[Guille1811]

Im modeling the effect of an axial fan via a cilinder subdomain with a general momentum source. I used the coefficient technique to force it to move air at 20 m/s.

I run the model with k-epsilon and the momentum source worked fine with a momentum source coef of -5E2 (see first picture attached) . The problem is the results were not so good in terms of temperature fields etc, so after doing tons of sensitivity analysis of mesh, boundary conditions, timescale factor, initial conditions, etc the only thing left to analize is the turbulence model.

I switched to SST model (with turbulence flux closure for heat transfer and transitional turbulence desactivated, i dont have any data), at first the velocity converged almost immediatelly to 19 m/s and it stayed there for like 100 iterations. During that time the simulation "results" were almost exactly as expected because of some other monitored variables, which indicates this model may be the best suited.

After that 100 iter, the velocity suddenly drop to negative values and stay there for like 100 iter, then it comes back to 20 m/s and stay there but this time the final streamlines are caotic and all over the place (see second picture attached).

I tried with different source coefficients in the range between -1E2 and -1E6 and nothing changed.

Any idea of how i can make the momentum source to work?

[evcelica]

Is your time step increasing automatically, pushing the subdomain into instability?

[sealcoga]

Nope, it stay practically the same. Ive tried with 0.1 timescale factor and 0.01 timescale factor, as well as 10 timescale factor (always in aggresive mode)

[ghorrocks]

Please attach your output file and an image of what you are modelling.

Also, -1e6 might not be big enough. Have you tried bigger numbers?

Also also, this flow may well be transient. Jet flows have a habit of going into flapping modes.

[Guille1811]

I tried up to -1E10. Here is the monitor of the velocity outside the momentum source (cant upload the output, the file is too large).
There is really no more images needed with respecto to the simulation, as you see in the first images the domain is simply a "box" of air and the cilinder wich acts the momentum source.

Boundary conditions:

Inlet: temperature profile, wind profile (same direction as the air blowed by the fan)

Face at the end of the flow: entrainment condition with static pressure profile

Lateral faces: wall with free slip condition

Ceiling: wall with free slip condition and fixed temperature of 300 K

Ground: wall with no slip and fixed temperature of 268 K.


Right now i managed to "kinda" make it work but after like a 100 mts the flow suddenly rises al the way to the top (see last picture attached), so it still isnt ready.

[ghorrocks]

Please attach your output file. It contains far more information than what you are posting and we need to see it to understand the details of what you are doing and how it is converging.

If you run it a few more iterations and look at the results again - does the kink in the flow just move along a bit? If yes then you simply need to run the simulation for more iterations to blow this kink out the outlet. It will converge quickly after that.

[Guille1811]

Nevermind, i made it work finally by setting relative pressure =0 Pa en boundaries.

But now i have another problem (which i also had the time before when i made it work with k epsilon). The air the fan is moving (which starts at 20 m/s) still has like 5 m/s of velocity after traveling 200 mts. According to the technical specifications, the fan has at best 125 mts of longitudinal reach, so having 5 m/s of velocity at 200 mts is far from coherent. Clearly there is much less air friction going on in the simulation than in real life, how can i adjust this?

[evcelica]

You are not appropriately modeling the fan:
Rotating blades, cylindrical velocity, vorticity and turbulence added by the spinning blades, as well as pressure pulses each revolution, vortex shedding over the blade edges....
You just have a magic volume that moves air perfectly axially at 20 m/sec.
How could you expect that to have that same flow characteristics of an actual fan.

Adjusting turbulence levels might dissipate the velocity quicker, but it is still not the same as the fan.

[Guille1811]

I run the simulation of the fan itself with all the proper machine design in a different smaller domain. The 20 m/s is the average outlet velocity of the fan according to that simulation results and, due to a special element in the design of the machine, the vorticity of the outlet flow is minimal so i felt free to ignore for the principal simulation.

Due to limitation of computstional resources, i cant run the big simulation with the real design of the fan (too many elements and nodes) so i must incorporate it as a momentum source.

If you have any suggestion on how to make it work this way i would be highly appreciated. Its important to say that there is no extreme presicion needed for this simulation (:

[evcelica]

You could try also putting in the same Turbulence Kinetic Energy and Turbulence Eddy Frequency as your fan simulation, and see if that makes it match any better.

[Guille1811]

Put them where?

In the advanced turbulence control settings of fluid models tab?
In the initialization tab on turbulence intensity options?
In the boundary conditions?

Only in the cilindrical "momentum source" domain or in the big domain as well?

All of the above?

[evcelica]

I would think in your volume source. That is the fan where you "know" the turbulence levels from your previous simulation.

[Guille1811]

I put the turbulence parameters in the cilindrical domain as the result was the momentum source became unstable again (exactly like the picture of the first post).

On other note, i did the experiment to expanding the domain to a ridiculously high value (500 mts long) and the air moved by the momentum source still had velocity after traveling 500 mts, which is absurd.

What input/condition might be causing this "perpetual" air movement?

