pipe flow heat transfer with high Prandtl numbers

[mikejcai]

Hi experts,

I'm using simulation cfd 2015 to study the heat transfer properties of some fluids, and I noticed something weird.  As a simple demonstration, I've modeled a long pipe with water flowing through it.  The boundary conditions are 40kW of total heat over the pipe wall, inlet volume flow of 0.004 m^3/s at temperature of 20C, and outlet of 0 pressure.  The temperature difference between the wall and the bulk of the water can be computed via well known correlations such as Gnielinski correlation.  There is indeed good agreement between CFD 2015's results and Gnielinski's for water (Pr ~ 7).  However, if I change to something that has high Prandtl numbers, such as ethylene glycol (Pr ~ 200), the temperature drop between CFD 2015 and analytic results can be as large as 50%.  In the attached cfz file, the analytic temperature drop should be 95C, while CFD 2015 gives 60C or so.  Can you suggest how to improve the results?

Thanks for your help in advance,

Mike

[srhusain]

1. From the properties shown below, it is clear that the viscosity varies significantly with temperature- have you considered using variable viscosity?
2. Also, without looking at your model setup, it is hard to tell, but i am guessing that the wall heat flux is applied throughout the length of the pipe. This could cause the solution to be inaccurate- maybe you could add an unheated/insulated entry length to the pipe?
3. In addition, check to ensure that the Reynolds number > 3000 as per the requirements of the GNielinski correlation
4. Lastly, you should (and probably are) ensure that you are applying the correlation on the fully developed flow portion of the pipe

Hope this helps

Physical Properties

Physical Properties (1)	Monoethylene Glycol MEG	Diethylene Glycol DEG	Triethylene Glycol TEG	Tetraethylene Glycol TETRA EG
Formula	C2H6O2	C4H10O4	C6H14O4	C8H18O5
CAS Number	107-21-1	111-46-6	112-27-6	112-60-7
Molecular Weight, g/mol	62	106.12	150	194.2
Boiling Point @ 760 mm Hg, °C (°F)	197 (387)	245 (473)	288 (550)	329 (625) Decomposes
Vapor Pressure at 20°C (68°F) mm Hg	0.06	0.002	<0.01	<0.01
Density, (g/cc) @ 20°C (68°F)	1.115	1.118	1.125	1.124
Density, (g/cc) @ 60°C (140°F) 1.096	1.085	1.087	1.093	1.096
Pounds Per Gallon @ 25°C (77°F)	9.26	9.27	9.35	9.37
Freezing Point, °C (°F)	-13.4 (7.9)	-9.0 (16)	-4.3 (24)	-4 (25)
Pour Point, °C (°F)	<-59 (<-75)	-54 (-65)	-58 (-73)	-41 (-42)
Viscosity, cP @ 25°C (68°F)	16.9	35.7	49.0	58.3
Viscosity, cP @ 60°C (140°F)	5.2	7.3	10.3	11.4
Surface Tension, dynes/cm @ 25°C (77°F)	48	44.8	45.5	44.0
Refractive Index @ 20°C (68°F)	1.430	1.447	1.455	1.459
Specific Heat @ 25°C (77°F) Btu/lb/°F	0.58	0.55	0.52	0.52
Flash Point, °C (°F)	116 (241) (2)	154 (310) (2)	177 (350) (2)	202 (395) (2)
Dipole Moment in Debyes	2.28	2.69	2.99	3.25
Coefficient of Expansion x 104 (0-60°C)	6.5	6.6	7.2	7.3
Thermal Conductivity, Btu hr-1 ft-1 °F-1 25°C (77°F)	0.1490	0.1175	0.1133	0.1106
Thermal Conductivity, Btu hr-1 ft-1 °F-1 25°C (77°F)	0.1490	0.1175	0.1133	0.1106

[mikejcai]

Hi srhusain,

Thanks for your advice.  These are excellent suggestions.  Please find my response to your itemized suggestions below.

1.  Since I'm comparing CFD 2015 simulation results to analytic calculations, I thought I'd keep things simple by choosing a constant viscosity.  If I wanted to compare to real experiment, then I'd have to use variable viscosities, as you have suggested.

2.  Adding an entry length is a good idea.  I added a segment 50cm long, which is 10 times the pipe diameter.  It is unheated, and I place the same inlet conditions there.  I checked "fully developed" box for the inlet volumetric flow rate too.  Unfortunately it didn't help.  The maximum temperature drop from surface to fluid bulk is about 20C (I misspoke in the previous message, it's not 60C), as opposed to the calculated 95C.

3.  The Reynolds number is 5200, and the Prandtl number is 204, which are supposed to be in the valid range of the Gnielinski correlation.

