Simcenter FLOEFD Simcenter FLOEFD : How to set up a simulation with water and propane (or any other fluids) defined at the same inlet BC

The simplest case is when both fluids are either “water” and “propane” gases or liquids. To analyze fluid mixtures, the fluids must be of the same type: either gases or liquids. In the General Settings > Fluids dialog box, specify the default fluids and the default fluid type to be assigned for all fluid regions.

Afterward, we can set their concentrations both for initial conditions and flow boundary conditions.

If “water” is a liquid and “propane” is a gas, they can be simulated as two immiscible fluids with a free surface.

To specify immiscible fluids, first enable the Free Surface option in the General Settings > Analysis Type dialog box.

Then, in the General Settings > Fluids dialog box, specify both fluids; they will be treated as an Immiscible Mixture.

You can then set the initial fluid distribution as either a constant or a tabular dependency on height, both for initial conditions and flow boundary conditions.

There is also a Real Gas approach, which allows for the simulation of phase transitions between liquid and gaseous phases.

However, this method is primarily intended for simulating gases rather than liquids.

Its applicability depends on the specific conditions of the simulation, but it is unlikely to be appropriate for this case.

In case the gas “propane” are bubbles dissolved in “water”, example : 

Propane is 10% of the water flow, than the situation is a bit more tricky.

The shredding of large bubbles and the coalescence of small bubbles have just not been implemented. There are two implemented approaches to simulates particles (if we consider bubbles as particles):

1. Particle Study (for Post-Processing only). The Lagrangian approach allows to calculate two-phase flows as a motion of particles in a steady-state flow field where the influence of the particles on the fluid flow (including its temperature) is negligible.

Also it's assumed that a size of each particle is constant during the simulation.

2. Particle Collection (for the Pre-Processor Simulation). The Euler-Lagrange approach allows to calculate two-phase fluid-particles flows by taking into account the influence of the discrete second phase (particles) on the first continuous phase (fluid flow=gas flow).

So both approaches have their own limitations which are not acceptable to simulate the shredding of large bubbles and the coalescence of small bubbles properly.

In the case mentioned a viable option is to use the Particle Study by specifying multiple sets of particles based on bubble size, while neglecting both the particles' influence on the fluid flow and any changes in particle size during the simulation.

So basically we simulate a base run with “water” only and then we enable a particle study introducing “propane” particles and check their behavior/distribution over the main flow and system.

As it can be seen above, for the generation of the study, we will need to choose the liquid or solid for the particles. Since gas is not allowed, just simply create a custom liquid or a solid material with the properties of the “propane” gas. Then choose it.

After this is set it up, we can just run it.

Reminder: there is no qualitative percentage feature available, since it is a post-processing tool and there is no density difference in the system.

However, you can use “surface parameters” in results to check how many particles are going through the faces (number of particles). And from here we can extrapolate percentage information based on the number of particles injected.

Of course, the inlet number should be same of the sum at the outlets (kind of mass conservation).
If there is a discrepancy, this is highly likely because of the mesh. Increase the cells count at the faces used to monitor the particles collection (avoiding vortex) and wait for full convergence of the simulation.
It is also suggested to let the calculation run for at least couple of Travels.

The term "travel" is an internal calculation terminology and from a user-standpoint can be imagined as the point of time when beginning from the defined inlet(s) a fluid particle passes the outlet(s) for the first time.