
[Sponsors] 
How To Calculate Average Heat Transfer Coefficient in CFDPost? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 29, 2016, 07:11 
How To Calculate Average Heat Transfer Coefficient in CFDPost?

#1 
Senior Member

Dear all,
Hi. Hope all are well. I am doing heat transfer analysis in a circular pipe. The fluid is water. I wanted to ask how can I get average heat transfer coefficient and local heat transfer coefficient in CFDPost along the length of the pipe? I searched for these variables in the variables list but all I found was wall heat transfer coefficient. When I used that in a line along the center of the pipe even though I got values I didn't get any values in the chart. Why is that? I couldn't change the boundary data from Hybrid to Conservative. Also is wall heat transfer coefficient equal to average heat transfer coefficient? Really urgently need to make graphs of average htc and local htc along the length of the pipe. Would be grateful for help. Thanks. 

April 29, 2016, 12:18 

#2 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,122
Rep Power: 21 
I'm sure this has been discussed many times. You should do a search for quicker answers.
Heat transfer coefficient is only a variable at the wall, not through the center of the pipe!?! It is equal to: Wall Heat Transfer Coefficient = Wall Heat Flux / (Wall Temperature  Wall Adjacent Temperature) Which is not equivalent to the standard engineering equation which uses "bulk temperature" in place of the wall adjacent temperature. When using wall adjacent temperature, the returned value is going to be completely mesh dependent, and a coarser mesh will give you answers approaching the standard definition using bulk temperature, and a fine mesh would give you very large values. You can plot Wall Heat Transfer Coefficient on a contour at the fluid side of the interface or boundary, or make a line along the pipe wall, and make a graph. If you want the HTC to use a different value for reference temperature instead of Wall adjacent temperature, can do a couple things: 1.) use the expert parameter "Tbulk for HTC" 2.) make your own expression for bulk temperature along the pipe. I'll let you figure this out. Then make a new expression for: MyHTC = Wall Heat Flux / (Wall Temperature  MyBulkTemperature). The tricky part is how do you get "Wall Temperature" Well from the original HTC equation: Wall Heat Transfer Coefficient)= Wall Heat Flux / (Wall Temperature  Wall Adjacent Temperature) Rearrange it to: Wall Temperature = (Wall Heat Flux / Wall Heat Transfer Coefficient) + Wall Adjacent Temperature Then make a variable from your "MyHTC" expression. You can then make a contour or plot it on a graph with a line running along the wall. 

April 30, 2016, 10:41 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
Hi Erik  Can you stick it in the FAQ page? Then just refer people to the FAQ page in future. It also means it can be reviewed by many people so we can make it the best response possible.
http://www.cfdonline.com/Wiki/Ansys_FAQ 

May 2, 2016, 17:43 

#4 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,122
Rep Power: 21 
Sure thing Glenn,
I just applied for the "user group" account so I can edit/expand the FAQ. I will clean up my response and add it there. EDIT: I added this to the FAQs, I feel special now :) Thanks, Erik Last edited by evcelica; May 3, 2016 at 16:59. 

May 3, 2016, 22:14 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
Excellent, thanks Erik. Feel free to do updates to any of the other comments on that page as well. Then you can feel even more special.


November 21, 2019, 09:05 

#6 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
Hello, everybody,
I just came across this thread and have a question about it: I activated the expert parameter t bulk and added the fluid temperature of the environment. If I now get the htc output, I get a realistic number (<20 for free convection of air). However, the value differs from the value I get when I divide the heat flux by delta T. What could be the reason for this? Many thanks in advance Last edited by bemomb; November 21, 2019 at 10:30. 

November 21, 2019, 10:28 

#7 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,122
Rep Power: 21 
What delta T are you referring to? What expression and location exactly?


