[TrII4d]

hey there,

i know this subject was discussed for many times ... but i didn't find the answer in one of this thousands threats.

of course the calculation for the HTC for laminar flow and steady state is:
HTC = areaInt(wall heat flux)@<interface> / (area()@<interface>*(areaAve(T)@<interface>-tbulk)

- i set tbulk to my inlet temperature
- the wall heat flux and area are for <interface> side 1 and <interface> side 2 equal
but i have a difference for the areaAve(T)<interface> side 1 and <interface> side 2

so my question is: what is the definition of T_wall ? is it the fluid side or solid side ...

anyway if i try both i get different values to the "direct" HTC calculation (areaAve(HTC)@<interface> side 1) ... what could be the reason for that? could be the reason that iam calculating conservative variables instead of hybrid values ? how is cfx calculating the HTC with conservative or hybrid ?

thanks in advance!

other b.c.:
grid: ggi
fluid: air
interface: fluid-solid

[ghorrocks]

At a solid-fluid interface the Twall parameter comes from the solid domain.

[TrII4d]

yeah that was my first impression, too ... and of course ... if i calculate the HTC with the temperature of the solid domain i will get a "better" result.

"better" means that the value is closer to the HTC value which i got from CFX with the CEL command areAve(Wall Heat Transfer Coefficient)@<interface>

But i won't get the exact value ... i tried to calculate the solid temp. with hybrid values but the result will not change ... actually i can not understand why i get different values if i calculate the HTC manually instead of using the CEL command ... :-/

In the CFX help i only found this explanation:
"For laminar flow modelling the wall temperature is just the local fluid temperature at the vertex adjacent to the wall." ... i have no idea what they suggest with that

[ghorrocks]

Be careful which variables you are using. The default conservative variables give you the condition assumed to exist over the entire control volume - sort of an average. The centroid of the control volume lies a little way into the domain, so represents the conditions a little way into the fluid or solid side from the domain. Hybrid variables can give you temperature of the interface, but you cannot do CEL expressions on hybrid variables.

"For laminar flow modelling the wall temperature is just the local fluid temperature at the vertex adjacent to the wall." is just a statement of the laminar heat transfer boundary condition. In laminar flow the control volume at the boundary is assumed to have the wall temperature. In turbulent flow the wall functions can mean there is a jump in temperature at the wall to account for the laminar sublayer which is not modelled directly.

[TrII4d]

hi ghorrocks,

first of all ... thanks for ur great support!

Originally Posted by ghorrocks

The centroid of the control volume lies a little way into the domain, so represents the conditions a little way into the fluid or solid side from the domain. Hybrid variables can give you temperature of the interface,

that's why i would prefer hybrid values (sounds more logical for me if i check the theory of heat transfer)

Originally Posted by ghorrocks

but you cannot do CEL expressions on hybrid variables.

that's interesting ... i didn't know that ... this will be a problem because i'm using a perl script for doing my post processing

Originally Posted by ghorrocks

In laminar flow the control volume at the boundary is assumed to have the wall temperature.

but i have a difference when i calculate the temperature of side 1 (fluid side) and side 2 (solid side) ... although if i set t_wall as one of this temperatures i won't get the same result as CFX with the wall heat transfer coefficient function ...

my problem is to find the CEL function which calculates the "real" wall temperature ...

[ghorrocks]

Let me clarify the laminar comment - the face of the control volume which forms part of the interface has the wall temperature. The control volume will have whatever thermal conductivity says the region that far away from the wall will have. So if the boundary is a solid/fluid interface then the fluid side and solid side control volumes will be slightly different as they represent control volumes slightly into their respective domains.

The CFX doco talks about a variabel called 'Surface temperature' but it does not seem to be listed in the available variables.

[TrII4d]

hmm ... where exactly did u find the variable 'surface temperature' in the docu?
can u tell me the version, name of the book and side pls (f.e. cfx 14.0 CFX-solver theory guide, page 55-56)

actually its very sad ... CFX is calculating the HTC but u r not able to find the equation in the theory guide to understand what CFX is doing

[TrII4d]

I did some small studies for a plate, cube and cylinder last week ...

the results are:
- calculating HTC with the formula in the first post and with the temperature (conservative) from the solid side it gives the same value as CFX (for hexa and tetra mesh)

- in a first study i used Tw=const. as BC ... in a second study i used q/(dt)=const. .... both give the result above

- i didn't check the calculation with hybrid values (cause of time problems)

- nevertheless if i calculate HTC for a complex geometry in a complex field size the difference are sometimes round <10% ... sometimes its <1% but i don't know why ....


if there are any other studies pls let me know ... thanks!

