Heat Transfer On Adiabatic
 

Hi,

How to calculate heat transfer coefficient on adiabatic surface in fluent. For example; I send 50 santigrad and 10 m/s air on surface as a parallel flow. when I assigned 10 santigrad on surface, there exist heat flux on surface due to temperature difference and I calculate heat transfer coefficient easily. But there are not heat flux on adiabatic surface in fluent. Heat flux is zero. How to calculate HTC on adiabatic surface.

The term "adiabatic" means that there is no heat flux across the boundary. So why are you trying to compute the heat flux using an adiabatic assumption. If you choose adiabatic, then you have already determined that the heat flux is zero. If I am misunderstanding your post then forgive me, but it sounds like the solver is behaving like it should.

I am not sure about the sense of the question, the heat flux is zero because is zero the normal derivative while the heat coefficient is not vanishing?

Even thought adiabatic wall conditions were applied in analysis, CFD post calculates heat transfer coefficient. does anybody can explain how CFD post calculates this? I'm also very curious.

CFD post has no idea that the surface is adiabatic or not so it will calculate heat transfer coefficient on anything.

I have thought about this more and I think I got the answer.
Please give me your comments about my conclusion.
Actually heat transfer coefficient(HTC) is calculated value base on measurement. In the test we can measure energy transfer between them and also temperature then HTC can be calculated.
But in CFD, "measurement" is NOT exist. so if we want to know Q then we should know at first HTC. How to calculate HTC? it should be based on experimental equation such as Petukhov-Gnielinski heat transfer coefficient. Nu=(hL)/k so if we can calculate Nu then can calculate h (HTC). the calculation based on this experimental data is free from Q so it doesn't matter whether the wall is adiabatic or diabatic.

Forget HTCs for a moment and just think about wall heat flux. It seems like you're saying that CFD solvers must rely on some empirical correlations (like those based on the Nusselt number) in order to be able to calculate wall heat flux. But that's not true, the temperature profile in the fluid near to the wall can be resolved "from first principles" without resorting to any empirical fits, and from the temperature profile and fluid properties the heat flux follows.
Having said that, there is the (uncommon) possibility to only solve an isothermal flow (without the energy equation) and approximately infer "what the heat flux would have been" at a wall. Even in this case though I doubt you would use a Nusselt number correlation, instead, I believe one would ask the user for Prandtl number and somehow work with similarity of the velocity and temperature boundary layers. In Star-CCM+ this is called Virtual local heat transfer coefficient, in other software tools it will be called differently. But I haven't seen it used much to be honest. After all, if you're interested in heat transfer, you probably don't want to resort to approximations.

CFD post is a post processing only calculator, not a solver. It uses fixed formulas. If the input into the calculator is garbage then the output will be garbage as well.

Engine cooling simulations at a major german car company were done exactly this way for many years with StarCD. When you can win Le Mans with this type of simulation, it's probably not completely useless :-)

Hi,

I have a quick question. Assume a case where a fluid is flowing through a pipe. There is no heat transfer happening between fluid and pipe (disabled energy equation). Does this mean that CFD software will not give you the value of HTC for this case? If it gives, I would like to know how does it calculate? Thank you.

Hello FliegenderZirkus,

Thanks for your comments. please let me clarify a little bit more.
"from first principles" it means CFD governing equations such as momentum, energy, turbulent model and etc. Is it correct? and actually CFD solvers (CFX) do NOT use empirical equation to resolve convection heat transfer.
HTC and empirical equation (Nusselt Number) might be necessary in other ways, e.g. to assign wall heat transfer boundary condition, to extract HTC in the post. Is it correct understanding?

That's interesting, thanks for the insight. If you know what you're doing, many things are possible. For someone fresh in the field looking into a heat transfer problem, I'd still recommend actually solving the energy equation though..

There are two different cases. 1) You solved the energy equation in CFD and have real heat flux data at the wall. Then you can use something like CFD Post to convert the heat flux to HTC (given a reference temperature). If your wall was adiabatic, then as LuckyTran already wrote, the calculated HTCs will simply be zero. 2) If you didn't solve the energy equation in CFD (this is the case you are referring to) then it still may be possible to approximately calculate the HTCs based on flow data only. As I already wrote, I believe this would typically be done by using similarity of the velocity and temperature boundary layers, so you'd need to supply the Prandtl number. Whether CFD Post can do this or not I don't know, but my guess is that it can't.

