My first deal with fluent were in 2005 in PhD thesis and passed 6 months before I detect the (h) in fluent is for only special cases. Trust me, calculate (h) with temperatures and heat transfer or fluxes extracted from fluent but not (h).

By the way...the h in fluent is changed with refernce temperature which is not logic to give variedh after processing to be changing according to other parameters

Hey,

Have you tried to plot the heat flux or Nusselt number? Do you obtain the same type of contours with these plots? If yes: there is some prob with the simulation, If no: it may be a just a post processing issue.

Cheers

 @Carlos

No, I have not plot them yet. I'll be getting back with an answer asap. Im checking these contours for one wall, not for a section.I guess that is the correct approach.

@Galina

On the mesh figure, the red surfaces indicate pressure outlet, the blue ones(they are opposite) indicate velocity inlets and the white surfaces(opposite) are walls(plates)

This question might sound too basic, have you turned on the Energy Equation in your model?

yes? Should I calculate it with no energy equation then turn it on?

It should be on for your calculation, please make sure this is activated (Image below). Why don't you try to get a surface integral over your faces of interest to check for the average heat transfer coefficient to find out if the calculations are throwing you a reasonable average value.: https://www.sharcnet.ca/Software/Fluent6/html/ug/node571.htm

If the number is good, then your issue is in the post-processing module. If not, something is wrong with the calculation.

Of course its turned on. Yes, I also had checked it through surface integral. I got a value but I still think it should have included different vaues on different locations. This attachment has a figure of velocity vectors of the middle plane. I think there must be higher  htc values where air passes. It doesnt make sense it is about 32W/m2K everywhere as you see in the first attachment.

I will suggest you first solve the 2D problem of flow over a heated flat plate to create the boundary layer problem. This is analytical solution and will give you some idea on how to solve the HTC problem.

Suggest you to look at the following link.

https://confluence.cornell.edu/display/SIMULATION/FLUENT+-+Forced+Convection

https://confluence.cornell.edu/display/SIMULATION/FLUENT+-+Forced+Convection

In the post processing software, can you get the plot for htc value along a line drawn on the surface of interest? It should give you different values if the line passes thought those different velocity regions.

I have seen this kind of problem and in many cases the problem is about the range used during the display heat transfer coefficient. Look to the auto range option and remove the check mark. write the expected range and look the differences. you can create a surface parallel to the plate but placed very close to the original and display the heat Transfer in this new condition. the result can help you to understand your problem. of course im considering the simulation process was fine.

Heat transfer coefficient is function of properties of fluid at film temperature, temperature differecne, temperature coefficient , buoyance force etc in natural convection. As Dr. Borrajo suggested, you can try auto range option.   

Nevet get Nu or h ftom fluent. calculate it using tepmerature and heat transfer

Perhaps，you should change the reference temperature

thank you all for your replies. 

@Mohamed

Are you sure that I should not trust the value h fluent gives? Have you experienced anything about it ?

Yes my dear 100%. Never use (not trust) the h values in fluent because its use for only special cases and your case is not from these specials.

My first deal with fluent were in 2005 in PhD thesis and passed 6 months before I detect the (h) in fluent is for only special cases. Trust me, calculate (h) with temperatures and heat transfer or fluxes extracted from fluent but not (h).

By the way...the h in fluent is changed with refernce temperature which is not logic to give variedh after processing to be changing according to other parameters

Most of calculation of physical parameters done by FLUENT is based on reference values. If you change the reference, the values will change. So the best way is solve for the values using FLUENT. Then export the x,y,z, values file to any text file or other software and perform the analysis there. Be it drag coefficient, nusselt number or whatever, if you depend on Fluent you may have to check the reference values regularly

h depends on many parameters like fluid velocity, temperature of fluid, specific heat of fluid and thermal conductivity of fluid and also boundary layer thickness, so it is not easy thing to find out the accurate heat transfer coefficient from CFD-Fluent. But if you model the problem correctly  then you will get almost nearest value. u can find the surface heat transfer coefficient from the wall fluxes contour. 

