Hi,

I'm simulating combustion in a furnace. I want to set the flue exit as a pressure outlet, however I am not sure what is meant by the boundary condition 'back flow total temperature' required by the model.

Is the back flow total temperature the temperature you'd expect at the exit or is it the atmospheric temperature? Fluent says to apply realistic values. My expected temperatures at the flue exit are 1100K approx and exits to the atmosphere of 300K.

Which value should I use?

Thanks

Eric

It would be the temperature/pressure/concentration or other conditions that would exist beyond the boundary layer. It is mainly there in case you have vacuum-type pressure conditions within your system that may cause reversed flow across the boundary. So if your end point was directly a vent into air, you could put the atmospheric air data, but if you are looking at a less-than-macro scale process and there would be additional piping or processes before that vent, you'd put in what you'd realistically expect to have after the unit you're modeling (which sounds like your 1100degC conditions).

While it sounds like you won't expect any weird backflow, there will be the cases of the first few iterations having such conditions, and thus it would be a good idea to match the backflow to what you expect to avoid introducing weird errors during the first few iterations.

Hi, We have a high vacuum Physical Vapor deposition cylindrical chamber (PVD). It contains 2 inlets and one outlet. I have to see gas-mixing pattern of this two gas inside this chamber. I mean Velocity, density and pressure of this mixture at the different point of this chamber. There are two gases in the vacuum chamber namely Nitrogen (20%) and Argon. Nitrogen and Argon are continuously feed to the chamber and the pumps maintain constant vacuum. The initial pressure inside the chamber before supplying the gases is .006 Pa (6e-5 mbar). After supplying Nitrogen and Argon into the chamber through small openings, the pressure inside the chamber is around 0 .6 Pa (6e-3 mbar).I know the velocity and volume fraction of these two gasses and also know the chamber pressure. (Vxar=5e-4m/s, Vxn2=1e-4 m/s, volume fraction of Ar=. 8 and N2=. 2, Vy=0 for both case).

Could you kindly give me details idea about vacuum pressure setting of this chamber and also backflow mass fraction? With best regards,Rahman

I've not dealt with vacuum systems in Fluent, but I would suspect that your backflow conditions should basicly be what you expect to be seeing in your output line (what the pump is pulling off): gas composition at 0.8/.2 Ar/N2, and temperature at some value (if you have the energy equation in place). The pressure to use at the end is probably (best guess) what your chamber pump is pulling, which sounds like around 0.006Pa. Remember that you're setting the gauge pressure in fluent, so you should be entering a negative number here (0.006Pa - expected atmospheric). What you should be seeing is that with the known velocity inlets, the pressure in the model should achieve the pressure you see by experiment (0.6Pa). But again, I've not dealt with vacuum systems in FLUENT, so it may be necessary to tweak the output pressure setting to get this correct.

As stated to the previous problem, the backflow conditions sound like they will never enter the final problem solution, as you'll always have 'positive' flow across the outlet face, but they should be set close to what's expected to be crossing as to keep the solver happy during the initial iterations of the solution.

Thanks for your suggestion. I have some question regarding ur answer...

I am using velocity inlet and pressure outlet boundary condition. According to your suggestion as i guess i have to set operating pressure=101325 Pa and gauge pressure at pressure outlet bc panel=(0.006-101325)Pa[absolute presure=OP+Gaguge pressure=.006 Pa].Is this pressure fixed or it will be become 0.6 Pa(absolute) after few iteration.

if not...will it be set up automatically roughly that pressure(~0.6 Pa) as u mentioned or where i have to set up working pressure(0.6 Pa) i mean pressure that will come after entering gas inside the chamber. And what about initial pressure?

[just for your remainder... before i used species transport model, laminar, compressible flow, steady state model with velocity inlet bc and pressure outlet. .i set OP=0 Pa, Gauge Pressure=.6 Pa and Initial pressure=0.006 Pa. and i set backflow mass fraction of N2=0.20....but i have not gotten any good result...it seemed to me during animation gas is starting flow from outlet like reverse flow...]