4.  Yes, I did the comparison in the fully developed portion of the pipe.

I've included some images from the simulation results below.  The first image shows the converged solution, with fluid flowing from right to left.  It's strange to see periodicity in the surface temperature distribution.  It can't be real.  The other two plots are taken along the axis of the pipe.  The linear variation of bulk temperature profile suggests that after the entrance length, heat flux is roughly uniform along the pipe.  The linear region in the temperature and pressure profiles allows me to identify the fully developed regions.  I used auto forced convetion option in the solver, so the flow part and heat transfer part are decoupled in the calculations.  From the pressure drop, I can calculate backwards the Darcy friction fraction f = 0.073.  However, if I compute from the Reynolds number, it gives f = 0.038.  Thus I think both flow and heat transfer calculations contribute to the problem.  (BTW, if I use f = 0.073 in the Gnielinski correlation, I get a temperature drop of 68C, which is still quite different from the 20C in CFD 2015 results.)

Looking forward to your further guidance.  Thanks,

Mike

[srhusain]

It appears that the temperature field in your screen-shot is wavy along the length of the pipe and I suspect that the solution is not fully converged. This will definitely yield poor thermal results.

Can you post your support file (rename the extension with a ".zip" before posting)?

[mikejcai]

Hi srhusain,

Here's the support file, with the extension manually changed from .cfz to .zip as you requested.  I've tried several mesh refinements, but didn't get much better results.

Thanks,

Mike

[srhusain]

Here is a revised support file. The main changes I made are:

1) Finer mesh and extruded for better accuracy

2) 10 layers of boundary layer elements for better resolution of the near wall sharp gradients

3) Using Adv5 along with the SST- turbulence model for better accuracy at low Reynolds numbers

Looking at the summary file, the energy balance is about 4.46 kg/s x 2382 J/kg-K x ( 23.7553 - 20 ) C = 39895 W, so that looks good. The temperature on the pipe wall and exit plane is shown below and looks smooth.

However, I am not clear how you are extracting the temperature drop that you are comparing with the solution from the GNielinski Nusselt number correlation.

[mikejcai]

Hi srhusain,

Thanks for the quick reply.  Yeah, I tried some of your tricks before, but wasn't very successful.  The way I check against Gnielinski correlation is to take a cut across the pipe and look at the temperature difference between the edge of the circular cross section and the center.  An easier way to check is just to look at the legend.  In your example, the highest temperature anywhere along the pipe is 37.10C.  We know the bulk temperature ranges from 20-23.75C along the pipe.  So the maximum temperature difference is 17.1C, no where near the 95C computed from Gnielinski.  

As I noted in the first message, this discrepancy becomes smaller for smaller Prandtl numbers.  If you replace the material with water and run the same simulation, the temperature drop is about 6-7C, while the Gnielinski correlation gives 8.8C.

Again, I appreciate your help in trying to solve this problem.

Mike

[srhusain · Accepted solution]

The bounadry layer mesh should be such that Y+ is around 0.3 to ensure that the thermal boundary layer is resolved accurately. The attached model results in a value of about 2.0, and the temperature difference between the center and the wall is around 30 C, which is a bit of an improvement.

Can you try making the pipe longer and a mesh fine enough for the Y+ requirement? You might try 15 layers of enhancement with a gradation factor of 1.2 and make the pipe twice as long, which might help to make the flow thermally developed (that is, the difference between the bulk and wall temperatures stop changing along the pipe)

[heath.houghton · Accepted solution]

I'd like to add an alternate approach to ensure proper y+ at the wall and not have to guess at the layer thickness, etc. is to use mesh adaptation and set the max y+ in the adaptation dialog.

Heath Houghton
Product Manager - Autodesk Simulation CFD

[Royce_adsk · Accepted solution]

I would advice you to listen to this section of the turbulence model support hangout.  High Prandtl number heat flux is much more difficult to solve and will require a very accurate representation along the wall. I would highly advise you to take Syed's suggest about tuning the mesh enhancement along the wall to make sure your Y+ value is 0.3 or less.  Using the extruded mesh is ideal, but not always possible depending on the geometry that you are looking at.

Also keep these in mind for these types of problems:

• 15 layers
• 1.2 Gradation
• 0.8 Thickness factor
• Tight convergence
• Enable Blending in the Mesh Enhancement Window (2015 UI Feature)

These are all a great place to start and not an end all.

When it comes to just pure pipe flows I am not a big fan of using adaptation.  For more industrial models I do become more of fan of using adaptation because tuning the mesh is much more difficult.  I say this because you can quickly do some guess and check with you enhancement options faster than waiting for 3 cycles of adaptation to run.

Best regards,

[mikejcai]

Hi srhusain,

Following your suggestion, I increased the number of layers to 15 and set gradation factor to 1.2.  The resulting Y+ is slightly below 1.  Now I'm getting maximum temperature drop around 85C, and the average temperature drop along the pipe is probably around 65-70C.  This seems to be the right solution to my problem.

Thank you so much for all the help,

Mike

[mikejcai]

Hi Royce and Heath,

Thank for further suggestions.  I just watched Royce's video on tubulence models.  Excellent overview on the subject.  I'll continue to explore some of the options.  For my particular problem, choosing the appropriate turbulence model and refining the boundary layer mesh did the trick.  It's been a pleasant learning experience for me.  Thanks again.

Best,

Mike