I'm analysing a Cyclone Sepetor in Fluent. So, i couldnt decrease the Y* under 60 yet. In this case, there is an air-powder mixture that enters the cyclone and i am observing escape/total mass ratio. You can assume that my model mesh is fine (good enough). Can any body tell me which equations and setting should i use in the in the physics solution.
Conditions for now:
-Steady State
-Turbulent: Reynolds stress,linear,wall eq.s,standart wall func. and buoyancy
-Solution: coupleds, gg node based,pseudo,warped
the others are default.
Thank you for your interest and help.
Hi Güven Nergiz ,
your settings are already well suited for simulation of cyclone separators. In terms of (U)RANS modeling you need to choose a turbulence model, which is made for:
a) flows with strong streamline curvature
b) anisotropic turbulence
From this perspective the point (a) could be addressed with the SST turbulence model as well, if the curvature correction term is included. The benefit over RSM models is higher numerical stability, i.e. better convergence behavior, and less numerical effort and hence higher computational speed because of the only 2 PDE's instead of 6 PDE's to be solved for a full RSM model. But the SST-CC model will not be able to address point (b), since it is a 2 equation isotropic turbulence model. But in tests we could not observe so substantial differences between the SST-CC and an RSM solution. You can test and compare by yourself.
With full RSM model the k-omega based RSM models are recommended for cyclones (or in general). RSM will address both points, in particular the effects from anisotropic turbulence.
Unfortunately your image does not show the lower end of the cyclone vortex chamber. It was found, that the flow along the apex cone and through the lower particle settling chamber of a real cyclone separator might have a substantial influence on the flow conditions in the cyclone vortex chamber and around the vortex finder.
Furthermore, it might be difficult to get CFD converged in steady-state. The reason is, that in many cyclones the flow conditions are inherently transient because of core vortex precession. The core vortex is in permanent slight rotational movement and this vortex is not just a cylindrical tube, but more or less formed like a thin helix vortex. So it moves permanently in space and time, which causes any steady-state simulation to stagnate rather early in terms of residual level and convergence. The remedy is to do the simulation (more costly) in transient mode and to apply statistical averaging to the simulation.
Hopefully that helps you a bit with your further progress for this intended simulation.
Regards,
Thomas Frank.
Hi Güven Nergiz ,
your settings are already well suited for simulation of cyclone separators. In terms of (U)RANS modeling you need to choose a turbulence model, which is made for:
a) flows with strong streamline curvature
b) anisotropic turbulence
From this perspective the point (a) could be addressed with the SST turbulence model as well, if the curvature correction term is included. The benefit over RSM models is higher numerical stability, i.e. better convergence behavior, and less numerical effort and hence higher computational speed because of the only 2 PDE's instead of 6 PDE's to be solved for a full RSM model. But the SST-CC model will not be able to address point (b), since it is a 2 equation isotropic turbulence model. But in tests we could not observe so substantial differences between the SST-CC and an RSM solution. You can test and compare by yourself.
With full RSM model the k-omega based RSM models are recommended for cyclones (or in general). RSM will address both points, in particular the effects from anisotropic turbulence.
Unfortunately your image does not show the lower end of the cyclone vortex chamber. It was found, that the flow along the apex cone and through the lower particle settling chamber of a real cyclone separator might have a substantial influence on the flow conditions in the cyclone vortex chamber and around the vortex finder.
Furthermore, it might be difficult to get CFD converged in steady-state. The reason is, that in many cyclones the flow conditions are inherently transient because of core vortex precession. The core vortex is in permanent slight rotational movement and this vortex is not just a cylindrical tube, but more or less formed like a thin helix vortex. So it moves permanently in space and time, which causes any steady-state simulation to stagnate rather early in terms of residual level and convergence. The remedy is to do the simulation (more costly) in transient mode and to apply statistical averaging to the simulation.
Hopefully that helps you a bit with your further progress for this intended simulation.
Regards,
Thomas Frank.
Hi Thomas Frank ,
First of all thank you for interest and help. I will make a transient analysis and share with you the results.
Secondly, this cyclone is our speical design. We are (as company) producing powder coating systems. So, at the bottom of the cyclone there is a sieve. And we did not need lower end yet. But due to analysis results, main design may be change. As i said, i will give you a feed-back after all.
Thank you so much again.
Best regards, Güven
Ps: I am waiting for other answers too. Please share Your comments.
