[SerSe]

Hello guys,

I am trying to model the flow inside a medical needle used to make blood plasma react with different reagents. The fluid is made up of liquid parts separated by air gaps. The problem is not stationary as the liquid parts/air gaps move during the supply phase.
How can I model this?
Should I use the discrete phase model or the multi-phase model?
And should I turn the dynamic mesh on, since the air gaps could either shrink or enlarge during supply?

Many thanks in advance.

SerSe

[mighelone]

It depends mainly on the amount of secondary phase on your flow.
DPM is good only for diluited flow (VOF is lower than 5-10%), otherwise Eulerian approach is better.

However Eulerian approach is able to evaluate very dliuited flow and high dense flow, but it is more complex from the numerical point of view.

Regards

Michele

[CFDtoy]

The problem mentioned here is a good VOF application (air / water interface clearly defined) with moving boundary. Use remeshing solution and make the boundary wall move. You should be able to see the frontal movement.

However, I am afraid that once the air bubbles start to penetrate the liquid, the mixing cannot be captured using VOF (since extremely fine meshes are required to do this)...so, in essence VOF produces smeared interfaces leading to results similar to Eulerian multiphase 2 fluid model.

So, the question is: if you want to see mixing effects - do eulerian multiphase model (multi fluid model) and if you are just interested in the air/water interfacial effects - VOF.

/CFDtoy

[SerSe]

Hi guys,

as I understood from Michele's help and from Fluent Users' Guide, I should not use the Discrete Phase Model since it treats the presence of small spherical solid particles - liquid droplets - gas bubbles within the main flow. That's not my case, since I have an inner flow bounded by adiabatic walls in which the air regions (which take up a considerable volume fraction) separate the liquid regions.

I would opt for using the VOF multiphase model in Fluent. Do you agree, guys?

Actually one more question arises... Does the VOF model take into account the gas region change in shape (e.g., shrinking of the air region or changing in shape of the interface air-liquid)? or should I introduce the dynamic mesh modelling to represent the behaviour of these air gaps?

Thank you in advance,

SerSe

[CFDtoy]

Definitely Discrete phase model approach is not the right one. They are intended more for spray applications or for purely tracking particles in air like dust particles, cyclone separators, mist to name a few.

Here, the process is different - you got 2 continuous phases liquid and gas and the problem is to check how they mix etc.

As I indicated earlier, VOF is model is good to track the interface of liquid with the gas. However, when these two fields mix - one cannot keep track of small air bubbles since they require very small meshes. So, essentially, the volume fraction of primary liquid smears which then becomes similar to the eulerian approach.

Does the VOF model take into account the gas region change in shape? Yes, the model itself is meant to track the interface and if you have specified that the air is going to impinge on the liquid, deformation of liquid-gas interface will be taken care of .

IF you have a snapshot of the process you would like to model, we can clearly indicate which model to use.

But i guess you indicated that your boundary may move like a piston compressing the air inside etc...so in that case use dynamic mesh to simulate boundary motion.

As of now, if you dont have any aggressive mixing - use dynamic mesh with VOF else, if these 2 fluids are going to mix very well and you want to see the distribution of either fluid after mixing in such a process, use dynamic mesh with eulerian multiphase modeling.

/CFDtoy

Originally Posted by SerSe

Hi guys,

as I understood from Michele's help and from Fluent Users' Guide, I should not use the Discrete Phase Model since it treats the presence of small spherical solid particles - liquid droplets - gas bubbles within the main flow. That's not my case, since I have an inner flow bounded by adiabatic walls in which the air regions (which take up a considerable volume fraction) separate the liquid regions.

I would opt for using the VOF multiphase model in Fluent. Do you agree, guys?

Actually one more question arises... Does the VOF model take into account the gas region change in shape (e.g., shrinking of the air region or changing in shape of the interface air-liquid)? or should I introduce the dynamic mesh modelling to represent the behaviour of these air gaps?

Thank you in advance,

SerSe

[SerSe]

Hello guys,
I am now proceeding to turn on the VoF model together with the dynamic mesh tool in a simpler test-case. I have a pipe with three cell zones, i.e., water at the right and left sides separater by air in the center of the pipe. The BCs are mass flow inlet and pressure outlet at the ends of the pipe, and interiors at the interfaces air/water.

If I have well understood, the VoF model will take care of tracking the change in shape of the interface (air/water) while the dynamic mesh will modify the air zone volume.

I will let you guys know the results achieved.
Many thanks for your help, and if you have some other tips, they are welcome.

My best regards,
SerSe

[SerSe]

Hi guys,
I have some problems with my CFD simulations.

Let's say I have a pipe with three cell zones, i.e., water at the right end, oil at the left end separated by air in the center of the pipe. The water pushes the air and the oil to get out of the pipe.

The BCs are mass flow inlet and pressure outlet at the two ends of the pipe, and interiors at the interfaces water/air/oil. I have turned the VoF model on, initialized the solution all over the regions based on the mass flow inlet BC and then patched the central domain with a secondary phase volume fraction equal to 1, so to have air in the central zone, and the left zone with a third phase volume fraction equal to 1, so to have oil in the left zone.

Do I need to introduce dynamic mesh or I could just specify the velocity of motion for the air domain (moving mesh) and keep stationary the other two mesh zones?
And should the mesh velocity be the same as the inflow velocity (I suppose that this way I would loose some interaction effects at the interface...)?

I thank you in advance.

Regards and best wishes,

SerSe