[Guille1811]

I need to simulate an oscilatting fan which oscilates 360º every 5 minutes, in other words, 0.2 rpm. This fan is operating on an stable atmosphere so temperature in the domain (more specifically in its boundaries) is an increasing function of height. The purpose of my simulation is to only obtain the temperature field at a certain height (1.5 m above ground) at the end of 1 cycle, in other words, after 5 minutes.

The whole geometry is basically a giagnt "cube" of air of 400 mts x 400 mts x 50 mts high with a cilindrical whole in the middle wich represents the fan (the hole is inclined 7º down so its not parallel to the ground, but almost). The fan is being modelled as a momentum source imposed in the front face of that cilinder hole (i obtained the data of the mass flow from the fan from another simulation).

The temperature of the ground is fixed (no thermal radiation) and the temperature in the "ceiling" is also fixed.

Boundary conditions:

in viento: inlet temperature profile imposed, as well as wind profile
out viento: outlet prssure profile
other 2 lateral faces: openings with temperature profile

Ive run some steady state simulations (both oscilating and without oscilating) with different timesteps but the residuals are always periodic so the problem has a transient nature.

I have running right now oscilating and not oscilating transient simulations with total time 300 sec and timestep of 1 sec. I know, its a huge timestep, but the total time is so large that due to time constrains of my project (every simulation cannot last more than 4 days) i aparently have no other choise. Anyway, there has been quite a lot of timesteps passed and neither one of them has converged after 5 coeff loops (convergence criteria: MAX<1E-3).

I would be highly thankful for any suggestion on how to approach this since the purpose of my simulation if VERY specific.

[ghorrocks]

You must do mesh size, time step size and convergence tolerance sensitivity checks to determine the mesh, time step size and convergence criteria you need to use. That will then determine how much computing resources you will need to complete the task. If you don't have that many computing resources then you need to do something like:

* Buy more parallel licenses
* Buy some time on a supercomputer (AWS for instance)
* Simplify the simulation so it is smaller
* Or give up and say the simulation is not possible with available resources.

If you choose to run large time steps, coarse meshes or loose convergence just so you can "complete" the simulation in available resources then can I suggest you save yourself time and effort and buy a dice. You can then easily generate random numbers which will be just as accurate as you simulation results will be.

[Guille1811]

Thanks for you response, you are definately right. Sadly im far from having those resources, any advise on how to redesign the simulation to get the result mentioned on a couple of days of running?

Greetings.

[ghorrocks]

Please attach some images of what you are modelling.

If you cannot simplify it then you are forced into option 4:

give up and say the simulation is not possible with available resources

[Guille1811]

Ok, here are some pics attached.

My geometry is extremelly simple, yesterday i reduced the size of the domain: its just a "cube" (of air) with a cilindral hole near on of its corners. The cilindral hole has a diameter of 2 mts and its like 30 cm long, the "cube" has dimensions of 200 mts long x 50 mts wide x 30 mts high. The front face oh that cilindrical hole has a momentum source of 80 kg/s (20 m/s) of air at a temperature of 277 K.

The "ground" temperature is fixed at 270 K and the "ceiling" temperature is fixed at 300 K (due to the vertical temperature profile).

My domain is rotating around a vertical axis near the hole so the net affect of this is that the momentum source is throwing "hot" air over the area near ground of the whole domain. This is a very slow process since the rotating speed is 0.2 rpm.

Basically all i want to know is that if after a whole rotation of the momentum source (5 minutes) which points at a 1.5 mts high plane dropped thier temperature instead of incrising it (drop because the "ground" is colder than the initial air at that height).

Every suggestion on how to achieve this result (or some result that can give information to infer it) is very welcomed (hopefully with a computational time of no more than 3 days since i have to run a lot of this simulations with varying source momentum speed and other things etc)

Greetings!

[ghorrocks]

It is very important to realise that the simulation time is whatever results from the validation process. It is not an input to it. Do not say what the simulation time must be and say the simulation must run inside that time. The tail does not wag the dog.

You have a very large box around your object. You should do a sensitivity study on the size of the box. Is a box that big required? You may well be able to make the box a lot smaller and that will speed the simulation up a lot.

