CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Onera M6

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 8, 2015, 10:57
Default Onera M6
  #1
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
Hello all,
I am working on reproducing the Onera M6 wing test case in Star CCM+, but I am having some issues that I cannot seem to figure out.

To start the pressure coefficient plot that is being generated is not smooth and has a lot of “bumps/waves” in the values. I would not think this is due to lack of mesh refinement, because as shown in the attached plot there is a sufficient amount of data points making that curve.

Also the values for my Cp are wrong. The Star CCM+ values plotted are values that I multiplied by -1. Once I make that multiplication, it appears to have a similar shape as the experimental data, but obviously the magnitude of the values is off also. Any idea why I am getting negative Cp values and the magnitude is wrong? I am defining the definition of Cp in the field functions with the setting listed below. The solver setting I am using are also listed below, and the case is being run on a 3,00,000 cell polyhedral mesh. My other concern is that some of my residuals are beginning to increase.

I attached pics of Cp plot, the mesh around the wing at a cut section, and the residuals. Could anyone give me some insight on my issue? Any help would be much apprciated, thanks!

Solver Settings:
Coupled Flow
Coupled Inviscid Flux – ASUM+ FVS
Ideal Gas
K-Omega
All y+
Steady
Courant Number = 10
Expert Initialization – Grid Sequencing
Solution Driver – Expert Driver

Flow Settings:
Mach = 0.8395
Pressure = 101325 Pa
Tinf = 288.15 K
Density = 1.2886 kg/m3
Dynamic Viscosity = 2.202875E-05 Pa-s

Mesh Settings:
Number of Prism Layers = 20
Prism Layer Thickness – 0.05m
Minimum Thickness Percentage = 5%
Layer Reduction Percentage = 10
Boundary March Angle = 85
Surface Growth Rate = 1.1
Attached Images
File Type: jpg Cp Plot at 0.2 of Span.jpg (33.1 KB, 80 views)
File Type: jpg Mesh Around Wing.jpg (87.0 KB, 115 views)
File Type: jpg Residuals.jpg (38.3 KB, 70 views)
mjaisit is offline   Reply With Quote

Old   March 9, 2015, 10:30
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
That is a mesh issue if I ever saw one. You may have 3M cells but, that doesn't mean you have a good mesh. A few things I would like to point out...

1. The volume change from your circular volumetric controls to the larger freestream cells is far too large and abrupt. You should keep it to less than 20% and try to smooth it out more.

2. It looks like your prism layer growth rate is a little too big. The default value of 1.5 is usually too high, I tend to stay between 1.1 and 1.3.

3. The final prism layer cells are larger than the core cells next to it. Idealy you would want them to be the same size, or maybe 20% smaller than your core cells.

4. Your residual plot does not indicate convergence. I would also caution you against relying on only residuals for convergence. Make a report/monitor/plot of lift and drag. When those stabilize you are finished, as long as your residuals aren't awful. Usually about 3 orders of magnitude is sufficent, although not always acheivable.

The good news is you can fix your model pretty easily. Do this:

a. Get a good surface mesh to start with. Your leading edge is sharp, that wasn't intentional right? Best way to do this is to create a Geometry>Operations>Automated Surface Mesh and select Surface Remesher and Automatic Surface Repair. If you already have one, modify it so that your minimum surface size is maybe 0.1% of your chord and your target surface size is maybe somewhere around 5%. (These values might need to change, but it's a starting point.) You can then also some custom controls to set surface sizes elesewhere int he model (like your freestream boundary conditions or symmtry plane). I would set these sizes to be something like 750% to 1000% of chord for target size and whatever 0.1% for minimum (orwhatever you settle on) You want the symmetry plane to be able to meet the mesh size on the leading edge. You will also want to change the surface growth rate to something between 1.05 and 1.1. Default value is too high for what you are doing. Oh, and surface curvature. Set that to 60 or better.

b. After you have a decent surface mesh, go back to your volume mesh and get rid of your volumetric controls (you may not need them, and you shouldn't start with them). Reset your number of prism layers to between 5-7 and set your prism layer thickness 10% of your chord. (Again, just starting values). Also, go into your mesh continua and set Tet/Ply Density>Growth Factor to something bewtwen 0.7-0.8. This will reduce how quickly your core mesh will grow away from your near wall mesh (that is essentially set by your surface mesh size). And.. Tet/Poly Expansion Max Cell Size, set this to be whatever your largest freestream cell size is (750%-1000%).

3. From there you may will likely have to tweak the prism layer mesh and maybe the polyhedral mesh, but it's a better starting point than what you have. Eventually, depending on pressure gradients and separation you may have to add in additional volumetric controls to help refine them, such as at the LE or TE. However, don't start with it. For a lot of moderate cases you won't have to deal with it.

