VOF mass loss
 

Again one more time as i havent got any repsonse

Hello all,

I am doing VOF simulation with 2ddp. Now using two phase air and water. Taking water as first phase and air as second. With small inlet with 96 m/s air impingement over water surface. Lance to water bath distance is 154 mm with 100 mm depth of water bath and having 100 mm radius of cylinder. Outlet is at top defined as pressure outlet. Now the problem is that when i am doing calculation it's diverging but the results are totally disappointing as the penetration depth of the air jet should have reached 14 mm while it simulation its stuck at 7.5 and further there is a mass loss of around 0.1 Kg out of 3 Kg.
Have used coarser mesh and its showing better result. Now according to the theory the finer mesh should have given better result but here it's 180 degrees. :(

And further i am using URF as
pressure 0.2
momentum 0.3
Tur. dissipation rate 0.8
Tur. viscosity 0.8
Step size 0.0001

Non iterative with Factional Scheme
Volume Fraction = geo reconstruct
Turb. KE = quick

Would be thankful if some would give suggestions.

Regards,
Smaras

http://imageshack.us/a/img23/6368/kepfinal.th.jpg

http://imageshack.us/a/img23/6368/kepfinal.th.jpg

You should not look at results before you fix the numerics.
Get a converging simulation!

Thanks Rodriguez but i have a converging solution that's the problem. And the numerical calculation and also some research paper i am consulting also giving the same depth of penetration which is not confirmed with fluent.

Therefore i am doing some mistake. I need help in this regard.

Regards,
Smaras

Do you say that in your originial post you meant "converging" instead of "diverging"?

Mistake,

I meant to say diverging from the numerical result and the results from the research paper

Thanks for correction.

Regards

Alright, now I get you.

Can you post some pics of your setup and mesh? And also the residuals...
What I don't understand: How can your simulation converge, when you have a mass loss?

That i cannot understand as well.

Mass-Loss:

http://imageshack.us/a/img441/5479/kepsmass0t.th.jpg

http://imageshack.us/a/img40/9773/kepsmasst.th.jpg


Mesh:

http://imageshack.us/a/img233/3048/kepsmesh0t.th.jpg

http://imageshack.us/a/img832/5681/kepsmesht.th.jpg

Penetration Depth:

http://imageshack.us/a/img402/547/ke...ondepth.th.jpg

Residuals:

http://imageshack.us/a/img502/961/kepsresiduals.th.jpg

Phases:

http://imageshack.us/a/img22/7638/kepsphaset.th.jpg


If anything else is left please i can post that as well. Vielen Dank Rodriguez

Regards,

Smaras

Just to be sure, I am getting your setup right:

1) The box you are simulating is a cylinder, the axis is on the left of your pictures?
2) On the bottom you got the water and a needle blasts air vertically on your water surface?
3) The needle is on the top left of your domain, where I can see the little gap in the green grid?
4) "Penetration depth" is the (average) difference of the height of the water surface at your symmetry axis, compared to the steady state without the needle fan?
5) Air from the needle escapes through the pressure outlet at the top?
6) On the right and on the bottom are walls?

http://imageshack.us/a/img90/8106/unbenanntgj.th.png

I hope this image will clear the queries. While for the 4th
Penetration depth is the depth difference between the stable condition and the impingement of air onto water surface. the distance calculated is from the top i.e. Outlet.

And all dimension are in mm.

Regards.

Correct me if I am wrong, but as I understand it, the needle (lower left in your last picture) shouldn't be an axis, but a wall boundary. There can be just one cylinder axis.

Ohh it was by mistake typing error. The top left is nozzle wall. While the lower left having length 254 is axis.

Ok, is your simulation time dependent? The residuals screenshot looks a bit strange... it looks like your first 2000 iterations have a residual in continuity equation of about 1.0

Yup it is time dependent since i am using Fractional Scheme with NITA.