Also depending on exactly how this thing works (I do not completely understand your description, so I will guess to fill in the blanks) this simulation seems to be an ideal candidate for separation of scales. This is because the time scale of the jet is likely to be fractions of a second to seconds, but the rotation of the jet is much slower (5 minutes). So then you can separate the scales and do a simulation of a stationary jet, and see what effect that has. You then model the slower rotation scale and impose the overall effects of the fast time scale jet simulation to it.

You can't do this separation of time scales in all simulations but it is a massive help if you can. And don't forget that often one of the time scales no longer becomes a CFD question - it might be just the heating up of a large body, and that is just simple heat transfer physics and can be done using a ODE solver. No need for CFD to model simple things like that.

You have not commented on my suggestion that you do mesh, time step and convergence sensitivity studies to determine what is required for your simulation. And in this case the size of the domain looks like it should be subject to a sensitivity study as well. You need to do this so you work out the simulation parameters you need for the accuracy you require - and then you can see if you have the computing resources to be able to do the job.

[Guille1811]

Thanks for your response.

"You have a very large box around your object. You should do a sensitivity study on the size of the box. Is a box that big required? You may well be able to make the box a lot smaller and that will speed the simulation up a lot."


The size of the domain cannot be reduced since it was determined according to the expected values of the performance of the machine. In other words, its said than the machine can protect an area of a circle with a radius of 150 mts aprox, so the distance of 200 mts long in my domain is there to give a margin to that value. The width of 100 mts maybe can be shortened a bit since i definately not going to model the whole 125 mts radius circle.

"I do not completely understand your description"

What exactly you dont understand? (:


"So then you can separate the scales and do a simulation of a stationary jet, and see what effect that has. You then model the slower rotation scale and impose the overall effects of the fast time scale jet simulation to it."

Do you mean run a transient simulation of the stationary jet, or a steady one) Cause i run a steady state simulation (with different timesteps and convergence criteria, my mesh is already super fine) with the stationary domain but the results are far from expected, probably because the real life scenario doesnt have the jet throwingng hot air to the same point all the time (due to its oscilation) so the behaviour of the temperature of that point is very different.

"You have not commented on my suggestion that you do mesh, time step and convergence sensitivity studies to determine what is required for your simulation. And in this case the size of the domain looks like it should be subject to a sensitivity study as well. You need to do this so you work out the simulation parameters you need for the accuracy you require - and then you can see if you have the computing resources to be able to do the job."


Yes i will be definatelly do that, but first i need to define my strategy for obtaining the result i need since there is no way i can simulate the whole 125 radius domain and/or the whole rotation.

[ghorrocks]

The size of the domain cannot be reduced since it was determined according to the expected values of the performance of the machine. In other words, its said than the machine can protect an area of a circle with a radius of 150 mts aprox, so the distance of 200 mts long in my domain is there to give a margin to that value. The width of 100 mts maybe can be shortened a bit since i definately not going to model the whole 125 mts radius circle.

This is saying that the domain may need to be bigger than what you have used. You should not guess these things, you should do a sensitivity study and work out what you really need.

What exactly you dont understand? (:

* Is the fan heated?
* What the purpose of this study is? Are you trying to stop frost forming or something like that?
* Why do a CFD study of it?
* How strong the external wind is relative to the fan.

A further point: This simulation appears to be strongly dependant on a jet flow, and how it mixes and breaks up. This is also being done in a buoyant atmosphere. These are challenging simulations to get accurate and you will need to make a careful choice of turbulence model, and depending on the sort of results you want you may need an LES model. Have you considered which turbulence model you are going to use for this?

[Guille1811]

* Is the fan heated?

No, its just a typical mechanical fan but because the temperature of the air increases with height, the air the fan is moving is warmer than the air near the ground.


* What the purpose of this study is? Are you trying to stop frost forming or something like that?

Yes, exactly that. Its a CFD study of the performance of a wind machine.

* Why do a CFD study of it?

Because its my graduate thesis work. Im a mechanical engineering student and i chose this proyect, there is no going back at this point.

* How strong the external wind is relative to the fan.

The external wind is 1 m/s at the height of interest (1.5 mts)

This simulation appears to be strongly dependant on a jet flow, and how it mixes and breaks up.