@ Güven Nergiz
Dear Güven
It is important to apply an appropriate turbulent model to solve complicated three-dimensional strong swirling flows in the cyclone. The RSM model, which can describe anisotropic turbulence has been proven to be an appropriate turbulence model for cyclone flow, although it is computationally more expensive than other unresolved-eddy turbulence models.
Also, you can read our newly published paper to help you for equations and setting of physical conditions.
Article Improving efficiency of conventional and square cyclones usi...
I will recommend you as a first approach use the K-omega STT menter model, you will find a good relation between computational cost and accuracy, however you must to ensure a good mesh treatment near the wall, in order to activate the damping function.
This two equation models ensure the acquirement of the buoyancy effects. if you use this model, please let me know your comments about it.
depending on your problem, The turbulence models that can be for your case are: 1) standard k-ε with curvature correction; 2) Shear stress transport (SST) with curvature correction; 3) SSG Reynolds stress model (SSG-RSM); and 4) large eddy simulation (LES). The comparison between the mean and root-mean-squared simulated velocity profiles and the experimental data is necessary. However, computational cost and the ability of the models to capture the significant phenomenon in a cyclone will be the main focus to decide which is the best one for your case.
you can find some intersting works added to this answer below:
My suggestion is:
- First perform a steady state simulation with K-w SST to obtain a initial flow field.
- Then swich to transient with RSM or smagorinsky / dynamic LES turbulence models (realy expensive). Comput at least three residence times before start averaging. Average for at least another three residence times.
Obs. You must ensure that mesh refinement and time step are approppriated for your simulation.
@ Oscar Alcocer : I disagree, that the SST turbulence model (without any additional precautions) is a good startign point for cyclone flow prediction. The so-called curvature correction for the SST model mandatory needs to be taken into account (see my post above). SST turbulence model for its own is an isotropic 2-equation turbulence model. It underpredicts without correction the effects in flows with strong streamline curvature and it is not able to predict anisotropy effects in turbulence, as they are very present in cyclone flows.
For high-enough Re, the turbulence problem has been solved, see attachments, even for non-Newtonian fluids. However, the curvature of r.m.s. streamlines is a problem which needs further research and empirical modifications. I know that from e.g. the Princeton Superpipe or the Cottbus superpipe. In case you have the means ($$$) for a research contract, I am ready to help.
You can use Reynolds stress turbulence model and unsteady state conditions. This is suitable for complex flow problems. Moreover u can use discrete phase model for particle simulation. If u use other models your article may be rejected by reviewers. Thesee models are accepted by reviewers.
Thank you
Hi, my recommendation, be practical, if you have enough computing power, just use RSM.
I do agree with @Thomas Frank, that the so-called curvature correction for the SST model mandatory needs to be taken into account for this case at which the flow has strong streamline curvature and rotation.
So, SST-CC (SST with curvature correction) is a good choice. Or, SST-CCM (modified SST with curvature correction) for easy coding if you prefer to write UDF.
Article Prediction of swirling cold flow in a solid-fuel ramjet engi...
Hi everybody, thank you all for your valuable ideas. I peruse them all.
But i need to know that what should the courant number be? Please share your toughts with me. At the end i will share my results with you. Especially Y+ number and all particle results, because this is a special cyclone design.
Short answer: always use Reynolds Stress for rotation-dominant flows.
Güven Nergiz : The Courant number to choose depends very much from the used CFD code and its numerical implementation and hence from its numerical stability. So a general advice is not possible.
Fully implicit implementations of (U)RANS modeling approaches are from a theoretical point of few numerically stable with no regard to Courant number. In practice usually there is nevertheless some limit to be observed. But high Courant numbers of 200 to even several thousands are not so rare. And for a steady-state flow simulation the end result should be fairly independent from the chosen Courant number in a pseudo-transient solution method. So I personally would start with an automatic timescale selection (if the CFD code does provide it, as CFX and Fluent do) and if that leads to numerical instabilities, I would wind down the Courant number, i.e. reduce the pseudo-timescale. If the code for Courant ~1 still diverges, something is wrong (with the setup, the mesh, the model selection or the implementation of the CFD code).
Probably you know the physical meaning of CFL number. In a bit generalized terms it means, that the CFL number gives you the number of cells in your mesh, which are crossed by the flow in a single timestep. So it means, that for CFL=1 the flow progresses for 1 cell width during the integration timestep delta t. Since cells in your mesh are not equally spaced, this is a bit generalized picture. But it gives you an imagination, what CFL number means.
Regarding y+: For a y+
- Badges
- Science topic