# Nusselt number?

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

 September 19, 2004, 08:35 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.

 September 19, 2004, 09:17 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! mohammed almaghrabi likes this.

 September 19, 2004, 10:07 Re: Nusselt number? #3 tash Guest   Posts: n/a stk,thanks,I'll try it.

 September 19, 2004, 10:21 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.

 September 30, 2004, 07:27 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

 February 14, 2010, 04:52 #6 Member   Mohammad Zakerzadeh Join Date: Dec 2009 Location: Aachen, Germany Posts: 40 Rep Power: 9 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 .

 October 1, 2010, 02:28 #7 New Member   P Kaushik Join Date: Oct 2010 Location: Kharagpur, India Posts: 5 Rep Power: 9 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.

 March 8, 2013, 10:10 #8 Member   Satish Gupta Join Date: Jun 2012 Posts: 30 Rep Power: 7 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

 March 8, 2013, 10:42 #9 New Member   P Kaushik Join Date: Oct 2010 Location: Kharagpur, India Posts: 5 Rep Power: 9 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.

 March 8, 2013, 10:48 #10 Member   Satish Gupta Join Date: Jun 2012 Posts: 30 Rep Power: 7 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

 March 8, 2013, 10:59 #11 New Member   P Kaushik Join Date: Oct 2010 Location: Kharagpur, India Posts: 5 Rep Power: 9 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.

 March 8, 2013, 11:11 #12 Member   Satish Gupta Join Date: Jun 2012 Posts: 30 Rep Power: 7 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

 March 8, 2013, 11:22 #13 New Member   P Kaushik Join Date: Oct 2010 Location: Kharagpur, India Posts: 5 Rep Power: 9 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.

 March 9, 2013, 16:32 dear #14 Member   farzadpourfattah Join Date: Mar 2013 Posts: 41 Rep Power: 6 first check your reference value, default value of fluent for length and depth is 1. set your length and depth.

 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 Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 42 January 8, 2017 13:55 maka OpenFOAM Pre-Processing 6 August 12, 2010 09:01 hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36 andre OpenFOAM 5 June 23, 2008 10:37 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 04:01.