Dear All,

I also face the same problem in calculating heat transfer coefficient in Ribbed tube application by FLUENT 17. I am still confuse how to calculate average nusselt number in it. I also confuse to decide which is bulk temperature to calculate the heat transfer coefficient. Is that film temperature or LMTD temperature?

Thank you for your helps

Best regards

I agree with M. H. Shedid. I calculated (h) with temperatures obtained from Fluent, fluid properties and velocities (or mass flow) (needed for Re and Nu). Than (h) can be obtained from Nu ...

The physical properties of a working fluid, which are generally temperature and pressure dependent, are used to calculate dimensional characteristics. For the precise calculation of these characteristics, it is necessary to clearly define the temperature at which the physical properties of the fluid are taken.

The temperature of the boundary layer changes from Twall on the surface of the plate (tube) to the free fluid temperature at the outer layer of the boundary. The properties of the fluid depend on the temperature and they are changing analogous to the boundary layer. In order to take into account the change in properties with temperature, the properties of the fluid are usually defined for the temperature of the boundary layer. The properties of the fluid are then considered to be constant in these values throughout the heat exchanger.

Nu number is calculated for the temperature of the boundary layer.

The temperature of the boundary layer can be taken to be approximately equal (Twall + Tbulk) / 2

...

I am currently working in force convection heat transfer through pipe with nanofluid by using mixture model two phase flow. I am getting the fluidflow result correctly (like average wall shear stress, velocity magnitude etc). BUT I AM GETTING HEAT TRANSFER VALUE (LIKE NUSELT NUMBER) OVER PREDICTED. What could be the reason for that?

Dear Mladen

I am agree with your statement but what is the value for Tbulk, is it the average of Tin and Tout of refrigerant?. Kindly reply. Thanking you very much.

Regards

Yes, Tbulk is the average of Tin and Tout of refrigerant.

Regards

Thanking you very much for the prompt reply.

To calculate the local heat transfer coefficient, Tbulk is the average fluid temperature along the tube allover the tube. Average of Tin and Tout of refrigerant will not give you accurate results.

yes, ...it should be careful whether it is a local or average coefficient of heat transfer ...

Dear Mohamed,

Thanking you for the reply but how could i find the average fluid temperature along the tube?. Or may be it is equal to the average of wall temperature. Is it? please comment and give your important suggestion.

Dear Hardeep

It is a little bit tedious to get the local Tbulk but its result is more accurate. Go to SOLUTION XY PLOT window and select Temperature from Y Axis Function and Direction Vector from XAxis Function. Default interior of fluid must be selected from Surfaces. If you tried to plot these options you will get all fluid temperatures at each location (according to your mesh size in the flow direction). Instead of the plotting, you have to use tick WRITE TO FILE in the Option. Open that file from Excel program and you will find two columns (location and temperature). You will find many temperatures for same X location. With small program in excel you can average the different temperatures for each X location. These averages is the local Tbulk.

I hope you got my technique. You are welcome for any question.

Dear Mohamed,

Greetings!

Thanking you very much for the prompt reply and technique. I really appreciate your important feedback and will follow your describe procedure. Thanking you.

Regards

Dear Mohamed,

I am facing the problem to calculate the local bulk, as per your direction i choose the temperature from Y axis and X- axis direction and surface wall. But what i need to select the second option from Y-axis function (i.e.) just below the Temperature. Is it wall temperature or Total temperature?. Kindly guide me. Thanking you.

Regards

The boundary layer temperature can be calculated by the expression:

Tbl=(Tam-out surf+Tam-bulk air)/2.

The term represents the arithmetic mean of the outer surface temperature of the tubes and fins and the arithmetic mean of the free stream fluid flow temperature.

Dear Mladen,

Thanks for the reply, i am finding for the fluid side and for that i using HTC(heat transfer coefficient ) = Heat flux/ [(Tin-Tbl)], Tbl is found as per your and Mr. Mohamed guidelines and recommendation. If i am wrong, please correct me.