4. I would also caution you to keep an eye on your y+ value. For the models you have selected it needs to stay between 1-5 OR 30-60 for best results. You can change this value by adusting the # of layers or thickness of your prism layer. However, you can't get a feel for the wall y+ values until you have a model that is converged (or close to it). You need the velocity field to be basically converged. Obviously, this means you will have to do some iteration with your mesh on top of a mesh dependency study.
fluid23 is offline   Reply With Quote

Old   March 9, 2015, 10:35
Default
  #3
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
Feel free to post pictures along the way for some feedback. A lot of the mesh sizing stuff is magic-gut-insticnt-voodoo that only comes after spending weeks and weeks meshing models over and over again.
fluid23 is offline   Reply With Quote

Old   March 9, 2015, 15:42
Default
  #4
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
Thanks so much for the help MBdonCFD! As you might be able to tell I am kind of new to meshing. I completely remade the mesh, but I am still having one issue. That is the trailing edge does not seem to be probably captured (its kind of triangular). I tried to just add volumetric controls to the trailing edge with a cylinder, but it didn't really work well. The only way it seemed to improve was if i really made the surface mesh really fine. Would you have any suggestions other than just setting the target surface mesh really low?
Attached Images
File Type: jpg Mesh.jpg (96.2 KB, 70 views)
File Type: jpg TE.jpg (78.0 KB, 69 views)
mjaisit is offline   Reply With Quote

Old   March 9, 2015, 15:55
Default
  #5
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
Your prism layer mesh is still too thick. Shoot for 1/2 or 1/3 of the thickness you have now.

As for the TE, it looks like you have a fairly flat surface and no blunt TE so the surface mesher doesn't try to apply small sizes here. It will always try to hit the target size first, then reduce from there to meet growth and curvature requirements. To get a small cell size you really need a small surface mesh, but I wouldn't try reducing your global size. Instead setup another custom control like you did for the freestream surfaces but assign just the last 10%-15% of the upper and lower surfaces before you get to the TE. (This may require a change to your CAD model). Then you can assign a target size that is much lower for this region and it should fix your problems.

Just out of curiosity, how far away are your freestream boundaries?
fluid23 is offline   Reply With Quote

Old   March 9, 2015, 17:24
Default
  #6
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
I think I'm trying to go too fine on the resolution now because I am getting a mesh around 10 million cells which is causing my computer to run out of memory when I initialize the solution.

My boundaries are 10x the chord length away from the wing in each direction. To reduce the cell count I am coarsening the boundary targets substantially to about 1500% of the chord. As there are no large jumps in cells sizes, is this an issue?
mjaisit is offline   Reply With Quote

Old   March 9, 2015, 17:39
Default
  #7
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
Probably not an issue. Hard to say without a picture. Like I said, the values I gave were just a starting point. Adjust as necessary. I wouldn't expect your model to have fewer than 3M cells, probably closer to 5M for a good model.

You probably want to go fruther than 10c downstream though. Your wake will not dissipate that quickly and you NEED the wake. Go for 15c downstream, that is probably a little better.

How much RAM do you have? For polyhedral cells (if I remember correctly) you need about 1GB/500k cells so for a 10M cell model you would need more than 20GB, for a 5M cell model over 10GB. If you do not have those kinds of resources, try switching to trimmed mesh with advancing layer mesher rather than poly/prism. That usues around 1GB/1M (I think) and is actually a good choice for external aero problems. That will let you retain fidelity if you are running low on RAM.
fluid23 is offline   Reply With Quote

Old   March 9, 2015, 18:49
Default
  #8
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
Oh, I would also be cautious about using grid sequencing for your initialization. You have a very high Mach number and it may crash on you or give bad results.

Usually, for something in the transonic regime I would start at a lower Mach, maybe 0.5 and then have a field function that ramps it up over time. That is very easy to do but I can help if you get stuck.
fluid23 is offline   Reply With Quote

Old   March 9, 2015, 19:57
Default
  #9
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
I have 16 GB of ram, so it's definitely a limiting factor. The main reason I was stuck on using the poly mesh is my colleague said he had really bad experience with the trimmer mesh on complicated geometries where it would crash every time a small change in the geometry would be made. It was a year a or two ago when he was using Star CCM+, so hopefully that is improved now. The plan is to paramtrize the wing, create a java macro for the mesh conditions that work well with this case, and run a DOE on the wing's design variables. Chances are that the DOE might generate a complicated/exotic geometry, so I was concerned with trimmer being able to automate the mesh easily for such a geometry.

But for this case, the trimmer mesh seems to capture the surface better. The TE is sharp now.

