CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Nusselt number 4.36 validation in a tube in constant heat flux situation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 2, 2012, 09:00
Post Nusselt number 4.36 validation in a tube in constant heat flux situation
  #1
New Member
 
Felix
Join Date: Feb 2012
Location: Qingdao,China
Posts: 5
Rep Power: 5
QustFelix is on a distinguished road
Hi,guys.

According to classic heat transfer knowledge ,the Nusselt number in a fully developed tube with constant heat flux should be 4.36 .

CFD code like fluent is so powerful ,so I want to validate the problem in fluent .And if I model right ,I should get the right Nusselt Number.

But maybe there is something wrong in my model process , I just can not get the Nusselt number as described above .

These is the process below.


according to experience :the length of entry region l=0.05Re×Pr。

Material is water : and I set Re=100.
Re=Rho×velocity×D/viscousity. then I get inlet veloctiy=0.1m/s.

Pr(30Celsius-60Celsius)is about 3 .then we get the entry length l=0.05×100×3=0.15m.


I build a cylinder in Gambit with the dimension below:
D=0.1m,L=0.3m.

Boundary condition:

inlet velocity :v=0.1m/s .T=300K. outflow in outlet。
heat flux of wall =q=400W/m^2.
the conductivity of water :lamda=0.6.

I use the 3D single precise solver to solve the problem. Set the residual to 10-4. At the same time ,I set a temperature monitor point in the middle point at the tube .


The calculation of Nusselt number:

Nu=h*D/Lamda.
h=q/DletaT=q/(Twall-Tref).
Twall is the temperature of wall of the tube ,Tref is the average temperature of the section I choose in the fully developed region.

I create a section in fully developed region .

plot temperature coutour of this section ,and I get max temperature in the wall is 300.948K .

The difficulty comes as I want to calculate the average temperature of the section I created.

According to heat transfer textbook ,Tref=Tm=(Intergral of(u×T)in seciton )/(pi×(D/2)^2×Veloctiy)。

The result of the section is 0.002341306。So Tref=Tm=0.002341341/(3.1415926×0.05^2×0.1)=298.2555K.

Then h=q/(Twall-Tref)=400/(300.948-298.2555 )k=148.560817084494 w/(m^2.k).

At last ,I get Nu=h×D/Lamda=148.560817084494*0.01/0.6=2.4760136180749 != 4.36.

I don't know what was wrong with the above process .Can somebody so kind to point the error in my process ?
QustFelix is offline   Reply With Quote

Old   May 2, 2012, 09:37
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 678
Rep Power: 13
LuckyTran will become famous soon enough
Quote:
Originally Posted by QustFelix View Post
According to heat transfer textbook ,Tref=Tm=(Intergral of(u×T)in seciton )/(pi×(D/2)^2×Veloctiy)。
Is your heat flux heating up or cooling the fluid? Check your calculation of mean temperature. For heating, the temperature cannot be less than 300K, neither can the wall temperature be less than 300K. Either way your bulk temperature must be between your inlet temperature and wall temperature, anything outside that range is non-physical and your simulation must be giving wrong results.

Lastly, you can more easily simulate fully developed flows using the periodic boundary conditions. If you don't care about entry length effects, I recommend you do fully developed flows this way. Just wanted to inform you that the feature exists.
LuckyTran is offline   Reply With Quote

Old   May 2, 2012, 09:54
Default
  #3
New Member
 
Felix
Join Date: Feb 2012
Location: Qingdao,China
Posts: 5
Rep Power: 5
QustFelix is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Is your heat flux heating up or cooling the fluid? Check your calculation of mean temperature. For heating, the temperature cannot be less than 300K, neither can the wall temperature be less than 300K. Either way your bulk temperature must be between your inlet temperature and wall temperature, anything outside that range is non-physical and your simulation must be giving wrong results.

Lastly, you can more easily simulate fully developed flows using the periodic boundary conditions. If you don't care about entry length effects, I recommend you do fully developed flows this way. Just wanted to inform you that the feature exists.
It is heating the fluid in the tube.

Thank you very much .
In fact I want to investigate the Nusselt number along the axial direction.
I am not very sure about the calculate method of average temperature in the section of the tube . Fluent provide so many method to calculate the average temperature in a section ,like facet average ,vertex average and area-weighted temperature and so on . But I don't know which is right for my problem. I use different methods and I get different answers . I was really confused by this.
QustFelix is offline   Reply With Quote

Old   May 2, 2012, 13:02
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 678
Rep Power: 13
LuckyTran will become famous soon enough
Quote:
Originally Posted by QustFelix View Post
Fluent provide so many method to calculate the average temperature in a section ,like facet average ,vertex average and area-weighted temperature and so on . But I don't know which is right for my problem. I use different methods and I get different answers . I was really confused by this.
You already showed me the correct equation for bulk temperature! The bulk temperature is calculated using the mass weighted average. Use a surface integral on a plane that cuts the cross-section of your pipe and calculate the mass-weighted average temperature to get the bulk temperature.
LuckyTran is offline   Reply With Quote

Old   May 3, 2012, 07:21
Default
  #5
New Member
 
Felix
Join Date: Feb 2012
Location: Qingdao,China
Posts: 5
Rep Power: 5
QustFelix is on a distinguished road
Thanks much to your suggestions . I use periodic boundary condition now and iterate again and at last I get a good result. I am not sure about the length of entry region .

I set the bulk temperature of inflow of tube as 300K,and transfer the velocity 0.1 m/s to mass flow rate as 0.0078437714588745 kg/s.

Here is my result :

bulk temperature is 300.0098 and wall temperature is 300.4001 .then I can get Nusselt number as 4.259307.

Now I want to use double precision solver to solve it again to get Nusselt number ,maybe it is closer to 4.36.

Thank you very much for your help again. You are really a nice guy.
QustFelix is offline   Reply With Quote

Old   June 18, 2015, 13:25
Default
  #6
New Member
 
shirin patil
Join Date: Jul 2014
Posts: 2
Rep Power: 0
shirin3151 is on a distinguished road
Then how will find the heat flux for constant wall temperature to find the nusselt number
shirin3151 is offline   Reply With Quote

Old   June 18, 2015, 22:09
Default
  #7
New Member
 
Felix
Join Date: Feb 2012
Location: Qingdao,China
Posts: 5
Rep Power: 5
QustFelix is on a distinguished road
Quote:
Originally Posted by shirin3151 View Post
Then how will find the heat flux for constant wall temperature to find the nusselt number
The report function will provide us the information of heat flux on bondary area.
QustFelix 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
Compressor Simulation using rhoPimpleDyMFoam Jetfire OpenFOAM Running, Solving & CFD 107 December 9, 2014 14:38
validating nusselt number in flows over parallel isoflux heat plate mkamalhilmi FLUENT 0 September 5, 2014 04:57
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 10:37
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 09:31.