[daf]

Dear all,

I am running 3D simulation of impinging air jets on a flat surface on CFX in order to study the wall heat transfer coefficient behaviour.

In the first part of my study, I simulate a single jet but I am having problems because the results of heat transfer doesn't match with similar simulations from other investigations.
In all studies I have found, at the stagnation region the heat transfer coefficient reach the highest levels, but in my simulations not.

I don't understand why I have this problem. I have changed the turbulence model, the mesh quality but I always get the same behaviour: at the stagnation region the heat transfer coefficient is lower than expected.
Another problem I amb having is about y+ value. Although I am doing the simulations with a very fine mesh, especially near the target surface the y+ value I obtain is very high..
Below I detail some details of one of my last simulations:
Geometry: 3D Impinging jet

Inlet: Air
v=40 m/s
T= 298 K (25ºC)
D=0,04 m
Target surface: Tconstant = 333K (60ºC)
Domain: Air 25 ºC
Turbulent model: SST
Mesh: 1003028 Nodes 996350 Elements

Would you please help me about it?

Thanks in advance

[Opaque]

I would not worry about the heat transfer coefficient until the heat flux distribution does not look correct. How does it look ? Does it make any sense ? and are the values within the expected behavior?

Once you cross that, you can define your heat transfer coefficient as it is done in the literature you are using to compare. What is their definition ?

Q_wall = HTC * A_ref * (T_wall - T_ref)

What is the reference temperature used by the literature ? How does it compare to the one used by CFX ?

HTC alone is useless for any engineering purpose until the companion reference temperature is defined. Most people tend to forget how HTC is defined.

Good luck.. Hope the above helps.

[daf]

Opaque, thanks for your response.

In the literature, they I trying to describe the radial distribution of the heat transfer coefficient in a impinging jet configuration.

They define:
q_wall= h ·(Twall - T_wall_adjacent)
q_wall(W/m^2)
h(W/m^2·K)

And then, they represent heat transfer coefficient adimensionally with the Nu number

Nu= h * Dh/lamda
Dh=Hidraulic Diameter of the jet (ctant)
lamda = thermal conductivity (for low differences between Twall and Tjet ctant)

I have not attached te the Nu distribution, but has the same behaviour of the h distribution.
The way they define the heat flux distribution, is the way used by ansys CFX...

[Opaque]

My apologies, but I will be surprised anyone reporting Nu, (or HTC) from experimental data based on T_wall_adjacent. Numerically, it is possible but experimentally sophisticated measuring techniques are needed not to perturb the flow conditions near the wall. Then I will start asking the following:
what distance is used to define adjacent ?
Is the same distance in your mesh used by CFX to report Wall Adjacent Temperature ?
How will you force CFX to use the temperature at a specified distance as the Wall Adjacent Temperature when computing HTC ? In particular, when you refine the mesh. Your near wall mesh may be closer to the wall than the reported experimental location.

A quick web search shows uses of adiabatic jet temperature (seemed like some king of total temperature), or the jet exit temperature. Nothing about near wall temperature.

[singer1812]

Opaque is right. Your definition should probably be Twall-Tjet_inlet (or vice versa) wth Tjet_inlet as your reference.

Also, you said similar experimental conditions dont match your profile. Since you said similar, I assume that the setup may not be exactly what you are modeling. Did you know that impinging jets are very suceptible to jet height (among other things)? It is not uncommon to see a secondary peak in h as you show, and that peak might also exceed the stagnation point value.

Read up on impinging jets in a basic heat transfer book.