I will definitely take your recommendation on the ramping up of the Mach number and look into that. I really appreciate all your help!
Attached Images
File Type: jpg Domain.jpg (99.5 KB, 49 views)
File Type: jpg Airfoil.jpg (96.8 KB, 56 views)
mjaisit is offline   Reply With Quote

Old   March 9, 2015, 20:14
Default
  #10
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
No problem. If you start having issues with the trimmed mesh talk to tech support, it's supposed to be ideal for flows that are mostly aligned like yours. I am not sure that I would call a wing all that complicated either. I could share some meshing horror stories that would make your skin crawl.

Also, it sounds like you would really benefit from using the adjoint flow solver. It's intended for optimization studies and will give you cost functions and all sorts of other fun stuff.
fluid23 is offline   Reply With Quote

Old   March 15, 2015, 08:57
Default
  #11
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
Sorry to resurrect an old post, but I am still having some issues with this case. I am getting decent looking Cp distributions, but there are mini-shock looking things behind the main shock. I attached two pics of the Cp distribution along the span on the wing. As you can see, immediately after the shock there is a significant amount of waviness in the in the distribution.

Originally I thought it was just that my surface mesh was not fine enough, and the leading edge was not perfectly round. I increased the curvature number of points substantially and really decreased the surface mesh size on the LE, but I can't seem to get this to go away. My residuals seem to be dropping by a fair amount and leveling out. Any ideas?
Attached Images
File Type: jpg CP at .2.jpg (49.4 KB, 45 views)
File Type: jpg Cp at .65.jpg (53.8 KB, 35 views)
File Type: jpg Residuals.jpg (51.2 KB, 34 views)
File Type: jpg Mesh of Wing.jpg (54.3 KB, 39 views)
File Type: jpg Mesh of Top of Wing.jpg (52.0 KB, 54 views)
mjaisit is offline   Reply With Quote

Old   March 16, 2015, 09:12
Default
  #12
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
I don't see any turbulence parameters on your residuals plot. You are still using k-w, right? Make sure you have sst turned on. I think it's default, I don't recall.

Looking at the mesh you posted, it looks like you have regressed from what was somewhat acceptable to wildly inappropriate. Your previous mesh from March 9th looked OK, but on this you have a lot of very big cells right on your surface. Your y+ value has to be very high. Have you checked this yet? I will post an image in a second of what I would call an a appropriate mesh and you will see what I am talking about.
fluid23 is offline   Reply With Quote

Old   March 16, 2015, 09:24
Default
  #13
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
This link shows a 2D mesh, but its a good represnetation how your cells should progress from surface to freestream. Your mesh isn't structured so it wont follow the curvature but the general idea is the same. Notice the enhancement of the wake? You may also need to refine cells along your shocks. There are very high pressure gradients there that can get wonky if you don't provide enough resoloution to resolve them fully. Look at the help documentation under User Guide > Meshing > Mesh Refinement > Field Function Mesh Refinement.

http://www.cfd-online.com/Wiki/NACA0012_airfoil
fluid23 is offline   Reply With Quote

Old   March 16, 2015, 09:32
Default
  #14
New Member
 
Michael Anderson
Join Date: Oct 2012
Posts: 14
Rep Power: 13
mjaisit is on a distinguished road
I was originally was using the k-w turbulence model, and will in the future to compare to the experimental, but I was struggling to remove this waviness/"mini-shocks" from the pressure distribution. In efforts to reduce the complexity of the problem I ran the simulation as inviscid.

I agree that I might have gone in the direction of overboard on the LE, but until I reduced the cell size down to around 1 cm the curvature of the LE of the airfoil looked somewhat sharp and not smoothed enough. I was originally thinking that the unsmoothed surface was causing the "mini-shocks". But maybe its just the transition.

I was also hoping to avoid having to refine the mesh along the shocks after an initial solution due to it cutting out some of the automation, but that might be necessary.

Thanks for the link to the NACA 0012 mesh, I will try to model my mesh after this.
mjaisit is offline   Reply With Quote

Old   March 16, 2015, 09:41
Default
  #15
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
I would keep viscosity, even during setup and troubleshooting. You could just end up having to solve a whole other set of issues if you ignore it right now.
fluid23 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Onera M6 Wing Mesh salvoblack OpenFOAM 10 January 23, 2021 12:52
Discrepancy between sectional Cp and experimental results on tip (ONERA M6) pdp.aero SU2 2 March 9, 2015 21:26
RANS optimization of Onera M6 wing diwakaranant SU2 Shape Design 8 October 21, 2013 15:57
Turbulent Onera Abhii SU2 3 March 21, 2013 22:41
Does anybody have onera M6 grid ? aeroman Main CFD Forum 0 November 7, 2006 01:48


All times are GMT -4. The time now is 17:57.