|
[Sponsors] |
No Slip Wall with Fixed Temperature Boundary Condition |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 9, 2011, 18:34 |
No Slip Wall with Fixed Temperature Boundary Condition
|
#1 |
New Member
Join Date: Jan 2010
Posts: 13
Rep Power: 16 |
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 |
|
March 9, 2011, 18:37 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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.
|
|
March 9, 2011, 18:44 |
|
#3 |
New Member
Join Date: Jan 2010
Posts: 13
Rep Power: 16 |
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 |
|
March 10, 2011, 08:54 |
|
#4 |
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 21 |
You're probably exporting conservative values rather than hybrid values. See the CFX doc for the difference.
|
|
March 10, 2011, 11:05 |
|
#5 |
New Member
Join Date: Jan 2010
Posts: 13
Rep Power: 16 |
Dear Stumpy,
You are correct. I was exporting conservative values! Thank you! |
|
March 10, 2011, 15:28 |
Heat Transfer Coefficient in Compressible Flow 3D turbine cascade
|
#6 |
New Member
Join Date: Jan 2010
Posts: 13
Rep Power: 16 |
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. |
|
March 10, 2011, 16:46 |
|
#7 |
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 21 |
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.
|
|
March 10, 2011, 17:23 |
|
#8 |
New Member
Join Date: Jan 2010
Posts: 13
Rep Power: 16 |
Do you know where I can specify tbulk?
|
|
Tags |
blade, fixed temperature, heat transfer coefficient, wall |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
how to set up a wall boundary condition according to calculated wall shear stress? | gameoverli | OpenFOAM Pre-Processing | 1 | May 21, 2009 08:28 |
No results for solid domain | Gary Holland | CFX | 10 | March 13, 2009 03:30 |
Deformation of wall by temperature condition | Jay | FLUENT | 0 | April 14, 2007 18:06 |
Free Stream Temperature wall boundary condition | emanuele | FLUENT | 0 | March 19, 2007 10:45 |
wall slip boundary condition | Federico | FLUENT | 0 | February 6, 2007 03:12 |