
[Sponsors] 
April 29, 2012, 06:46 
low heat transfer and nusselt number below 1.

#1 
New Member
Join Date: Mar 2012
Posts: 12
Rep Power: 5 
Hello all
I'm trying to do 2D model of the convection heat transfer in the pipe with dimension of 0.047m *1.8m. the water flow enters the pipe with the velocity of 1 m/s and the temperature of the 300 K, the wall temperature is kept constant at 400. i have chosen kepsilon turbulence model. but the total surface heat flux on the wall is 520 w/m2, and by putting the volume average temperature(344K) as the refrence temperature. and according to nu=hD/K, D=0.047 and k=0.6 W/m.k for water, the nusselt number would be 0.3627, i want to know does it make sense to have a nusslet number under 1? i think there is something wrong, can anyone tell me what is wrong with my model thank 

April 29, 2012, 11:19 

#2  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 
Quote:
Also what are you trying to solve in this simulation? Either way this problem can be solved easily without CFD. Use the DittusBoelter correlation or similar for fullydeveloped flow and/or use developing flow correction. this is not the reason for your error but the volume average temperature is incorrect reference temperature. It shall be the logmean temperature difference. You are probably better off just using the inlet temperature as a reference. 

April 29, 2012, 12:02 

#3 
New Member
Join Date: Mar 2012
Posts: 12
Rep Power: 5 
thank you so much for your reply,
in fact i want to check the validity of my model with comparing it to DittusBoelter correlation. there is something wrong with the value of total heat flux from wall, because its 520 W/m2. and its too small, because when i calculate the rate of the enthalpy increase between the inlet and outlet based on the average outlet temperature and inlet mass flow rate, its so much higher than this value and the nusselt number will be higher than 1000. i'm wondering why the total surface heat flux calculated in the fluent is so low?? thanks 

April 29, 2012, 12:30 

#4  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 
Quote:
How are you calculating this magical total surface heat flux? First, there isn't even such a quantity as total surface heat flux. Did you mean surface average heat flux? Did you mess up when scaling your mesh when you imported it? 

April 29, 2012, 13:28 

#5 
New Member
Join Date: Mar 2012
Posts: 12
Rep Power: 5 
thanks again for your attention.
the average outlet temperature is 366 K I calculate HTC and nusselt according to this process: volumetric flow rate= A*velocity=(0.0235^2*pi*1)=0.00173 m3/s mass flow rate= density*volumetric flow rate= 998*0.00173=1.73 kg/s enthalpy increase along the total length of pipe= mass flow rate*cp*deltaT=1.73*4182*64=463626 [J] its the enthalpy increase in the 1.8m of the pipe but since the velocity of the fluid is 1 m/s and it passes through the pipe in 1.8 s for obtaining heat flux i divide the enthalpy increase of pipe by 1.8 so: 463626/1.8=257459 W then, HTC=257459 /((400344)*Area)=17298 W/m2.K then, nusselt=h*D/K=17298*0.047/0.6= 1355 I mean the average heat flux from the wall with the unit of W/m2, that in fluent I obtain it from surface integrals>total surface heat flux, and by choosing area weighted average as report type. about the scale i checked it again and its ok, the diamter is 0.047m at lenght is 1.8m Dittusboelter predict a value of about 300 for my case for fully developed flow. 

April 29, 2012, 13:42 

#6  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 
No real fix, but some small errors.
This needs to be mass weighted average and not areaweighted average. Which did you use? Either way, it will not affect the Nu that much. this part should give you [W] Quote:
This area should be pi*D*L = pi * 0.047m * 1.8m, is that how you calculated it? Quote:
Your calculated heat flux using mdotCpdelT is the same as that reported by Fluent or no? Since all the calculates seem to be mostly correct, but guess now lies with the accuracy of your simulation. Any problems with convergence? Is your grid consistent with wall function approach used? Last edited by LuckyTran; April 29, 2012 at 14:03. 

April 29, 2012, 15:43 

#7  
New Member
Join Date: Mar 2012
Posts: 12
Rep Power: 5 
Quote:
Quote:
Quote:
Quote:
Quote:
I did very fine mesh near to wall and yplus is less than 0.05 at the wall 

April 29, 2012, 15:54 

#8  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 
Quote:
Since this is 2D, it is done with axissymetric type domain correct? Check your convergence by monitoring actual engineering values. I seriously doubt your solution is converged at 1000 iterations. For y+ < 0.05 and 40D domain length, your mesh is huge (relatively). For starters, you can check your velocity profile at multiple crosssections to verify that the flow becomes fully developed. Quote:
For DittusBoelter, the fluid properties are evaluated at the mean bulk temperature (average of inlet and outlet). But again, the properties would not change by that much. Again, I would ignore this little detail for now. Last edited by LuckyTran; April 29, 2012 at 16:10. 

April 29, 2012, 16:42 

#9  
New Member
Join Date: Mar 2012
Posts: 12
Rep Power: 5 
Quote:
yeah its axisymmetric. the mesh size near to walls is that fine but the size of mesh increases going away from it. i have already plotted the velocity profile in different sections and i attached the plot. i didn't understand this "Check your convergence by monitoring actual engineering values" can you explain more? 

April 29, 2012, 16:47 

#10 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Nusselt number calculation in Fluent  Sharadkumar Yeri  FLUENT  36  June 5, 2015 05:08 
Nusselt Number  Heat Transfer over a rotating cylinder  leomec88  CFX  3  March 7, 2012 18:09 
Reynolds Number and Heat transfer Coefficient  panos_metal  FLUENT  0  January 7, 2011 07:37 
Flow around pipes  heat transfer coefficient on the wall of pipe  doodek  Main CFD Forum  2  November 23, 2009 09:48 
Water vapour condensation in CFX5.7.1  hdj  CFX  1  November 27, 2005 08:15 