[vincenzolights]

Hello everybody, I'll be very grateful if some could reply to my unsolved question.
I'm dealing with a discharger in an open space. I have a velocity inlet condition at "Inlet1" and "Inlet2" and an outlet condition at "Outlet" (see the picture below for more detail about the geometry). From "Inlet1" the fluid has a density slighter bigger than the fluid from "Inlet2" and a velocity magnitude 10 times greater than "Inlet2", which leads a flow streamline spread both towards "Outlet" and "Inlet1". When the flow from "Inlet1" reaches the "Inlet2" deviates in an unphysical way due to Inlet boundary condition.
I know that a possible solution is to increase the length of the domain of a length necessary to reduce the momentum generated from "Inlet1" to 0 (I prefer to avoid this option due to computational costs), but I would like to know if there is a way to change the "Inlet2" boundary condition to allow that some portion of it became an outlet.
I know that CFX allows this situation with the "Open boundary" permitting to set the reversed velocity. I would like to obtain the same boundary in FLUENT because for other reasons I can't use CFX.
I read in other threads the possibility to use outlet boundary even at "Inlet2" and to allow the reversed flow but, in this case, I don't know how to set or control the velocity reversed flow. Could anyone help me with this issue?

[vinerm]

It depends on the setup. What is the reason for density to be higher at Inlet 1. Is it because of lower temperature at inlet 1 or is it because the fluids are different or their composition is different?

Just like pressure outlet, pressure inlet also allows flow reversal. In this case, you should use Pressure Inlet. In reality as well, flow will reverse on some fraction of the surface because of adverse pressure. Pressure Inlet will allow that while maintaining incoming flow on rest of the faces.

[vincenzolights]

Originally Posted by vinerm

It depends on the setup. What is the reason for density to be higher at Inlet 1. Is it because of lower temperature at inlet 1 or is it because the fluids are different or their composition is different?

Thank you very much for your fast reply. The fluid from "Inlet1" has a different composition from that one from "Inlet2".

Originally Posted by vinerm

Just like pressure outlet, pressure inlet also allows flow reversal. In this case, you should use Pressure Inlet. In reality as well, flow will reverse on some fraction of the surface because of adverse pressure. Pressure Inlet will allow that while maintaining incoming flow on rest of the faces.

My simulation has two incompressible and mixable fluids in subsonic regime. I have a velocity as input for my analysis. How could I convert it in "Gauge Total pressure" for "Pressure Inlet"?
I imagine that I should use the Bernoulli equation, but I don't know anything about static pressure.
The equation should be:
p_tot= p_stat + 1/2*rho*v^2 + p_ref
where my "Gauge Total pressure" is p_tot;
density and velocity and reference pressure are known and what about p_stat?

Thank you very much,
Vincenzo

[vinerm]

As long as the fluid is incompressible, static pressure is arbitrary. You can use any value and best is to assume 0 Pa gauge pressure. All that matter is pressure drop and not the absolute value.

[vincenzolights]

Originally Posted by vinerm

As long as the fluid is incompressible, static pressure is arbitrary. You can use any value and best is to assume 0 Pa gauge pressure. All that matter is pressure drop and not the absolute value.

I am truly grateful to you because your solution seems to work well. I lost a lot of time thinking about how to figure out this problem and the solution was so simple.
Thank you very much.

Vincenzo

[vinerm]

It is good that the option works.