free surface problem with capillary effect
 

hi, everbody. I need some help from you with my simulation in CFX. I am trying to solve a free surface problem with capillary effect. It's part of a brazing process. The model is in the attach. The three wall boundaries are the boundarie of two parts to be joined. There ist a gap between the two parts. The two fluids in the domain are molten copper and argon. The molten copper has a intial sharpe of a triangle and is placed directly outside the gap. I want to see how the molten copper flows in the gap and if the intire gap can be filled (there are also other models with different size of gaps).
Here are my settings in CFX:
I used adaptive time steps with both initial time step and minimum time step of 1e-6 s.
The buoyancy model is actived with the ref. density of the argon (which i caculated with the equition: (p*M)/(R*T)).
Free surface model : standard
interface compression : 2.
Heat transfer: isothermal
fluid temperature: 1357.77 K (melting point of copper).
surface tension model: continuum surface force
primary fluid: copper
volume fraction smoothing type:none.
interface transfer: free surface
mass transfer: none
The hydrostatical pressure caused by the molten copper war included.
Adhesiv is actived for every wall boundarie with a contact angle of 5 degree.
A relative pressure of 0 Pa was setted for all opening boundaries. At openings is the volume fraction of copper 0 and is 1 for argon.
The Coeff. loops is setted to be 3 to 5.
There are two reference pressures (the pressure in the brazing oven), 1 bar and 40 mbar respectively (which affects also the density of argon).
When i simulated it with 1 bar, the RMS went down after few time steps until under the 1e-5 (i have setted the residual target as 1e-5). The solver beginned then to increase the time step. I have runned the simulation for a total time of 30 ms. The result seemed to be good.
But when i simulated it with 40 mbar (the argon density reduced also), the RMS went under the 1e-5 limit after more time steps and the solver has never increased the time step. After some hundred time steps a peak of RMS appeared. I stopped the simulation and had a look at the result, there are some weird change of the sharpe of the molten copper.
When i once changed the reference pressure from 1 bar to 40 mbar, i forgot to change the density to the density at 40 mbar. The simulation then has a similar RMS trend with the one with 1 bar and density at 1 bar.
It seems, that the lower pressure and density (more likely is the density) have caused some problems with the simulation. Can someone help me with this problem? What can i do to solve this problem?
Attachment 23188

My comments:
* Do not set a minimum time step size. Make it 1e-20 so it never gets reached. It is needs small time steps let it.
* Are you sure buoyancy is significant?
* What do you mean by "The hydrostatical pressure caused by the molten copper war included."
* When you run with argon at 40mbar that makes the density difference across the interface enormous. This will lead to convergence difficulties. Try using double precision numerics, but you might have to limit the minimum Ar pressure. How does Ar pressure affect this anyway?

hi, Glenn Horrocks, thank you for your reply! As i was setting up my simulation, i have learned a lot from your posts in the forum, i want to thank you for that too.
to the comments:
*i will try with this minimum time step size. Should i also set the initial time step size to 1e-20 s?
*the buoyancy shoul have small or no effect for the flow into the gap, but i think, it will effect the change of the fluid (molten copper) sharpe outside the gap.
*"war" is an "was", sorry for the error. I gave an expression for the relative pressure in the domain initialization: VFcopper*(5[mm]-x-y)*7997[kg m^-3]*g. VFcopper is the initial volume fraction of molten copper. 5 mm is the height of the triangle.
*How can i set a double precision numerics in CFX? Actually the argon pressure should have nothing to do with the flow behavior. The pressure of the oven is setted to be 40 mbar during the brazing process, that's why i setted this referenze pressure for the simulation.

i have found the double precision option in solver manager, i will try it.

No, start with a time step size of your best guess of what it needs. If the adaptive algorithm shows that you were way off then start again using the time step the algorithm suggests.

Only include buoyant effects if buoyant effects are important. It complicates the analysis so if you do not need it then remove it.

If Ar pressure makes no difference then just use any Ar pressure which works. As I said, free surface modelling is tricky because of the big density change across the interface, and running with low Ar pressure makes this situation worse.

I have tried the double precision, the same problem occoured. I will use 1 bar for further simulations.
Where can i find the theoretical explanation to this problem with the big density change across the interface? Is there something about that in the user's guide of CFX?

I have no idea about a reference - but it is obvious if you understand the numerics. Air (at atmospheric pressure) and water have about a 1:1000 density difference. There is also likely to be viscosity and pressure variations also of this order. This is going to be hard work for a numerical scheme. If you lower the air pressure you make this difference even bigger, so it gets worse.

the RMS trend now goes well with the 1 bar pressure. The imbalance stay most of the time under 2%. I setted the timestep update freq. to 1. The solver increases the timestep size continuously every several time steps. At this time the imbalance went up to over 10%. When the solver decreased the timestep size, it went down to under 2 or 1%. Will this effects a lot over the accuracy of the result? Should i change the timestep update freq. to a biger value, like 5 or 10?

