[ZiadElSayed]

Hello everyone,

I am trying to model an infiltration casting process of aluminium through a packed bed of salt particles.

Right now I am using Eulerian-granular multiphase model, the model geometry is as follows:

- Cylindrical mould
-Proportion of the mould is filled with salt packed at a certain limit
- Aluminium is being pushed through the packed bed at given pressure

Currently I am able to simulate the model using velocity-inlet by defining the velocity of the aluminium phase and using pressure outlet on the same side of the inlet (top of the mould).

In reality, its slightly different, I have a specific volume of Aluminium initially stationed on top of the salt particles, then gas pressure is used to push the aluminium inside the packed bed.

Right now I am not including any energy calculations till I get hold of the flow of Aluminium. Only then will I include the energy equation and heat transfer properties.

Can anyone give me tips on how to make this model? And what are the data needed to calibrate the used models.

P.S. I am new to CFD, fluid and thermodynamics.

Thanks in advance.

[vinerm]

Inclusion of gas may not show much difference in the results, however, it depends on the objective of the study. If the objective is to study the flow of the aluminum, then you don't need to include the pressurized gas since it will add another set of momentum equations as well as would require thermal energy because gas would be at high pressure.

[ZiadElSayed]

Well, the objective is to determine the infiltration time of the aluminium and how it changes with changing the particle diameter and the packing density of the packed bed.

Is there any other way to model the flow of Aluminium under a specified amount of pressure? I tried changing the velocity-inlet to pressure inlet but that makes all three phases have velocity in -Y direction. Even when I initialise the velocity of Air phase and solid particles phase at 0 velocity, I still get error "floating point exception".

Any idea what might be the problem here?

[vinerm]

Pressure field is shared across all the phases, however, velocity field is specific for each phase. So, when you apply velocity inlet, it is applied only to the phase for which you provide a non-zero velocity, such as, aluminum in your case. However, when you apply pressure inlet, it acts on all phases. Since aluminum can be considered incompressible under the given scenario, you can use velocity inlet and then look at the pressure predicted by Fluent for the inlet. This should give you values matching with those you want to apply as pressure inlet.

[ZiadElSayed]

Okay then I'll try that.

Regarding the process, after the pressure is applied I am supposed to model solidification of the aluminium+packed bed composite, in that case, I should stop the flow of the aluminium at the inlet the initiate energy equation? when I stop the flow of aluminium at the inlet, air seems to be entering the system from the outlets, so I set the back flow volume fraction of aluminium at the outlet=1, I seem to get some disturbances in the system at the beginning, then it settles down. I am not sure if what I am doing is physically correct or is there another way to do it??

Sorry if I am asking many questions, and thank you very much.

[vinerm]

If you want to stop an inflow-outflow, convert all openings to walls.

[ZiadElSayed]

Originally Posted by vinerm

If you want to stop an inflow-outflow, convert all openings to walls.

I tried doing that before, but when I turn the inlet and outlets into walls, I get error "floating point exception" and the system seems to be heavily disturbed. Residuals of continuity and pressure rise up to 10^5 which I don't understand.

Also, I read in the manual that solidification/melting isn't possible when using Eulerian multiphase model, I need to use Eulerian model to simulate packed bed and then simulate solidification of the aluminium+particles composite, is there any other way to do that and include the solidification model?

[vinerm]

If the velocity field is not almost 0 and pressure field is not homogeneous, conversion to walls will cause issue. You can convert to walls only if the flow has almost subsided. If the solidification takes place while the aluminum is still flowing, then do not convert openings to walls. However, if the solidification starts when the flow has almost stopped, then there is no need to solve for flow. You can just initialize with filled aluminum.

Solidification & Melting is unavailable with Euler-Euler, however, if really have to use Euler-Euler, then you can write your own UDF for solidification. Otherwise, as mentioned above, if solidification starts after the flow has subsided, then you don't need Euler-Euler.

[ZiadElSayed]

Well there the fact that I am simulating the pressure in terms of velocity flow is actually far away from what happens but it seems the only way since using pressure is inconvenient, the solidification should start after full infiltration takes place, in practice, the whole medium has the same temperature, then after infiltration everything is left to cool off together. So I guess after the flow stops. If I begin the model with presence of Aluminium, how do I model the particles within the Aluminium matrix without using E-granular model? Is it possible?

I think in that case I can divide my model into two models, one for the flow(infiltration) of the particles and another one for the solidification.

[vinerm]

What is the objective here? Since, once the flow has stopped, it is only about thermal diffusion and nothing else.

[ZiadElSayed]

The objective of the 2nd stage is to model the solidification of particle composite.

[vinerm]

I understand that solidification is the objective, however, it needs to be clarified elaborated further. Are you interested in knowing the time required for solidification or does it have segregation during solidification and you want to predict that or do you want to predict any contraction or expansion during solidification. In other words, solidification is composed of multiple phenomena and the simulation has to be set as per the objective.

[ZiadElSayed]

Well I don’t believe there should be any segregation, any segregation would result from the flow during infiltration, I believe I am more interested in the solidification time and conraction.

[ZiadElSayed]

Originally Posted by vinerm

I understand that solidification is the objective, however, it needs to be clarified elaborated further. Are you interested in knowing the time required for solidification or does it have segregation during solidification and you want to predict that or do you want to predict any contraction or expansion during solidification. In other words, solidification is composed of multiple phenomena and the simulation has to be set as per the objective.

I am sorry but have you been able to figure out something for my case? As I stated, I am looking for solidification time and contraction of the entire composite if its possible.