mass not balance in multiphase simulation
 

I'm setting a fluidized bed simulation, which has two phases: gas and solid. Eulerian model is used. Geometry is a 2D rectangle with around 5500 square-shaped cells. Gas comes in from the bottom velocity inlet and goes out from the top pressure outlet. Solid is initially patched within part of the bottom area with volume fraction of 0.55.

The problem is that, the total mass of solid phase keeps dropping, with the solid mass flow rates of all the boundaries to be 0. Since I use constant density, the total volume of solid phase is dropping in the same way, while volume of gas phase is increasing.

I'm checking for the total mass of solid phase because I had a chemical reaction in the case, and change of total mass may indicate the progress of reaction. Then the problem happened, and I reduced the case to be without chemical reaction to still find the problem.

Now I have no clue where could those masses go? Or is this just a normal situation?

solved
 

Still don't know what is wrong.
Good thing is, after I use syamlal-obrien in stead of gidaspow for the drag law, all things turned normal. That's actually a UDF from Fluent tutarial 6.3, which is a modified version of syamlal-obrien.

Hi,

I actually have a similar problem for stirred tank (gas/liquid) - the mass of liquid is not conserved, even though there are no sources for liquid in the domain, and drainage at the top through the pressure outlet does not explain the imbalance (for one, liquid mass is often growing and the outlet-backflow is gas only)

Did you find any reason so far?

Hi, CeesH

I still don't know what specific reason caused this. But I would guess it's some computing issues rather than model setup problem. Once I tried mixture model rather than Eulerian model for the multiphase, then problem solved. But mixture model is only for extremely low fraction of solid.
The new thing is, after I refine my mesh to 4 times the original cell number, without decreasing time step, that imbalance mass occurs again. So I would suggest you to set a smaller number for you time step, or coarsen your mesh. Even try mixture model maybe, if you are using Eulerian.

Hi guys,

I am also facing the same problem, my case is a static bed placed at the bottom of an annuls, water is coming into the domain from inlet and my goal is to see if the bed begin to erode at a given water flow rate,
the weird thing is that I tried Eulerian-Eulerian model and monitored the total mass of the secondary phase, it keeps dropping continually, I conducted a test with DDPM model I still see the total mass of the secondary phase dropping but when I check the fate of particles they all are still in the domain, how is that possible?

anyways I am going to try your suggestion of changing drag law to see if it helps,

Thanks

Has any one found solution to this mysteriously disappearing mass?

In general in Euler-Euler you need to find a suitable time step size for a given mesh size and make sure the calculation converges in each time step. Also higher order discretization shemes should be used. Once these factors can be ruled out and mass imbalance still persists, deeper investigation into the problem is needed.

Thanks for the advise.

I am trying a simple case where initially particles are suspended in the air and they are allowed to settle down with time. I am interested in packing pattern once everything is settled down.

I suppose the issue in my simulations arose from the fixed flowfield approach during mixing. What we did is first solve the flowfield (residuals ~E-4) in steady state, after which mixing was conducted with the transient solver. since no flow periodicities were expecte, the flowfield was frozen (i.e. not solved every timestep), and only the scalar transport equation was solved each step.

Although the residuals were decently low, the equations are of course not exactly satisfied, and by freezing the equations there may be a consistent net. imbalance in momentum locally. Since this is frozen, it consistently exists every timestep, and may act as a "source" of tracer material via the convective terms in the scalar transport equation. Indeed, unfreezing the equations and conducting a fully transient simultation solves the issues - but at a huge time penalty.

Thanks Cees Haringa for sharing your experience.

The case we were trying seems to be working alright now. The continuity residual is still high (around 0.1 with smallest time-step I can afford), but the good thing is that the mass is not disappearing as in earlier cases. The higher continuity is perhaps due to open surface boundary condition where air is allowed to move in-n-out freely or due to coarse mesh.

Anyways, its moving in a positive direction.

Also, when we consulted Ansys about it, they recommended us to switch to DDPM. But since tracking 20 millions of particles could make simulation very long, we are sticking to Eulerian for now.

Hehe, did they make a quote for a new supercomputer as well to run those ddpm simulations ;)

Hi vasava

I'm facing the same problem the mass is continuously decreasing, can you please explain how you are able to solve the problem using Eulerian model

Thank