[hsn]

Dear friends,
I am modeling a simple duct. there is an inlet and an outlet in my model and since my model is just a slice of a very long duct, I used a domain interface condition for the inlet and outlet and I just specified the mass flow rate. (completely like a periodic condition in fluent). this way, my output condition will be completely like my input condition as the problem converges. My goal is to see the heat transfer characteristics of the duct but because of the conservative interface flux condition, the fluid will become warmer and warmer as iterations go on. this means that in the result file, the temperature of the whole fluid is reached to the temperature of the wall. which is completely reasonable under these conditions.

In fluent, the situations is better. you give your upstream temperature to it and after each iteration it starts from that temperature at the inlet. and in this way the temperature of the fluid will not increase on and on. in better words, it is like you completely solve your velocity domain and after it is converged, temperature field is calculated based on its boundary condition and the velocity field available.
As you may know, velocity field is not coupled with temperature field but temperature field depends on the velocity field.


now, can any one give me any advice how can I set my problem so that the mass and momentum to be solved under the periodic condition but the energy to be solved by a constant temperature at the inlet and not going to a periodic loop of warming and warming...

Any help is highly appreciated as the deadlines are really near...
thank you.

[galap]

The velocity field of a compressible medium is coupled to its temperatur field due to density changes. So I assume you are simulating an incompressible fluid. As far as I know you can't implement a periodic condition for your velocity profile whereas your inlet temperatur is fixed.

So I would perform an isotherm and periodic simulation and then would use a velocity profile as inlet boundary condition for your actual simulation. The profile can be saved in CFD-Post.

[hsn]

Dear galap,
thank you for your reply. I think it works for a steady state case...
but what can I do for a transient simulation?

[ghorrocks]

CFX has a periodic boundary condition which can have a specified mass flow, so that will do what you want. I can't remember what options you have for heat transfer but hopefully you can do something similar.

Don't know about the transient case. I have never tried something like that, just give it a go and see if it works. I suspect it can be done, can't see any reason why not, but that is just a guess.

[hsn]

Dear ghorrocks,
Thank you for your answer. You have always been a great help...
you are right. but the only way to put a periodic condition is to use the interface. but as I said not only the momentum, but also the energy is also coupled on the 2 faces. this is the problem... iterations increase, temperature increase on and on. mathematically it is true, but physically, we dont have a thermally periodic condition...

[stumpy]

If your duct walls use a specified wall heat flux boundary, then you can use CEL to take the areaInt of Wall Heat Flux over the duct walls. Next apply a boundary source at the outlet to the energy equation that removes areaInt(Wall Heat Flux)@DuctWalls. This adds/removes the correct amount of energy before the profile gets wrapped around back to the inlet. This does not work with a temperature specified wall.

[hsn]

Hmm...
I see...
thank you stumpy...

[joey2007]

Hi HSN,
I was on conference some weeks ago. There was somebody who did it for chip cooling. They used user fortran.

Pin-shape assessment for interlayer cooled chipstacks with periodic boundary condition modeling (Gözde TöRAL et al.). One of the authors has a ANSYS address. Guess he implemented the code.

http://cmp.imag.fr/conferences/therm...Technogram.pdf

You may ask these guys. The fluent solution is quite limited by the assumptions used.

Joey2007

[hsn]

Thank you Joey2007
for your great help...