[kgschuch]

Hello all. I am trying to model a process in which a viscous fluid is injected into a stream of high-velocity air jet wherein it should be accelerated.

I have formulated a Fluent model as follows

Multiphase with K-e turbulence
-3 phases: air (to fill my domain), a low velocity viscous fluid (secondary phase), and a high velocity air jet (Secondary phase). The secondary phases are immiscible, suggesting a multiphase VOF model.
-VOF model with standard options

I have specified my boundary conditions, initialized, and patched the fluid volumes to the domain (and verified them prior to solving).

I initially solve a steady-state case with only high-velocity air to generate its flow fields, then initiate a transient case wherein I specific the velocity of the viscous fluid flow, and calculate that solution.

I'm solving with the SIMPLE algorithm and standard options there.

The high-velocity air jet behavior (VOF & velocity decay), once computed in steady-state, is as expected. Once I initiate the viscous fluid flow, the high-velocity air jet behavior computed by the transient case also is as expected (both VOF and velocity).

Once the viscous fluid flow is initiated though, its VOF behavior is as expected, but its velocity remains the same as it travels through space (fundamentally, through drag and frictional forces it should be accelerated by the high-velocity air) throughout space and time. Does anybody have any suggestions?

[vinerm]

Is your viscous fluid a liquid? If yes, then VOF is alright but why the third phase. Primary phase and the third phase are same, air. Even if one is air and other is, say, pure oxygen or argon or some other gas, it should not be treated as another phase. Could you share more details of the multiphase model you are using and the expected morphology, i.e., do you expect high viscosity fluid to behave like a separate layer of fluid with a clearly defined free-surface or do you expect it to be broken into droplets, assuming it is liquid?

[kgschuch]

Originally Posted by vinerm

Is your viscous fluid a liquid? If yes, then VOF is alright but why the third phase. Primary phase and the third phase are same, air. Even if one is air and other is, say, pure oxygen or argon or some other gas, it should not be treated as another phase. Could you share more details of the multiphase model you are using and the expected morphology, i.e., do you expect high viscosity fluid to behave like a separate layer of fluid with a clearly defined free-surface or do you expect it to be broken into droplets, assuming it is liquid?

Hey there. Thanks for the response! Yes, I expect the viscous liquid to behave as a free surface (free liquid jet) under these conditions and have observed such experimentally.

I was under the impression I needed 3 Eulerian phases in the model: two secondary phases to which I assign velocity inlet conditions: one for the high-velocity jet (inlet), one for the low-velocity fluid (inlet), and one primary phase for the stagnant air existing in my domain.

For the setup I use 2D DP, pressure-based, transient time, absolute velocity formulation, with 2D planar space, and gravity -9.8 in the appropriate direction.

For model I choose multiphase, VOF, 3 phases (as described above), I've tried with/without Level Set on, explicit velocity formulation, volume cutoff 1e-6, courant number 0.25, implicit body force on, sharp/dispersed interface.

For phases: ambient air in the domain is primary, with the two jet moving phases as secondary (as described above).

For phase interactions I do not have surface tension modeling on.

I have viscous flow set to either Laminar or K-e with standard options there.

Anything I'm missing? I'm still new to CFD so apologies if this is amateur.

[vinerm]

Set up only two phases; one air and other liquid. High or low velocity at the inlets do not make those fluids as separate phases. If the domain is not large, surface tension would certainly be required but do not enable this in the beginning. Do not enable Level Set Method. Use explicit formulation but do ensure that the time-step is small. If you expect a stable free-surface, then you can use steady-state solver as well. This will only work with Implicit VOF and not explicit.

[kgschuch]

Originally Posted by vinerm

Set up only two phases; one air and other liquid. High or low velocity at the inlets do not make those fluids as separate phases. If the domain is not large, surface tension would certainly be required but do not enable this in the beginning. Do not enable Level Set Method. Use explicit formulation but do ensure that the time-step is small. If you expect a stable free-surface, then you can use steady-state solver as well. This will only work with Implicit VOF and not explicit.

Hey thank you so much for the reply. I've implemented that model, it definitely makes sense to only use two phases.

However, I'm still not seeing the viscous fluid deform or change velocity, making me think that there is some interaction that's not being captured? I've tried reducing the fluid viscosity significantly and increasing the velocity of accelerating air, but no changes. Time step size is 1e-5.

[vinerm]

VOF automatically takes care of the momentum interactions across phases since the interface is resolved. If you are not observing a lot of interaction, then try including the surface tension model.

[kgschuch]

Originally Posted by vinerm

VOF automatically takes care of the momentum interactions across phases since the interface is resolved. If you are not observing a lot of interaction, then try including the surface tension model.

Hey thanks so much. That definitely seems to have helped. Are you aware of any general ranges of surface tension coefficients between air and different materials?

[vinerm]

Refer

http://www.surface-tension.de/