hi, i've just used CFX in this past 3 months. i am trying to simulate the flow passes a curve channel using CFX. the purpose is to study the counter-rotating vortices due to the imbalance between the pressure gradient and centrifugal force inside the boundary layer. i use a small wall perturbator placed at the leading edge. but, this disturbance was always damped out. so, i cannot observe counter-rotating vortices (Goertler vortices) inside the boundary layer.

can anybody help me? can we use CFX to study the phenomena inside the boundary layer? if yes, what are the important things that we have to consider?

thank you very much..

Make sure you are using an appropriate turbulence model and near wall mesh.

but the flow is still in laminar region. for the near wall mesh, i used inflated layers inside the boundary layer. so, it should be no problem.

Are your current results grid independant?

I think so, since i have done some cases with different geometries (and of course different grid sizes), but all results show that the disturbance were damped out. i suspect that CFX cannot be used to study this vortex, or may be i miss some features in this software. but, what is it? Petitjeans (1997) managed to simulate this vortex using Fluent by applying the SIMPLEC (Semi Implicit Method for Pressure Linked Equation - Constant) algorithm with an iterative line-by-line matrix solver. What is the similar feature in CFX?

Trying different grid sizes != grid independance study.

Are you properly resolving the boundary layer?

Paste your command file here + pic of your geomeetry + pic of near wall mesh.

The type of solver used shouldnt affect the final simulation results.

If Fluent can model this flow so can CFX.

The geometry is very simple, i.e. a curve channel with a small perturbation at the leading edge. The geometry and the mesh near the boundary and the perturbator can be seen in this link. http://www.box.net/public/1kuph4ohrg

And this link is the command file. http://www.box.net/public/qf5xxjiu60

please let me know if i have a mistake in this simulation. thank you very much.

Hi Tandiono,

Do you have a turbulence model set, or are you running it laminar? This isn't clear from your answer.

Is the phenomenon you are interested in steady or transient?

Regards, Robin

this vortex occurs inside the laminar boundary layer, and we only interest in the steady state condition.

You have about 15 cell layers in your prism mesh. I dont think this will be enough to resolve recirculation in the laminar sublayer. What is your yplus value? Make sure the prism layer lies with the boundary layer i.e. there are enough prism layers inside the boundary layer. 50 prism layers inside a boundary layer is not unreasonable. There is a section entitled something like "advice on near-wall meshing" in the modelling section, turbulence modelling subsection of the manual. Read this and make sure your boundary layer mesh conforms to its recomendations.

I would try to run this problem transiently and then produce a video of the flow vectors in the laminar sublayer downstream of the perturbation.

A proper grid independance study seems essential for a simulation like this. You dont seem to have done one.

If it turns out you have to solve this transiently make sure your final results are also timestep independant.

You are solving this as a laminar problem which means your mesh needs to be fine enougth to resolve all scales of motion ala DNS. This, again, makes it essential that your perform a proper grid independance study.

As recirculation is an inherently transient phenomena it would point to the need to solve the motion transiently.

I would also suggest solving this as a 2D problem initially which will dramatically speed up your grid and timestep independance study.

Another thing: You may be terminating the solver too early. Do a test run with unattainable convergence criteria to observe the long term convergence behaviour. i.e. Residuals may start to ocsilate pointing to vortex formation / transient behaviour.

Yes. I understand that it occurs in the laminar portion of the boundary layer, but what I am asking is whether you activated a turbulence model. If you did, it may interfere with the vortex generation.

Regards, Robin

Another factor would be the aspect ratio of the elements. In order to resolve the vortex, you will need a fine resoluiton in the streamwise direction. If the aspect ratio is too high, you won't get a vortex.

-Robin

Hi, I have tried in the past to reproduce with CFX 5, TG vortices inside a lid driven cavity with periodic end walls (setup can be seen from for example Albensoeder et al, Physics of Fluids, 2000 I think). I used a fine mesh (essential) and a laminar model and the vortices appeared as expected. Regards, Ulian