CFD Online URL
[Sponsors]
Home > Forums > FLUENT

Nusselt number?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 19, 2004, 09:35
Default Nusselt number?
  #1
tash
Guest
 
Posts: n/a
How to get the local surface Nusselt number and the average Nusselt number in the fluent? For example,at a square cavity the top and the bottom are adiabatic,and the left wall is with low constant temperature and the right wall with high constant temperature.I have try to get the surface Nusselt number from the Report>Surface integrals,choose the Report Type with Integral,and the Field Variable with wall Fluxes and get the surface Nusselt Number, but is seems not the Nusselt what I want.What on earth the Nusselt number on there? Thank you for any help.
  Reply With Quote

Old   September 19, 2004, 10:17
Default Re: Nusselt number?
  #2
stk
Guest
 
Posts: n/a
I think you can define Nusselt number by its definition(i don't remember the equation) and see the Nusselt variation all over the field.You can do it really easily with out any code, by DEFINE>CUSTOM FIELD FUNCTIONS (PUT THERE THE EQUATION DESCRIBING NUSSELT), Hope this helped you!
  Reply With Quote

Old   September 19, 2004, 11:07
Default Re: Nusselt number?
  #3
tash
Guest
 
Posts: n/a
stk,thanks,I'll try it.
  Reply With Quote

Old   September 19, 2004, 11:21
Default Re: Nusselt number?
  #4
tash
Guest
 
Posts: n/a
the definition of the Nusselt number. By default Fluent uses:

Nu=(q")*(1m)/k/(T-288.15K)

but I can't input the equation in the Definition of the Custom Field Functions.stk,thanks for more details.
  Reply With Quote

Old   September 30, 2004, 08:27
Default Re: Nusselt number?
  #5
venu gopal
Guest
 
Posts: n/a
Hi, The main problem with the fluent is, it will not give the Nusselt number values correctly for most of the cases. So, what you have to do naa, just take the temperature values of the wall/surface on which you want to measure the Nusselt number and by using the above equation you can find the Local or Average Nusselt number. This is the way you have to do for getting good results.

Venu Gopal
  Reply With Quote

Old   February 14, 2010, 04:52
Default
  #6
Member
 
Mohammad Zakerzadeh
Join Date: Dec 2009
Location: Aachen, Germany
Posts: 40
Rep Power: 7
moh1367 is on a distinguished road
Hi guys!

My case is very simple , its laminar flow in a pipe with constant wall temperature. I take the length as long as the flow can reach to fully thermally and Hydrodunamically developed. When I get the Nusselt Number from the xyplot/Surface Nusselt Number it can seemed that the Nu begins from a large number(as predicted by theory) and go toward zero at the end of pipe (the theoric value is 3.66). Can anybody help me?
I can send my case to you for more information.

Thanks alot
.
moh1367 is offline   Reply With Quote

Old   October 1, 2010, 03:28
Thumbs up
  #7
New Member
 
P Kaushik
Join Date: Oct 2010
Location: Kharagpur, India
Posts: 5
Rep Power: 6
kaushik is on a distinguished road
Fluent has some way of calculating Nu, What I suggest is that you make certain surfaces(lines for 2d) on the pipe and calculate average temperature, wall heat flux and separately calculate at each location. You will see that after the entrance length your Nu will tend towards 3.66 for constant wall temperature case and 4.36 for constant wall heat flux case.
kaushik is offline   Reply With Quote

Old   March 8, 2013, 10:10
Default
  #8
Member
 
Satish Gupta
Join Date: Jun 2012
Posts: 30
Rep Power: 4
Rahul123 is on a distinguished road
Sir,
I am simulating a cavity with a cylinder rotating in it using fluent. I am getting the nusselt number as 0. can you plz suggest a way I get the correct results.
Thank you
Rahul123 is offline   Reply With Quote

Old   March 8, 2013, 10:42
Smile
  #9
New Member
 
P Kaushik
Join Date: Oct 2010
Location: Kharagpur, India
Posts: 5
Rep Power: 6
kaushik is on a distinguished road
Hi,

It may be easier if you export the basic parameters such as u,v,w velocities, Temperature, etc and do the post processing externally. The reason is that fluent has a very different way of calculating the calculated parameters, so hence we usually find errors. Hope that helps.
kaushik is offline   Reply With Quote

Old   March 8, 2013, 10:48
Default
  #10
Member
 
Satish Gupta
Join Date: Jun 2012
Posts: 30
Rep Power: 4
Rahul123 is on a distinguished road
Can you help me on how to calculate it. I got the temperature gradient on the wall..what to do next...
thank you for your previous reply
Rahul123 is offline   Reply With Quote

Old   March 8, 2013, 10:59
Default
  #11
New Member
 
P Kaushik
Join Date: Oct 2010
Location: Kharagpur, India
Posts: 5
Rep Power: 6
kaushik is on a distinguished road
Hi,

What you do is:
1. Export the Coordinates along with the temperatures.
2. Calculate the bulk mean temperature as Tbulk = (1/Area)*Integral(T*dArea) across the Face
3. Then find wall heat flux as qw = -k(deltaT/deltaY) at the wall.
4. Find heat transfer coefficient h = qw/(Twall-Tbulk)
5. Nusselt Number Nu = hD/k

Hope this was helpful.
kaushik is offline   Reply With Quote

Old   March 8, 2013, 11:11
Default
  #12
Member
 
Satish Gupta
Join Date: Jun 2012
Posts: 30
Rep Power: 4
Rahul123 is on a distinguished road
I am solving the problem in the non dimensional form. I have used k=1. It is two dimensional problem. so i need to calculate the nusselt number on the face(line). I defined a surface(line) in fluent a cell distance away from wall. using surface monitors I found the temp. on the wall and found temp. gradient. I didnt understand the part of finding the bulk temperature. It would be very helpful if you could elaborate the process.
Thank you very much
Rahul123 is offline   Reply With Quote

Old   March 8, 2013, 11:22
Smile
  #13
New Member
 
P Kaushik
Join Date: Oct 2010
Location: Kharagpur, India
Posts: 5
Rep Power: 6
kaushik is on a distinguished road
Hi,

Bulk mean temperature is the basically the average temperature. If you take the mass weighted average of temperature using the surface integrals over a line perpendicular to the mean direction of flow. You will get it. Please go through any standard heat transfer textbook for finding the definition of bulk mean temperature. In case of any further doubts please feel free to post.

Hope this was helpful.
kaushik is offline   Reply With Quote

Old   March 9, 2013, 16:32
Thumbs up dear
  #14
Member
 
farzadpourfattah
Join Date: Mar 2013
Posts: 38
Rep Power: 3
farzadpourfattah is on a distinguished road
first check your reference value, default value of fluent for length and depth is 1.
set your length and depth.
farzadpourfattah is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
DecomposePar unequal number of shared faces maka OpenFOAM Pre-Processing 6 August 12, 2010 10:01
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 08:36
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 11:37
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 05:15


All times are GMT -4. The time now is 11:19.