I created wing in inventor and did a smimulation in CFD. In results I got 66N of lift and -0.8N of Drag. Lift looks OK but drag is insane.
Please see CFD file. What can be wrong?
I set 15 degrees angle of attack. I NASA simulator I have 70N lift and 15N drag. So I agree to 66N of lift but not ot drag.
I have one more question. When I am doing simulation in the way I attached, May I analyze more complicated airfolis such as delta wings or swept wings?
And one more thing, I need to check what is the maximum angle of attack before stall appears and air starts to "tear off" from the wing, causing turbulent flow and loosing lift. I know I can do it manually to pick up next angles and observe when lift starts to loose but is there any automatic option to do so?
I had a quick look through your file, few observations:
1) Mesh is too coarse. You need to do a sensitivity analysis for your mesh size and distribution, before even hoping for any meaningful results of separation point and stall angle.
2) The walls of enclosure are way too close to the airfoil, you need a lot more room aroudn the airfoil so they don't affect the physics of airfoil. And you want them with symmetry condition instead of "no slip" condition as it is now. Also, why not 2D simulation for this?
3) Why laminar model, are you sure the flow is laminar? Using laminar model for a turbulent flow at sufficiently fine grid will result in modelling of voriticities that result into turbulence and you are not likely to get a convergence (at least in steady state). All the while, any results being completely wrong. Be aware that laminar layer detaches easily than turbulent one and hence choice of laminar or turbulent physics may have implication on the stall angle.
4) You don't need to model an inclined air domain. Keep it parallel to the chord line and just use the components of velocity at the inlet to represent the angle so you can use the same geometry for all angles.
As far as I am aware, there is no automatic way of obtaining it in the software and you have to do a series of simulation to find the stall angle, for this and any other wing section. Generally, you may want to refer to some literature to understand the characteristics of the airfoil so you know the range of stall angles you are looking for, and then design your experiment... And of course, the trustable results can only be possible with adequate mesh, BCs, model, advection scheme and convergence...
It seems simple but accurately getting the drag of a streamlined shape in CFD is actually quite tricky.* Most of what Omkar said is very true and good advice, though I would disagree with inclining the inlet flow. It is important that the walls of the domain are aligned with the free stream velocity, and angling the domain (or the wing) is the right way to do it.
This and other useful tips for getting accurate results in external flow are here: http://help.autodesk.com/view/SCDSE/2014/ENU/?guid
Something that is not mentioned there is the importance of capturing the wake. To get accurate wing drag and lift, the fluid in the wake region for several chord lengths should be meshed as tightly as the area near the wing. The flow details that determine the drag actually happen behind the wing.
One other note regarding your model - compared to reference 2D airfoil data, since it is a 3D wing the drag will be higher and the lift lower due to induced drag (tip vortex formation). If you are just trying to match the book values you should either do a 2D simulation (which is much quicker with a fine mesh) or extend the wing to the edges of the domain and make those side walls slip/symmetry boundaries.
* numerically this is because we are subtracting one relatively large number from another very similar number, and the difference (several orders of magnitude smaller) is the result we're interested in for drag. Also drag is a combination of friction (boundary layer effects) and pressure. Lift is easier because it's of the same magnitude as the pressure forces, and doesn't need accurate shear forces due to viscosity. That's why good meshing is so important, as well as using the right turbulence model, advectionscheme, modeling the wake, etc.
Thanks for posting the link, to be honest, I wasn't aware of the section of guidelines! Will be interesting to see what else is there...
Having noted the guideline about rotating the domain, as I think aloud, if you use the uninclined domain, use components at inlet and use periodic bounday conditions at the top and bottom, symmetry at the front and back (for 3D) etc, do you anticipate any problem? As long as the mesh is fine enough and adequate modelling is used (ADV5/ SST-kw), numerical diffusion will be smaller. And since boundaries are sufficiently away from the airfoil, the results are not sensitive to them. You can always initialize the next angle of attack with the results of current one, and prescribe BCs without remeshing the domain, thus saving time.
I haven't tried the periodic boundary condition on the "top" and "bottom" as you suggest. It seems like it should work, as long as the boundaries are far enough away and the mesh is good enought to capture the wake regardless of orientation. I have always treated it as a virtual wind tunnel, so have gone with rotating the foil relative to the free stream (or vice-versa). It would definitely be nice not to remesh each time, though if I were using a mesh refinement region I would rotate or redefine it so it always captured the area straight downstream and the downwash from the wing.
So your approach as an infinite cascade with large spacing ought to be alright.... especially for quick multiple angle analysis... but my remaining concern is that the outlet (P=zero) surface will "try" to make the flow to be normal to the outlet surface. This turning doesn't make sense in the desired scenario. This is why for cascades the domain is usually a paralellogram or similar shape, with the inlet and outlet faces parallel, but inclined to the domain sides so the inlets and outlets of each periodic section line up. In your setup the infinite cascade is staggered at different angles depending on the angle of the flow, and the inlets & outlets don't quite line up. But again, it shouldn't matter much if the boundaries are far, I guess.
I agree on the "turning" of the flow with pressure BC and it just seems strange. I witnessed this first when I was simulating a periodic section of a perforated plate for inclined flow where inherently, the inclined flow had a tendency to straighten out towards pressure outlet, without any apparent motivation. This happens even with a simple box with periodic conditions to some extent. I may be wrong, but I thought what I was seeing was unphysical!
Would you say that to mitigate this, specifying the inclined velocity at the outlet as well may make sense? Thus the locally disturbed flow because of the airfoil eventually aligns to the inclined flow direction prescribed at the outlet. And since the domain is big enough, this transition is not abrupt and not too sensitive to the far field boundary conditions. In a way, this will mimic the actual sky? I have seen some CFD codes employ a pressure far field BC that prescribes the zero pressure and velocity components (for compressible flow) to all the boundaries (except front and back symmetries).
Omkar, I'm pretty sure the flow turning to be normal to a P=0 surface is correct mathematically. So an outlet in an external flow analysis needs to be perpendicular to the far-field velocity.
You do not want to specify velocity on inlet and outlet planes. This will make the simulation incorrect - it is the velocity difference (downwash) due to the airfoil that causes the lift! Also, it will tend to make the simulation less stable numerically. For an incompressible analysis to be stable you need pressure and velocity BCs, and at least one inlet/outlet surface must have velocity free and one other inlet/outlet must have pressure free (you can use mass or volume flow too since those just divide by density and area to get velocity). [Compressible flow is different - you need temperature too, and you can have an unknown BC on a downstream surface in some cases.]
I hope someone from Autodesk will chime in if this is incorrect or poor guidance for Simulation CFD. The above is based on general principles. Omkar, I don't know about the other codes you mention, and it's possible that's correct in those cases... but for getting lift and drag on an airfoil simulating a wind tunnel is the way to go.
I don't want to get too far off the main topic or into the weeds, and it's been a while since my university days doing actual CFD math. So this is probably as far as I will go in this discussion. There are lots of good references for CFD and fluid dynamics on the web (or even in real books!) and even though SimCFD is easy to use, in my opinion people who use it regularly should get familiar with the principles so they don't create misleading simulations. I commend the original poster for comparing his results to published values and trying to figure out why they didn't match up.