CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   reversed flow in xxxx faces on pressure outlet (

franzdrs June 23, 2009 10:42

reversed flow in xxxx faces on pressure outlet
Hi all,
I have a small question: during iterations I get the warning message "reversed flow in xxxx faces on pressure outlet". The number xxxx goes down with iterations. then the solution converges and there are still about 1000 faces in the outlet with reversed flow. If I continue the iterations the number keeps falling, and probably it will reach zero (no more warnings). What does this mean? Is the solution not really converged when FLUENT says so
(according to the default residuals criteria)? IS the solution converged when finally there are no more faces with reversed flow or when this number stays constant?

-mAx- June 24, 2009 01:33

you have an vertex at the outlet.
It can slow the convergence, but it's harmless

Trev June 24, 2009 05:21

It also depends on what you are actually modelling aswell where reversed flow may physically occur. Such as in the modelling of hydrocyclones where the reversed flow message is desirable. If this isn't the case the messages will eventually subside but if they don't you could also try extending the boundaries where reversed flow occurs or reduce the back pressure on the outlet to suck the flow out of the domain.

franzdrs June 24, 2009 06:00

Hi, thanks for the answers. Trev, I am modeling a dryer for agricultural products. It is a pretty simple system. Yes, there could be a reversed flow if the bed of product does not make much resistance to the flow. In my case, this resistance could or could not be small enough to create reversed flow. I model the bed of product as porous media. If I disable the porous media region then I get reversed flow for sure. The problem is that the reversed flow starts happening at the beginning of the iterations at a high number of face elements of the outlet, it grows even more, and then it starts to drop. When the solution converges (when the residuals reach all 0.001) there are still around 1000 face elements with reversed flow. If I continue iterating after this convergence, the faces with reversed flow keep dropping and reaches finally 0. My guess is, that if the number of face elements with reversed flow stabilizes at some point before reaching 0, then that would be what is physically happening, but if the message eventually subsides, then the physical situation is without reversed flow. Am I right? Could somebody tell me? Thanks.

Trev June 24, 2009 10:51

If the number of faces with reversed flow keeps decreasing it is unlikely that the physical problem would exhibit much if any reversed flow. As a rule of thumb convergence isn't achieved until your residuals have flattened out and the mass flux is negligible. The standard 10-3 convergence limits fluent automatically imposes are not really sufficient for most cases so try iterating further till 10-4 or lower and put a surface monitor on the outlet for mass flow rate. Keep iterating till the mass flow rate has flattened out and the mass flux error is around 10-6. Then you can see if reversed flow is still occuring in which case it is likely to occur physically as the solution can be considered converged.

maysmech October 18, 2010 11:56


Please tell me the solution of this problem. i mean, how can we revise the problem to remove this error?

aalisha March 19, 2014 04:16

Reverse flow on faces
Hello, I am also facing the similar problem. I am working on a 3 blade tidal turbine and doing the calculations for the drag force on blades. It has a velocity inlet and pressure outlet. However, on every single iteration it shows a message saying that "reversed flow on XXXX faces on pressure outlet 11. The XXXX numbers first decreases and then increases again keep flowing this increase decrease thing. If any one can explain me what is the physical significance of this.

I mean what impact it will have on the turbine working. The results starts converging after 60 iterations.

rajann_786 February 26, 2017 02:23

It happens due to a poor quality of mesh, abnormal boundary condition at inlet/outlet, short downstream length etc.
Remedies are:
> if vortex formation/recirculation of flow near an outlet boundary, increase the downstream length.
> check the mesh quality, improve it.
> use higher order scheme
> At last reduce the relaxation factor if necessary.

All times are GMT -4. The time now is 23:51.