Heat loss from a steam pipe in windy air
 

Hello,

I want to prepare basic model of heat transfer described below. This is an example form Cengel's Heat and Mass Transfer.

A long 10-cm-diameter steam pipe whose external surface temperature is 110oC passes through some open area that is not protected against the winds. Determine the rate of heat loss from the pipe per unit of its length when the air is at 1 atm pressure and 10oC and the wind is blowing across thepipe at a velocity of 8 m/s.

The answer based on empirical correlation is about 1090 W. But my computation in Fluent gives about 1760 W and I cant find source of error. Please help me. Below is my model description.

mesh.jpg is screenshot of my mesh. Its coarse, but changing elements to be twice smaller doesnt change result significantly. So there must be problem with model.

I use Fluent 16.2.
Model:
- energy equation - On
- viscous - standard k-epsilon, enhanced wall treatment,
Material - air (default)
Cell Zone: fluid, air
Boundary conditions:
- velocity inlet (blue) - velocity magnitude 8 m/s, temperature 283.15 K,
- pressure outlet (yellow) - temperature 283.15 K,
- pipe wall (red) - temperature 383.15 K,
- surrounding wall (green) - heat flux=0,
Solution methods:
- Scheme - Coupled
- Gradient - green-gauss node based,
- pressure - second order,
- momentum, turbulent kinetic energy, turbulent dissipation rate - second order upwind
- pseudo transient - On
Solution controls - left default.
I used hybrid initialization.
Calculations converge quickly. But the result which i get using Reports -> Fluxes for pipe wall is far too large.

I hope I provided necessery information. Any advice and suggestions will be appreciated.

hi,

1. you can increase the dimension of tunnel/box i.e. far field boundary to avoid effect of wall on flow & thermal field.
2. Change BC from Adiabatic to symmetry/free slip.
3. Why coupled solver ?
4. Reynolds number in current case ?
5. Fluid properties are constant or function of temperature ?


Devesh

Hello,
I improved my model somewhat. I answer your questions below:
1. I increased dimension below and over the pipe as well as beyond. To gain precision I added density block around pipe and in wake region. This results with fine (IMO) flow field. Pics rel attached.
2. I've changed BC to symmetry for all surfaces around pipe except inlet and outlet.
3. I,ve used coupled solver because it was recommended in ANSYS tutorial. Which one should be better in case like this?
4. Reynolds number based on pipe diameter and free stream velocity is 42190.
5. All properties I assumed to be constant from table for air at 60oC. I can use some characteristics from Fluent database for air, but which one exactly should I pick? There is a lot of options.
I know that calculation in book are just rough approximation, but my result should be +-20% of that. (about 900-1300 W) But after presented improvements I still got 1730 W.

Thank You

Since you are using enhanced wall treatment, did you check to see if your Y+ values are less than one? When you did your mesh independent study did you increase the number of prism layers as well as increasing the number of tetrahedral cells? Also what is the minimum quality of your mesh? These factors could influence your computed heat transfer rate.

But how to obtain y+ value for pipe? I found this calculator: http://www.cfd-online.com/Tools/yplus.php
In my case free stream velocity is 8 m/s, density and dynamic viscosity are for air at 60oC (film temperature) 1.059 and 2.008e-5 respectively. But im not sure what to put in boundary layer lenght. Should it be pipe diameter? I left default value of desired y+ (1). The Reynolds number which I got (4.2e+4) is obviously correct, but how to understand estimated wall distance? (4.0e-5 m)
I was also changing number of prism layers, but this doesnt change result. I just set initial high of prisms 0.2 and height ratio to 1.2. growth law - expotential. Below you can find quality report from ICEM:

Histogram of Quality values
0.95 -> 1.0 : 53747 (15.211%)
0.9 -> 0.95 : 43732 (12.377%)
0.85 -> 0.9 : 37484 (10.608%)
0.8 -> 0.85 : 42336 (11.982%)
0.75 -> 0.8 : 43569 (12.331%)
0.7 -> 0.75 : 41685 (11.797%)
0.65 -> 0.7 : 39516 (11.184%)
0.6 -> 0.65 : 37797 (10.697%)
0.55 -> 0.6 : 12898 (3.650%)
0.5 -> 0.55 : 250 (0.071%)
0.45 -> 0.5 : 38 (0.011%)
0.4 -> 0.45 : 1 (0.000%)
0.35 -> 0.4 : 0 (0.000%)
0.3 -> 0.35 : 0 (0.000%)
0.25 -> 0.3 : 0 (0.000%)
0.2 -> 0.25 : 0 (0.000%)
0.15 -> 0.2 : 0 (0.000%)
0.1 -> 0.15 : 0 (0.000%)
0.05 -> 0.1 : 0 (0.000%)
0.0 -> 0.05 : 0 (0.000%)
Quality metrics criterion: Quality (Min 0.449497 Max 0.99919)

I think mesh quality is quite good. Prism layer has very good quality (above 0.8). But maybe I should change prisms parameters? Or mesh is not a problem in this case and I should change something in Fluent? Maybe disable enchanced wall treatment or try another model?

Thanks in advance

Mesh quality looks good. Transitions are gradual as well which is good.

y+ depends on the wall shear stress which we don't usually know before we run a simulation. The calculator you used only estimates the first prism height based off of a Reynolds number and a desired y+

To obtain the real y+, obtain iterative convergence in Fluent, then go to contours of turbulence, then select y+ and select all your walls. The contours you see will tell you the value of y+ on all your walls. They should be below 1. If they are not, then you have to move the first prism height closer to you walls. Stick to enhanced wall treatment as it is better for heat transfer calculations. You can search the forums for more detailed explanations of y+ and also take a look at the books "Turbulence Modeling for CFD" by Wilcox and "Viscous Fluid Flow" by Frank White.

If you still cant match to your experimental results, try the k-w model or the kw-sst model. Let us know if any of these factors get you closer to the experimental data.