We have been conducting our own attempt to validate Simulation CFD 2015 by modelling the well researched and documented NACA0012 aerofoil section in 2D. We have been very disappointed with our results and would be interested if anybody else has attempted a similar test. Following the advice in the Autodesk help files, we have the following settings:
Over a range of settings we have never achieved an error in lift force lower than 15%, and computed drag is typically 6x higher than published data for these conditions. I have seen considerably better results published on-line from Fluent and Cosmol simulations.
Is this really the best we can expect for this software, or am I doing something wrong ?
I have sent this also to Autodesk Support, with relevant files included.
Solved! Go to Solution.
Solved by Royce_adsk. Go to Solution.
Hello All,
Though I have not tried to coorelate to published foil data, I do set the Y+ parameter to on and always set it to 35 and the boundary layer growth factor to 1.3 from its defalt value of 1.05 in the adaptation section. Perhaps this may be of help.
Mike
I looked into this and it appears that its been logged with the support team. I spoke to them this am and they are looking at the settings and running the models as we speak. Their plan is to close the loop on the support side as well as provide an update to the broader community on the forum.
More to come soon...
I am looking at the model on my end.
Looking over some NASA notes we should be able to solve this fairly well using the newer SST models.
http://turbmodels.larc.nasa.gov/naca0012_val_sst.html
and
http://www.cfd-online.com/Wiki/NACA0012_airfoil
We'll see what we find out!
Anyone like the idea of turning this into a Support Hangout Session in the near future? Would be a fun one to just talk about.
This is exactly the NASA validation data we have been using. I'm surprised that Autodesk have not tried this before !
Hi Wolfgang. We did this validation a few years ago at Blue Ridge. I am trying to dig up the report. While it's a good airfoil or 2d aero validation model, it's not used commonly to benchmark the code in general, unless you are doing this sort of thing in reality. In other words, if you are looking to use Autodesk CFD for an airfoil project, it's probably a good representative test case. But, like all of the commercial codes that have used this for validation, it will take a unique combination of mesh and solver settings to dial it in. So, like I said, if this is your commercial application it's probably worth investigating further.
If you are looking to validate CFD, in general, I'd advise you look at the particular type of application you are interested in and there is a good chance we have a validation model we can share or work on with you.
All depends on what you are trying to accomplish with you benchmark testing. Settings for one type of CFD simulation, may not be the same as what you need for another. I'll keep digging for the report and will post what I find.
We are doing this validation for a commercial project. We are lucky enough to be so busy with paid-for project that we are not using CFD software just as a pastime. BTW, I'm presently on holiday (this is pastime), hence replies might take a while.
Hi Wolfgang,
Here is a summary of the results using below recommended settings for this analysis in Simulation CFD 2015:
Recommended Settings for this analysis:
Scenario level flags:
Solve Dialog Options:
Mesh:
Overall Strategy
There are 2 areas to concentrate on to get best results for external aero airfoils like the NACA0012.
o Leverage solver options that work well for sensitive external aero analysis like the NACA0012
o Ensure the flow gradients in the boundary layer are captured within the wall layer elements
o Avoid an abrupt change in mesh height at the transition from prism wall layers to tetrahedral elements
o Ensure close enough first node at wall to keep y+ < 50
Description of Solver Configurations:
The necessary solver adjustments that need to be leveraged to correctly study very sensitive airfoil shapes is to enable these two flags.
Once you run your models with these options you will notice that the drag force starts to fall considerably (typically within 20-30% without concentrating on the mesh at the wall layers)
Mesh Considerations:
When you want to start to dial this model in with more a validation frame of mind you really need to focus on the mesh enhancement sizing.
A study was performed to understand sensitivity of the mesh enhancement on this model to the overall lift and drag results. The 100 x Cord geometry, provided by Wolfgang was used although the notes at NASA mention that it really should be 500 x Cord.
