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

Confuse about Nu Number in Laminar Flow

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 30, 2014, 08:40
Default Confuse about Nu Number in Laminar Flow
  #1
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Hi I did simple heat transfer problem of flow throw a circular pipe with constant heat flux at wall. Usually for laminar flow with constant heat flux the Nusselt Number should be 4.36 ? when I view surface nusselt number from Report>Wall Fluxes>Surface Nusselt number it give me Nusslet number as 11.61 ? Why this deffer from the theortical value as (4.36)?

Mariam
mariam.sara is offline   Reply With Quote

Old   January 30, 2014, 08:54
Default
  #2
New Member
 
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 4
Alek is on a distinguished road
dear mariam and sara,
In fact FLUENT compute h (heat transfer coefficient) and NU number wrong and you should compute them manually as follows:
h=mdat*cp*(Twall-Tbulk)
Nu=hD/k

Sincerely
Alek is offline   Reply With Quote

Old   January 30, 2014, 08:59
Default
  #3
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Hi Alek thanks a lot for the quick respond. You mentioned in your relation Twall & Tbulk? the problem I not have both of these temperatures because I used fixed heat flux at the wall not fixed wall temperature? So how I can predict Twall in this case?
mariam.sara is offline   Reply With Quote

Old   January 30, 2014, 09:23
Default
  #4
New Member
 
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 4
Alek is on a distinguished road
The Twall which is computed with FLUENT is right and you can use it.
Alek is offline   Reply With Quote

Old   January 30, 2014, 09:25
Default
  #5
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Do you mean I need to plot Twall along the wall? what about Tbulk how i can compute it?
mariam.sara is offline   Reply With Quote

Old   January 30, 2014, 09:27
Default
  #6
New Member
 
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 4
Alek is on a distinguished road
If you send me an email I can send you a good document.
Alek is offline   Reply With Quote

Old   January 30, 2014, 10:33
Default
  #7
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 381
Rep Power: 9
macfly is on a distinguished road
Quote:
Originally Posted by Alek View Post
dear mariam and sara,
In fact FLUENT compute h (heat transfer coefficient) and NU number wrong and you should compute them manually as follows:
h=mdat*cp*(Twall-Tbulk)
Nu=hD/k
Sincerely
Careful maria, the equation Alek gave you for h is wrong: It's not the equation for h, it's the equation for the heat transfer.

Fluent calculates the heat transfert coefficient (h) from various correlations depending on the physics. It's your homework to verify in the Theory Guide which correlation Fluent uses according to the physics of your model, then decide if you should modify it or not.

Last edited by macfly; January 30, 2014 at 12:00.
macfly is offline   Reply With Quote

Old   January 30, 2014, 11:44
Default
  #8
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Hi Macfly I not have problem with the theory. I tried solve problem with constant heat flux at a cylinder wall with laminar flow case it must give me Nu=4.36 but it give different value? I am not one of fluent designer to know how FLUENT predict Nu values you answer is vague to me?
mariam.sara is offline   Reply With Quote

Old   January 30, 2014, 12:08
Default
  #9
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 381
Rep Power: 9
macfly is on a distinguished road
Quote:
Originally Posted by mariam.sara View Post
Hi Macfly I not have problem with the theory. I tried solve problem with constant heat flux at a cylinder wall with laminar flow case it must give me Nu=4.36 but it give different value? I am not one of fluent designer to know how FLUENT predict Nu values you answer is vague to me?
You don't have problem with the theory but it seemed like you bought what Alek said.

- maybe your mesh is not fine enough?
- maybe the flow is not fully developped?

