[navi]

hello

i have done simulation of water sloshing in rectangular tank, in empty space of water tank there is air,
i have selected for water as dispersed fluid with mean diameter of 0.05 [m] and air as continuous fluid,

i am showing two images one is simulated image and other is experimental,

my question is in both experimental and Ansys simulated videos motion are similar, but in Ansys i am not getting bubble/drops/spray formation as same as experiment (shown in image please seen)
i guess i need to change physics setting of dispersed fluid diameter, or is there anything i need to change, do can i put air as dispersed fluid

help me

thank you

[ghorrocks]

I think you need to do some research on droplet formation. There is plenty of literature on it, and it is important background information what you need to know before you simulate it.

You will need:
1) A surface tension model
2) A finer mesh
3) A very small time step (don't guess this, use adaptive time stepping to home in on 3-5 coeff loops per iteration).
4) Plenty of computer time. It will be a big simulation.
5) Most simulations of this sort of thing use a homogenous free surface model. You don't need to set droplet diameters for this model as it models the formation of the droplets itself.

[navi]

Yeah thanks. I have seen so many papers but i dint get any details about mean diameter for dispersed fluid

If i don't give diameter. Then i should give both as continuous fluid.
And
I am in fine mesh tetrahedral .i know i cant ask mesh detail in cfx form. But this mesh is important for vof modeling
Can i use for this simulation an hexahedral mesh pr tetrahedral mesh. Due to large time of simulation

[ghorrocks]

Then i should give both as continuous fluid.

Correct.

I am in fine mesh tetrahedral

Surface tension is highly sensitive to mesh quality. You will want to use hex meshes with 1:1 aspect ratio if at all possible.

[navi]

Thanks. Ill simulate it

[navi]

hello glenn

I have changed hex mesh with aspect ratio details i have given in attachment,

and I have used surface tension model > in that there is volume fraction smoothening type is there , i searched about that I didn't get THEORY about that,and what to select in that,
similar in solver setting , there is initial volume fraction smoothening is automatically selected (volume weighted) , what is this in surface tension model, now i have put for simulation ill check ill get water droplet or not,
check my setting given right to get droplet

[ghorrocks]

1) Your mesh has some wonky bits in it. You want it to be perfect hexas. Use mapped mesh faces to make sure they are perfect hexas.

2) You have shown a few of the free surface modelling options. Surface tension models are very sensitive to some of these parameters and often you can do better than the defaults. But exactly what option works for you will depend on many factors. So I recommend you try all the options and see which ones work for you. Do a short benchmark simulation to test it and script it up so you can run lots of options quickly. Then you can find for yourself which options work (and don't work) in your case.

[navi]

Originally Posted by ghorrocks

1) You have shown a few of the free surface modelling options. Surface tension models are very sensitive to some of these parameters and often you can do better than the defaults. But exactly what option works for you will depend on many factors. So I recommend you try all the options and see which ones work for you. Do a short benchmark simulation to test it and script it up so you can run lots of options quickly. Then you can find for yourself which options work (and don't work) in your case.

from your experience any suggestion to get droplets by changing free surface model, shown in initial message in this thread,,

[ghorrocks]

My posts #2 and #7 list what you need to look at.

[navi]

hey,

i tried lot to get droplets, but result is still negative,

i want to know that do really cfx Ansys tool , in vof model do we get droplets like experimental type exactly.
i tried everything using continuous fluid for both fluid, with surface tension model,

[ghorrocks]

Have you drawn isosurfaces of volume fraction = 0.5?

Also if you could describe what you have tried that would help. I have already explained several times what you need to get this working but I cannot be more specific until you explain what you have tried - in enough detail that we can comment on it.

[navi]

yeah i tried isosurface, ill take a clip image all what i did in cfx outline tree, with expressions few min

[navi]

i need to get droplets like experimental image, but i am not get droplet when fluid hits wall, other than droplet movement fo fluid is same as experimental

just check my setting in outline tree,
i changed for different simulation the relaxation factor, and volume fraction smoothening type (laplacian and volume-weighted both i tried)

[navi]

other images of cfx pre setting

[urosgrivc]

Hi

I have a question: Is mesh addoption appropriate for cases like this? or is extra computational effort (extra nodes in the mesh and time spent to refine the mesh) not worth the extra resolution.

-Maybe even to obtain the same amount of nodes but higher resolution where is needed (gas-liquid border)

-Mesh adoption could be done where fluid volume fraction has some value (or is between two walues)

-I imagine that it would look and work similar to a cut cell mesh, but would be able to run within cfx for simple geometries like this, as cutcell is not suported.

Well that is the idea anyway
just a thought
It seems an interesting case to me

[navi]

Its interesting only
But
I dont get about mesh adoption.

[ghorrocks]

Surface tension models are extremely sensitive to mesh quality. You get a significant error with elements with an aspect ratio of just 1.2. So in my experience the mesh adaption methods used in CFX cannot keep the mesh quality high enough to remain accurate.

Fluent has a hanging node mesh refinement which keeps mesh quality high. I have used this in fluent and had good results. But to make it dynamically track interfaces is not easy It took me several months of work to get the mesh refinement to dynamically track the interface.

So unless you want to spend several months developing a hanging node dynamic mesh refinement algorithm in Fluent, then just use a 1:1 aspect ratio hex mesh with no mesh refinement.

I have seen no comment that naveen has done sensitivity studies of mesh resolution, time step or convergence. He is wasting his time looking at other things until he has checked these basic parameters.

Also I note you have set a maximum of 4 coeff loops per iteration. That appears unnecessarily restrictive. It should be 10 and you should use adaptive time stepping homing in on 3-5 coeff loops per iteration.

[navi]

actually, i need to learn more about mesh resolution ill do that thanks,
as i am doing in cfx, and i dint try in fluent.

and can you tell me exactly in mesh what to study , because i am new to mesh ansys everything

[navi]

hey
i need to get this job done ASAP, can u tell me just procedure to mesh and physics, and ill see steps and i can learn easily, i have a very short dead line

[ghorrocks]

One key factor is to ensure that the tunable parameters of your model are set correctly. For most models they are the mesh density, converge tolerance and time step size (if transient).

The time step size is the simplest - just use adaptive time stepping homing in on 3-5 coeff loops per iteration and it will automatically find the correct time step. If you manually set the time step you will need to do sensitivity studies on time step size as well.

You will need to do sensitivity studies on mesh density and convergence tolerance. The procedure is:
1) Run your simulation with the current settings
2) If doing mesh sensitivity then remesh with the element edge length halved (so 8 times the element count in 3D).
3) Run your simulation on the new mesh.
4) Compared the simulation results of 1) and 3) using a parameter of interest to you. It could be pressure loss, lift, drag, flow rate... what ever is important to your analysis.
5) If the two simulations give values of the parameter closer than an error tolerance you are happy to live with then you are finished and you have found the mesh density your require.
6) If the two simulations give different results you need to halve the element edge length again and go to step 3 - repeat this process, refining the mesh until you converge within a tolerance you are happy to live with.

For convergence tolerance also do a sensitivity study, but start with your current residuals tolerance, and do 10 times tighter for the next step. Keep refining convergence tolerance by a factor of 10 until it converges.

You should now have found a time step, mesh and convergence tolerance which you have shown to be suitable for your application. You can now proceed knowing that you have done some basic accuracy checks on your simulation.

There are more sophisticated ways of doing this with converge much faster. As mesh refinement gets very expensive very quickly this becomes important for real world cases (for instance: http://journaltool.asme.org/Template...umAccuracy.pdf). But I would not use these techniques until you can manage the simple process I have described.