Hello All,

I have a problem with reversed flow in a pressure outlet. I have a large model (1.15e6 cells) which has a single velocity input and single pressure outlet. The model geometry is of a cooling jacket of an exhaust manifold with the approximate dimensions 20 inches x 8 inches x 15 inches.

The coolant or water enters the manifold via a single water rail inlet port. From there, the flow is divided and ported into 4 seperate runners to cool the individual exhaust gas runners. Towards the back of the exhaust manifold, the 4 seperate cooling jacket runners merge together and exit out a single outlet located at the back of the exhaust manifold.

I fully expect a lot of turbent flow, especially in the portion of the manifold where the flow merge together.

Running the analysis over 500+ iterations with the standard k-e turb. model, the residual plot seems to oscillate. I then reduced some of the under-relaxation values and reran the analysis. That seemd to help with the residual oscillations, but I still continue to have periodic times of reversed flow in the pressure outlet.

I am running a steady state analysis, so I am at a loss as to why I have periodic regions of reversed flow. I tried the same problem with identical boundary conditions in another CFD package and obtained good results without the oscillations. The alternative package used the standard k-e turb. model as well.

Not sure what is going on. Would love to hear from someone who might have an idea as to what is happening.

Thanks in advance.

Steve

hi, I had this problem before. I think the boundary condition of pressure outlet is not correct. You can modify the pressure outlet by adding a long hydraulic pipe, and define the pressure outlet at the end of the pipe. It doesn't influence the flow patterns in the domain. Good luck. Lisa

It may be due to disparity between velocity inlet and pressure outlet. is it possible to use outlet pressure at 1 atm (0.0 gauge)? also, can ou use pressure inlet instead of velocity inlet? it may be possible to use pressure inlet as a forcing pressure and pressure outlet open to atmosphere (hence 0.0 gauge).

Sometime, this can also be due to a badly constructed grid. However, if your flow is indeed splitting up due to some kind of a solid boundary, then I guess intermittent reversed flow sounds ok.

Thanks for the advice Lisa. I will give it a try.

I don't think it would be possible to use a pressure inlet BC for this problem. I have tried both a velocity inlet and a mass flow inlet BC, but both result in reversed flow in pressure outlet.

Lisa recommending to extend the outlet geometry. I can try that soon.

The current pressure value on the outlet I have set at 0 gauge pressure. I could try setting that at some no zero guage value, but I shouldn't have to.

[Lisandro Maders]

Steve, I would like to know if you have already solved your problem.. Because I have a similar problem in a simulation I'm doing,with the same boundary conditions.. If you want, you can send an e-mail to lisandro_maders@hotmail.com

Thank you

[rambex001]

The problem is often caused because of the fact that the position of the outlet is not really good. So that means that you have backflow conditions at the face of the boundary. You can handle that problem by setting the outlet boundary on another position.

The other thing you can do is to extend the outlet. This would not really influence your fluid flow. A good approach is to extend the outlet 7 to 10 times the pipes diameter.

I hope this would help.

[Lisandro Maders]

Yes, I will try to extend the outlet so.. Thank you for your reply!

[yuhehuan]

Hi,

I have a similar problem. I have already extended the outlet. But I am not sure the boundary condition of the original outlet. Is it interior? The result of simulation is that the mass flow rate of one of the outlets is minus and the other two are positive. The extended mass flow rate are minus. Does it make sense? I am so confused that why mass flow rate of the original outlets are not minus. Can I use the simulation results of velocity and static pressure at the original outlets directly? I am looking forward to your reply. Thank you so so much!

Regards

Originally Posted by rambex001

The problem is often caused because of the fact that the position of the outlet is not really good. So that means that you have backflow conditions at the face of the boundary. You can handle that problem by setting the outlet boundary on another position.

The other thing you can do is to extend the outlet. This would not really influence your fluid flow. A good approach is to extend the outlet 7 to 10 times the pipes diameter.

I hope this would help.

[rambex001]

Originally Posted by yuhehuan

Hi,

I have a similar problem. I have already extended the outlet. But I am not sure the boundary condition of the original outlet. Is it interior? The result of simulation is that the mass flow rate of one of the outlets is minus and the other two are positive. The extended mass flow rate are minus. Does it make sense? I am so confused that why mass flow rate of the original outlets are not minus. Can I use the simulation results of velocity and static pressure at the original outlets directly? I am looking forward to your reply. Thank you so so much!

