Hi all

Well, I know the convergence topic is pretty common here, and I have read through the threads. Unfortunately, Im still stuck.

Im running a simulation of an automobile chassis in a wind tunnel. Convergence (RMS) seems to level out at between 1-e3 and 1-e4, and remains very stable at that level from iterations 30 -> 200+. I have tried most every suggestion I found (reduced/increased time step, dropping advection scheme mix to .75, using a conventional gas instead of 'air ideal gas,' changing from Outlet to Opening for the exit, etc). I have also tried refining the model's mesh. In some cases, convergence becomes unstable or diverges, but with a bunch of tried combinations, I can't get RMS residuals anywhere below 1e-4, which is probably not a very tight result.

The basic setup is: Tunnel using symmetry plane, with a length/height/width 3x that of the blunt body. SST turbulence model, 1%, Isothermal Inlet = Normal, 130mph Fluid = air, 65F Ref pressure = 1 Atm Outlet = Static, 0 pa Walls/Floor = Free slip

Mesh is approx 2M nodes Inflation = 15 layers

I understand that I may always have a high MAX residual due to turbulent flow, but RMS seems to me to be way too high. Any thoughts on a next step are appreciated.

Roland

Hi,

Your suggestion that turbulent flows always lead to high MAX is not correct. A well posed turbulent simulation should converge.

I assume you are using steady state simulations. Automobile aerodynamics are well known to have large scale flow structures in the wake which are not captured very well by a steady state approach and a turbulence model. Have you considered doing a DES simulation?

If you don't want to go there, maybe try the k-e turbulence model. It tends to over-estimate the turbulent viscosity at separations and this may improve simulation stability.

A final point: You should also consider the behaviour of important variables when you assess convergence, rather than just the residuals. If the drag is the important parameter, make drag a CEL variable and output it to the solver manager. If the drag has converged ages ago but the MAX residuals are still high then you may well have reached adequate convergence anyway.

Glenn Horrocks

Hi, It seems your problem formulation is okay. you may remesh your geometry using CFX MESH and rerun. outlet should be outlet. Do not change it. Set reference pressure to zero. or And you can also run your problem with k-epsilon model to get a converged flow field later on you can change it to SST.

Thank you

Hi Glen

Thanks for your insight here, and for your many posts in support of those of us who are fumbling our way though the learning process.

My thoughts on the RMS vs. MAX came from a thread you addressed last year, where you mentioned that in some cases areas of high max can occur outside the area of interest, or may be focused in such a small area as to not have a significant impact on the global results.

Yes, it is steady state, as Im not yet focused on things like vortex burst, etc- just wanted to validate the model against some knowns (CD for example).

I have not attempted the k-e model. I will give it a try, but am primarily concerned about drag estimation; I understand that SST is generally considered a more accurate estimate, but perhaps I am mistaken here.

I did include the normal force (X axis for drag) as a plotted value in solver, and generally, it stabilizes (along with lift) by about 30 iterations. And, the drag value as calculated post run leads to a C/D which is within a few percent of actual (from the validation in a wind tunnel). My concern was that using this solver criteria/grid approach may not be accurate with the addition of aero devices (i.e. wings, spoilers) since convergence is not what I had hoped it would be; I dont want to build on a faulty base.

Thanks again for your help Regards, Roland

What mesh type do you use? Hex or Tet? If geometry is not too complicated, try hex and see if the convergence is improved.

I have a case where I rerun steady simulation in transient and the max residuals dropped by an order of 2. If you expect unsteady flow in your problem, you should give transient simulation a go.

I did a mesh dependency test on various turbulence models and I found that SST model captured different flow topology when mesh was refined and convergence was more difficult when mesh density dropped below certain values.

Hope it helps.

Cheers.

A 3X fit of domain to model isnt very big. Recirculating flow downstream of your model could easily intersect with the outlet plane. An opening type outlet BC could be usefull to solve that.

"15 layers" means jack shit ... you need 15 layers INSIDE THE BOUNDARY LAYER. That meanns you have to analytically estimate the BL thickness and get a decent minimum yplus value. Read the section in the modelling section "Addice on near wall meshing"...

You need to post your command file + sketch of your domain with BC types and locations and a representative section of your mesh to get proper assistance.