No, let the solver find its own point with as much resolution as it needs. If the imbalances concern you (you should do a sensitivity analysis to find out) then add imbalances as a convergence critereon then it will always converge to the imbalance you request.

hello, Mr. Horrocks. How can i find out what is the timestep the algorithm suggets? For example, when i started a simulation with the timestep 1e-6s, the programm decreases the timestep until the RMS reachs the convergence criteria. It turns out that the timestep is now 1e-8s. Now should i start the simulation again with the timestep 1e-8s?

If you want to capture the flow at the very start of the simulation accurately then yes, rerun using the 1e-8s time step size. If you do not care about the first millisecond then don't bother, but if you do you want to have it properly converged right from the start.

I have read from another post of you, that the coef. loop should be setted to be from 3 to 6. Does this mean that the target min./max. coeff. loops in analysis type, or do you mean here the min./max. coeff. loops in solver control?
Now i beginn to deal with the simulation with 0.5 mm gap. I started with 1e-7s timestep. It was decreased to 1.6e-8s. Then the programm started to increase it. It can reach a timestep of 1e-5s, but every several a peak appears. The RMS went to 3e-5 - 1e-4 (i have setted the residual target as 1e-5) at the beginning of the peak, then it went down to under 1e-5 again in 3 to 5 timesteps. Based on the experience of ealier simulations, in which i setted a min. timestep of 1e-6s, these periodical peaks lead to a much greater increase of the RMS (more than 1e-2) at a timestep later. And there is a big and weird sharpe change of the copper at this time point.
I am wondering why there are these peaks. I think it might beacuse i have set the target min. coeff. loops in analysis type to 4 and the min. coeff. loops in solver control to 3. This causes the programm to increase the timestep more easily. Will it help, if i set the target min. coeff. loops in analysis type to 3 and the min. coeff. loops in solver control to 2? I think that will force the programm to increase the timestep only when the RMS can be less than 1e-5 within 2 coeff. loops, it might stop the programm increasing the timestep to a too great value.

3 to 5 target coeff loops. Put the maximum at somethign like 10 and no minimum.

I have tried again. This time i set no minimum to the timestep. The first Bild in attach is the RMS. It started to have peaks from about 7000. timestep. Before i stopped the simulation there are three greater peaks.
The second picture shows the sharp of molten copper at 1 ms. There are some weird wave on the longest side of the triangle. The third pichture shows the sharpe of the copper at 29.8 ms. As the simulatin further running, the copper flowed into the gap and has a sharpe simmilary to that in the third picture, only the flow length is shorter. But the copper turned into the sharpe in the last picture at 29.9 ms (i saved the result every 0.1 ms). This big change of the copper in the gap within 0.1 ms seems to be unrealistic. What's might be wrong in the simulation?
Attachment 23630 Attachment 23629 Attachment 23631 Attachment 23632

Yes, you are having stability problems with your free surface model.

When I last did free surface models with surface tension I was greatly assisted by having a little time to do some preliminary work. I chose some benchmark simulations: spherical drop on a plate with a wall contact angle and capilliary driven flow up a thin tube and looked at the effects of the main convergence parameters (convergence tolerance, time step size) and the options specific to free surface modelling (free surface smoothing, coupled versus segregated VF solver and many others) and found a solver setting which was faster and more accurate than the default settings.

I recommend you do the same. I remember seeing this sort of wobbliness, and I remember I found the fix for it. But I cannot remember what the fix is. (Sorry, you will have to find it yourself!)

Thank you for your suggestions. I'm examining now the relevant settings. I have some questions about the effect of some options.
1)The initial volume fraction smoothing in the multiphase control. What does the word "initial" here means? For example, if i set the initial volume fraction smoothing to volume-weighted and the volume fraction smoothing type in the fluid pair models to none, then when does the programm use the volume-weighted volume fraction smoothing and when for none?
2)What is the curvature under relaxation factor in fluid pair models?

1) I am not completely sure on this but I think the initial smoothing is for the VF equations, and the fluid pair one is for the surface tension model.
2) This is under-relaxation of the surface motion for surface tension modelling.

I have runned the simulations only with 1 CPU, because there will be "overflow" error at sometime during the simulations, when i run it with parallel model. I have read from somewhere, that it would be problematical, if any portion of a partition boundary is aligned with the free surface. Is there a solution, so that the parallel caculation can be used?

If serial works and parallel does not it is usually because a partition boundary lines up with the interface. I would move to a different partitioning algorith,

Hi, Mr. Horrocks. I'm doing some setting research as you suggested. Meanwhile i reexamined the old results. I've found a weird thing. As you can see in the pictures in attach, the contur shows the volume fraction of copper. I also setted a isosurface with a volume fraction of copper of 0.99 to caputure the free surface. The black line is the intersection of the isosurface and one of the symmertry plane.

Most of the time there are some dictance between the black line and the boundary of the red part of the volume fraction contur, as in picture1. Sometimes the black line has a weird sharpe as in picture2. When i decrease the volume fraction value for the isosurface to 0.95, the black line will then be near the boundary of the red part.

Have you seen this problem before? Do you know what cause it?
Attachment 23836 Attachment 23837