CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)
-   -   BCs for pressure driven flow using rhoCentralFoam (https://www.cfd-online.com/Forums/openfoam/92055-bcs-pressure-driven-flow-using-rhocentralfoam.html)

eric.m.tridas August 31, 2011 16:41

BCs for pressure driven flow using rhoCentralFoam
 
1 Attachment(s)
Hey Foamers,

I'm attempting to model the airflow through a capillary into a vacuum system. The pump flow rate is 33 cubic meters per hour (which corresponds to an average velocity of 18.67 m/s through a KF-25 flange). The capillary is 65 mm long and 0.5 mm in diameter. I am trying to calculate the pressure in the vacuum chamber based on this pumping rate, therefore I do not want to impose any pressure boundary conditions on the vacuum side of the capillary. The inlet conditions are atmospheric.

The problem is that the simulation doesn't do anything when started. I believe the problem lies in my inlet boundary conditions. My BCs are as follows:

p:
inlet - fixedValue, value 101325
outlet - zeroGradient

U:
inlet - inletOutlet, inletValue uniform (0 0 0), value uniform (0 0 0)
outlet - fixedValue, value uniform (0 -18.674 0)

I've attached an image of my geometry for reference. The pump (outlet) boundary is on the middle of the face starting at (0.075, -0.05). If anyone is working on something similar or has encountered problems of this type your help would be greatly appreciated. Also, I can post my case if anyone is interested. Thanks in advance.

-Eric

tomf September 1, 2011 02:40

Dear Eric,

I think you should change your inlet velocity boundary condition. To a pressureInletOutlet boundary condition. This gives a similar behavior as the inletOutlet, but the inletValue is calculated from the pressure field. You may want to give a small initial velocity into the domain using the value as below. Or you may want to leave it at uniform (0 0 0)

U:
inlet -
{
type pressureInletOutlet;
value uniform (0.1 0 0);
}

Hope this helps,

Tom

eric.m.tridas September 1, 2011 13:19

Thanks for your reply Tom. Unfortunately the performance of the simulation remains the same while using your suggested boundary conditions. Do you have any other potential solutions?

-Eric

tomf September 2, 2011 04:01

Hello Eric,

Unfortunately I do not have any other suggestion regarding the boundary conditions. Did you check if the simulation would run if you apply a pressure at the outlet and some inflow at the inlet? If it does not run then either, something else may be wrong.

Tom

umer.chaudrey September 2, 2011 09:54

Hello Eric,

Try giving a pressure boundary condition at the outlet but lower value than the inlets atmospheric. Or even for a test case, try giving "0" pressure at the outlet and try running the case. It should run that way, I have been working on a slightly similar case and I used these boundary conditions.

Regards,

Umer

eric.m.tridas September 6, 2011 13:38

3 Attachment(s)
Hey guys,

Thanks for your replies. I've actually figured out part of the problem. I was expecting some transonic behavior from the system as the air flowed from atmosphere through the narrow section shown in the geometry. Because of this I had set my writeInterval as 1e-8. Even though I had put my writeControl as adjustableRunTime wtih a maxCo of 0.5, the flow wasn't moving as fast as I had anticipated. This forced the deltaT to be the value of my writeInterval. My simulation wasn't actually stalling it was just being forced into a very small time step which caused the appearance no motion.

Unfortunately I get some strange/unrealistic velocities and pressures as the simulation progresses in the narrow region of the model. As the simulation is started, the imposed velocity on the outlet begins to "pull" on the surrounding fluid, and this influence propagates from the outlet through the chamber. These strange velocities and pressures observed occur even before the fluid near the exit of the capillary is affected. I've attached a few pictures to show how the simulation looks before and after the strange behavior occurs as well as a close up image of the narrow region.

anon_a October 28, 2011 10:08

Hello Eric

A very important note: You must calculate your Knudsen number. If Kn > 0.01 (or maybe 0.1) your solution will be wrong, the Newton-Fourier constitutive equations are not valid and you need to use kinetic theory. You might want to check F. Sharipov & V. Seleznev, Data on internal rarefied gas flows. J. Phys. Chem. Ref. Data. 27(3), 657-706 (1998). Not even the dsmcFoam solver will work due to the very low velocities (your channel is extemely long compared to the radius so you will not reach transonic velocities).

It would also help to plot a legend along with your results to have an idea on the magnitude of the velocities.

Regards,
S.P.

Moslem January 10, 2015 10:31

Dear Eric,
I see that this is an old post. I wish you can help me on almost the same problem. I'm working on a similar problem. I want to simulate a nozzle flow expanding into the vacuum. I've implemented different pressure boundary conditions at the outlet. unfortunately non reproduced the correct flow condition. Would you please suggest the correct outlet boundary condition?
Regards.


All times are GMT -4. The time now is 15:25.