[changhee.kim]

I'm conducting the pilot calculation to investigate internal flow field in simple duct.

From that, I want to see the htc distribution.

When I used 'defalut' in CFX, htc value can be shown (this values are based on 'wall adjacent temperature.' however, when I applied 'tbulk for htc' in expert parameter, htc value is all zero, exactly.

Why does it happen?

I know that the htc value can be calculated using the turbulent wall function.

What seems to be the problem? I need your help.

[ghorrocks]

Did you enter a valid value for "tbulk for htc"?

Please attach your CCL.

[changhee.kim]

Thank you

I have attached ccl file.

[ghorrocks]

Try setting the expert parameter to "300 [K]". Looks like you forgot to give the value units.

[changhee.kim]

Dear ghorrocks,

There is no option to enter the unit for 'tbulk for htc.' I can just enter the number.

I think the unit of this value follows inlet condition.

[ghorrocks]

What thermal boundary condition have you applied to the walls?

[changhee.kim]

I applied adiabatic wall condition at the walls. And total energy equation was solved.

[Thomas MADELEINE]

your walls are adiabatic (default condition for wall).
so there is no heat flux between the fluid and your walls.

htc (Wall Heat Transfert Coefficient) is calculated by :
Wall Heat Flux / (Twall - Tadjacent or Tbulk)

so here it is 0 divided by something without value (no temperature is given for your walls).

every thing seems normal to me.

[changhee.kim]

Thanks,

As far as I know, even if I applied adiabatic wall, htc value can be calculated using turbulent wall function. but these values are not real physical quantity.

So I just want to know why htc values are exactly zero after applying Tbulk for htc at expert parameter.

[Thomas MADELEINE]

I have just checked in the documentation and I confirm that the HTC is calculated from the heat flux :

CFX > Modeling guide > 2. boundary condition modeling > 2.7. Wall > 2.7.5. Heat Transfer > 2.7.5.4. Heat Transfer Coefficient and Wall Heat Transfer Coefficient

[changhee.kim]

Thank you so much,

I have a little bit confusing

Applying adiabatic wall assumption, htc value is calculate based on wall function (that is, wall function based heat transfer coefficient).

However, after reference temperature was specified, htc value was calculated using newton's cooling law. So I obtained 0 htc value because wall heat flux is zero.

What do you think about it?

[ghorrocks]

Thomas is correct. HTC is calculated from wall heat flux, so if there is zero wall heat flux (as an adiabatic boundary requires) then the HTC=0.

Wall functions do not return a HTC so your explanation is incorrect. Also I have no idea what your sentences "However, after reference .... flux is zero" mean.

[changhee.kim]

In CFX document,

wall heat transfer coefficient is given by the thermal wall function. the theory of thermal wall functions can be found at Heat Flux in the Near-Wall Region in ANSYS CFX-Solver Theory Guide.

[ghorrocks]

Yes, that is correct. Thomas's posts #8 and #10 describe how the HTC is calculated from the thermal wall function.

[changhee.kim]

Thank you for your help. That is very helpful.

[Opaque]

As far as I can read in the documentation, the behavior you observed is described here

CFX-Solver Modeling Guide

Chapter 17: Expert Control Parameters | 17.3. CFX-Solver Expert Control Parameters |

tbulk for htc

When the Heat Transfer Coefficient (HTC) is computed for a temperature specified wall, by default a near-wall fluid temperature is used for a temperature scale. However, for consistency with traditional 1D analyses, you may want to enter a reference bulk temperature to compute the HTC. This parameter is that reference value.

Thus the HTC computed when this parameter is provided is equal to the local heat flux calculated by the solver divided by the difference of the specified wall temperature and this specified bulk temperature.

I read that as "once you use this parameter, the HTC is evaluated as described here and not elsewhere"

Hope the above helps,

[sircorp]

Originally Posted by ghorrocks

Thomas is correct. HTC is calculated from wall heat flux, so if there is zero wall heat flux (as an adiabatic boundary requires) then the HTC=0.

Wall functions do not return a HTC so your explanation is incorrect. Also I have no idea what your sentences "However, after reference .... flux is zero" mean.

In relation to HTC I need bit help.

Some expert help please. "Pipe(inside) Cooling Test"

I have insulated copper pipe(Filled with Secondary Fluid). During cooling test, the cooling fluid (Primary Fluid) is injected inside the pipe vertically to carry out cooling test for both Secondary Fluid & Pipe Walls.

In Fluent, I set the temperature settings of the wall (pipe material, properties wall thickness and insulation material, properties & thickness and pipe wall temperature).

Problem is system is assuming my Wall Temperature stays constant which is not the case. Pipe should cool as the fluid starts flowing inside the pipe, but does not (heat source was switched off prior to "Cooling Test", so there is no heat source)

The fluid (inside the pipe, Pipe was filled with a Fluid & Heated Prior to Cooling Test) starts cooling down but Copper Pipe temperature stays same.

I only meshed the Fluid Zone not the Pipe's ? Pipe is added in the wall boundary conditions.

How to couple the pipe cooling with inside fluid cooling ?

Help is highly appreciated.

Thanks

Shane

[ghorrocks]

Sounds like you need to think about what is really happening. If you apply a defined temperature on the walls then of course you won't get any cooling as you have defined it to be fixed. You need to think about what are appropriate initial and boundary conditions so the correct physics can occur.

I suggest you should consider an initial condition of your fixed temperature, with the wall being a convective boundary condition.

[sircorp]

Originally Posted by ghorrocks

Sounds like you need to think about what is really happening. If you apply a defined temperature on the walls then of course you won't get any cooling as you have defined it to be fixed. You need to think about what are appropriate initial and boundary conditions so the correct physics can occur.

I suggest you should consider an initial condition of your fixed temperature, with the wall being a convective boundary condition.

Thanks Ghorrocks for the prompt response.

(During experiments, I did record temperature and pressure both along radial and axial directions. Since fluid is highly viscous so I needed to record radial temperature too)

Back to CFD, since walls are part of the system (no heat source) I have created a new geometry where pipe becomes part of the system.

Only bad part is I got several hundred walls and interfaces now. In case of error tracing them is a slight issue.

I need to get correct numbers for pipe cooling else it will be difficult to valid the model in a two phase viscous fluid.

With Regards

Shane

[Thomas MADELEINE]

Since there is no big change in the flow (except for temperature) the thing you can do is extract the HTC (W/m²/K) from a steady state simulation with a rough temperature at wall. This value should be more or less constant no matter of the wall temperature.
and export it to a mechanical software for a transient run.

It is not the most accurate simulation but you don't have to get all the interfaces right.

2nd choice :
on CFX you can create a solid domain and create interface for only heat flux.
I think the same is available on Fluent but I don't know this software as well as CFX.