Hi everyone! I am simulating a cylindrical mixing section with two inlets in the same plane (inner jet is faster than the outer flow and they are concentric). I used k-epsilon turbulence model and incompressible air. My results show that the velocity profile in some sections are not symmetric with respect to the centerline, and sometimes the maximum velocity doesn't lie along the center. As far as I know, it should be symmetric with maximum pt at the center as the flow becomes fully developed. I tried to lower (from 5% to 1%) the intensity of turbulence for the inlet conditions but the results were the same. Do you have any explanation for this guys? The most unsymmetric profile is located in the region where there are sudden change in turbulence kinetic energy(TKE). Is it okay to assign similar inlet TKE eventhough the inlet velocities are not equal? Thank you so much guys for your time!

Michelle

Hi Michelle,

Welcome to the non-linear world of fluid dynamics, where the obvious is rarely right!

This is a classic problem of instability. A pin standing on its head is symmetric and it should be possible for the pin to remain in the standing position. However, the solution is unstable; the slightest deviation will cause the pin to fall because a pin laying down is at a lower energy level. Another physical example would be that of a sphere sitting on the top of a hill; again symmetric, but unstable.

Physical examples such as these are easy to visualize, but fluid dynamics is often less obvious. In the case of an axisymmetric jet within a tube, the slightest movement of the jet towards one of the walls will cause the static pressure on the side nearer the wall to drop, drawing the jet even closer and causing asymmetry in the flow. The solution isn't always steady either. As the jet is pulled to the wall, a recirculation zone may develop upstream due to the blockage. This recirculation zone may push the upstream portion of the jet towards the other side or at least away from the current impinging position. As a result, the jet will wander or fluctuate. This is a good example of unsteady behavior that can lead to convergence problems in steady state solutions; because there is no steady state.

It all depends on Reynolds number of course. At low Reynolds numbers, the viscous transport of momentum will keep the jet stable, but as the Reynolds number increases, the advective transport of momentum will dominate and lead to instability.

-CycLone

Hi Cyclone! Thank you so much for your very informative response. Actually there are negative velocities inside the mixing section which imply that there's recirculation/swirling inside. However,I made a refined mesh (reduced the body spacing to half and doubled the no. of inflation layers) and the results were very different though they both converged using the same criterion. Is it right to assume that I have to improve the quality of mesh?I'm using 6inch(diam)x 30ft long cylinder. Do you have any suggestion about the appropriate inflation layers? Also, I've read that there's specific range of yplus for every turbulence model, is the yplus of my mesh equal to the maximum yplus given in cfx post? I'm so sorry for many questions. I'm quite new to cfx. My simulation results is quite far from experiment results. I really appreciate your response and any other recommendations is much appreciated.

Regards, Michelle

Hi Michelle,

The only way to ensure you have a fine enough mesh is to continue refining it and evaluating the error. At some point any further decrease in the mesh size (and timestep, if it is transient) will not improve the solution appreciably, at which point you have acheived mesh independance.

Near the wall the mesh resolution is particularly important due to the high gradients. Not only is the hight of the first layer important, but you also have to take care that you have enough layers to sufficiently resolve the boundary layer. If your first layer is within an appropriate Y+ range and your expansion rate does not exceed 1.3x for each layer, you should be in good shape.

The Y+ limit depend on the turbulence model and how it is implemented. With some codes the k-epsilon model is limited to a minimum Y+ of about 11, below which the profile goes from logarithmic to linear as you enter the viscous sub layer. CFX does not share this lower limit. If you are running a k-epsilon model, the scalable wall function will handle this (see the doc for details), the k-omega type models, such as SST do an even better job with an Automatic wall treatment. As the Y+ is reduced (i.e. as you add more resolution near the wall), these models will switch from a logarithmic to a linear profile, allowing greater resolution of the boundary layer profile.

For k-epsilon, in this case I recommend a Y+ of 15 to 30, which should put about 5 nodes within the boundary layer. Any lower than 15 and you probably aren't getting much benefit for the added computational cost. For SST you could use the same grid, but as you reduce the Y+ you will get improved prediction of boundary layer development. If the flow is separting, this can increase you simulation fidelity.

As a final note, be careful comparing to your experimental data. Undertand how the data was collected and processed, including any averaging that was done and try to compare the raw data where possible. As I mentioned previously, this situation can lead to transient flows, so even though you have a steady state solution, it may be the turbulence model that is damping out the transients. You could try running a transient using the SAS SST model instead and comparing the time average solution to your experimental data. You should also take care to match the conditions upstream as closely as possible as well. The velocity profile at the inlet will have a significant influence on the results of this case.

Best of luck to you!

-CycLone

Thank you so much Cyclone! Your response is much appreciated. It helps me a lot! I made some mesh refinement and then the results of the velocity profile became more and more symmetric. I followed your advise to refine the mesh until there's no appreciable difference in results, I'm still simulating with some more refined mesh. I hope I'll reach that point of having independent mesh. But what if the results continue to change significantly eventhough the mesh size is very small? would that mean that i really need to simulate it in transient? Thanks again cyclone! I really appreciate it!

Best regards, Michelle

It really depends on what you are studying and how you are refining your mesh. If your meshing strategy is correct, solver may capture more unsteadiness, as the mesh is refining. The question is whether it will affect what you are studying. If you are solving steady flow problem, don't waste your time doing transient simulation, unless you are sure that it will have significant effect on your problem.