing in the right direction would be good. A uniform pressure which is lowe than your inlet pressure and higher than you outlet pressure will help things move in the right direction.

Lastly, if you want to update the timestep during the run you will have to wait for 5.6. With 5.6 you can specify the timestep as an expression of iteration number (or time if it is a transient simulation). You can also update the timestep manually during the run using the new Dynamic Update feature (which also allows you to modify boundary conditions and other things).

Good luck. If you are still having trouble, contact technical support. You have some funky setup by the sound of it and support staff will be able to help you out a lot more if they can look at the problem.

Best regards, Robin