turbulence models
 

Hello to everyone,

I'm currently trying to simulate a nozzle used for HVAC, and I was wondering if anyone could give me any advice about it.

So far I've tried the k-e (standard and RNG) and the k-w models, always in steady-state.

My domain consists simply in a box, with an inlet and two outlets. Through the inlet (which is in the middle fn the top face) hot air enters to the domain. The outlets are on the sides of the top face.

The results I obtain show always higher velocity than expected. Also the residuals plot start to oscilate after a number of iterations (usually over 1000) and the heat flux is never 0.

Which boundary conditions would you recommend me (velocity inlet, mass flow inlet, outflow etc.) and which turbulence model and other settings (discretization method and so on)?

Thank you very much!

Lots of questions there. Starting with the turbulence model, I would recommend the v2-f if you have the license for it (it comes with the standard version of FLUENT, but you need to buy a new license from ANSYS. It's available via text commands.) The v2-f model is particularly good at capturing heat transfer. If you don't have or can't get the license for that, I'd go with the k-w-sst model, with a grid that gives you y+ < 1. The k-w model is typically better at near-wall interactions since it doesn't use wall functions, at least in my experience.

Oscillating residuals could be because of high under-relaxation factors. Try reducing those and see if it controls the oscillations. But, oscillating residuals aren't a problem if they're low enough. How low are they oscillating at? And at what amplitude?

Velocity inlet is good for incompressible flows only - if you're using an ideal gas as your fluid, you'll need a mass flow inlet.

I've had no luck with outflow boundary conditions. I tend to use pressure outlets instead. That could be due to errors on my part, I don't know.

Discretization method is another hard one to give advice on. For most applications, I use 2nd order wherever possible (in some cases, some equations won't converge at 2nd order; in other cases I've gotten away with all 3rd order.) I don't know how to finesse a solution to improve the order of accuracy, I just pick the highest discretization scheme I can get away with.

I'm a bit confused about how to calculate the Re number.

If I calculate it with the velocity at the inlet and the inlets area, that number leads to a very thin grid spacing to have an y+<1. So that would be the spacing needed near the inlet.

Then to calculate the grid spacing near the walls of the room, do I have to calculate the Re number with the inlet velocity or with a much lower velocity (what it's expected near the walls)??

Thanks

Calculating the spacing you need for a particular y+ is a bit of a guessing game. NASA has a nice website to help though: http://geolab.larc.nasa.gov/APPS/YPlus/

i assume that i have to calculate 2 grid spacings.

one near the inlet (velocity 6,7 m/s and area of 0.1x0.1sqm)
and another one near the walls of the domain (velocity about 0.2 m/s and area of 2x6sqm).

am I right?

also I'm not sure of the velocity near the walls, 0.2 is more or less what i've calculated in previous tests, but i think is more realistic to use 0.2 m/s to calculate y+ than 6.7m/s, as this velocity only appears in the region close to the inlet.

Thank you for your responses
Regards

Use the reference Reynolds number in your flow. I only do external flows, so for example for an airfoil I use the Re at the trailing edge and the chord length as the reference length. In your case I don't know what the reference Re number and lengths would be.
The point of having y+ less than 1 is to get the first cell in the laminar sublayer (near walls.) There's no reason to have y+ < 1 near an inlet.