I am facing big times problem with the Lagrangian particle tracking model in CFX. I simulated flow in a hydrocyclone and once I obtained quite good flow field, I started tracking the particles with all the applicable forces applied (Turbulent dispersion force, pressure gradient force, gravity, byouancy) BUT I get wrong results all the time.

Could some one comment his experiences with Lagrangian model and accuracy of it in CFX-11? I have heard from other people as well that they have been facing the same problem as that of mine.

Please help. Thanks very much.

Regards, Kushagra

[rvallejo]

I´m facing the same problem. Could anyone help us ?

Thanks

[John]

Originally Posted by Kushagra
;87439

I am facing big times problem with the Lagrangian particle tracking model in CFX. I simulated flow in a hydrocyclone and once I obtained quite good flow field, I started tracking the particles with all the applicable forces applied (Turbulent dispersion force, pressure gradient force, gravity, byouancy) BUT I get wrong results all the time.

Could some one comment his experiences with Lagrangian model and accuracy of it in CFX-11? I have heard from other people as well that they have been facing the same problem as that of mine.

Please help. Thanks very much.

Regards, Kushagra

Can you provide details what's wrong with your results?

[rvallejo]

Lagragian model provides a result where all the particles go to the underflow. I 'm using turbulent dispersion and Schiller Naumann drag force. I've tried virtual mass force and pressure gradiente force in addition, but they didn't work as well.

I'm using ANSYS CFX 11.01.

Best Regards,
Vallejo

[rvallejo]

Originally Posted by John

Can you provide details what's wrong with your results?

Lagragian model provides a result where all the particles go to the underflow. I 'm using turbulent dispersion and Schiller Naumann drag force. I've tried virtual mass force and pressure gradiente force in addition, but they didn't work as well.

I'm using ANSYS CFX 11.01.

Best Regards,
Vallejo

[leeportnoff]

When the particle diameters become small (less than 10 microns in air) the fluid can no longer be considered continuous. The drag coefficient on each particle, which is calculated using standard correlations (Schiller Neauman), must be divided by the Cunningham correction factor. The correction factor is greater than 1 which means that the effective particle drag coefficient goes down.
The cunningham correction factor is not used in CFX but if you use the "Particle Transport Drag Coefficient" in the Momentum Transfer tab in Pre you can specify any drag model that you need using CEL relations. First try to redo the Schiller Nauman relation, verify it with the CFX implementation and then correct it with the Cunningham factor. The Schiller Nauman will be the hardest part because it is an implicit relation.

[gravis]

Originally Posted by leeportnoff

When the particle diameters become small (less than 10 microns in air) the fluid can no longer be considered continuous. The drag coefficient on each particle, which is calculated using standard correlations (Schiller Neauman), must be divided by the Cunningham correction factor. The correction factor is greater than 1 which means that the effective particle drag coefficient goes down.
The cunningham correction factor is not used in CFX but if you use the "Particle Transport Drag Coefficient" in the Momentum Transfer tab in Pre you can specify any drag model that you need using CEL relations. First try to redo the Schiller Nauman relation, verify it with the CFX implementation and then correct it with the Cunningham factor. The Schiller Nauman will be the hardest part because it is an implicit relation.

Does anyone have experience carrying out this implementation in CFX?

[sei2006]

check your turbulence model firstly.

[leeportnoff]

LEVEL OF DIFFICULTY: ADVANCED
To get this working, I had to write a custom FORTRAN routine based on the pt_mom_source.F file included in ANSYS.
I compiled a custom pt_mom_custom.dll,
Expressions, functions, and variables > user routines > insert user routine and call 'drag'
option: particle user routine
calling name: pt_mom_custom
library name: pt_mom_custom
library path: <path to winnt> containing pt_mom_custom.dll

Then insert User Function
user routine name: drag
argument units: []
results units: []

Now, in your domain, under the 'Fluid pair models'
for 'drag force' select 'none'
check 'particle user source'
you should see your 'drag' routine for particle user routine

Lastly choose arguments and return variables.
** important ** the order you select these variables must match the order in your pt_mom_custom.h routine. i.e. It is by order of appearance, that cfx knows input DIAM_PT means particle.Mean Particle Diameter.