Learning Forum

[s.petley]

I am modelling an oil-water hydrocyclone using the Eulerian model and RSM turbulence. nI believe my solution is converged without issues, however compared to experimental results the model is considerably underpredicting seperation efficiency. The tangential velocity is also underpredicted (which partially drives the seperation). nI have checked mesh and timestep and while there are some differences it is less than difference between numerical and experimental result. nI am wondering then if it is an issues with regards to turbulence modelling and perhaps this model is overly diffusive. I'm already using RSM which is the recommended for stongly swirl flows. Being not totally familiar with the mathematical formulation of this model could it be possible to change the coefficents?nAny advice would be greatly welcomed, thank you. n

[Rob]

I'd leave the coefficients alone, they're fine for most applications and work well for cyclones. Assuming the mesh is well refined and is hex and/or poly check the convergence and post some images of the velocity components with the node values off. nI assume you're running PRESTO! & second order for everything but turbulence? n

[s.petley]

Dear Rob,nThanks for your comment. The mesh is poly.nIn previous results I was using only First Order for the momentum, I switched to Second Order and the results are much improved, both for the pressure contour and tangential velocity. In fact the velocity is somewhat overpredicted but since the results between the two meshes are very similar I then modelled Eulerian with the coarse mesh given we are time restricted. nI’ve now run with the Eulerian model. I think we can only afford First Order volume fraction – even QUICK is very slow to solve. Results are much better however we are still about 25% away from the reported separation efficiency. I've uploaded contour of x velocity and pressure for your reference (apologies I tend to use CFD post so the figs are not great). nI guess this is a result of all of the above but I think about as far as we can stretch the computing resources in the time available. Unless you have any other tips?nKind regards,nSeann

[DrAmine]

Ensure that you are using high order discretization schemes. Volume fraction QUICK is not a must and might have some caveats. Do a grid sensitivity study if you can afford it and read about Richardson Extrapolation.What are the other models and interracial forces you are using?n

[s.petley]

Dear Dr Amine,nThanks, yes I would normally do a full grid convergence study with 3 or 4 homegenously refined grids and find the value at zero spacing, but as you say in this instance we are time restricted.I use the standard Schiller Naumann drag law, Lopez de Bertodano turb dispersion and Troshko Hassan turb interaction, everything else is as standard. n

[Rob]

Looking at the pressure I'd expect to see more of a velocity range in the inlet section. I know you're mesh limited but have you enough in that region? n

[s.petley]

Dear Rob,nSorry for delay. I am now running a mesh independance test based on the coarse grid and refining x1.5 for 2 more grids. But I see what you mean, perhaps I could use an automatic mesh refinement within Fluent here rather than globally refining the whole region?nAnother thing, it is off the original topic somewhat but I was reading the User Guide and in there it notes that outflow bc's cannot be used with multiphase models. Initially we missed this since we followed the setup details in the published paper we are using for benchmarking. What is the effect of outflow bc's and the Eulerian model?nThanksnn

[Rob]

Outflow bc's don't provide a back flow condition or pressure. Other than that there's not a reason they won't work; however we stopped using outflow before Euler models were added so it's possible there just isn't enough coding linking the two. nYes, adaption will probably be a better option now as you can just focus on the chamber. Just watch the cell count as it can increase significantly very quickly. n