No Slip Wall with Fixed Temperature Boundary Condition
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 Ogrid 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 postprocess 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 
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.

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

Dear Stumpy,
You are correct. I was exporting conservative values! Thank you! 
Heat Transfer Coefficient in Compressible Flow 3D turbine cascade
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 Ogrid 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. 
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.

Do you know where I can specify tbulk?

All times are GMT 4. The time now is 03:42. 