5 Replies Latest reply on Apr 14, 2017 8:29 AM by Josiah Lund

    Mesh for NACA 0012 - Mach 0.1 Re 3,000,000

    Josiah Lund

      I am trying to calculate the lift coefficient for a NACA 0012 wing section. I am experimenting with different meshes and am strangely finding better results for my coarser meshes. I have am setting up a mesh with zero gradient and setting a number of cells per cord. I first ran only 10 cells per cord with no refinement for partial cells. I am running for a level 2 and 4 refinement for partial cells, and also doubling the mesh precision to 20 cells per cord, and when those are done, I will keep going to 40 and so on. Computation domain is 10c behind, and 5c behind, top and bottom.


      I was expecting the 10 cells per cord mesh to be far too coarse to give good results, so I was very surprised to find that I was getting good correlation. Can anybody explain how a mesh this course is giving me good results when making my mesh more fine is making things worse. Also, I recently learned about Courant-Friedrichs-Lewy condition. Is this something that need not be satisfied within the solution that solidworks uses?


      The plot below shows the results of the parametric study I ran varying angle of attack for the two shown cases. The blue CL curve was created using XFLR5 for the same foil, Re, Mach, and fluid properties.


      Mesh from computational domain level

      10x10 no refine.PNG


      Airfoil detail

      10x10 no refine close up.PNG


      Solution at 15 deg AoA with no partial cell refinement

      10x10 solver.PNG


      solution at 15 deg AoA with level 4 partial cell refinement and 1 global refinement while the solver was running

      10x10 4 refine 1 refine.PNG

        • Re: Mesh for NACA 0012 - Mach 0.1 Re 3,000,000
          Josiah Lund

          Can anybody shed some light on this?

          • Re: Mesh for NACA 0012 - Mach 0.1 Re 3,000,000
            Rudolf Van den Berg

            HI Josiah


            I ran into a similar issues on previous flow studies, I don't have an answer for you regarding why the coarse mesh is giving better results. There is so many variables that plays a role in this.

            In SOLIDWORKS FLOW 2016 there is this new mesh called Equidistant meshing this works superbly with these kind of airfoils and also any kind of blades from impellers. 

            In this mesh you can specify the amount of shells (1-3) and for each shell you can define the size.



            Have a look at this, I am sure you will get more accurate results.


            Kind regards


            Rudolf vd berg


            MECAD Systems.

            • Re: Mesh for NACA 0012 - Mach 0.1 Re 3,000,000
              Dave Bond


              Thanks for taking the time to post the question, it has made me think more about my problems and as a result gain more insight into modeling.


              The first thing that occurred to me was your reference to XFLR5. My initial assumption was on reading your post, that XFLR5 was a complex model that you were using to compare your Solidworks result to. After reading this article http://www.rcsoaringdigest.com/pdfs/RCSD-2008/RCSD-2008-02.pdf it is clear that the XFLR5 model was developed to help design RC gliders rather than some CFD model run on a super computer! The author of the article Andres Deperrois concluded at the end of the article "


              My conclusion is that a simulator such as XFLR5 may be a valuable and useful tool, provided that the user knows what to look and ask for, and that he always keeps in mind the limitations of the underlying mathematical model and the finite precision both of our tools and of our beloved planes.


              Given you are comparing one model against another and rightly or wrongly, my impression is your belief is the XLRF5 model is the correct result. It might also explain why you are getting an answer closer to XLFR5 with a course mesh compared to a refined one. The XLRF5 model is a 2D model that was used to integrate across a variety of wing airfoils to get a 3D answer. Solidworks on the other hand is a 3D model even when you call it a 2D one because the Z direction has a physical dimension other than zero (assuming X&Y are the 2D directions). Therefore as you simulate with a course grid, you are most likely simulating in a similar fashion to the XLRF5 2D model. In a 2D model as transition occurs from laminar to turbulent the true effect of that can't be modeled accurately in 2D because it becomes a 3D problem due to the air moving in the Z direction instead of purely in the X&Y direction as assumed in the 2D simulation.


              Given that, I would suggest that wind tunnel tests are a better starting point (although not always!). It would I think make a more robust case to calibrate Solidworks to a published wind tunnel result (or your own test data) rather than comparing to another model result. Your post of February 12th 2015 Re: Lift Coefficient on 2D Airfoil and the following responses are a good starting point to some of the important calibration issues. Some things that come to mind:


              1. Start with an airfoil that has some good wind tunnel data of a similar size and the Reynolds number (Re) you are using.

              2. Set Computational Domain 10+Cord lengths (C) Ahead, 10-15C Above, Behind and Below ,change until no discernible difference in result. 5C seems too small in your examples. see Re: Lift Coefficient on 2D Airfoil further down

              3. Change the Y slice dimension to see how it affects the result, increasing should should allow you to better a more accurate Cl or Cd as less influence from side effect errors at the expense of longer computational time. Dividing the Lift or Drag force by a bigger area reduces the side errors since these are the same

              4. Use local meshes in an assembly if you don't have access to 2016 to create a finer mesh around the airfoil as was suggested above. This video is a great explanation SOLIDWORKS Flow Simulation - Mesh Controls - YouTube

              5. Refine the mesh as you have been doing too again until little change to the result

              6. Increase the Travels or consider using a dummy plate 1 or 2 cord lengths behind the airfoil to measure velocity and use it for convergence in addition to lift and drag to ensure sufficient simulation across the entire Computational domain. Solidworks is iterating like a spreadsheet ie in a particular order so cells down stream may not have time to effect those upstream. This is a good example Propeller wash does not seem accurate

              7. Try altering the Turbulence Intensity(TI) and length after the above have been done (one at a time not both together) Turbulence kinetic energy - Wikipedia, the free encyclopedia If you plot Re versus TI on a log scale you will note TI getting flatter after about Re= 1,000,000

              8. Keep the mesh the same and change the X&Y velocity vectors to simulate Angle of Attack. If you have the time don't do that change the model orientation instead and see what difference it makes to the result!

