[umran]

And Wang, do not forget to run the mech check by typing these lines...

checkMesh -allGeometry -allTopology

If there are no warnings or cautions, then rhoSimpleFoam should be able to run... and do play around with the relaxation factors especially during early running of the simulation.

At times, some might not understand that the relaxation factors are there to prevent a solved variable to be used directly for the next step solution. It seems that without the relaxation, the solution may converge early but on contrary as other parameters may not be ready for such a drastic change of the solved variables and leads to simulation blowup.

If there are slightest warnings on the mesh, better to get it corrected first before anything else. simpleFoam may run on not a proper mesh but rhoSimpleFoam definitely won't.

[dkokron]

Umran,

Thank you for posting your work!

I have the case running under OpenFOAM-4.x. Your use of an unbounded divergence scheme for (phid,p) appears to be critical. Using "bounded Gauss limitedLinear 1;" results in very slow execution as the solution for p fails to converge within 1000 iterations. Did you notice this behaviour? Did you disable the following warning for your runs?

Reading "/scratch/dkokron/OpenFOAM/dkokron-4.x/tutorials/compressible/rhoSimpleFoam/OneraM6/system/fvSchemes.divSchemes.div(phid,p)" at line 37
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/home/dkokron/OpenFOAM/OpenFOAM-4.x/etc/controlDict"

[umran]

Dear Dan,

As expected there will be shockwave/shockwaves formed and therefore I allow the pressure to go wild prior to settle down.

I leave the switch to the unbounded warning as it is i.e. selected to '0' as it doesn't actually stop the simulation from running.

[dkokron]

Umran,

The case you provided ran fine with OpenFOAM-4.x after a few changes to the initial conditions. I also converted it to run in parallel. This required setting the consistent flag to yes in fvSolution I will share the case if there is interest.

Did you use the 'sample' utility to extract data for plotting the top and bottom Cp values? Would you share your sampleDict file?

Dan

[umran]

Dear Dan,
In the spirit of OpenFOAM as an open-source CFD package, sharing findings would be great especially in this cfd-online forum. There are many researchers browsing this forum and they (including myself) would be very grateful to those contributors.

Off course, there were some sensitivities involved when dealing with proprietary research, however, in this case of onera M6, I guessed it should be shared openly. Anyway, it is nice of you to extend it to run in parallel!

With regards to extracting the data, as mentioned in my paper, I used the paraView line filter located exactly at the percentage of the wing span (as per the Agard 138 report). From the extracted pressure raw data, by using the calculator function, you'll obtain the Cp values. Off course to align the data with the available data from the experiment, the cross-sectional length of each span section being normalized into 1.

[moser_r]

Dan,

Were any other changes required to get the case to run in parallel? I have added the consistent flag into my fvSolution file, but it is still crashing.

Many thanks

Richard

[dkokron]

Sorry for the delay.
see attached file containing the full working case. The file is actually a bzipped tarball.

tar jxf OneraM6P_CFDOnline.gz

Let me know if you have problems.
Dan

[dlansigan]

Hello,

I'm trying to recreate this case with a mesh generated using snappyHexMesh. How long did it take you to run your simulation, with and without parallelization?

Thanks!

[Ash Kot]

This is an excellent thread to follow; my suggestions will be to make it sticky on forum wall!

[umran]

Originally Posted by Ash Kot

This is an excellent thread to follow; my suggestions will be to make it sticky on forum wall!

Thanks, Ash.

It seems many would like to see the case file running. Our friend Mr. Don there have already got it running parallel on OpenFOAM 4.

So, to those interested in rhoSimpleFoam and OneraM6 solutions, kindly browse thru this thread.

[Tobi]

Hi all, old thread moved to the top again
I would suggest to move the thread into the validation sub-forum based on the fact, that the thread compares measurement and simulation in a nice manner. To stick it to the top is not recommended. There are a lot of good threads out which are not pinned. If we would do so, we would only have pinned threads.

However, we are trying to keep the forum clean and move the stuff to the corresponding sub-forums. It is indeed a lot of work because everybody just posts on the main forum and there are too less moderators available.

[manahara]

Appreciate your work in the validation case for the Onera M6 wing. Unfortunately none of the Dropbox links seems to work. If you are still up for publicly sharing your work, can you please include links to download your work. Thank you in advance,