What I'm saying wouldn't sound vague if you took a look at the theory guide in order to understand what Fluent is doing. I guess you're doing some engineering homework and you have to put some thinking into it. You don't become an engineer just clicking on buttons expecting to get the right number on the output.
macfly is offline   Reply With Quote

Old   January 30, 2014, 12:19
Default
  #10
New Member
 
Smith
Join Date: Jan 2014
Posts: 9
Rep Power: 4
Alek is on a distinguished road
Dear maryam and Sara
you can use the following relations to compute h and NU manually:
Q=q''Px=mdat*C*(Tbulk,x-Tbulk,in)->Tbulk,x=(q''Px/mdat*C)+Tbulk,in
h(x)=q''/(Twall-Tbulk,x)

Twall is calculated by Fluent
macfly and mariam.sara like this.
Alek is offline   Reply With Quote

Old   February 9, 2014, 02:12
Default How to make inlet velocity fixed along a pipe
  #11
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Hello
I have a query to how i can make the inlet velocity value fixed from pipe inlet until pipe outlet? is that possible in Fluent? knowing that the flow is laminar?
mariam.sara is offline   Reply With Quote

Old   July 28, 2015, 11:41
Default
  #12
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
ghost82 will become famous soon enough
Question is not very clear to me; do you mean have a fully developed flow so to have a constant velocity profile?
If so, just use periodic boundary condition.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   July 29, 2015, 03:28
Default
  #13
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
Hi ghost if I want fully developed flow I can use periodic boundary by defining inlet as periodic boundary?? I need to know how to use periodic boundary??

mariam

Quote:
Originally Posted by ghost82 View Post
Question is not very clear to me; do you mean have a fully developed flow so to have a constant velocity profile?
If so, just use periodic boundary condition.
mariam.sara is offline   Reply With Quote

Old   July 29, 2015, 03:43
Default
  #14
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
ghost82 will become famous soon enough
Yes, just change the inlet/outlet to periodic.
Then in periodic settings set the pressure gradient or mass flow rate.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   July 29, 2015, 04:47
Default
  #15
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
ghost82 will become famous soon enough
The main problem is how the heat transfer coefficient (h) is defined: as you know there is bulk temperature into the equation, but what is bulk temperature?
Adjacent cell to the wall? Or temperature on the axis? Or....?

For each defined bulk temperature you will obviously obtain different values of h, and so different values of Nusselt number.

Related to your problem (fluid flow in pipe, laminar, with constant heat flux) I suggest to:

1- Draw 2D axisymmetric pipe
2- Set a periodic translational pipe
3- Enable energy equation, but disable in solution controls the energy equation (1 step: solve the momentum equation)
4- Once the velocity field is converged, eneable energy equation and disable momentum equation (2 step: solve the enrgy equation)
5- Create a line in y direction at a predefined x location (in the middle of the pipe for example)
6- Go to Reports->surface integrals->area weight average: select temperature and the line you created (This will be the mixed mean temperature, n other words Tbulk)
7- Evaluate the temperature on the wall, at the line you created
8- Calculate h as h=Q/(Twall-Tbulk), where Q is your heat flux (Watt/m2).
9- Evaluate Nusselt as Nu=h*D/k, where D is pipe diameter (m), k thermal conductivity (W/m/K)

This should give you a good approximation.
esinticik likes this.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   July 29, 2015, 05:04
Default
  #16
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
really thanks ghost82 for the valuable illustration. I will told you what I did, I run my case as described previously it converged and the contours of temperature is quite good when compared to the literature. I want now to predict h & Nu at a distance (0.69825 m) from the pipe inlet hence I draw a vertical line at this distance I evaluate Tbulk and used surface integral>area weighted average along the line Tb=298.6429 K then evaluated Tw at the wall which be 308.17706 K now I predict h from the relation knowing that heat flux at the wall is 8846.4 W/m^2 as below:

h=8846.4/(Tw-Tb)=8846.4/(308.17706-298.6429)=927.8635978 W/m^2.K

this value is higher than that predicted from experiments which is 888 W/m^2.K??

I can sent you my case file and the paper I compare with if you want have a look?