Would u kindly give me some idea from where will i get idea about vacuum system modelling in details (say any documents, log file etc)?

Thanks again and waiting for your reply…

rahman

First, after I posted, I completely forgot about the operating pressure setting. You can change that to zero, such that you can enter your pressure directly instead of subtracting out atmospheric. Make sure to place the reference point near/at your exit port so that this is considered as the reference pressure.

I just tried a simple version of your problem, and had no problem getting the conditions set up using a simple 1cmx1cm 2d cell. Velocity inlets were as stated through 0.02cm holes, outlet was 0.04cm. The pressure outlet was set to 0.006Pa, with 0.2N2 in the backflow composition. All temperatures kept at 300K. I used an initial guess of P as 0.006Pa through the system. After a few iterations, the flow pattern was pretty much developed, and the system had a higher pressure around 0.1-0.2Pa, though the profile through the cell varied. The 0.6Pa value should be what you'd get near the point where the pressure is being probed in your system, but you shouldn't enter this into the problem statement. (Alternatively you could set up the initial guess to be 0.6Pa, but again, your outlet should be at 0.006Pa -- this may help prevent the initial reversed flow that you're seeing since you're driving flow with pressure, but you should let the solution iterate for a while to see if the reversed flow eventually goes away in your problem).

If this isn't converging, you may need to check the grid and refine it near the inlets and outlets as, as by my quick test, that's where the largest gradients in flow profile and concentrations are, as well as near the walls.

Many many thanks for your suggestion...

Would u kindly send me the sample version of my problem that was u done as reference? i will be pleased for that. still i have faced some problem ..if u want i can sent my cas file with details of my modelling to you for your kind review... my email address is md.rahman5@mail.dcu.ie Thanks again for your time Rahman

Unfortunately, I don't have any easy way to send or recieve case files, but I can briefly summarize how I set up the problem in GAMBIT:

- Created a 2x2 XY centered plane

- Using the line split tool, I split the face on the left to create vertices at y=0.74 and 0.76, and -0.74 and -0.76; these will be the entry holes. (Use the coordinate part of the panel, setting x=-1 and y to the values above, instead of trying to playing with the U value)

- Same split line tool, split the right plane with vertices at y=0.02 and -0.02 for the exit hole. (same as above, x=+1 now)

- Mesh all edges with 0.01 spacing

- Mesh the face with the default meshing scheme (should work out to be Hex/Map since the edge meshing should have equilvalent # of points and resulting in a mostly rectangular grid)

- Assigned the small edge on the top left as the Ar inlet, the bottom edge as the N2 inlet (velocity inlet), and the right small edge as the outlet (pressure outlet). Left everything else as the default (walls and fluid).

- Export 2-d mesh to FLUENT

- Scaled mesh in FLUENT to reflect construction in "cm" scale. (make sure to "Change Lenght Units" AND to "Scale", otherwise your size will still be weird and you'll get odd results).

- Added species model, and rest of steps as designated by the problem.

Another thing if you are still getting a reverse flow to start with from the exit port, is to set your velocity initial condition to push the flow towards the hole. So if you have your 4e-4m/s and 5e-4m/s flows as stated and the exit direction on either the x, y, or z axis, I'd set the velocity to 5e-4m/s in that direction for the entire problem space and work from there.

thanks for your reply.. i am going to model first as u described...then i will let you know about my soluion.Regards...rahman

Hi, i am writing you after a long break. I have modelled as you described. But i have still gotten problem with pressure value. Pressure was increased initially inside the chamber but after some iteration pressure became very low value again...i used species transport model also...could you kindly outline me your fluent set up of this model that was you done before. Thanks for your time..Rahman

[ksiegs2]

Is there a way to disable the possibility or reverse flow in a pressure outlet? I have a low-flow simulation case in a flow-through reactor and my residuals keep blowing up when the simulation detects reverse flow across one or more cell faces in the pressure outlet.

[hello123]

Hi Kate, I am currently trying to simulate a low-flow simulation case and am facing the same issues as you were, may I know whether you have managed to solve your problem?