[Swish31]

Hi

I am currently working on a project that involves CFD simulation on ANSYS and i need some help as it has got me stuck. I am designing a faucet atomizer and it's functioning is similar to a nozzle.

I have designed it on CATIA and am trying to analyse it on ANSYS Fluent.

I am using the following conditions:

-Pressure based solver, absolute velocity, steady flow

-Flow characteristics: Laminar at inlet, turbulent at outlet

-Boundary conditions: inlet velocity: 0.041 m/s, inlet pressure: 300000 Pa,outlet pressure: 0 Pa

-Fluid: water(liquid)

I have the following doubts:

1.)I read that turbulent models give accurate results even if flow is laminar but not vice versa so i chose turbulent but which turbulent model should i apply?

2.)My geometry has swirl, complex curves and rotational flow and i read that k-epsilon, k-omega models do not handle such flows and curves well so which model should i adopt(my geometry is very small in dimensions so swirl may not matter?).

3.)How should i do the meshing of my model? I did it multiple times according to my understanding but due to some reason the solution didn't converge and diverged a couple of times as well. My system also does not have a lot of computational power hence less elements and nodes in mesh.

I have attached the link for the images of extracted volume, my mesh and the part.
I will be able to share the geometry file with you if you require.

I will be very grateful if you can help me out.

Thanks
https://drive.google.com/open?id=1Tk...bbRwx0Z7kTBhV_

[vinerm]

It all depends on whether you are analyzing the inside of the atomizer or the outside, i.e., the surroundings where outlet of faucet is considered as inlet. Or it may have both; the faucet as well as the surroundings.

[Swish31]

Sir i want to analyze the inside.

[vinerm]

Since the flow is wall bounded, prefer SST model. Eddy viscosity models, such as, and do not handle anisotropy in turbulence well, however, this needs to be tested for your case; the turbulence in your case may or may not be isotropic. However, would work to a good extent. The most important part in your case is the pressure. You have mentioned a pressure of 3 bar. Is it gauge or absolute? If you consider fluid to be incompressible, then the pressure won't have any effect. So, you have to consider it compressible. With compressible fluid, you should not use velocity inlet; use either pressure inlet or mass flow inlet. I'd suggest you to start with incompressible fluid and velocity inlet. Once that case works fine, then you should start working with compressible fluid.

As far as mesh is concerned, if you cannot generate hex mesh, generate a fine tet mesh, close to 1.5 - 2 million cells. Then, in Fluent, convert it into polyhedral. This will reduce the count below half a million and may also improve the quality. However, the conversion requires good amount of RAM. For 1.5 mn cells, you will need at least 8 GB. If you can't do that, then try to put good quality tet mesh with at least 4 layers of boundary layer mesh, called inflation in Ansys Meshing. This is required for using SST .

[Swish31]

Sir the 3bar pressure is gauge pressure as the water that generally flows in our pipes is 3 bar. The fluid is water so how to go about the compressible fluid part since it is incompressible.

If using the k-Omega model will generating a good quality tetrahedral mesh with inflation layers work or do i have to give some other features as well?

[vinerm]

3 bar at inlet and 0 bar at outlet imply a drop of 3 bar across the nozzle, which is significant. If that is required for the mass corresponding to 0.041 m/s velocity at the inlet to go through, then you won't have to use compressible fluid. That you can check by running a case with constant density. Fluent will predict the pressure at the inlet for the required mass to go through. If it is closer to 3 bar, then it is good. If it is way too less than that, which I expect, then you will have to use compressible fluid. That option is available under material properties as compressible liquid. The coefficients given are as per water so you don't have to change those.

[Swish31]

So ill use the pressure based solver with k-omega velocity inlet only.

[Swish31]

Dear sir,
I solved the problem using velocity inlet and pressure outlet and the inlet pressure i got was 2.2 bar as opposed to the expected 3 bar.
Why is this difference there? Is there any error? The fluid is water hence incompressible.

[vinerm]

Any particular reason that you want it to be 3 bar? Is it a value reported from some test? If that is the case, then you will have to look at other aspects, such as, roughness of the impeller blades and casing, length and roughness of the inlet and outlet ducts. As per the setup, assuming mesh is fine enough to resolve the shear stresses at the blades and the casing of the pump, results would be within 10% error. So, if for a certain flow rate, 2.2 bar is the pressure drop, then that's it. Do note that you have to compare total pressure drop and not static pressure drop.

Every fluid is compressible, even lava and molten steel. All that matters is Mach number. Any flow above Mach number 0.25-0.3 is considered compressible, provided it is in continuum.

[Swish31]

Thank you ! I was able to get it done. Now onto the spray pattern.