Thanks
mariam
mariam.sara is offline   Reply With Quote

Old   July 29, 2015, 05:09
Default
  #17
Senior Member
 
Join Date: Jan 2011
Posts: 235
Rep Power: 8
mariam.sara is on a distinguished road
I forgot to mention my case not fully developed from inlet it a startup flow which be fully developed at the end pipe section only. So i think I do not need for periodic boundaries.
mariam.sara is offline   Reply With Quote

Old   July 29, 2015, 05:12
Default
  #18
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
ghost82 will become famous soon enough
Quote:
Originally Posted by mariam.sara View Post
really thanks ghost82 for the valuable illustration. I will told you what I did, I run my case as described previously it converged and the contours of temperature is quite good when compared to the literature. I want now to predict h & Nu at a distance (0.69825 m) from the pipe inlet hence I draw a vertical line at this distance I evaluate Tbulk and used surface integral>area weighted average along the line Tb=298.6429 K then evaluated Tw at the wall which be 308.17706 K now I predict h from the relation knowing that heat flux at the wall is 8846.4 W/m^2 as below:

h=8846.4/(Tw-Tb)=8846.4/(308.17706-298.6429)=927.8635978 W/m^2.K

this value is higher than that predicted from experiments which is 888 W/m^2.K??

I can sent you my case file and the paper I compare with if you want have a look?

Thanks
mariam
EDit post: Sorry, I deleted what I wrote as it was wrong.

Send me the paper; I think that 927 vs. 888 should be acceptable, it's a 4% "error", I don't know..

Moreover: are you sure your simulation reflects 100% the experimental setup?

Daniele
__________________
Google is your friend and the same for the search button!

Last edited by ghost82; July 29, 2015 at 15:24.
ghost82 is offline   Reply With Quote

Old   July 30, 2015, 11:04
Default
  #19
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
ghost82 will become famous soon enough
Just to make public my thoughs I wrote you by email:
I think Tbulk could be calculated better by mass-weighted-average and not area-weighted-average.

Moreover,
Book "Fundamentals of heat and mass transfer" by Incropera defines a Tm (Tbulk), as in the attached picture.

I think you can create a custom field function named for example numerator:

density*axial-velocity*specific-heat-cp*temperature

Then evaluate the integral on the radial line you defined:
Reports->Surface integrals->Integral and choose Custom field function->numerator

Then divide this number by the (mass flow rate*cp).
Mass flow rate can be obtained in reports->fluxes.

If your cp is a function of temperature you can evaluate an average cp by mass-weighted-average.

Results of Tm should be similar to Tbulk evaluated by mass-weighted-average.

Daniele
Attached Images
File Type: png Tm.png (5.2 KB, 10 views)
mariam.sara likes this.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   November 23, 2015, 15:21
Default
  #20
New Member
 
Join Date: Mar 2009
Posts: 14
Rep Power: 9
sfalsharif is on a distinguished road
Quote:
Originally Posted by mariam.sara View Post
I forgot to mention my case not fully developed from inlet it a startup flow which be fully developed at the end pipe section only. So i think I do not need for periodic boundaries.
Hi Mariam,
I realize this thread is a bit old now, but can you explain further what you mean by the above statement? If your case is not fully developed it is not surprising that you would get a higher Nu than the theoretical result for fully-developed conditions. The temperature profile is flatter in the developing region, and the difference between the bulk temperature and the wall temperature is smaller than in the fully developed region. For a given fixed wall heat flux, this means h will be higher in the developing region. So it is important to use periodic conditions for temperature, not just velocity.
sfalsharif 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
decomposePar pointfield flying OpenFOAM Running, Solving & CFD 28 December 30, 2013 16:05
AMI interDyMFoam for mixer danny123 OpenFOAM Running, Solving & CFD 4 June 19, 2013 04:49
parallel code samiam1000 SU2 3 March 25, 2013 05:55
Stable boundaries marcoymarc CFX 33 March 13, 2013 07:39
AMI speed performance danny123 OpenFOAM 19 October 24, 2012 07:44


All times are GMT -4. The time now is 23:22.