Hi. I am trying to perform a simple Lift and Drag Force calculation on a aerofoil. Are the steps I have followed correct:
1. Loaded an Inventor model of a simple aerofoil into the Steady State Fluid Flow environment.
2. Created an external fluid surrounding the aerofoil, essentially a large box.
3. Meshed the model.
4. Added a nodal velocity to the 'front' surface of the box to simulate the freestream.
5. Added a inlet/outlet condition to the 'back' surface of the box to simulate the exit.
6. Set the Material for the fluid to air, and suppressed the model of the aerofoil itself.
7. Run the Simulation
Now everything seems to have worked to this point. To find the Lift force and Drag Force I am a bit more sketchy, this is what I have done
8. Selected the Reaction Force in the Z direction to be displayed from the REsults Contours Menu (This is for Lift, for Drag I would select Y direction)
9. Selected the surfaces from the Air Part model that surround the aerofoil (essentially all surfaces except the box boundaries, and the 'Interior Surfaces'), and then asked to select nodes as subentities.
10. Clicked on "inquire Results", and "Sum" to give me the total force in the relevent direction (force in Z direction for Lift force, and force in Y direction for Drag force).
Is this correct? Because my drag force seems to be very very small (e-7 N!) and I do not trust this
The word airfoil usually indicates 2-D planar, so if you want performing Lift and Drag Force calculation on an airfoil, 2-D planar simulation will simplify your workflow. 3D simulation is for plane, wing or other 3D objects. Anyway, it's some fashion of waste in computational resource and setup time to do airfoil in full 3D simulation. But it is still good to go if you set it up correct (see next).
Be careful doing the 2-D case in 3D simulation, especially in result evaluation. First, the experimental result (or your comparison result) for airfoil has assumption of infinite depth, or depth effect needs to be ignored. However, in your 3D box, you do always have front and back walls and which impacts the flow patterns, this applies to the top and bottom walls, so you should have reasonable offset for this effect, this is called wall effect in experimental aerodynamics.
To get the total drag and lift force from FEA analysis, only select the nodes on the airfoil surfaces(Don't select any other nodes) , then you can do any summation on x,y,z directions.
Also notes the reaction force counts the pressure (normal to airfoil surface) and shear stress (tangential to airfoil surface due to velocity gradient and fluid viscosity).
Ok- clarification I was using 3d elements as I was modelling a wing, whose profile is obviously an aerofoil.
So in summary the steps I was following are correct? As in I just select the surfaces that make up the surface of the aerofoil/wing itself and sum in the 'up' direction for 'Lift' and the Left/Right direction for drag?
Your steps are correct :-), but as said before, the result accuracy could be skeptical, which depends on your model setup of the box, the wall effect is one of the factor.
And again, if you are doing wing which has different airfoil profiles in wing's aspect direction(wing's root to tip), the 3-D modeling is necessary. If the airfoil profile keeps same in wing's aspect direction, I would suggest to do 2D planar simulation which is much cheaper and avoids the issue the wall effect in depth direction. It sounds your case is in second category according to your most recent reply, I am just trying remind that the wall(front and back) effect in 3D modeling is probably not trivial depending your enclosure box setup.
Here is something else to check. It doesn't occur very often, but I have seen it happen before. Is the size of the model correct in Autodesk Simulation? For example, you expect the wing to be 60 m long, but in the model it somehow turned out to be 60 mm long?
The only other factor that comes to mind is the air density. Depending on what units are shown, the density could be in units that are unfamiliar and/or difficult to work with. In this type of situation, expand the "Unit System" branch in the browser (near the top) and activate one that is more comfortable to use. For example, either SI so that the density is in kg/m^3, or whatever the english system is that uses lbm/in^3.
John Holtz, P.E.
Senior User Experience Designer, Simulation
Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)
FYI, Attached a simple 2D fluid flow model which demonstrates the lift/drag force calculation.
- Full pre-defined model (2200_2Dsubm_10deg_un.zip)
- Simple description/result (.pdf)
- Pressure animation (2200_2Dsubm_10deg_un_pressure.zip)
(download and unzip it to .mp4 to play animation)
- 2D sub moving at speed of 8.3ft/s, attack angle 10 degree
- 2D planar unsteady fluid flow analysis
- Symmetric BC at top and bottom boundaries
- Model geometry imported from CAD
- Results include velocity, pressure, flow rate and reaction force, you have to re-run the model to get all results I deleted all result because of the upload size limitation
Unzip attached .zip file to open Autodesk simulation Multiphysics, click "Run analysis" you will get all result.
Does someone have a 3d version example of a wing simulation in a windtunnel? I am working on something like this but I can't make it.
Thanks for any response.
Post two pictures for 2D airfoil in 3D modeling by one layer element in depth direction.
(2) It is perfered to setup 2D planar model for airfoil. (See my previous post and example model in this thread)
From pressure pattern, one can image the the lift and drag force directions.