changing velocity (outlet) BC to pressure outlet
 

the main purpose of this thread is how to change a velocity BC or the so called velocity inlet BC in fluent to pressure outlet. I did not have the pressure at outlet so I used velocity inlet (with negative sign in order to assign an outlet BC) in order to find the pressure.does this way work? cause there are some reverse flow on outlet although the same flux is passing through this BC



MORE DETAILS?



I will try to be very brief in explaining my problem if anyone needed further details feel free to ask.
in my case which is a distillation sieve tray
I have two inlet and two outlets.ALL OF THE liquid enters from one of the inlets and exits from one of the outlet
the same happens for the vapor phase.
I did not know the pressure at the outlets at first but the mass flow rate at the outlet is obvious.so velocity inlet
condition is used for the outlets.
I simulated hydrodynamics successfully and now I am tring to change BOTH of the outlets into pressure outlet BC.
when the pressure of velocity inlet BC is used reverse flow is reported by fluent at the vapor outlet.(and not the liquid outlet)
the reports showed that the same rate of vapor is exiting from Vapor outlet (although there are some reverse flow).
this reverse flow does not change as the iteration continues.
am I doing somthing wrong?
thanks in advance

Sometimes it is not realistic to have a pressure outlet. Have you specified the Operating Density in the Cell Zone Conditions panel to be the same as the gas phase? If not you may have a static pressure difference over the face of the outlet and consequently you may get reverse flow. Are the outlets perpendicular or parallel with the gravity vector. Also are you sing the full Eulerian model?

yes I have set the density in Cell zone condition to be the same as the gas phase
the outlet is parallel to the gravity vector and (g is on the opposite direction).
I dont understand what do you mean by FULL. but Im using eulerian model.



actually I realized somthing else too. when I set velocity BC I demand the BC to pass ONLY the vapor phase but there are a little liquid near the outlet. (volume fraction of liquid is about 10^-5) so the liquid velocity at this condition is on the opposite side of vapor and in to the system. (cause it cannot exit)
so when I change the BC to Pressure outlet there are some reverse flow for the liquid phase and not vapor.(I have checked it in report).
Ive let velocity BC to let a little liquid pass through this BC lets see what happens if I change to Pressure outlet afterward

Have you tried setting the gas outlet to pressure as this will remove the liquid without causing any continuity concerns. Keep the liquid outlet as a velocity inlet (with negative velocity as you have already done). This is the approach used for alot of multiphase separation equipment and works well.

yes I agree with you.
but I think I should re init my case. :(

You should not need to reinitialise as long as you have some solution still. You may need to lower the URF's though for it to stabilise but then it should not be an issue.

as I said earlier there is no divergence about pressure outlet. but there are some reverse flow(does not disappear even after long time) I said that its because of velocity vectors of liquid that is on the opposite directions of vapor at vapor outlet as I was using velocity BC. URF is used in order to reduce the risk of divergence or to reach a better convergence (correct me if I'm wrong) so I don't think URF is going to help
thanks in advance

I only meant that you should reduce the URF's when you change any boundary from say velocity to pressure whilst keeping the same solution as the starting point. URF's can then be increased afterwards. Very often I find that without a URF reduction when making a BC type change you get divergence. Hope all goes well.