[Karkoura]

Hi,

I am using CFX to model a 3D turbine cascade. My ultimate objective is to compute the heat transfer coefficient distribution at the blade surface.

The flow is subsonic compressible so I am using "Total Energy" and "Air Ideal Gas" for the working fluid.

I am also using the SST turbulence model, with an O-grid mesh around the blade, and a small distance of the first node away from the wall in order to obtain a yplus of around 3.

Since I would like to compute the heat transfer coefficient distribution at the blade surface, I defined the blade walls, to be no slip and applied a fixed temperature of 296K.

However, as I post-process the simulation and export the variables at the blade loading line, I do not obtain a temperature of 296K at the blade wall.

How can that be since I did specify a temperature?

I would really appreciate any comments you may have. I would also benefit from the experience of those who did heat transfer calculations in a turbine cascade.

Thank you in advance

[ghorrocks]

If you correctly defined a fixed temperature then they have the temperature you defined. Either you set it up wrong or you are post processing it wrong.

[Karkoura]

Dear Glenn,

Thanks for the answer.

First of all there are not so many ways of specifying a temperature at the blade. Under "Boundary Details" > "Heat transfer" option, I choose "Temperature" and apply a fixed temperature of 296K.

So it seems plausible to me that I am post processing it wrong. I have a question concerning that. What is the "Blade Loading Line" in CFX?

You see what I do in CFD post in that I go to "
File > Export
for the Location, I choose "Blade Loading Line"
for the Boundary Data, I choose "Current"
then I select all the variable I need (of which the temperature) and I save it to a .csv file.

Are you familiar with this procedure? Would you know of any other way for computing variables at the blade surface, at a certain span location?

Thanks

[stumpy]

You're probably exporting conservative values rather than hybrid values. See the CFX doc for the difference.

[Karkoura]

Dear Stumpy,

You are correct. I was exporting conservative values! Thank you!

[Karkoura]

Hi,

I am using CFX to model a 3D turbine cascade. My ultimate objective is to compute the heat transfer coefficient distribution at the blade surface.

The flow is subsonic compressible so I am using "Total Energy" and "Air Ideal Gas" for the working fluid.

CFD Post outputs data for two particular variables. The "wall heat flux (q) " and the "wall heat transfer coefficient (h) ". From the CFX manual, I understand that these two are related by:
h = q / (T_wall - T_adjacentwall)
These values are very high and not in agreement with experimental data.

I tried to compute the wall heat flux myself by using the following:

q = -k * (Twall - Tadjacent wall) / y

where
k is the thermal diffusivity
Twall is the wall temperature (which I had specified as a boundary condition)
Tadjacent wall is the temperature of the first node away from the wall.
and
y is the distance of the first node away from the wall to the wall itself (this value I defined when I was creating the O-grid mesh around the airfoil in ICEM CFD)

Still I see that the variable are underpredicted compared to experimental data and the trend of heat transfer distribution with streamwise direction on the blade surface is not smooth and fluctuating.

I would appreciate any comments and knowledge you can share about computing the heat transfer coefficient in compressible flow.

Thank you so in advance.

[stumpy]

If you are comparing to experimental data then their HTC is likely based on a reference temperature other than Tadjacent wall. You should use the expert parameter "tbulk for htc" to set a reference temperature for the HTC calculation.

[Karkoura]

Do you know where I can specify tbulk?