Learning Forum

[Mepal]

Hello everyone,

I've been using a macroscopic particle model (MPM) to create a group of particles (1 cm. diameter) inside a cylinder.

The whole fluid inside a chamber is only air.

After I initialized a system, I checked a contour of a MPM-volume-fraction. Everything went well.

Then, I checked a contour of air volume fraction. I found something strange. The air volume fraction was 1 but it should not be like this.

I think the MPM volume fraction was already recognized by the software. My question is why the air volume fraction is full-on plane 3?

I mean should it be blank in the area that was occupied by particles?

Your help is greatly appreciated.

[Rob]

I suspect the fact you're using a CFF for volume fraction means the particles don't actually exist in the continuous phase as a volume. Looking at the Theory Guide I suspect something else is done (it's good bedtime reading) so you may find that you either check it's not already defined in the CFF list or need to create another CFF of (1- mpm-volume-fraction). 

[Mepal]

Thank you so much for your help, Rob.

I did not use CFF. I used an available MPM techniques in Ansys Fluent 2022R1.

Below pictures are the way I created a group of particles.

After that, I initialized a system.

Then I found the problem that I already explained above, a contour of a MPM-volume-fraction looked logical but a contour of air volume fraction did not make sense.

I am still curious that

(1) Do I understand correctly that Fluent already recognised there is a group of particles in a domain after I initialized MPM functions and particle (fig 6 above).

(2) If the MPM volume fraction was already recognized by the software, why the air volume fraction is full on plane 3?

By the way, I will check at the Theory Guide as you suggested. Thank you again for your valuable time.

 

[Rob]

The particle volume fraction is reported via a Custom Field Function, first contour panel. What else is available in that section?  MPM is not a normal multiphase model and uses a different approach, hence my comment that the particles may not exist as a physical volume in the domain. 

[Mepal]

Thank you Rob for your reply.

In the panel of the contour of custom field function, there is a list of mpm-.....

This morning, I changed between CFF and Legacy in preferences (if I understand correctly this is what you mean in your first comment).

It still has the same problem, the air volume fraction is full on plane 3.

If you have any suggestions I would appreciate it.

[Rob]

Custom Field Function - CFF. The file format option is for legacy (.cas.gz) of cff (.cas.h5)    Ansys are very good at reusing acronymns without warning people.... 

The Custom Field Function for the macro particle volume fraction can be used to create a CFF for carrier volume fraction if you want to view that. 

[Mepal]

Maybe you are right that particles may not exist in a physical domain.

When I created an MPM-volume-fraction by using contours, the result indicated there was a physical volume of particles.

 

However, when I tracked an MPM-volume-fraction by using particle tracks, the result indicated there was not a physical volume of particles.

This was an interesting result for me ?.
Do you know what is the possible reasons I tracked the CFF of MPM-volume-fraction by using between contours and particle track, the results of VoF were different?

 

[Rob]

I suspect it's linked to the way the data is stored.    https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v222/en/flu_ug/flu_mpm_using_limit.html 

[kasidit.phanpa]

 

After I read the link you attached, I am still curious about this line, The MPM is not compatible with mesh interfaces.

Do you know what is the meaning of not compatible with mesh interfaces?

I mean I am not sure whether this is the cause of MPM-volume-fraction was different between tracking by using contours and particle track, and whether this is the cause of the air volume fraction is full on plane 3.

 

 

 

[Rob]

It means the model will react badly when the macro particle hits a non conformal interface. 

[Mepal]

Hello Rob, thank you for your help as always.

I am sure a real MPM volume fraction did not recognize in a domain!

To test my assumption, I started again with a simple small domain.

1) I created a cemented ball in a simple cylinder by using an MPM technique.

2) I patched the water over the cemented ball to notice when the water falls, whether it interacts with the ball.

3. I ran a simulation. The result is shown below.

The result indicated the VoF of water overlaps with the VoF of MPM. It means both MPM and water did not interact.

I've tried to fix it by adjusting many possible ways (following an Ansys Fluent User's guide), but the MPM still did not recognize in the domain (although the MPM volume fraction shows in a domain!).

Do you have any general suggestions I should try?

[Rob]

As I don't know why you want to use MPM it's hard to make a suggestion! What is the purpose of the simulation work?

[Mepal]

I use MPM to create particles because of the size of the particles.

According to Ansys Fluent User's Guide (Ref, https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/flu_ug/flu_ug_models_mpm.html), MPM is used when the total particle volume is significant within the flow domain volume.

I did not use a traditional Lagrangian discrete phase model (DPM and DEM) because it is applied when particle sizes are small enough to be regarded as point masses within a single cell.

In my case, I need to create a real volume of particles inside a domain. That is the main reason why I use an MPM.

[Rob]

A real volume that moves, or are you modelling a packed bed?

[Mepal]

In my work, I would like to create a stable (and moving) packed-bed with real volume inside a cylinder.

After that, I will fill a solution in its porous region.

[Rob]

Do you need to model both large (MPM) and small (DPM) particles at the same time? By definition a packed bed isn't moving, so which is it?

[Mepal]

Thank you so much Rob for your reply.

My work has two phases.

In the first phase, I need to create a stable packed-bed (that cannot move) inside a small chamber. Then I will fill a solution into its porous region to notice the movement of the solution.

In the second phase, I will create a group of particles (that can move) inside a small chamber to notice its interaction with an external force.

[Rob]

OK. For the non-moving part, if the particles are "big" you may need to model them in CAD. However, if you're after the pressure loss only for porous media you won't need to model the whole bed. Additionally, there are empiracle equations for bed pressure losses for most packing materials (spheres, rings, saddles etc). 

If the particles can move then you can use Eulerian Granular, DPM (watch the volume fraction limits), MPM or Ansys Rocky. The latter two are either designed for large particles or have some options (Rocky) to account for it. 

[Mepal]

Thank you for the ideas and the suggestions

 

I am happy to update you that I can activate an interaction (coupling) between MPM and the fluid phase.

 

As you remember, I had a problem with the MPM particle and fluid phase do not interact with each other (picture below).

I used a mixture model as a multiphase, the primary phase is air and the second phase is water. I let an MPM particle settle down by gravity into water.

or

Now, I can activate a coupling between MPM and multiphase (picture below).

 

Just only one thing it was strange.

If you notice the above picture carefully, the volume fraction of the particle did not recognize in a primary phase (in my case, it is air). 

I've tried to fix it but I've not found a way to handle it.

Do you have any general suggestions to fix it?

 

 

[Rob]

 

I have a feeling of deja-vu with the answer to that…..

So you may need make a custom field function based on the MPM fields.