[Svetlana]

You can simulate 20m/s with fixed particle flow rate if you wish. In this case each particles has less momentum compared with 40m/s, and the flow is different.



There is no "better" or "worse" case between these two different speeds: they are two different cases, and they are both valid.



You need to know your velocity to decide what to model.

[pigei]

Dear Svetlana,
really thank you for your support but if i simulate 20 m/s as for my "real" model, results are not valid... flow goes on a specific direction without any reason (see picture).

If i made the same simulation changing only speed with 40 m/s finally i have what i expect (see picture)...

I'm really surprised and confused....

[pigei]

I made other tests...

Now I leave velocity (and diameter) fixed and varying flow rate...

The behaviour is the contrary compared to velocity.

With high flow rate (50 kg/s) results oscillating. With low flow rate (2 kg/s) i get "good" results...

See picture attached.

I still don't understand why...

[ghorrocks]

Your water appears to be bouncing. I don't think you want that, I would turn the restitution coefficients to zero to stop bouncing.

The instablility you are getting is probably because the droplets are exciting a transient flow in the room. This is likely to be physically correct, and you will probably need a transient model to accurately capture this. This is all discussed in the FAQ I linked to, I hope you read it https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[pigei]

yes ghorrocks, you are right... this is not what i want, i will put to zero restituition coefficient.
In any case frankly speaking actually this is not my problem...
I would better know the relation between velocity and flow rate. Basically they should be independent and related to my physics, but it is not.

I made several simulation now and i estimate that velocity must be about 4-5 times flow rate otherwise i have oscillating and bad results.

I explain it better...with velocity 5 m/s I can have maximum 1 kg/s as flow rate...

With velocity 1 m/s i have to put about 0.1 kg/s as flow rate...and so on...
For example if i put 1 m/s and 1 kg/s i noticed bad results.

In addition also timescale have a influence.... i have increased it to 0.1 from 0.01 and a simulation that results "good" turn now in "bad".

You can see picture attached (first number is velocity - second is flow rate).

[ghorrocks]

Please explain what you are doing in enough detail that we can understand. What velocity? Flow rate of what? What do you mean by "bad results"?

Please attach an image of your geometry and your output file.

[pigei]

Dear Gleen,
surely i can explain better...

I want to simulate the effects of a water barrier in case of a toxic gas release.
This water barrier is generated by some sprinklers. A situation very simular to the picture attached.

In order to better understand and to have confidence on how sprinkler works, I started with a very simple simulation without gas release and a simple geometry.

I started with particle tracking becasue i want to fully understand how lagrangian works and because i think that this will be the best model for my physics.

I put only one sprinkler in the easiest situation: in air (that is the continuos fluid) with no turbulence, isothermal, no inlet air speed.

The geometry is a cube where at the top (a wall) is located the water inlet of the spinkler and so where my particle of water coming from.

At the bottom there is the floor considered a wall. The other 4 lateral faces of the cubes are opening.

You can see the geometry of my water inlet attached in red (cilindrical slice area: diameter is 60mm, lenght is 30mm).

In my previous post velocity was the particle water velocity and flow rate was water particle mass flow rate. As explained before only particle water have speed, air is put to 0.

I expect to have as results of particle tracking something similar to a water fan so this is what i call "good" results. This is not happen if i put for example the condition 20 m/s and 20 kg/s, 0.5mm diameter (see attached in my previous post)... in tjis situation the particle moves to an opening faces and if we go in details on inlet, particles seem to go out with strange angles and not normally to surface.

So I noticed that the shape of the water barrier is dependent of the parameter that i put for velocity, mass flow rate and diameter and this is ok but i guess if there is a relation or something else because if i consider data coming from my physics results are "bad".

I made other tests and so for example if we compare a simulation at 40 m/s and 2 kg/s changing diameter from 0.5 to 0.1 mm i get a fan that is not properly "good" (see attached)...why?

[pigei]

please do not consider the bouncing on the floor that as you have said i can eliminate putting to zero restituition coefficient...

Thank you very much in advance for your support....

