Learning Forum

[Waruna Maddumage]

Hi,

I am currently working on a steady-state heat transfer simulation using Fluent, focusing on a two-phase system involving oil and air. The setup includes a heated copper solid plate with oil injection for cooling, where approximately 20% of the metal is in contact with the oil jet stream, and the remaining part is exposed to surrounding air.

Here are some key details of my simulation:

• Computational domain with one velocity input (only oil injection, no air) and one pressure output (oil and air escape, backflow of air is seen during simulation. But backflow of oil is not allowed).
• Adiabatic walls and coupled solid-fluid contact surfaces.
• Metal geometry defined as a constant heat source.
• Multiphase model using VOF with Implicit formulation.
• Turbulent model: K-omega SST.
• Steady-state simulation with pseudo-time stepping and enabled high-order term relaxation.
• Mesh properties: Orthogonal quality (2.3), aspect ratio (90), 10 boundary layers at the thermal boundary layer, Max y+ value around 1.5, average y+ below 1.

While the temperature values from the simulation match well with the experimental data, I am facing a significant issue with the heat transfer coefficient. The experimental values are around 800, but the simulation results yield a much lower value of around 50. I also get unrealistic surface heat flux values in areas where the metal is in contact with air, with many regions showing zero or negative values. The average temperature difference between the fluid and the metal is around 10 degrees.

I would greatly appreciate any insights, suggestions, or recommendations to improve the accuracy of the heat transfer coefficient and surface heat flux values in my simulation.

Thank you in advance.

Waruna

[Federico]

Hello, 

which HTC are you using in Fluent? If using, Surface Heat Transfer coefficient, this will be based off a reference temperature in your Reference Values. The default is 300 K. For most flows however, a constant reference temperature is not applicable.

There is also the Wall Function HTC, but this should only be used for average y+ between 30 and 60.

Finally, since your boundary mesh is fine, you may use the y+ based HTC and Ref. Temperatures. This method uses the temperature found at y+ ~ 300 (again, the 300 value is the default value, but you can change this in References Values). The theory is that when y+ = 300 away from the wall, the fluid temperature approaches the bulk fluid temperature. However, this method may not be applicable on closely spaced fins, where the mesh does not reach y+ away from the walls.

You can check this article which summarizes this: Defining heat transfer coefficient (HTC) - Ansys Knowledge

[Waruna Maddumage]

Hi Federico, 

Thanks for the quick reply. I used the Surface Heat Transfer coefficient to get the above values. The reference temperature I used was the coolant oil inlet temperature. Could you please clarify a few points, 

1. When you said ''y+ based HTC and Ref. Temperatures'', do you mean the second method defined in Defining heat transfer coefficient (HTC) - Ansys Knowledge. Where HTC is defined as, HTC =(‘Total Surface Heat Flux’ – ‘Radiation Heat Flux’)/(‘Wall Temperature (outer surface)’ – ‘Static Temperature’).
   
   
2. You mentioned this method cannot be used in closely meshed fins. In my geometry, I do have a closely spaced area (clearence 0.25 mm). Is there a way to figure out whether y+ reaches 300 or not within this 0.25 mm gap?

Best,

Waruna

[Federico]

1. The y+ based HTC is different and not mentioned in the link provided. You can read its definition here 41.4. Alphabetical Listing of Field Variables and Their Definitions (ansys.com) (find the last 2 variables defined at the end of the page).
2. Unfortunately, there is no direct way to do this. I would not expect y+ to reach 300 on such closley spaced area. Eventhough you can lower the reference y+ value, you would need to have a sense of what y+ your flow does reach. You can estimate y+ by creating a Named expression for yplus and plot it along a line normal to the surfaces in question, but this y+ will only be valid along this line. 

Since you have experimental data, you might want to just use Surface HTC and try to find a reference temperature that will match experimental HTC.

[Waruna Maddumage]

Hi Federico,

Thanks again for your excellent suggestions. 

Changing the reference temperature and trying to match the experimental HTC is doable and I will try it.

But what about the surface heat flux? With this HTC approach, I will be relying on the Total Surface Heat Flux. I am not entirely sure that my total surface heat flux is correct. In some regions where the metal geometry contacts the air, I'm obtaining zero and negative results. As far as I understand, having zero or negative Total Surface Heat Flux values in areas where the metal temperature is higher than the fluid seems improbable.

Do you have any advice about my heat flux values? 

Thanks,

Waruna

[Federico]

Hello Waruna, 

to be sure, do you have a coupled Wall/shadow pair where the copper meets the air? This is required for heat transfer to occur.

[Waruna Maddumage]

Hi Federico, 

Yes, I do have a wall/shadow pair at the fluid-metal boundary and I have selected the 'coupled' option as the thermal conditions setting. 

Best,

Waruna