Non-Newtonian turbulence modelling
 

Dear all,

I've been tasked with setting up a simulation to which the details I describe below:

• There are two fluids that come into contact and mix and the goal is to capture this mixing as better as possible
• The whole system is pressurized (at around 24 MPa)
• On one side there’s hot compressed water (temperature around 350 C)
• The other fluid is a biomass slurry close to ambient temperature
• The biomass slurry presents strongly shear-thinning, viscoelastic behavior and to have a significant concentration-dependent yield stress
• The Reynolds number for most flow rate cases is around 1000, but can vary from 300 up to 5000
• The system’s geometry consists of 2 concentric tubes, with the hot water entering through the smaller tube and the slurry through the bigger one
• The tubes are of small dimension (in the order of mm) so I’m unsure about the influence of wall effects on the fluid flow and behavior

I do have a k-epsilon model with custom wall and damping functions to deal with the non-Newtonian behavior of a similar fluid, although I'm unsure if the fluids are similar enough for this approach to be applicable for my case.

With the absence of any results to validate my simulations, I'm thinking about testing the results from the k-epsilon model I have against a k-omega model (it should at least confirm whether the wall functions are applicable).

Can any of the k-omega models implemented in Fluent deal with multiphase flows or should I just use the k-epsilon model I have?

Any suggestions would be greatly appreciated (even a different approach that I haven't considered).

Kind regards,
Dinis

Wall Functions
 

You can use almost all of the RANS based models in Fluent with multiphase, non-Newtonian systems. However, the wall functions are not really applicable. The only solution is to resolve the boundary. uses Enhanced Wall Treatment, which is a two-zone model and is independent, however, to ensure that it does not go in SWF zone, use a fine mesh.

As I understand, the may use wall functions if is high enough. While I have a fine mesh and the values are low enough, which should be fine for the , what would I gain if I'll use the Transition SST or models?

Thank you in advance,
Dinis

Ewt
 

always uses Enhanced Wall Treatment.

Transition models are meant for prediction of the transition to turbulence position. These will not improve the results you expect snce even with the current setup, you will get less than 1 eddy viscosity ratio where flow is more or less laminar.

Thank you for the clarification, but my doubt still persists. I'm not expecting to have laminar flow, I will simulate several cases with varying flow rate, falling into the transition regime. Hence, the transition model.

You're saying that this is not necessary or that actually I will have cases in the laminar regime?

The ultimate goal is geometry optimization and/or flow rate increase of the system I'm simulating so a model that can account for turbulence is necessary.

Kind regards,
Dinis

Transition model vs its existence
 

What I meant is that the transition models are meant for use if the objective is to predict the location of the transition. If that is not the objective, then you should continue with either or .

Thanks a lot, Vinerm!

I do have another question regarding the wall treatment. I've checked this post and from what I understand, the uses a blending functions for the velocity and the k equation but not , correct?

If so, the blending function will still use pre-defined values to achieve this smooth transition between layers. This treatment will still be valid for non-Newtonian multiphase flows?

In the end, high accuracy is not of utmost necessity, but I need to have confidence that my results are realistic (especially because the fluids and condition to model are not at all typical). With this in mind, and if the wall effects are not that significant for the properties mean values, or the model is sufficient for this purpose, then I will go with that approach.

Again, thank you for your help!

Kind regards,
Dinis

Blending Functions
 

Blending functions are used by SST to blend and at the outer boundary layer. This transition is not a fixed value, rather a function of k, as well as mesh resolution and fluid properties. This is applied to both k and but not to velocity. I suppose what you are talking about are enhanced wall treatment. But there as well the blending function is not used for momentum or k. It is used to define eddy viscosity in a manner that makes it compatible with the eddy viscosity in the outer layer

I've come across a video describing how the blending functions work in the SST to which I leave a link for anyone else interested.

I don't quite understand what you mean regarding the enhanced wall treatment though. Just to clarify, there are no wall functions here and the wall treatment is just the application of the model near the wall, correct (which then is blended with the model to be applied far from the wall)?

Yet another question that has popped up when watching the video I linked. I guess checking the value is not really what I should be doing to see if my mesh is adequate for my simulation case but rather the blending function and values?

If so, how can I check these in Fluent?

Not available for selection
 

For models, Fluent does not give an option for the selection of wall treatment, however, EWT is applied by default. In the newer versions of Fluent, default is M-L.

I do not wish to select or modify the wall treatment in any way, but to check the blending function values. As I understand, these also vary with the distance to the closest wall.

Can I plot them in Fluent?

Use expert options
 

Those are available under Turbulence category if you tell Fluent not to free up the temporary memory (use the following command)

sol set exp