[ghorrocks]

First of all I would recommend you look at Eularian particle tracking. This is much easier to use and very good at capturing entrainment effects (which is the key physics you want in the technology you are looking at). So try some Eularian particle models rather than Lagrangian particle tracking.

For "good" results, I am suspicious that those results are not converged adequately. Do a convergence sensitivity check to tell whether they are converged. I bet they are not. If you cannot get convergence look at the FAQ I have linked to already.

You did not attach an output file - please do so.

[Svetlana]

I am confused by "I made several simulation now and i estimate that velocity must be about 4-5 times flow rate otherwise i have oscillating and bad results.".


You can specify either the velocity or the flow rate. But not both simultaneously?

[pigei]

Dear Gleen, yes, my idea is to go with Eulerian approach after I have well investigated Lagrangian model.

I would like to compare them first for the easiest geometry (single sprinkler) and then with complex and real geometry.

I start with Lagrangian because i know that it is more complicated to set up...

Dear Svetlana, yes, you are right, you have to put both. What i want to say is that if i put for example a mass flow rate of about 5 kg/s, velocity must be about 30-40 m/s. If i put flow rate 1 kg/s, velocity must be 5-10 m/s. This allow me to a have a fan shape and RMS not oscillating. So this is the reason why i said that the "number" of velocity must be at least 5 times the "number" of flow rate.
If i put for example 5 kg/s and 5 m/s or (20 and 20) RMS start oscillating too much and results are "bad".

Attached you can find output for 2 simulations:

- velocity 5 and flow rate 1: good results
- velocity 20 and flow rate 20: bad results

diameter is fixed for both simulation: 0.5mm.

Do you see any bad or unusual setting?

PS: I decided to stop the simulation after about 65 iterations...i know that it is too soon, but also after more iterations the situation is more or less the same.

[ghorrocks]

You are using a laminar flow model. Are you sure the flow is not turbulent? A turbulence model will also tend to add dissipation and make convergence easier.

You still have some walls with a restitution coefficient of 1. The water drops will bounce off these which does not appear realistic. They will also make convergence harder, so fixing this will help you obtain convergence.

Have you read the documentation on obtaining convergence? There is a section in the documentation which comments specifically on obtaining convergence for Lagrangian particle tracking models.

Also, you have only run this model for 9 minutes. You can easily run it longer and see if it converges.

There is a whole heap of suggestions I could make but they are all listed in the FAQ I have already linked to twice. I won't link to is again as you have ignored all the other times I mentioned it so it seems pointless to repeat myself yet again.

[pigei]

Dear Gleen, i don't put turbulence assuming that this will help and make easier the simulation.

Wall with restituition coefficent is my "sky", so opposite to particle direction. Ok, I will put it to 0, but i don't think this will have effect.

I haven't ignored FAQ and I've read it... I assume to have done all correctly...but i don't find any specific section on obtaining convergence for Lagrangian.

I run only 9 minutes but i have simulated also longer (24h) with same results...

I tested also Eularian model with no particular problem.

[ghorrocks]

Using a laminar model on a flow which is actually turbulent will make it much harder to converge, and often impossible to converge. So that is a big mistake you need to fix up. If it is a turbulent flow you need a turbulence model.

The key features on the FAQ are - adjust the time step size, double precision, check whether the flow requires a transient simulation. But don't bother doing any of this until you have applied a turbulence model. The turbulence model is critical.

[pigei]

If i put a turbulence model (k-e scalable), simulation failed immediately after 4-5 iterations also with water conditions where i had "good" result with no turbulence...see output for error attached

[pigei]

I reduced timescale (0.001) and simulation run...waiting the results...

[ghorrocks]

If the flow is turbulent then you need a turbulence model. If the turbulence model diverges then you fix it, you don't turn it off and use incorrect physics. Also, it is unusual for a k-e turbulence model to make a simulation less stable than a laminar model. The turbulence model can only add dissipation and this stabilises the flow. So with a little work with the tips in the FAQ I linked to you should be able to get it to work.