I meant to say that if you know the temperature profile in the wall-normal direction and conductivity of the fluid, then you also know the wall heat flux. So in CFD with the energy equation on, you don't need any Nusselt number correlations. I think this is what you're saying in the first part of your post too. I don't quite follow the second part, can you elaborate?

Hello. FliegenderZirkus,

Thanks for your reply.

By the way, I think we need more clarification. at first, the question from me and the first post was how to calculate HTC with adiabatic wall. sometimes we make adiabatic CFD to provide HTC & Tbulk for structural FEA (e.g. ANSYS mechanical). Definitely we can provide better results with CHT analysis but it is too time consuming process and even for complicated system, it is almost impossible. So for this purpose we made adiabatic CFD and provided HTC & Tbulk to FEA engineers. It is some kinds of regular process which is well validated when I worked in Germany company. Even in adiabatic wall conditions, CFD post calculates a certain value of HTC which is actually unrealistic and too big. There are many way to improve its accuracy but I think accuracy is not the matter in this post. Since there is no heat flux, HTC should be zero as you wrote. But anyway it's NOT. So I think HTC is NOT calculated from the equation q=h*delT. then how it did? it was my question. Was it calculated based on empirical equation Nu number based on?
My second part you asked me elaborate is about this. More exactly saying, since we can calculate heat transfer through basic governing equations, why and what for we need HTC? And I thought it is necessary for, e.g. FEA or wall boundary condition setting. please give me your comments. Thanks.

I am not sure about the real issue but in the fluid the adiabatic condition is
q=k dT/dn=0 at the wall.
If you evaluate that in a post-processor software, are you sure it will be able to compute the discrete dT/dn exactly like in the CFD code?? It is sufficient to use a different formula for the derivative and you get differences.

Why don't you describe the process you're using in more detail? As already stated, many things are possible and depending on context, they can either be appropriate or not.

It sounds like you are fixated on doing the thermal simulation on the solid side in FEA instead of CFD. You say it would be almost impossible to do in CFD. What makes it possible in FEA? Aren't there the exact same challenges?

If I were asked to provide HTC and Tref as thermal BCs for, say, a combustion engine coolant jacket. Let's say the thermal simulation of the engine block and cylinder head need to be done in FEA for whatever reason. Then my first idea would be to do CFD on the fluid with energy equation on and assume a constant wall temperature slightly higher than the fluid inlet temperature. You can estimate approximately by how much the coolant warms up as it flows though the engine based on engine power and efficiency and prescribe a wall temperature that is slightly higher than the outlet coolant temperature. For example: inlet temperature = 95 degC, estimated coolant warm-up 5 degC, assumed wall temperature 105 degC. Not sure about the exact values. This way you get a physical heat flux at the wall and can extract any type of HTC you need without having to worry about the adiabatic condition. Now of course in reality the wall temperature is not constant, there will be hot-spots, and this is where the Newton's law of cooling assumes a linear dependency of heat flux on temperature difference between fluid and wall. Is this accurate? Often it's good enough, but if there's anything nonlinear going on, like boiling, then of course not. Such an approach is only a tiny bit more computationally expensive than not solving the energy equation and you save yourself the hassle of leveraging boundary layer similarity or anything like that...

Hello.

Finally I got the answer about the question what I & the first poster asked.
In CFX, but I think it would be the same for Fluent, it is different between laminar & turbulence.
Laminar flow : it will be calculated from q=hdelT, so CFD post does NOT show any HTC. it is zero.
Turbulent flow : HTC will be calculated directly from turbulence equation. The equation will be applied differently for each turbulence equation, SST or KE. The equation is in CFX manual.

Actually my question is about above.

Thanks for your comments.

CFX has nothing to do with CFD-post.

And are you sure it has answered your question? Because you are exactly where you started... lol What do you think happens when you have a laminar adiabatic wall and try to calculate an htc? Well I guess some questions can be answered by just listening to yourself.