[GasHighSpeedMixer]

Hi everyone

I'm currently simulating a high speed mixer for two gases. For that I'm using the solver reactingFoam (disabled combustion / chemistry).

At a certain / near outlet region, the mixture does not experience a perfect diffusion of the gas, since there is some backflow. However, I would like to avoid backflow and therefore I set the following boundary condition for the outlet:

outlet
{
 type            inletOutlet;
 inletValue      uniform (0 0 0);
 value           uniform (0 0 15);
 }

The flow direction is the z-direction. The inletValue is set to 0, so why do I have backflow? What could the reasons be?

Thank you for your help!

[geth03]

to guarranty mass conservation.
i suggest to extend the outlet pipe and do your postprocessing
at the area where backflow does not occur.

otherwise there is a BC available which extrapolates the flow from
the cells before the boundary, so you won't have backflow. for that
you specify the flow rate.

flowRateOutletVelocity:
Velocity outlet boundary condition which corrects the extrapolated velocity to match the specified flow rate

other BC:
https://www.openfoam.com/documentati...conditions.php

[Bodo1993]

Hi, I have the same issue for some of my simulations. In two dimensional domain, I have a single inlet and two outlets. The flow re-enters the computational domain and messes up the results. I have tried many outlet boundary conditions, extended the geometry and refined the mesh, but the problem persists. Please let me know if you would like to know more about the geometry I use.
I would greatly appreciate your assistance.
Best Regards,

[Tobi]

Originally Posted by Bodo1993

Hi, I have the same issue for some of my simulations. In two dimensional domain, I have a single inlet and two outlets. The flow re-enters the computational domain and messes up the results. I have tried many outlet boundary conditions, extended the geometry and refined the mesh, but the problem persists. Please let me know if you would like to know more about the geometry I use.
I would greatly appreciate your assistance.
Best Regards,

I am not sure about your experience and your analysis but the inletOutlet condition prohibits re-entering of flow. It acts as zeroGradient condition for outflow and a fixedValue condition for inflow (based on the sign of phi). Hence, if you set-up your things correct, you should not encounter any inflow there.

[geth03]

multiple outlet simulations can be problematic if boundary conditions are not correct or not specified sufficiently.

i face this problem myself a lot. i also tried every possible BC or combinations of those, to prevent backflow or even to prevent non-sense flows.
the best thing which works most of the time is when i use one fixed outlet velocity BC and one fixed pressure BC at the other outlet. in that case backflow at the pressure outlet might occur, but thats what works most of the time for me.

i do multiphase simulations, so it is much more complex bc complex physics is involved and sub-models play a role, too.

if backflow occurs, i further analyse the flow field. if backflow doesn't enter my area of interest, i do the analysis at the nearest pipe cross section. i also have situations where fluid flows from the velocity BC pipe back in my domain and then exits from the pressure pipe. it is really difficult to find out why it happens in this certain situation and works well in all others.

to sum up, multiple outlet problems (in combination with multiphase flow) is kind of complex and not as easy as normal one phase pipe flows or air flows around wings.

[Bodo1993]

Originally Posted by geth03

multiple outlet simulations can be problematic if boundary conditions are not correct or not specified sufficiently.

i face this problem myself a lot. i also tried every possible BC or combinations of those, to prevent backflow or even to prevent non-sense flows.
the best thing which works most of the time is when i use one fixed outlet velocity BC and one fixed pressure BC at the other outlet. in that case backflow at the pressure outlet might occur, but thats what works most of the time for me.

i do multiphase simulations, so it is much more complex bc complex physics is involved and sub-models play a role, too.

if backflow occurs, i further analyse the flow field. if backflow doesn't enter my area of interest, i do the analysis at the nearest pipe cross section. i also have situations where fluid flows from the velocity BC pipe back in my domain and then exits from the pressure pipe. it is really difficult to find out why it happens in this certain situation and works well in all others.

to sum up, multiple outlet problems (in combination with multiphase flow) is kind of complex and not as easy as normal one phase pipe flows or air flows around wings.

Thanks for the reply. I agree. I work also with miscible fluids, so the density of the mixture is not constant (although the two fluids are incompressible). Unfortunately, I do not know any information about the outlet velocity to set it as a boundary condition to one of the outlets.

In some cases, I just get some circulations at the outlets and in some others the flow exits one outlet and re-enters from the other outlet!

Kindly, I did not get "i do the analysis at the nearest pipe cross section", would you please clarify what is meant by the nearest?

[geth03]

what i am interested in is the separation process of two immiscible fluids, basically droplets in a continiuous phase.
so i have two outlets, which are pipes, one for each phase.
i have different kind of fluid properties (density, viscosity, droplet sizes, distributions, concentration, ...). for that i define a constant outlet velocity at one outlet and for the other i define a constant pressure.

so basically, backflow can occur at the pressure outlet, bc velocity doesn't need to point out from the geometry. it is system and geometry dependant, but i can't figure out why it works for one setup and fails for another.

one other problem is that my velocity BC is not correct (but there is no solution to this). droplets with different sizes move with different velocities, so there is a velocity distribution, but at the outlet they are forced to move in unison. so they are slowed down at that end, and if i am not lucky and the slow down happens fast, this phase will accumulate and change the flow field.

so when either backflow occurs or the accumulation changes the flow field, i analyze the flow in my main domain. if it looks good, i.e. no effect of those two, i will analyze the separation efficiency at the entries of those pipes.

[Bodo1993]

Right. Basically, we should ensure that whatever happens at the outlets (e.g. backflow) should be far from the region of interest (i.e. the one being investigated) so that the inaccuracies at the outlets do not affect the solution.