MixSim V2.1 - Modeling solids suspension

The user wants to calculate just suspended velocity using Mixsim. I coudlnt find out any reference regarding that calculation in the guide. Also the user wants to know how the beads would move in to domain. I think he is assuming a multiphase simulation can be done in Mixism, to my knowledge that is not possible. I needed you confirmation on this. Can just suspension analysis be done using Mixsim using multiphase model or some other means?
MixSim is an extension to FLUENT, adding application-specific pre- and postprocessing capabilities to it. These capabilities are limited to single-phase analyses. For multi-phase problems, you can always, after having prepared the single-phase problem, switch to the FLUENT GUI and do whatever FLUENT_6 offers. (In this case, you would go for an Eulerian-granular two-phase flow simulation.)
I recall Kumar Dhanasekharan talking about a scheme source code file that provides a user input panel and process automation for the running of such kind of solids suspension simulations. If you believe this may be the right thing to offer to the customer, please consider contacting him. He may however advise to not give this tool away for free, but sell it.
I've once compiled the necessary steps to transition from a single-phase simulation to a solids suspension simulation. Here they are, written down at the time when I worked with FLUENT_6.1 (...!):
- This assumes you are doing a multiple-reference-frames simulation.
- For accuracy, consider using PRESTO & QUICK (for momentum and volume
fraction -- not for turbulence equations: keep them at first order
- Also for accuracy, consider using node-based gradients!
- Converge the single-phase calculation.
- save the single phase case & data.
- Enable the mixture multi-phase model withOUT slip; enable implicit
body force treatment.
- Create a new material for the dispersed solids.
- Set the phases, assign materials to them etc.
NOTE: The primary phase is the liquid...
- check the settings for turbulence model and gravity (!)
- patch the solids volume fraction in the complete domain to a sensible
- Switch OFF the volume fraction equation.
- run some iterations, until the start-up transients in the residuals
have calmed down a bit.
* Save case & data!
- For the mixture multi-phase model, switch on the slip.
* The following may help avoid a bug in the next step:
Solve -- Controls -- Solution: click OK.
- Set the particle diameter in the phase properties.
If you cannot access the entry field, you've run into the same bug as
I did. To get out of the mud, re-start in a new FLUENT session from the
case & data you saved just a few steps above. Again, do not hop over the
previous step that also helps avoid the same bug.
After having come here again in the new FLUENT session, do not forget
to actually set the particle diameter.
- run more iterations, again to settle the start-up transients in the
residual plots.
- Switch from the mixture multi-phase model to the Euler/Euler
multi-phase model.
- check the turbulence model: It should use the "mixture" version.
- Activate the "granular" option for the secondary phase.
- A couple of new settings will appear in the phase properties list --
set them carefully. Syamlal-O'Brian is generally a good choice.
(Use Lun-et-al for the Granular Buld Viscosity.) Where there are
no default models available (i.e. only "none" and "constant" or
"user-defined"), choose "none". Also, set the "frictional viscosity"
choice to "none". For the coefficient of restitution, consider lowering
the default value, because 0.9 is usually too high. I used 0.7...
- Now you will have to use the "ABgranular.c" UDF. I'm attaching the
source code. As you may not need any instructions, I'll not give any
to begin with. If you feel that you need some, let me know.
- Calculate some more iterations, again to go over the new start-up
- Finally, enable the volume fraction equation again!
Disable all automatic convergence checks, and monitor the volume
fraction on the impeller surface or at some other appropriate location.

Some additional notes:
- I mentioned the node-based gradients already.
WARNING: These should not be used in FLUENT_6.2 when there are
zero-thickness (double-sided) wall zones!! That bug has been fixed in v6.3.
- The under-relaxation factors I used:
pressure/continuity: 0.7
velocity/momentum: 0.5
granular Temperature: 0.2
volume fraction: 0.2
k, epsilon: 0.5
all others: 1.0
- To get the turbulent dispersion of the particles right, you must use
the following TUI switch:
"interphase momentum source?" --- *yes*!
Unfortunately, this may have negative effect on stability.
A crude alternative that adds to the stability is, instead of the
above mentioned TUI command, to type in the following:
(domainsetvar 3 'vof/diffusion-on? #t)
To get rid of this setting again (it will be saved in the case file!),
type in the same line, but replace "#t" by "#f".
- You should also type in the following in the FLUENT TUI:
(rpsetver 'pressure/mp-dissipation? #t)
[This will not be needed in FLUENT6.2 any more.]
- The ABgranular UDF *may* not be needed any more in
FLUENT_6.3. It is provided at the following address:
<a target=_blank href="ftp://ftp.fluent.de/outgoing/jos/ABgranular.zip">ftp://ftp.fluent.de/outgoing/jos/ABgranular.zip</a>ftp://ftp.fluent.de/outgoing/jos/ABgranular.zip

Show Form
No comments yet. Be the first to add a comment!