low heat transfer and nusselt number below 1.
 

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 k-epsilon 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

Nusselt number can't be less than 1.

Also what are you trying to solve in this simulation? Either way this problem can be solved easily without CFD. Use the Dittus-Boelter correlation or similar for fully-developed 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 log-mean temperature difference. You are probably better off just using the inlet temperature as a reference.

thank you so much for your reply,
in fact i want to check the validity of my model with comparing it to Dittus-Boelter 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

What's the outlet temperature? Is it above 400K?

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?

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 /((400-344)*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
Dittus-boelter predict a value of about 300 for my case for fully developed flow.

No real fix, but some small errors.

This needs to be mass weighted average and not area-weighted average. Which did you use? Either way, it will not affect the Nu that much.

this part should give you [W]

No. Don't do that. That makes no sense. The pipe length is taken care of by area.

This area should be pi*D*L = pi * 0.047m * 1.8m, is that how you calculated it?

Was your simulation fully developed using periodic-bc? If not, you should expect higher than Dittus-Boelter.

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?

yeah i did mass weighted average

yes, you are right, but unfortunately not dividing by 1.8 made the nusselt worse and now its above 2000 :D

yeah, i did that to obtain surface area. do you think that choosing bulk mean temperature as reference is ok since i want to compare it with dittus-boelter??


it is not fully developed, but the pipe is long enough, and it would be fully developed after about L/D=10, so i think at least it should be near the theoretical value for fully developed.
No, my main problem was that the value shown by matlab is very low, so my nusselt calculated is, i dont have problem with convergence, i put all the residuals euqal to 1e-6 at converges after a bit more than 1000 iterations.
I did very fine mesh near to wall and yplus is less than 0.05 at the wall

well you're certainly not helping yourself. Stick to the physics, not arbitrary divisions.

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 cross-sections to verify that the flow becomes fully developed.

For internal flow, bulk temperature is typically (almost always) used as reference temperature in heat transfer coefficient. You will have to write a UDF or find one to calculate this temperature and modify the reference temperature if you want super accurate results. But you can calculate HTC using the entrance bulk temperature and correct for the change in bulk temperature (it is an algebraic correction using an energy balance). But I think this error would not be that great to explain why your Nu ~ 1300. So I would set this aside for now.

For Dittus-Boelter, 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.

thank you again for your patience and your help
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?

Check pressure, temperature, velocity
residuals don't say anything about convergence