Two sweeps of runs where performed. One sweep only the layer thickness was changed and the other held the thickness at 200% (2.0 in UI) and varied the enhancement gradation factor.
Here is the plot of the results. Keep in mind for those that are reading this on the forum. The target forces is approximately 5.26N Drag and 488N Lift. This is based on the notes that Wolfgang provided in his excel file to me.
For the layer factor results as the factor was increased to 210% the results improved. As the gradation value was reduced to 1.15 the results also improved, but was not as sensitive as compared to the thickness factor.
These findings gave guidance which was used for the best results case referenced above:
Now the question should be asked how to approach this regarding best practices?
The study actually validates one aspect of the Turbulence Model Hangout conducted a few weeks back. The suggestions in the Advanced panel is a great place to start. From there you need to make sure that the mesh enhancement thickness is thick enough to capture the boundary layer along the walls and maintain a Y+ value of less than 50 for the K-omega SST.
Lastly as a general note, the NACA0012 airfoil problem is very sensitive to meshing/solver configurations due to the dynamics of the physics, but many industrial models aren’t nearly as sensitive. This difficulty/sensitivity to physics is why it is used for validation.
Topics have been added to the Simulation CFD help to describe the three flag descriptions that were missing:
resid_bdry_force_calc: http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-94A16B55-01E2-4739-8340-E14123E1A5D4
sst_new_iwf: http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-F1EEF97E-686E-4D63-ADED-6F1BE07EA85D
use_sst_rc: http://help.autodesk.com/view/SCDSE/2015/ENU/?guid=GUID-E01069FA-E14B-4374-99C5-CE495FF33975
The model we received back includes an additional flag not mentioned in the response, it is called "default_adv5" (ON), again this is not included in the on-line documentation. How is using this flag different to just selecting ADV5 through "Solution Control"->"Advection Options"?
I would like to try out the effect of the two new flags mentioned above. Although the search window of the Flag Manager offers the "use_sst_rc" flag, if you select it nothing appears the Flag Table, so I am unable to set it. Same goes for the "sst_new_iwf" flag too.
IDBateman,
Those flags are scenario level flags, and you are trying to add them at the default flag level. Make sure you are selecting the scenario on the left hand side of that dialog, and then RMB in the right side canvas and hit add....
I've included two images to illustrate.
Hope this helps
Thank you for such a prompt response. Understood and works as you suggest at my end.
Its just the fact that it was included in the drop down list of available default level flags made me think that it was a valid option.
Maybe it would help if the documentation for each flag indicated what level it was applicable too.
Ian
Hold that thought 😉
So I am starting to build the content for this as a hangout, but curious what people really want me to talk about!
If you have specific things you want me to try to cover in 30-40 min start asking your questions here please.
Cheers,
Would like to know how you knew the correct y+ range to be in as well as the reasoning behind using the flags that were used. Mainly interested in the mesh and solver setup choices if you think that would be of interest to other users?
cheers,
Niall
1/ I thought your "Understanding the Turbulence Models" hangout was excellent, and would like to see some of the points covered during the Q&A session at the end covered as formalised slides. (ie: effect of TurbLam ratio in different turbulence models). Maybe you could provide similar details for each of the 'advanced turbulence parameters', for example ... does the SWF have any effect on the k-omega SST solution, where there is no 'wall function' as such. That window seems to offer me a lot of parameters that are probably only applicable to specific turb-models.
2/ Of course we would like a more detailed explaination of what the three flags do, (resid_bdry_force_calc,sst_new_iwf,use_sst_rc) the documentation is still very brief on these.
3/ Problems such as the NACA0012 should be sensitive to surface roughness, if I set a surface roughness to the air (not an intuitive quantity) how does that interact with the surface roughess of a soild wing?
4/ Is there any way to determine the Y+ of the mesh nodes other than those nearest the wall, ie at the outer edge of the mesh refinement region ?
Can't find what you're looking for? Ask the community or share your knowledge.