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

Fluent Tutorial on Heat transfer

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

Like Tree4Likes
  • 2 Post By Far
  • 1 Post By Far
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   August 25, 2013, 16:18
Default Fluent Tutorial on Heat transfer
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,954
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Here I have prepared tutorial on Heat transfer and calculation of local heat transfer coefficent and local Nusselt no in Fluent.

It is well known test case "Baughn Pipe Expansion at ReD = 40750



ICEM CFD, Mesh and Fluent Files are attached along with excel sheet and PPT slides.

https://dl.dropboxusercontent.com/u/...n_ReD40750.zip

1. Units = meters

2. Boundary condtions Velocity and temprature are given in excel sheet

3. Materials properties : K calcualted from prandlt number and Cp as 1005

4. De in the formula for Nu (see image) is calcualted as 2*D*3.14

5. Data is normalized with Nu from Dittus-Boelter correlation for a straight pipe. Value comes out to be 97.79

6. Two models are also compared V2F and SST

7. Yplus is below 0.06

8. Local heat transfer coeffcient is found from Fluent. Go to Wall Fluxs > Surface heat transfer coef. Please note that I have used local heat transfer coefficent in formula for local Nu nuber instead of q/(Tw-Tb). Heat transfer coefficients for both turbulence models are also saved in the zip folder attached herewith.
sadegh1068 and siefdi like this.
Far is offline   Reply With Quote

Old   August 28, 2013, 20:44
Default with different turbulence models
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,954
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Results with different turbulence models are shown in following Fig.


tiandabeiyang likes this.
Far is offline   Reply With Quote

Old   August 29, 2013, 03:27
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,954
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Above results were obtained for mesh size of 17000 nodes. Mesh is also refined and fine mesh has size 34000 nodes approx. There is no difference in results for V2F and SST model with baseline and fine mesh Results are attached...

Y+ for both meshes (baseline and fine) is below 1. It is approx 0.3-0.5

To match the Reynolds number, one must run the simulation and get the mass flow rate and put in the formula of Reynolds number. keep on iterating until you get the required Reynolds number

Moreover to provide the fully developed flow condition at inlet, one must run the simulation for pipe of dia d and import the velocity and turbulence profiles to the simulation. Or one must extend the length of the smallar cylinder by 35-40 dia upstream.

Far is offline   Reply With Quote

Old   September 1, 2013, 00:47
Default
  #4
New Member
 
ousegui
Join Date: Oct 2010
Posts: 18
Rep Power: 6
ousegui is on a distinguished road
hi
Great efforts
thx
ousegui is offline   Reply With Quote

Old   December 30, 2013, 09:59
Default great!A question about heat transfer coefficient
  #5
New Member
 
saisai
Join Date: Sep 2013
Posts: 4
Rep Power: 3
tiandabeiyang is on a distinguished road
Thank you for your effort.Here I have a question:the local surface heat transfer coefficient in dependent on the reference temperature.Different temperature get different heat transfer coefficient .So if we need a UDF to get the Tbulk at different position,and then from the fomular:h=q/tw-tbulk?
this is my thesis,so i do really appreciate if you can give me some advices.thank you very much.
tiandabeiyang is offline   Reply With Quote

Old   December 30, 2013, 13:13
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,954
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
yes we need local Tb and we have to use udf.
tiandabeiyang likes this.
Far is offline   Reply With Quote

Old   December 30, 2013, 23:02
Default Udf
  #7
New Member
 
saisai
Join Date: Sep 2013
Posts: 4
Rep Power: 3
tiandabeiyang is on a distinguished road
thank you for your reply.Rencently i spent a lot of time on the UDF,but it is too much for me to read,because i am not familiar with UDF.So i want to kow if it is convinient for you to send me a copy of your UDF?thanks very very very much.
this is my email:xusai1206@gmail.com
thanks again.
tiandabeiyang is offline   Reply With Quote

Old   January 1, 2014, 03:43
Default Hi,Far
  #8
New Member
 
saisai
Join Date: Sep 2013
Posts: 4
Rep Power: 3
tiandabeiyang is on a distinguished road
I want to know how to get a specific region of Tbluk?I mean how can we get local region Tbluk which is normal to the local wall face.If we need a position judge to realise it?Thank you very much.
tiandabeiyang is offline   Reply With Quote

Old   January 2, 2014, 12:53
Default Just few ideas !!!
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,954
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
i have few ideas and i would to have comments on my opinion from experienced members in this field:

1. Draw a vertical line where you want to have the heat transfer. Take the vertex average fluid temperature on that line.

2. take a point just outside the boundary layer (thermal boundary layer)


I have UDF for this purpose sent by some one for the case i have mentioned above.
Far is offline   Reply With Quote

Old   February 16, 2014, 22:35
Default
  #10
New Member
 
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 4
siefdi is on a distinguished road
Hi, great effort, thanks.

Sorry for a noob question, but could you please explain in more detail about this step:

Quote:
Originally Posted by Far View Post

To match the Reynolds number, one must run the simulation and get the mass flow rate and put in the formula of Reynolds number. keep on iterating until you get the required Reynolds number

thanks and regards,
siefdi is offline   Reply With Quote

Old   February 21, 2014, 15:39
Default I need you udf!!please
  #11
New Member
 
Mahdy jamaly
Join Date: Dec 2009
Posts: 4
Rep Power: 7
stalon67 is on a distinguished road
Quote:
Originally Posted by Far View Post
i have few ideas and i would to have comments on my opinion from experienced members in this field:

1. Draw a vertical line where you want to have the heat transfer. Take the vertex average fluid temperature on that line.

2. take a point just outside the boundary layer (thermal boundary layer)


I have UDF for this purpose sent by some one for the case i have mentioned above.
hi far.may you send me a copy of your udf? really i need it.thank you so much.(jamalim3@gmail.com)
stalon67 is offline   Reply With Quote

Old   April 28, 2014, 11:47
Default Udf
  #12
New Member
 
Ismael
Join Date: Oct 2012
Posts: 2
Rep Power: 0
Ismael is on a distinguished road
Hi. I have seen the discussion and a have the same problem with the Tbulk temperature calculation. I will be very grateful with you help me to develop this UDF code or send me the UDF file from this calculation?(ismael.marchi1@gmail.com)
Thanks for your attention.
Ismael is offline   Reply With Quote

Old   December 18, 2014, 05:24
Default
  #13
New Member
 
vahid Goodarzi Ardekani
Join Date: Jun 2013
Posts: 14
Rep Power: 4
vga67 is on a distinguished road
hello

excuse me if here is not the right place for asking such question.

i am simulating a two phase (water and air bubble) model which is the interaction of a shock in water with an air bubble. my problem is that when the shock hits the bubble the temperature of the bubble should rise but the fluent does not show this(i have selected the energy equation to be solved). i do not know what the problem is. should a UDF be written for heat transfer inside the bubble?
can anyone help me on this?
thank you in advance
Hamid
vga67 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
Radiation interface hinca CFX 15 January 26, 2014 18:11
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
How to find the inbuilt equation in fluent for Heat Transfer Flux? rohitjvbibin Main CFD Forum 0 October 26, 2010 05:51
How to find the equation for Heat Transfer Flux in Fluent?? rohitjvbibin FLUENT 0 October 26, 2010 05:50
How can I increase Heat Transfer at Domain Interf? B.Simon CFX 3 October 28, 2008 19:53


All times are GMT -4. The time now is 06:50.