              9. Once you have a good calibration put in a different airfoil shape (again assuming data is similar to your conditions from wind tunnel testing) and see if Solidworks can get a similar answer. If so then you have confidence in the model's ability to correctly compare different shapes as you refine your design. If not then you have curve fitted rather that calibrated and can't have confidence in the answers unless you don't change the shape of the airfoil.

              10. Finally do what you originally intended to do, simulate your model in 3D using the calibrations.

              11. Publish your results on the forum. Publishing allows others to peer review your results (ie replicate them) and also suggest improvements.


              My experience with both Solidworks and Flow simulation is not the precise answer but gaining understanding of the flow behavior which then can guide your idea/product development to a robust solution rather than spending time and money on a physical model too early. Unfortunately the calibration bit is very time consuming. Once completed though, the iteration of the idea can go quickly with good confidence of a good solution. The technical engineering term "Shit in Shit out" comes to mind!


              Hope that helps and have a great New Year

                • Re: Mesh for NACA 0012 - Mach 0.1 Re 3,000,000
                  Josiah Lund



                  I appreciate your response. To make this as easy to follow, I will respond to your suggestions in order.


                  1. I actually was copying data from a study that has already been done (Aerospaceweb.org | Ask Us - NACA 0012 Lift Characteristics). I used XFLR5 so I could have the data without having to read it from a chart. Just some background on XFLR5 is that it as basically Xfoil that has been modified to allow the user to analyze 3D wings, but it drops Xfoil's capability to reverse design an airfoil. As you can see below, it is very accurate at low angles of attack. In future posts, I will compare against data from wind tunnel tests, but that limits the analyses I can validate my methods with as I do not have access to one to collect my own data.



                  2. You were referencing another post that I had made on an airfoil I was matching to another XFLR5 simulation I had done. The conclusion that I made from that post was that 5c for top front and bottom and 10c behind WAS a sufficient computation domain. This may not be true for the larger angles of attack that I am attempting here, so I will take my previous findings with a grain of salt.


                  3. The mesh is currently set up to be only 1 cell thick. I was under the impression that this would make my simulation as close to 2D as SolidWorks gets. My goal is to find a setup that is relatively accurate in 2D that I can scale to 3D and analyze a wing or entire aircraft.


                  4. I am familiar with the meshing tools like local meshes, and while I do not have access to SW2016, with some work I can manually do the same thing and the "equidistant refinement". Again, my goal is to find a mesh that is as time efficient as possible so that it can be applied to a 3D region without creating too fine a mesh in a region that is not critical and slowing the analysis down. In the post you referenced in suggestion 2, I did use a local refinement, and was able to get a match within 3% of what I got for XFLR5, so this time I was trying to use a different approach and let the solver do automatic refinements. I am currently re-running the simulation with a manual local mesh.


                  5. I think this suggestion is too vague to be useful as there is a number of ways I can refine my mesh. I believe the surface mesh is much more fine than necessary, but in the outer regions I am guessing that the mesh is far too coarse. I have no way to tell if this is true without much trial and error.


                  6. This is a new technique to me. I will add a plate like is done in the post you linked to as to see what my downstream flow is like.


                  7. I am not really interested in seeing this phenomena unless it has a direct influence on my simulation. My goal is to work towards simulations of full aircraft (or at least their components) in outside air, so this parameter is not something that is under my control as in a wind tunnel.


                  8. I have heard this suggestion before. I too am curious to see its result, but I would like to have convergence using both methods before doing a study of the two.


                  9, 10, 11. I completely agree. I was hoping to attract someone with this post who has gone through the same struggles I have faced and come out the other side. It appears I am pioneering with the airfoil flow which is very perplexing to me. I thought there would be a flood of people pointing out flaws in my approach, but I don't think I have seen a concrete solution yet.


                  Again, I very much appreciate your input and you have brought a few new things to light for me (and also reminded me of thing I had heard but forgotten). I will continue to stumble through this and I hope to eventually have something to share with the community. I try to keep my simulations simple but true, with a tight focus (in this case, only the Cl). If you can thing of any other specific corrections to make, let me know and I will try to implement them. I think I'm going to put together a spreadsheet to track all the changes I make because it is already beyond what I can remember.



                • Re: Mesh for NACA 0012 - Mach 0.1 Re 3,000,000
                  Josiah Lund

                  I think I found an underlying flaw in my analysis method. As I approach stall AoA, I should be using the transient solver, rather than the stead state solver that I did use. When I have a chance, I will try this again using a transient analysis.


                  Ref: unsteady flow, when do you use steady when do you switch to transient -- CFD Online Discussion Forums