Yes, i did a simulation of this specific fan itself so i have all the relevant data for the main simulation.

Have you considered which turbulence model you are going to use for this?

Im using k epsilon, do you think its not a good idea?



Thanks a lot for your time!

[ghorrocks]

Thanks for the background, I have a better idea of what you are doing now.

I would recommend you do some research into jet flows and how the different turbulence models handle it. The different turbulence models are likely to produce quite different results in your case so you need to choose carefully.

About how to make this model tractable: The basis of the sensitivity studies I mentioned is what mesh, time step and convergence criteria is required to give the accuracy you require. In your case it may be better to turn this around and say what accuracy can I get for the resources I have. So if you determine that, say, a 1M node mesh with 0.1s time step and 1e-4 convergence criteria gives you an estimated 5% error range but a 2 week run time, you could ease that back to, say, 0.5M node mesh, 0.2s time step and 1e-3 convergence criteria and this gives an estimated 20% error range but a 2 day run time. This type of approach means you know the implications of the simulation settings you use.

[Guille1811]

So if you determine that, say, a 1M node mesh with 0.1s time step and 1e-4 convergence criteria gives you an estimated 5% error range but a 2 week run time, you could ease that back to, say, 0.5M node mesh, 0.2s time step and 1e-3 convergence criteria and this gives an estimated 20% error range but a 2 day run time.

Ive run a transient simulation of 15 sec with timestep of 0.01 sec and convergence criteria of MAX res < 1E-03 and after like 500 timesteps neither one of those has converged. With 0.1 sec timesteps or higher it definattely wont converge in any timestep :/

[ghorrocks]

Don't use fixed time steps. Use adaptive time stepping, homing in on 3-5 coeff loops per iteration. Then it will find its own time step, and that is one less parameter you need to do a sensitivity analysis for. Make sure the min and max limits are wide enough that you never hit them, and the initial time step size is reasonable (if you don't know what it should be then guess small and let it increase it to the correct value).

[Guille1811]

Thanks for the advise, i did that and the simulation is running right now (:

I came up with a possible strategy on how to approach this and it would be awesome if you gave me your opinion on it:

Well, as i said before, the purpose of my simulation is to determine the protected area due to the machine. My criteria for this is spoting the points (at 1.5 mts high) that dont decrease in temperature after a whole oscilation of the machine (in other words, the points that the increase in temperature due to the machine is greater than the decrease in temperature due to natural convection with the colder ground, after a whole rotation). The points that meet this criteria conform the protected area.

First of all, i need to check if the steady state solution of the jet fan without oscilating is applicable for the transient scenario. To do this, i plan on running a steady state simulation with the jet fan stationary and on cfx post see the temperature of some point (80 mts in front of the jet for example). Then, run a transient simulation (of 1 minute for example) with the jet fan oscilating (at 0.2 rpm) and monitor that same point 80 mts away. If the max temperature reached in that point on the transient run is equal to the one obtained in the steady state solution, then it means that steady state is reached at every angle of rotation of the jet fan. In other words, if this is the case, i can simply run steady state simulations instead of transient ones and extrapolate the rest.

Now, with respect to the latter, my strategy would be as follows:

1. Run the steady simulation
2. Pick the furthest point from the jet fan with temperature rise
3. Register its temperature (lets say 273 K) and the temperature of the points below it
3. Do a hand calculation (or maybe matlab) of the natural convection problem with air at that height at 273 K, temperature below equal to the simulated results and ground temerature of 270 K and evaluate the temperature of the air at that height after 5 minutes.
4. If that temperature is less than the initial temperature in that point (271 K), then that point is unprotected.

With that i can determine the maximum longitudinal reach of the jet fan affect, and since the problem is symetric, the protected area would be a circle of a radius equal to that lenght.


Sorry if it sounds complex, i didnt know how to explain it simpler. Looking forward to hearing your opinion of this and if you find any flaws in my reasoning please let me know.

Greetings!

[ghorrocks]

That sounds reasonable. Good to see you are investigating whether the steady state simulation can be used to extrapolate the full transient results.

Note that some jet flows will look quite different steady state versus transient. This is because the large scale structures are averaged out in the steady state flow but can be directly modelled in transient flows depending on your turbulence model and other factors. This may significantly affect results.