[flotus1]

Not sure if this is related to your problem, but the last time I used CFX for heat transfer simulations I had to activate the expert parameter "Tbulk for HTC".
Otherwise, CFX takes a temperature value somewhere in the flow as the local reference Tbulk temperature, which is inconsistent with the usual formula for heat transfer coefficients.

[ghorrocks]

Note this Tbulk for HTC expert parameter just affects the value reported for post processing. It does not change the heat transfer modelled in the solver at all - so it just changes the reference temperature used to report the HTC in the post processor.

[flotus1]

I didnt mean to imply anything else. Sorry for being a little unclear.
I just thought that when comparing heat transfer coefficients manually calculated from wall temperatures and heat fluxes to the ones calculated by CFX, the Tbulk for HTC option is the better choice.

[TrII4d]

Originally Posted by flotus1

the Tbulk for HTC option is the better choice.

yes it is ... u will find this statement in "Heat transfer coefficient calculation for analysis of ITER shield block using CFX and ANSYS" Xiujie Zhang et al., too.

[flotus1]

So you were already aware of this and used the expert parameter?
Then I have some doubt about the expression you use for calculating the average heat transfer coefficient manually.

Instead of:
areaInt(wall heat flux)@<interface> / (area()@<interface>*(areaAve(T)@<interface>-tbulk)

try to use:
areaAve(wall heat flux/(Temperature-Tbulk))@<interface>

[TrII4d]

yeah i already used it ...

your equation is still the same ... iam calculating with the heat flux and you are calculating with the heat flux density ... both is possible and both give the same result

[flotus1]

They dont give the same result if the wall temperature or heat flux is not constant. I just tried that in CFX.
My alternative expression recovers the area average of the heat transfer coefficient in this case.
The other expression does not.

[TrII4d]

okay this can be possible ... but in my case i always calculated steady state .... so there were only three options for BC and i chose two of them (Tw=const. or Q=konst.) ... but your statement is an interesting information ...

[flotus1]

I didnt mean constant in time, but constant in space. The case I tried is a laminar steady-state flow with =const.

[TrII4d]

oh ok ... interesting study ... now i got your point ... i will try your alternative equation for the complex geometry (because in this case Q is not constant in space) ... hopefully i can give feedback by next week !

[Shaheer]

Hello, I was having some problem obtaining the heat transfer coefficient on the wall of the body i want to heat up. Technically since the body heat up and the heat flux decrease the heat transfer coefficient should more or less be same at given location of the body. However the problem i am facing is there is a steady decrease of the Surface heat transfer coefficient to 0. I put the reference temperature to the highest temperature of the system in which case i chooose the inlet plane from where heated gas comes in.
I tried to find the wall heat flux and it says that its undefined.

[MiloslavDohnal]

Hi everyone,
yesterday, I have faced the very same problem. I have spent almost whole day by hacking it. The problem is not in the equation itself, but if you check temperatures on each side of interface, you will find they are different. And CFD-Post calculates HTC as a difference between those two temperatures. Which means:

in CFX:

areaAve(Wall Heat Flux)@<interface fluid side> / dT

where dT is defined as areaAve(Temperature)@<interface Side 1> - areaAve(Temperature)@<interface Side 2>

in CFD-Post

areaAve(Wall Heat Transfer Coefficient)@<interface fluid side>

The difference between those two values in my study case was aprox. 0.4 % which is nothing. It can be caused by different interpolation that CFD-Post is using compared to the CFX. (I don't know that exactly, it's my guess).

If HTC value is negative, don't worry. It means it has reverse flux than is defined in dT. Just rearrange dT as areaAve(Temperature)@<interface Side 2> - areaAve(Temperature)@<interface Side 1> and it should be fine now.

Hope it will helps everyone in future

Have Fun