MixSim V2.1 - Modeling solids suspension
|
The user wants to calculate just suspended velocity using Mixsim. I couldn't 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 discretization). - 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 value. - 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... - Calculate some more iterations, again to go over the new start-up transient. - 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. |
||
|