You cant just force a realife transient problem (separated flow from a chassis) into a numerical steady state shoebox and expect decent convergence or results. It may be possible that this problem can be solved steady state if the flow separation and recirculation are of such a nature that they can be captured by a turbulence model. But this isnt very likely. Pics of your current postprocess results would allow us to asses that. However you must certainly try a transient run to establish whether it converges properly. That would be an important clue to the source of the poor steady state convergence.

The ke model is very poor at predicting flow separation (almost inevitable in chassis flows) so I wouldnt bother going up that road.

Goind DES for turbulence at this stage is silly you first need to establish the root cause of your poor steady state convergence. Dont try to crack an egg with a sledgehammer...

have you checked y+

Hi Roland,

You will find an option in Pre under Output Control for both the Results and Backup files that allows you to output the equation residuals to the results and backup files. I generally enable this for the backup file as it allows you to look at where the solution residuals are high.

The residuals are normalized but maintain their sign, so it is useful to create a new variable in Post which is equal to the absolute value of the residual you are intersted in (i.e. CEL expression would be abs(U Mom.Residual)). With this variable you can create an isovolume (Volume object using isovolume method) in Post and see where the residuals are high and make some determination as to the nature of the instability. The solver generally behaves in a physical way, so for instance if it as the edge of a shear layer, it is the turbulent flow that is giving you trouble.

In terms of settings, try running with a bigger timestep. In some cases this may wash out transient turbulent effects and allow the turbulence model to do it's job. If the eddy viscosity isn't high enough, however, this won't help much.

The forces on all the boundaries are always written to the mon file, so you can easily go back and plot these. Just create a new plot in the Solver Manager and expand the "Force" list. You can also plot flows, imbalances, etc.

Overall, it sounds like you are doing a good job. If it helps, you can also download a CFX validation case on the AHMED body from the CFX Community Site at http://www-waterloo.ansys.com/commun...orts.asp?id=14 .

Finally, don't hesitate to call CFX support for help.

Regards, Robin

Hi Joe

Thanks for your feedback. I did try moving the model forward in the tunnel substantially (early on in my testing), and this did help with recirculation (into the domain) problems but not with high RMS. Perhaps I should try doubling the dimensions of the tunnel just to see the impact.

On the BL, the inflation layers are largely or completely within the boundary layer.

I ran a transient simulation, and results for lift and drag were within .5% of the stady state results, but convergence was not improved; it was stable at approx 8E-4 for U/V/W Mom, which is higher than that obtained for steady state.

You are right about k-e, that was very unstable.

I may re-mesh this more carefully to see the impact; most of the other variables have been addressed or eliminated from consideration.

Regards, R

Robin

I will try your guidance on the isovolume technique- seems a great approach to track down the potential culprit here.

I have tried fairly broad adjustments to the timestep (ranging from .01 sec through 2sec)- which for a 15M tunnel length seeing 190 ft/sec air velocity seems to cover the spectrum. It seems more stable at the higher end of the timestep for whatever reason.

Best, Roland

Your transient convergence is poorer that your steady state convergence?! I assume you used sufficiently small dt's and tried at least dt and 0.5*dt?

You must be making some kind of error in your command file or have a poor mesh.

I suggest looking carefully at your mesh quality and make sure it falls within accepted limits for all mesh parameters calculated in CFX post.

Also take another look at your BC types, locations and values specified.

If the turbulent structures are large, their timescales are big. If your timestep is smaller than the larger turbulent timescales, the solver may resolve some of the transient fluctuations. Increasing the timestep effectively washes out these transient effects.

Regards, Robin

Robin

Thank you for your guidance here. By further refining the mesh, and by modifying the inflation/prism layer to better capture the flows at different areas (thanks to the Y+ suggestion), the convergence trends are very smooth compared with the sharktooth trends of the prior approach. By increasing the time step, convergence has improved to approx 2E-4, which is substantially better than previous attempts. It does not want to continue on down towards E-5, but the C/D values agree with actual, and surface streamlines parallel the old wool tufts test quite well. So, perhaps I have a (usefully) converged solution even at this RMS level.

Just for the sake of trying, I will double the length of the test tunnel, to see if that better captures some of the larger turbulent flows (as are typical with most production cars).

Thanks again for all your help- much appreciated

Best, R