But look at your residuals. Something ugly happens during the first 2000 iterations.

You can also do this: Under "Monitors" add a surface monitor and integrate the water density over your domain. Plot it each timestep to a window. I guess when your residuals start to converge (after about 2000 iterations), your integrals won't change any more over time, thus the total mass will be conserved.

Rodriguez i decrease the time step size to 1e-3 from 1e-5.

You could also try to keep the current stepsize and get convergence here! Maybe increase the number of iterations of each time step or change the solution algorithm.

By currewnt step size you mean 1e-3 or 1e-5

I mean the old one (1e-3). I guess in your post above you meant "i decrease the time step size from 1e-3 to 1e-5" and not vice versa...

other way i.e. from 1e-5 to 1e-3 that why its such a drastic change

I am confused... you can not decrease to 1e-3 from 1e-5. This is an increase.

ok that's increase and yes that what i did i.e. increase from 1e-5 and change the time step to 1e-3.

Now if i am using directly 1e-3 from the start. The courant no. is increasing surpassing 250. So what to do now?

Alright! Now, in your residual picture it looks like the first 2000 iterations did not converge at all, is that right? How many iterations per timestep did you set as maximum, 25? That means that the first 80 time steps did not converge? Maybe the loss of mass happens right there. Every single timestep of your simulation should converge in a satisfactory manner, otherwise you can not expect mass conservation.

I would try to increase the maximum number of iterations and see if you get convergece for the first timesteps.

Did it work out Smaras?

Well thanks Rodriguez,

i tried to refine the mesh (adopt) in the regions of inlet and the interaction of two phases and used 10 iterations per step. Using 1e-5 as step size and 10000 steps. Got convergence after 3000 iterations i.e. 300 ts. And then onward every step got convergence.

I don't know why there is mass loss, may be because of viscous heating even though i have not selected that option or either it was something else. But in this run i have got relatively less mass loss and was getting almost similar penetration as in the research papers.

now i want to use K-w SST model what would you suggest???

Hold on. You really need convergence every single timestep. Otherwise you can not take things such as mass conservation into account: What, if during your first 100 non-converged time steps something unphysical happens? Your equations are not converged and it can easily happen, that you lose some mass or whatever. You need to do as many iterations as it takes to get a converged solution right from the start, for time step number one, number two...

Ok got it....ill try to make more iteration i.e. 20 now an see

Yup getting convergence in K-eps with 20 iteration per step and step size being 1e-6 and for k-w with 25 iteration per step and step size being 1e-5. From the start.

Now running both simulations and will take around a day or so to complete. Then see what is the penetration. And hope now there would be no mass loss.

Thanks once again Rodriguez fro help.

Regards,
Smaras

Thanks Rodriguez,

For the help, the problem lies in the pressure residual monitor. Even though it wasn't not changing too much but it wasn't giving converging.....i have also change it to 0.01 and now getting converging at every iteration. Further no mass loss and the penetration is also kept the step size 1e-5 and iteration per step 20. Getting converge solution. Better results in both models.

Thanks for the help, learnt a lot. :)

Regards,
Smaras

Just one more comment:
By "change it to 0.01" i guess you mean that you increased the residual convergence criterion to 0.01 ?
You should better try to increase the max. number of iterations (and lower the residual) than relaxing the threshold of "good" and "bad" convergence.

Ok doki...am working on it.

Thanks for the help Rodriguez. Had increase the number of iteration and getting the desired result i mean the result approximately matching the research results.

now working on 3D. Need some help, do you have some idea where to find good resource on meshing techniques in ICEM. And mesh refinement for 3D.

Regards.

Watch the youtube tutorial by Simon (PSYMN in this forum). Search for "ICEM CFD Hexa 2D Airfoil meshing" in youtube. It has three parts and is really helpful, although it's just 2d.

Mesh refinement can be done pretty easy in ICEM since you can increase the number of gridpoints on edges quickly.