# Fluent Tutorial on Heat transfer

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

 August 25, 2013, 16:18 Fluent Tutorial on Heat transfer #1 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,914 Blog Entries: 6 Rep Power: 38 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.

 August 28, 2013, 20:44 with different turbulence models #2 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,914 Blog Entries: 6 Rep Power: 38 Results with different turbulence models are shown in following Fig. tiandabeiyang likes this.

 August 29, 2013, 03:27 #3 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,914 Blog Entries: 6 Rep Power: 38 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.

 September 1, 2013, 00:47 #4 New Member   ousegui Join Date: Oct 2010 Posts: 18 Rep Power: 6 hi Great efforts thx

 December 30, 2013, 09:59 great!A question about heat transfer coefficient #5 New Member   saisai Join Date: Sep 2013 Posts: 4 Rep Power: 3 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.

 December 30, 2013, 13:13 #6 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,914 Blog Entries: 6 Rep Power: 38 yes we need local Tb and we have to use udf. tiandabeiyang likes this.

 December 30, 2013, 23:02 Udf #7 New Member   saisai Join Date: Sep 2013 Posts: 4 Rep Power: 3 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.

 January 1, 2014, 03:43 Hi,Far #8 New Member   saisai Join Date: Sep 2013 Posts: 4 Rep Power: 3 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.

 January 2, 2014, 12:53 Just few ideas !!! #9 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,914 Blog Entries: 6 Rep Power: 38 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.

February 16, 2014, 22:35
#10
New Member

CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 4
Hi, great effort, thanks.

Quote:
 Originally Posted by Far 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,

February 21, 2014, 15:39
#11
New Member

Mahdy jamaly
Join Date: Dec 2009
Posts: 4
Rep Power: 7
Quote:
 Originally Posted by 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.
hi far.may you send me a copy of your udf? really i need it.thank you so much.(jamalim3@gmail.com)

 April 28, 2014, 11:47 Udf #12 New Member   Ismael Join Date: Oct 2012 Posts: 2 Rep Power: 0 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.

 December 18, 2014, 05:24 #13 New Member   vahid Goodarzi Ardekani Join Date: Jun 2013 Posts: 14 Rep Power: 4 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post hinca CFX 15 January 26, 2014 18:11 sunilpatil CFX 8 April 26, 2013 07:00 rohitjvbibin Main CFD Forum 0 October 26, 2010 05:51 rohitjvbibin FLUENT 0 October 26, 2010 05:50 B.Simon CFX 3 October 28, 2008 19:53

All times are GMT -4. The time now is 16:26.