Fluent airfoil help
Hello everyone,
I'm new to CFD and need some help modelling an airfoil in Fluent. I'm modelling both NACA 0012 and NACA 0015 airfoils in 2D. My lift coefficients are very close to experimental values, but drag coefficients are too small (by a factor of about 10). I am using a Cgrid mesh of 40,000 elements and a Reynolds value on the order of 200,000. Currently I am using the viscousinviscid model and I assume that this is the source of the error. I have played around with SpalartAllmaras and komega models but I don't know what to do and can not get these to converge. Any advice on constructing a more accurate simulation would be greatly appreciate. Thank you. 
Quote:
Bests. 
Hi,
Thank you for your response. Do you mean the "Modelling External Compressible Flow" tutorial? If so, then I have been trying to use that one as a guide. However, because it uses compressible flow and I am not, because of my lack of understanding of the software I don't know what I need to change. Currently the Reynolds values for my simulations are around the 100,000 mark and all less than 200,000. Later, once I get these simulations working, I will be modelling Reynolds values on the order of 1,000,000. My understanding is that, for airfoils, values less than 500,000 indicate laminar flow. I have tried using the ViscousLaminar model in fluent, but it did not converge. I am beginning to have more success with the SpalartAllmaras model, but now my lift values are 10% too low and drag 45% too high. I was wondering if anyone knew of a reliable model for Re=200,000 airfoils in fluent that I could basically copy and then modify? My main aim is to compare maximum L/D ratios for a selection of aerofoils and find the best one. However, with my current model, the AoA for the maximum L/D is out by 2 or 3 degrees. Thanks again. 
can you share a picture of your mesh ??

Hi Jonathan,
I am no airfoil expert, but here are some general thoughts: 1) If you choose "inviscit model", you switch off the natural "noslip" boundary condition that occours at real (surface) boundaries. Your fluid's velocity isn't set to zero at the airfoil any longer. Thus, the fluid slips at the airfoil boundary without creating drag. I guess the lift is produced by pressure effects (?!) which can be reproduced even by this strongly unphysical boundary condition. This would be in good agreement with your observation. 2) If your flow is actually laminar, you should not use any turbulence model at all  so take "viscous  laminar". If your simulation does not converge, it could be a meshing problem or a numerical problem (or ...). This is, what Diamondx indicates by asking you for your mesh. Also plot the velocity along some line perpendicular to the surface of your airfoil (maby in the middle of the airfoil) to see if the boundary layer is resolved correctly. 
Quote:
As I know in most simulation flow is considered to be turbulent in Re numbers equal or higher than 100,000 .It is comparable with flat plate problem. You should show us the grid. In laminar flow, there is a rule of thumb saying there should be at least 20 cell in adjacent the solid boundary to capture velocity Gradient(from zero to free stream) of boundary layer. But in the turbulent case, you should consider an expansion ratio equal or less than 1.2 for boundary layer cells. Of course, y+ criteria is very important in turbulence modeling and you should adjust the first cell height regarding to the y+ recommended for turbulence model in use. In this case, I suggest SpalartAllmaras because it usually converges fast and is appropriate if there isn't any Big! separation or steep pressure gradient in the flow. According to AOA you've mentioned below, you can use this turbulence model easily. 
Quote:

Good lift and bad drag agreement is a typical representation of bad viscous mesh, so it means your boundary layer is not resolved properly. What type of mesh you are using hybrid or fully structured? what is the chord length? SST kw is the best model recommended for airfoils if the flow is fully turbulent but if the flow is transitional then you have to use 3 or 4 Equations transition models in fluent to properly capture the physics. Show us the mesh and tell your chord length so that we can suggest you proper solver settings.

2 Attachment(s)
Hello all and thank you very much for your replies.
Here are the pictures of my mesh. I hope they are high enough resolution for you to get the information you want. The chord length is 1m, the mesh boundaries are 12.5 chord lengths from the airfoil and the mesh is 40,000 cells. I don't understand the terminology "unstructured", "hybrid" and "structured". When I created the mesh I followed Fluent tutorials and simply selected the number of divisions along a certain boundary and the bias type and factor. My main aim is to find L/D max for each aerofoil and compare them. Using my current models, the AoA for L/Dmax is 2 or 3 degrees off the experimental value, which is insufficient for my purposes. I believe I understand the maths and theory behind the models and I think SpalartAllmaras should be sufficient. I believe my problems lies in not understanding how to use the software effectively. Again, thank you for your help. Attachment 15994 Attachment 15995 
Quote:

From pics, I can infer that Y+ is too large. What is the minimum and maximum Y+ on the air foil surface.

Showing my ignorance here.
I'm not sure what you mean by the y range. The airfoil has a chord of 1m and thickness of 15%. The arc radius of the Cgrid is 12.5 chord lengths (12.5m). Cheers 
Quote:
In this range flow is transitional and you should not model is as laminar flow. Bette try to use the higher Reynolds numbers (fully turbulent flow) to get comfortable with it. Moreover in the low Reynolds number regine boundary layer is thick and you should put the more mesh in it and with increasing the Reynolds number, boundary layer get thinner. 
Quote:
Also: As far as I know, grid lines should always end perpendicular to surfaces  if possible. It looks like they don't do it on your airfoil. 
2 Attachment(s)
Hello again.
I had to take some time off from this project to get some other work done. I found out how to find the y+ values and I increased the number of mesh cells and the bias factor until it reduced (from about 20) to 1. The simulation is producing better results now, but the mesh looks a bit funny to me. Does it look alright to those of you with experience? I am operating with a Reynolds number in the region of 300,000. Cheers Attachment 16109 Attachment 16110 
Hello All,
I want to do analysis of heat transfer from water flowing through pipes submerged inside concrete. I am modelling in GAMBIT and wish to analyse it on Ansys FLUENT. Can anybody help me out, how to model and simulate? Does any tutorials exist? 
Hey. To me it looks allright. But I am no airfoil specialist.

Quote:

Sensitivity analysis?
How do I do one of those? Cheers. 
sensivity analysis means trying different size mesh to have an optimal mesh, less elements and without affecting solution. solution becomes mesh independent

All times are GMT 4. The time now is 08:51. 