[cfdsolver1]

Dear all,

I am trying to solve the attached problem using Fluent. This problem is very simple; however, I get "reversed flow in 102 faces on outlet 11" -kind problems.

The defined problem is mixed convection problem. Left wall is kept at 20 celcius degrees while right wall is kept at 100 celcius degrees. Inlet velocity is 0.0822 m/s. I define outlet as outflow. I have uniform mesh in my problem and x direction is divided into 60 and y direction is divided into 1000. The length of the channel is 3 cms and the height of the channel is 1000 mm.

Because of these "reversed flow" error, my solution(especially continuity equation) does not converge and this causes my solution not to reach steady-state and fully developed region.

Can you help me to find the error in my problem?

Thank you very much

[villager]

Maybe, you have forgotten to scale your mesh - default units for FLUENT are meters. And you have mm.
Also it can be a problem with mesh.

Best regards, John.

[jafarizade]

hi
how do you solve the problem?
using steady state solver or transient solver?
is it in laminar region or in turbulence one? i think it is a laminar case. right?
did you check the pressure outlet boundary condition too?
best regard

[Aaron_L]

Hi,cfdsolver1

have you solved your problem? I encountered the same problem too, can you give me some suggestion?

best wishes,
Aaron

[cfdsolver1]

Hello Aaron. I have solved that problem by adding a dummy region at the outlet. I suggest you adding a dummy outlet region to your problem.

[Aaron_L]

hi, actually I have encountered a "reversed flow" in openfoam, then I doubt maybe it's my openfoam solver wrong, so I took fluent for comparison, but I also encountered the "reversed flow" in fluent

At first, I doubt that a reversed flow should not be happened, but I found some experiment,see this article[1], show that "reversed flow" can happened in experiment.

Then I doubt maybe somewhere I misunderstood, what's your code validation benchmark? and can you recommend some mixed convection article(just in Upflow, buoyancy-assisted flow, mixed convection in vertical duct/pipe)?

[1]Gau C, Yih K A, Aung W. Reversed flow structure and heat transfer measurements for buoyancy-assisted convection in a heated vertical duct[J]. Journal of heat transfer, 1992, 114(4): 928-935.

best wishes,
Aaron

[cfdsolver1]

Dear Aaron, reversed flow at the outlet region, if you increase Richardson number significant, must occur due to satisfy fixed flow rate. The main problem of Fluent is outlet boundary conditions are designed to work through main flow direction. For instance, OpenFOAM has InletOutlet boundary condition for this kind of mixed convection problems. Which means, the outlet boundary condition acts as inlet or outlet. So, it might be easier to model it using OpenFOAM but I have no experience.

I suggest you the study of Aung and Worku (doi:10.1115/1.3246919). This study is old study, however it is analytical study. It is a good starting point for a comparison with Fluent or OpenFOAM numerical result.

[oozcan]

Originally Posted by cfdsolver1

Dear all,

I am trying to solve the attached problem using Fluent. This problem is very simple; however, I get "reversed flow in 102 faces on outlet 11" -kind problems.

The defined problem is mixed convection problem. Left wall is kept at 20 celcius degrees while right wall is kept at 100 celcius degrees. Inlet velocity is 0.0822 m/s. I define outlet as outflow. I have uniform mesh in my problem and x direction is divided into 60 and y direction is divided into 1000. The length of the channel is 3 cms and the height of the channel is 1000 mm.

Because of these "reversed flow" error, my solution(especially continuity equation) does not converge and this causes my solution not to reach steady-state and fully developed region.

Can you help me to find the error in my problem?

Thank you very much

First, you should calculate hydrodinamics diameter in 2d

what dimension is needed for developing ''fully development'' in your hand-calculations and is it inside in your geometry that you drawn?

for ınlet, you should define inlet temperature as well as velocity

inlet parameter is cooling down or heating up? So, mesh is changeable.

for steady state, coupled is best choice and URF could be decreased 20%