Preprocessing

Preprocessing

Need Help! – Boundary layer micro structure meshing for riblets on an airfoil

    • DanJ85
      Subscriber

      Hi all,


      I have spent 170 hours+ unable to solve this. I need to simulate a 3D NACA0012 for my thesis so that I can modify the airfoil boundary to add riblet microstructures (others have done it in research papers using Solidworks) but I want to use ANSYS Fluent.


      What I need to do is simply compare lift and drag coefficients for a model with and without riblets, but so far I can't mesh it with riblets due to their micro size in the boundary layer (perhaps).


      So far:



      • I can get a 2D mesh on a plain NACA0012 airfoil and simulations to work perfectly

      • in 3D, I can only get a 1x1m NACA0012 airfoil to achieve results in line with NASA (https://turbmodels.larc.nasa.gov/naca0012_val.html). If I make the airfoil thinner (0.1 or 0.01m depth) to save computations, I can mesh but I can't get Sparat-allmaras, k-e or k-omega sst to work without many issues and backflow, etc.

      • when I model riblets they are 0.1mm x 0.05mm repeating pattern and the mesh fails everytime, I think they are too small for it to function??


      Please see attached document for images and clarification.


      I have tried every tutorial I can find including Cornell University tutorials (2D) and CFD Ninja plus many many more. I've tried different boundary layer conditions, different field shapes (curved nose, rectangular), structured mesh and unstructured and I've tried them on all manner of airfoil dimensions, I've even upgraded my PC. I'm at a complete loss to make this work.


      Please if someone can help show me a viable method I would be forever in your debt.



      • 1. Simulate plain NACA0012

      • 2. Simulate NACA0012 with riblet microstructures


      I seem to only be able to attach one file here so I've put in an overview. I am happy to somehow share my actual project files and/or step files to anyone that might be able to see what I'm doing wrong.


      Warm Regards,


      Dan McEvoy


       

    • Keyur Kanade
      Ansys Employee

      As ANSYS Staff, we can not download attachments. Please insert images using insert image functionality. 


      please use tet mesh with inflation. you may need to use edge/face sizing to get desired refined mesh. also you may need to use body of influence (boi) as well. 


      please check some videos for the same. 


      Regards,


      Keyur


       


      If this helps, please mark this post as 'Is Solution' to help others.


      Guidelines on the Student Community


      How to access ANSYS help links


       

    • DanJ85
      Subscriber

      Hi,


      Sorry for the late reply, I have been very busy trying to solve this using Solidworks but I really want to do it in ANSYS as I know it is far more professional and in-depth, including things like y+ plots, etc. I flip back and forth with no luck in either.


       


      Summary:



      •   NACA0012 Airfoil

      •   NASA result, Coefficient of Drag (Cd) = 0.00809

      •   My Fluent Result: Cd =                             0.00816 (less than 1% difference which is terrific!)

      •   Problem: Can't mesh my proposed variation


       


      Process:


      Following references:


      NASA: https://turbmodels.larc.nasa.gov/naca0012_val.html


       


      Calculated Parameters:



      • Re:        6 million

      • Chord:   1 m

      • Span:     0.1m

      • Temp:    300K

      • U:          94.458 m/s



       



      • Y+ of 1 and first inflation layer 4.5e-6 from online calculator


       



       


      Geometry:




      • H1 (forward): 8m

      • H2 (aft): 16m

      • V3 (vertical): 20m

      • Airfoil: 1m NACA0012 (Boolean subtracted from body)


      Mesh:




       


      Airfoil Edges (x2) - 420 dividions, hard, no bias



      Tail internal edge - 310 divisions, hard, no bias



      Inflation - airfoil internal face, first layer 4.5e-6, 50 layers, growth 1.2



      Internal airfoil face sizing - 1e-2, hard, no bias



      Tail flow rectangle Body of influence - 4.2e-2 



       


      Setup


      PC:



      • Processor i9-9900k

      • GPU: 2080ti

      • Memory: 64GB DDR4


      Boundary Conditions:



      • Front = Velocity Inlet

      • Rear = Pressure outlet

      • Sides = Symmetry

      • Top and Bottom = Symmetry

      • Airfoil = Wall


       



