[mehranjangh]

Dear All

I am trying to simulate a multiphase flow in the annular space btween two pipes in FLUENT, I have tried using the outflow boundary condition but my solution does not converge and FLUENT itself recommends using a pressure BC for multiphase flows. However I have no idea what the outlet pressure would be (Cannot find experimental data either) and I fear that if I choose a wrong outlet pressure, this would affect the results (I am trying to determine the concentration of sand in the annulus) and render them useless.

Could anyone please suggest a reasonable way to guess the outflow pressure and would that choice actually affect the results in a significant way?

Best regards
Mehran

[sbaffini]

Not a multiphase expert but:

1) Following the Fluent guide is usually ok

2) For single phase incompressible flows, the outlet pressure value is meaningless if you also DON'T HAVE an inlet pressure but, say, a mass flow rate (that is, if you don't specify pressure on more than a boundary). But I don't know if this also applies to multiphase flows in general.

[mehranjangh]

Since I am modeling an incompressible flow I am using a velocity inlet condition for the inlet which also asks an inlet pressure (which I usually leave at 0) so an outlet pressure would be reasonable (it should be negative of course since the inlet pressure is 0). The preblem is that I have absolutely no idea what to put and without it the steady steady solution does not converge (I have tried several values but I still have a backflow problem and the solution does not converge)

[sbaffini]

Originally Posted by mehranjangh

Since I am modeling an incompressible flow I am using a velocity inlet condition for the inlet which also asks an inlet pressure (which I usually leave at 0) so an outlet pressure would be reasonable (it should be negative of course since the inlet pressure is 0). The preblem is that I have absolutely no idea what to put and without it the steady steady solution does not converge (I have tried several values but I still have a backflow problem and the solution does not converge)

What solver are you using and which multiphase model? I don't recall any pressure required for inlets but, if any, that should be a value used in case an inlet cell face becomes temporarily an outlet, so 0 should be ok because if it is used it is a problem in itself, independently from the value.

For what have you tried several values? Outlet pressure? So it doesn't work neither?

[mehranjangh]

I am using the pressure based solver since the flow is incompressible and the velocities are small (0.5 m/s) As for the multiphase model, I am using the Euler-Euler model. In this case the inlet boundary conditions for the mixture requires the input of an initial gauge/supersonic pressure.

[niranjan863]

You don't have to worry about initial gauge/supersonic pressure. Fluent uses this pressure when inlet flow is supersonic. Since the flow is incompressible you can leave it as 0 and fluent will not use it in the calculations.
As far as the reverse flow is concerned is gravity included in the simulation? If the direction of gravity is not normal to the outlet, you are likely to get a reverse flow.

[mehranjangh]

Yes, gravity is included and its direction is perpendicular to the flow direction (I am simulating flow in the annulus between two concentric pipes)

[niranjan863]

If gravity is perpendicular to the flow direction, then you will likely get reverse flow.
This is because the pressure at the outlet is will to be hydrostatic, but pressure outlet BC will make the outlet pressure constant.
One way to over come this is to create an 90 degree bend at the outlet. The new outlet will now be along the direction of gravity and reverse flow will be avoided.

[mehranjangh]

Thank you, so in order to prevent reverse flow should I set the gauge pressure to zero (the same as the velocity inlet gauge pressure)? Or should I put a negative number (which I cannot calculate since the flow is multiphase in an annular geometry and there are no good formulas for that which I could find and there are no experimental results directly translatable to my case)?

[aero_head]

Originally Posted by mehranjangh

Thank you, so in order to prevent reverse flow should I set the gauge pressure to zero (the same as the velocity inlet gauge pressure)? Or should I put a negative number (which I cannot calculate since the flow is multiphase in an annular geometry and there are no good formulas for that which I could find and there are no experimental results directly translatable to my case)?

It would help to do a literature survey to see what has been done in papers for cases similar to yours.

[LoUcAsss]

Originally Posted by mehranjangh

Thank you, so in order to prevent reverse flow should I set the gauge pressure to zero (the same as the velocity inlet gauge pressure)? Or should I put a negative number (which I cannot calculate since the flow is multiphase in an annular geometry and there are no good formulas for that which I could find and there are no experimental results directly translatable to my case)?

One important aspect to know is that the Fluent solver (as many other solvers I guess) works with relative pressure as in the Navier Stokes you need to solve a pressure gradient. If the flow is incompressible, whatever the pressure you set up at the outlet (+1atm, 0, -1atm,...), you should get the same pressure gradient in the pipe.

One must know as well that Fluent works with an operating pressure Pop. And the absolute pressure Pabs is following:
Pabs = P + Pop.
P would be the local pressure computed by Fluent.
To change that operating pressure you need to double-click on boundary conditions and at the bottom of the task page a button "Operating conditions" appears.

Therefore if you're working on flows which strongly depend on the pressure such as cavitating flows or compressible flows you have to set up correctly both the outlet pressure and the operating pressure.

Another point to mention, in multiphase flow, the speed of sound varies greatly with the volume fraction. For a continuous air flow the speed of sound will decrease with the increase of the particle volume fraction. It will reach a minimum and rise again. Why am I pointing out this ? In the case of air and water flow, the speed of sounds drops to a few dozens of m/s. Better double-check the volume fraction, the averaged speed, to be sure that you're not expecting shockwaves in the flow.


To finish concerning the reverse flow, if you have some reverse flow at only a few cells, Fluent can easily deal with it. Otherwise you can follow the suggestion of Niranjan or you could stretch the pipe far away from the area of interest.

Cheers,
Lucas