[ghorrocks]

perpetual motion:
Is your moment source correctly applied?

If that is OK then you have not modelled the jet dispersion correctly. You have too little dissipation in the model. Modelling dispersing jets is a standard CFD benchmark simulation and I would strongly recommend you spend some time looking into it. When you can accurately model a benchmark simulation of a jet flow then you will be in a good position to simulate this case with more confidence.

Here are some links on jet flow to get you started:
http://www.sciencedirect.com/science...10465593901475
https://www.youtube.com/watch?v=iELFWDuSoe4
turbulent jet flow RANS validation

[Guille1811]

Thanks Glenn for the references. I read them but nothing really solves my problem. All fan simulations are made via one of 2 ways: either a general momentum source or an inlet/outlet mass flow boundary condition.

In my case i cannot do the last one because for my simulation the temperature of the air being moved by the fan is very important for the actual results. That being said, if i would do the secon approach i would have to specify an specific inlet temperature and that would be messing with my results, so im forced to do the general momentum source approach.

As i said earlier, i already did a simulation of the fan itself so i have available all the cfx post data. The thing is i dont know how to incorporate it the right way so the air moved by the fan actually behaves like a real fluid in term of its losses while moving...

[ghorrocks]

I think you missed the point of my last post.

Modelling a jet flow (such as the exhaust from a fan) is a complex thing to model and is the subject of many benchmark simulations. Your question is "how do I accurately model the jet coming from my fan" and my answer is "do some benchmark simulations of jet flows so you know how to accurately model them. Then use these approaches on your model." This is why the benchmark jet flow results are important.

You need appropriate validation and verification of your simulation approach and proper select of a turbulence model. If this is your question you can start at this FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[Guille1811]

Glenn i searched for jet flow simulations and all i found was either simulations utilizing the general momentum technique or the simulation that i already did (the fan with all its mechanical parts etc). I really dont know what else you are refering to. On the other hand, i dont need extreme accuracy in my simulation results so modelling the fan as a momentum source with a fixed velocity is more than enough for me (if i get the technique to work, of course)

That being said, i had to change some boundary conditions and now the streamlines coming from the momentum source are caotic no matter what setup I define. Ive tried docens of combinations of turbulence models, turbulence initialization settings, other boundary conditions, momentum source coefficient and always the momentum source become caotic. Funny enough the velocity at the "outlet" of the momentum source always converges to a good value, but the streamlines are extremelly caotic and all over the place.

Does anyone have any tips on how to fix this? Im getting kinda desperate since ive tried almost everything and my project deadline is oming closer and closer.

Thanks in advance!

[ghorrocks]

Please attach your output file.

I really dont know what else you are refering to.

I will try to explain it more clearly. This is basic fluid mechanics so if you don't have some knowledge of the basics it is unlikely you are going to get far in your simulations.

Here is an image of a basic single phase fluid jet flow. Fluid enters a domain at velocity V. How far does the jet go before it breaks up? Does it break up at all? Or does it go wiggly?

SinglePhaseFluidJet.png

This is a simple benchmark case which you should be able to find lots of good experimental and numerical studies of. Then you can simulate these cases and see if you can get the correct answer. You will probably need to adjust mesh, time step and convergence parameters to get answers accurate enough to be useable. And once you have determined what is required to give the accuracy you require you can then use the same settings in your case with some confidence that the results are going to be accurate.

Hopefully this explains what the jet flow I am talking about is and why it is important to use it as a benchmark case to make sure you are accurate.

[Guille1811]

Yes Glenn, i know exactly what you mean (refering to your diagram).

In fact, ive found some papers online that simulates jet flow but sadly neither one does anything very complex or out of the ordinary to execute the simulation (which apparently you are insinuating needs to be done)

If you ask me it makes absolute sense thst if you put a momentum source with some velocity, due to the air and turbulence model the program employs, the flows end up reaching velocity 0 at some coherent point.

Well anyway, my major problem now is the issue of the caotic streamlines from the momentun source i talked about (no need to attach pic, simply imagine absolute caos on the domain)

Do you (or anybody) know the possible causes of this?

[ghorrocks]

The chaotic streamlines could be either real or a numerical problem.

If it is real it is because you have triggered an instability which goes chaotic. Transition to turbulence is like this. If the effect is real than you should not try to change the model to eliminate it - the effect is real so your model should predict it. But then you need to think about how you are going to get representative statistics out of it. You might need to do a time average or something like that.

Also check whether the flow is chaotic (random and non-repeating) or periodic (a fixed pattern repeating). Chaotic is typical of turbulence, periodic is typical of instabilities such as jet and bluff bodies.

Or the effect could be a numerical artefact. Check your convergence is tight enough (ie, run tighter convergence and see if it remains chaotic), and use double precision numerics. Also check whether it goes chaotic for coarse or finer meshes. Consider the turbulence model you are using - is it suitable for this flow and Re number? It might not be adding enough dissipation to stabilise the flow.