November 21, 2019, 10:39 

#8 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
Hi evcelica,
I have a free convection of air on the outside of a cylinder. With tbulk I get a htc (wall heat transfer coefficient) around 4. My air has a temperature of 298 K. When I want to verify the htc by dividing the heat flux by (twalltfluid) I get a value that is around 11. But it has to be in the area of 4 hasn't it? Thx 

November 21, 2019, 20:54 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
Where does twall and tfluid come from?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

November 22, 2019, 01:29 

#10 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
Tfluid is my ambient temperature, that i chose to be 298 K (that's why tbulk has that value). And twall is the temperature on the cylinder surface, that I get from post. So what I want to do is basically compare the htc I get from post (which is around 4) and the htc I get by taking the heat flux on the cylinder surface and dividing it by delta t (around 11) and my problem is that they are different.


November 22, 2019, 01:54 

#11  
Senior Member
Join Date: Feb 2011
Posts: 495
Rep Power: 16 
Quote:


November 22, 2019, 04:32 

#12 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
I just read the post and it sounds quite complicated. So basically the main problem is that Twall is computed conservative? When I change it to hybrid in post, the difference is .03 K. I don't get it.
In addition: I want to simplify my simulation by replacing the big atmosphere domain with a htc bc on the outside of my cylinder. Therefore I tried to find the htc in that first simulation. 

November 22, 2019, 04:53 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
As Antanas states, details are important. Even the way you average it over the surface is important. So please tell us exactly how you have calculated the numbers you are comparing. Include the integration/averaging scheme you used, which exact variable and if you select hybrid or conservative values.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

November 22, 2019, 05:15 

#14 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
So I have calculated the WHTC with areaAve(T) on the fluid side of the interface, where the same value comes out for conservative and hybrid, namely 4.8 W/m^2K.
For comparison, I also calculated the wall heat flux with areaAve(T) on the fluid side of the interface, 210 W/m^2. Again, it doesn't matter if conservative or hybrid. Then I calculated the wall temperature also on the fluid side of the interface, also with areaAve(T). Here conservative and hybrid differ by only 0.03 K. In the appendix you can see a picture. What might be important is that the convection takes place only on the outer surface, the side surfaces are adiabatic. Maybe this causes problems, on the picture you can see on closer inspection that the WHTC rises towards the edges. Many thanks in advance and a compliment from me that all of you really try to help! Edit: The temperature scale is for the plane, the colours on the surface of the cylinder represent the WHTC! Last edited by bemomb; November 22, 2019 at 06:29. 

November 23, 2019, 05:32 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
No, your problem is more fundamental than that. If A and B are field variables, then, in general; average(A)*average(B) does not equal average(A*B).
This means you cannot use an average of T in this calculation. You should define a new variable as Wall Heat Flux/(TTamb). This is the number you should be comparing to the HTC from CFX.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

November 23, 2019, 06:05 

#16 
Member
Benni
Join Date: Oct 2019
Location: Germany
Posts: 33
Rep Power: 5 
Okay, but how do I define T? What's also interesting is that if I enter the two different htc into the simulation as Bc (without atmosphere), the temperatures in the simulation will match for the calculated htc 11 (wall heat flux/delta t), not for the htc from cfx 4. This means that the problem is not the value calculated by myself (wall heat flux/delta t), but the value calculated by the system


November 24, 2019, 19:57 

#17 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,266
Rep Power: 136 
This means that when you are comparing heat transfer coefficients they need to have the same averaging process. So if you are comparing the areaAve(HTC) then you need to define your value as a variable field defined as Wall Heat Flux/(TTamb), and then you do an areaAve on that variable.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
please can any one explain producer to calculate the heat transfer coefficient in sid  reslan  FLUENT  0  February 12, 2016 05:24 
Question about heat transfer coefficient setting for CFX  Anna Tian  CFX  1  June 16, 2013 07:28 
Error finding variable "THERMX"  sunilpatil  CFX  8  April 26, 2013 08:00 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
Average Heat Transfer Coefficient vs. local  safikhani_hamed  CFX  3  August 20, 2011 11:45 