Regards

Hi,
I'm not familiar with your problem. So if I understood it right you have on the one hand a inlet boundary condition (either a velocity or a mass flow inlet). On the other hand you have an outlet where the fluid exits the simulation area. Therefore i would not set the outlet boundary as interior (they are often used to replace them with physical models). I would set a pressure outlet with gauge pressure zero, so Fluent interprets a static pressure of environment in which flow exhausts.

[oj.bulmer]

It may help to understand your problem if you share some snaps of your fluid domain, along with the boundary conditions

OJ

[Destiny]

one of my student did thesis on diffuser and now am trying to get same results but am not able to get those again. am using same geometries as created by him but the difference in results is huge. There was no problem of flow separation in case of my student thesis but when i try the flow start to separate. so i need ur help guys. coz am not able to contact my student..

[yuhehuan]

Hi,
Thank you so much for your reply. I have a velocity inlet and three outlets. I set the boundary condition at outlet is outflow because I don't know the pressure at outlets. It's unknown. Because the distance from inlet to outlets is very close and I tried it there is reversed flow during the converging process. So I extend outlets to some place. Then the boundary condition at the original outlets is interior. The boundary condition at extended outlets is still outflow. So what do you think about the boundary?

Regards,

Rong

[oj.bulmer]

I am not sure how you extended the outlet. But if the outer most outlet is defined as outflow, then all the other interfaces that come before should be interior. From what you describe, it seems fine.

The minus flow rates are artifacts of circulation. Do you see a strong circulation in any of the simulations (using vector plot etc)? Also, are you sure the solution is adequately converged? Can you report the mass imbalance at inlet and 3 outlets?

Regards
OJ

[Destiny]

Thankx for ur reply..

bro can i send u my problem through mail..

my problem have 1 inlet(velocity inlet) and other is outlet(pressure outlet) and everything else is wall.

when i look at work of my frnd there was no separation at same point but in my case separation starts very early even at low angles of diffuser cone and swirl.

[imnull]

I do have same problems with reversed flow in FLUENT.

I did solve the problem in CFX with using opening boundary. And I know that my nozzle is over-expanded (back flow from the atmosphere at the end of the nozzle wall).

Is anybody knows how to solve the reversed flow in FLUENT???? (I need FLUENT because of CUT-CELL mesh). I did try - first order, solution steering, limits.. nothing helps... once I got reversed flow the solution is down..

WHY FLUENT DOES NOT HAVE opening boundary as CFX DOES.

BTW: my CFX simulation data are 95% in agreement with experiment

[asal]

Hello!

In this case if you have incomprehensible fluid, then the best for the outlets would be the outflow. you should assign the percentage of the inlet flow for each outlets, if you have multi outlets. Extend the outlets also work in this case. the original outlet should be specified as interior. moreover, course mesh specially at the outlets could be one of the reason of the reverse flow.
In most of the cases, after a certain iterations, this will disappear. other option is to apply a bit positive pressure over the outlet in the case of pressure outlet or outlet vent.
If you know the exact volume flow rate over each outlet, you can set the outlet as velocity inlet, but in opposite direction. you need to just calculate the velocity based on the mass flow and outlet area.
Hopefully it works!

[imnull]

Originally Posted by asal

Hello!

In this case if you have incomprehensible fluid, then the best for the outlets would be the outflow. you should assign the percentage of the inlet flow for each outlets, if you have multi outlets. Extend the outlets also work in this case. the original outlet should be specified as interior. moreover, course mesh specially at the outlets could be one of the reason of the reverse flow.
In most of the cases, after a certain iterations, this will disappear. other option is to apply a bit positive pressure over the outlet in the case of pressure outlet or outlet vent.
If you know the exact volume flow rate over each outlet, you can set the outlet as velocity inlet, but in opposite direction. you need to just calculate the velocity based on the mass flow and outlet area.
Hopefully it works!

Thanks. solved by Explicit + adapt gradient. 70K iterations (reversed flow was over 70K, but converged OK).

about outflow....
Note that outflow boundaries cannot be used in the following cases:

If a problem includes pressure inlet boundaries; use pressure outlet boundary conditions (see Section 7.8) instead.
If you are modeling compressible flow. (outflow can not be used with ideal gases!)
If you are modeling unsteady flows with varying density, even if the flow is incompressible.
With the multiphase models (Eulerian, mixture, and VOF (except when modeling open channel flow, as described in Section 23.3.9).
For an overview of flow boundaries, see Section 7.2.