Hello everybody,
I am trying to solve a heat transfer problem(conjugate heat transfer )by the fluent, which is a heat transfer enhancement in a rectangular channel with baffles. The problem is a rectangular channel with a 1 m length and there is heating by constant heat flux from the above and lower plates(The aluminium heating plates are 3 mm in thickness) in the channel and there are solid baffles in a staggered arrangement on the lower and upper plates. During my calculations, I noticed that there is a reverse flow in many faces(about 1750 faces) at the pressure outlet, this number started small at the 25th iteration and increased to 1750 faces at the 450th iteration and remained constant after that. Before the exit section, there is a baffle on the upper surface and it is about 5 cm away from the exit section. I think this small distance between the baffle and the exit section is the main cause of reverse flow at the outlet, so I need to shift the exit section with enough distance from the baffle to prevent this phenomenon, What should I do in order to do this without any effects on the boundary conditions and the calculations?
Thanks in advance.
Ramy H Mohammed
I already made adiabatic section but I am confused about the boundary conditions of the plates' sides of the adiabatic section. Also, adding this section directly to the exit section will overwrite the boundary condition at the back sides of the aluminium plates, moreover whin I keep the back sides of the aluminium plates as a named selection and go to the boundary conditions list in the fluent, I explore that this B.C turned to a wall in coupled condition and I can't insert convection heat transfer coefficient.
Best Regards,
Hi Mohamed A. El-habet,
First, there is nothing wrong if you get a reversed flow. It will definitely not influence your solution much. You can check this by integrating energy and mass during the computation and see how much mass/energy is "lost/added" to the domain compared to the total values.
But I need more information in order to give a piece of appropriate advice! What are the forces in your model making the air move? What about the left side of the domain? Do you have an inlet BC? I assume you used the Boussinesq approximation to account for the buoyancy force? Are you interested in the transient or steady-state solution (in the case such a solution exists)?
I would consider an outflow BC. It would be correct for a fully developed flow, but again, it depends on what you are looking at :).
Best,
Antoni
Dear, Antoni Artinov
Thank you very much for your response. I used a velocity-inlet boundary condition with velocity magnitude normal to the boundary. The remaining boundary conditions are the same as these shown in the right side photo. My case study is time-independent(steady-state) and forced convection with higher Reynolds numbers (Re=12000,22000,32000).Your assumption about using the Boussinesq approximation is correct. I enabled this parameter by giving gravity value to the solver in order to account for the free convective losses from the sides shown in the figures.
Best Regards.
Dear Mohamed A. El-habet ,
I agree with Antoni Artinov , there is nothing wrong if you get a reversed flow. However, I do not really understand what you expect about this calculation. Please tell me.
Regards,
Increased the domain 2.5 times to that of the inlet. The reverse flow will disappear
Hi
you could use outflow pressure condition , it might help to disappear reverse flow. On the other hand, if the flux dose not have discrepancy between inlet and outlet , so let it go, there are not any problems. Also maybe using low under relaxation factors be helpful.
Hi Mohamed,
I think you should begin by investigating the quality of the mesh especially at the oulet BC. Try by refining more the mesh at the outlet and the reverse flow problem should diseappear. In addition, what is the temperature of the fluid that you have fixed at the outlet ? Do you have some experimental datat to compare with, especially heat transfer coefficient ?
Good luck for your simulation,
Hi Mohahamed, if you have Ansys fluent 19, you can use "Generalized K-w(GEKO)" turbulence model, I did it and there was good effect on the reverse flow after some iteration and it disappeared,
in addition
check your aspect ratio and skewness of your mesh, it should be near to good values ,, for aspect ratio try to it be between 1 and 70,
if you can set it more close to 1 it is better(However, up to 100 is acceptable) ,
for skewness the value between 0 and 0.8 it is good range , try to close it to 0 more(However, up to 100 is acceptable).
B.R
Ramin Alipour
Dear, Nazaruddin Sinaga
I use a pressure-outlet B.C at the outlet with backflow temperature of 300k which appears to be cooler than the upstream temperature of the flow before the exit. This appears when I view a temperature contour of the entire domain and I think It may affect the solution.
Dear, Ramin Alipour
Thank you very much for your response. I have tried the outflow boundary condition but I think this B.C requires a precise position of the outlet so that the reverse flow could not affect the solution. Also, the backflow temperature, in this case, is unknown which could cause a problem in the solution in case of reverse flow. My mesh is hybrid and combines between structured and unstructured meshes but I have modified it until I have reached reasonable qualities of orthogonality, skewness and aspect ratio, my problem is in the inflation region and it is the source of bad qualities . My model is K-omega (SST), but I am going to try the GEKO model due to its flexibility and its broadness in covering wide flow scenarios.
Thank you very much,
Best regards, Mohamed.
Dear Mohamed
If it is possible give me the inflation detailed and send some pics from your inflation areas that you fell with problem with it.
- Badges
- Science topic