       



       


      Modification (Riblet microstructures)



       


      Mesh


      With the same meshing (except mesh defeaturing turned off):



      • Airfoil Edges (x2) - 420 dividions, hard, no bias

      • Tail internal edge - 310 divisions, hard, no bias

      • Inflation - airfoil internal face, first layer 4.5e-6, 50 layers, growth 1.2

      • Internal airfoil face sizing - 1e-2, hard, no bias

      • Tail flow rectangle Body of influence - 4.2e-2 



       


      It said a warning along the lines of "some topologies defeatured" but it disappears before I can click it and I have defeaturing turned off.


      Please, how do I mesh this airfoil with these small detail features? Otherwise I am lost for my dissertation!


      I think the simulation will work with my parameters but I just can't get the mesh to work (I have tried changing a lot of things to make them smaller, etc.).


      I would be very very thankful for any advice that helps me get past this sticking point!


       


      Warm Regards


      Dan McEvoy


       


       


       


       

    • DanJ85
      Subscriber

      Also, I tried your suggestion for tetrahedrons (is this just in the master mesh settings?). It has great quality, but it removed my features. Is there a way to make this very fine and mesh around my riblets?


      These are my settings and outcome:



      Thank you



      Dan

    • Rob
      Ansys Employee

      You've got a few issues to work out here:


      - the geometry is smaller than most CAD tolerances. Scale up by 100 in geometry, mesh it & scale back in Fluent.  Hopefully it'll not be too big to cause problems due to the bounding box. That's an old micro-fluidics trick so public domain


      - the inflation layer set up isn't working as you've got some very silly looking mesh. 


      - mesh resolution. To resolve features you need several cells over their height & spacing.  That's going to be a huge mesh in 3d, use 2d


       

    • DanJ85
      Subscriber

      Hi,


      Thanks for the quick reply! I'll try the scaling trick. Did you read my first post by chance? The second one was just a quick go at tetrahedrons but the first one I was able to validate against NASA and is the real issue I'm having.


      Unfortunately I am trying to modify the aerofoil surface in line with other CFD studies and so 2D wouldn't work for my research. There are other papers that have done the basic of what I posted up above but none detail how they mesh it (and many use other programs).


      Can you please help me how I could do this in 3D? 


      Update: I've modelled it to 100m so the smallest channel/feature is 5mm. Attempting to mesh soon..


      I will let you know how it goes.

    • Rob
      Ansys Employee

      It'll work in 3d but the mesh count is gong to be very high.  Given the model looks to be an extruded section then 2d & 3d results should be the same. 

    • DanJ85
      Subscriber

      Hmm that would be a major problem. So even though it's extruded and these features are modelled on the upper surface, Fluent won't calculate any difference between 2D and 3D?


      This is what my current model looks like:


      Isometric view:



       


      Front View of aerofoil top surface (flow path):



       

    • Rob
      Ansys Employee

      It'll calculate a difference as you'll have an extra velocity component. But in this case, what changes across the swept direction? 

    • DanJ85
      Subscriber

      So the riblet microstructures are parallel to the swept direction on the top and bottom airfoil surfaces (or just top). CFD studies and wind tunnel experimentation have shown that they can reduce drag on airfoils but they have to be less than 100 micrometers or they become detrimental. It is thought that they raise, pin and separate turbulent vortices above or at least higher in the boundary layer, away from the skin surface. Here are a couple of studies, but there are many others of varying complexity:


      https://www.researchgate.net/publication/305359068_Riblets_for_airfoil_drag_reduction_in_subsonic_flow


      https://www.sciencedirect.com/science/article/abs/pii/S0960148112005630


      Unfortunately I am only able to mesh and simulate the plain airfoil (with great results). If I could just get the riblet model to mesh and validate against some of these other studies I could move on to further research. So I am very stuck!

    • tazia
      Subscriber
      Hi Dan nI?m trying to do the same thing and haven?t had any luck yet.nI was just wondering if you had managed to model the riblets succesfully? nI would really appreciate any help or advice you could give me.nthanks you so muchnTazian
Viewing 10 reply threads
  • You must be logged in to reply to this topic.