Excuse me sir,
i just want to ask that why when i am using autodesk simulation cfd 2013 to get the lift coefficient for naca aerofoil 2415, i can't get the accurate result. according to experiment for naca 2415, angle of attack 0 degree, reynold number of 3x10^6 , the lift coefficient should be 0,2. when i am using this product, it's resulted lift coefficient is not even close to it.
in this post i have attached my ipt file and the cfz file. please
i solve it using solve mode :
- steady state
- tight convergence
- incompressible flow
- RNG turbulence mode
- enable adaption (max y+ 300)
- other settings are default
please help me solving my case...
Solved! Go to Solution.
Could you be more specifc about what value you are mesauring? Are you using the wall calculator to do this?
One item that we should change is the Advection scheme, 5 would likely be best here.
A couple items.
First, I would consider starting this in 2D as you can get a better understanding of the mesh required while still maintaining a quick running model.
I would position the airfoil in the center of the domain as the sharefile you posted has it adjacent to a wall.
Some external aero applications can take a little longer to develop so you may need more than 300 iterations per cycle.
I would also recommend starting out with ADV5
i am using wall calculator method to determined the lift coefficent on this naca aerofoil 2415
the result was after 250 iteration..( i stop at this iteration because i thought that more iteration wouldn't give more significant change anymore..)
from this result i assume that FY is the lift force, Fx is the drag force
then i calculate the lift coefficient, the lift coefficient that i got is 0,02 .., the published naca aerofoil said that the lift coefficient for that condition should be 0,2...
What Apolo said is very true, you will definitely need to run for longer within each mesh adaption cycle.
i am already have done the simulation with RNG mode, 3 adaptive cyle y+ 100 with a lot of iteration (300 and more), no matter how many times i tried...
but still when i am calculating the lift coefficient, it's not even close to the published experimental result...
(i am using wall calculator for calculation)
is there anybody that can help me solving this case... (example with any aerofoil would be very helpful)
or can anybody give me the rope how to calculate aerodynamic force (lift coeff, and drag) of aerofoil properly..
i don't know anymore what to do..
it would be very helpful if someone can give me the example how to calculate it accurately..., i am very grateful for your help, since i am working this case as my one of my project...
btw i also want to ask that when we are doing simulation in 3d model, is there any different / effect whether i use steel, wood dll.., i think since the surface roughness for all material by default is zero, maybe there are no different whether using different material (my taught)...
so far many people using ansys fluent to solve this case.. i wonder if this autodesk product can also calculate it accurately..
waiting for good reply
Please understand that the recommendations we made were good replies and are for a reason so that you can learn the requirements of external aero. While you are using Mesh Adaptation, we do need to ensure that the initial mesh is appropriately tight enough to capture some of the flow gradients that will be detected and refined upon.
My recommendation for you to start in 2D is one that most users would have followed so that they can understand the meshing requirements.
Simulation CFD can do well for these applications as long as you have an appropriate mesh to capture the flow characteristics. The solid material will not make a difference in these cases as the listed Surface Roughness is zero for all of them
Attached you'll see a 2D model that I ran out that produces ~261N of Lift which would give you an appropriate lift coefficient for the NACA-2415.
As I was running this overnight I did run it out for 6500 iterations, however looking at the convergence monitor this was done ~3500 iterations.
Now, you can continue moving forward with this in 2D (my recommendation) as that will be the easiest for changing profiles or angle of attach and seeing performance changes. If you decide to move to 3D understand the meshing requirements I'm showing in the attached 2D results and consider the initial mesh (if using adaptation) and ensure that there are enough iterations run for each cycle.
First i want to apologize to inventor's team if i unintentionally offended them.. "good reply" < i don't mean that the replies are dissapointing...
btw i have seen apolo attachment and explanation...
actually i have some question in my mind..
1 : is there any different result betweeen 2d simulation and 3d simulation ??
2 : for calculating car's aerodynamic force, should i using 3d model like explained in tutorial, or just using 2d model like the one u showed me..
3 : what is the different between 2d simulation and 2d planar (like extruding your model into the solid box by cutting operation, thus creating model's like hollow) (2d planar http://forums.autodesk.com/t5/Autodesk-Simulation-
as far as i seen, this model was created by extruding the aerofil solid's body into the box's solid by cutting operation thus creating a hollow like aerofoil in the box's solid .. (this one is just like my first model..)
also i have question regarding creating mesh..
i have opened and studied the cfz. file that u sent to me. i still don't get it how can u make the mesh so beautifully (preview mode),
i only can see edge 10 and 15 (aerofoil), so where is the rest of the edge ???
also is there any way to hide the UCS (x,y,z), it's really bothering me..
Most of us who reply here are part of the Simulation CFD Support team so our recommendations come from our experience of working with new and experienced users on a wide variety of models. It's ok, no offense was taken by your comment.
Yes there are some obvious differences between 2D and 3D. If you are studying profiles/angles of attack, 2D is by far the easiest to start with. You can then work your way to a 3D model.
With 2D planar it is assumed to be 1 unit depth. The next progression would be taking the 2D model and building a 1unit deep extrusion with Slip/Symm on the front and back faces as that would be similar to the 2D run.
We use 2D often to get an understanding of meshing requirements for certain models and then we can try to mimic that setup in the 3D environment.
You are also linking to one of our other products as that forum post is on Simulation Multiphysics which is different then Simulation CFD. In CFD, you can do a 2D Planar (built as a sketch in Inventor and then using a Boundary Patch to build a surface), or you can do a 3D model that is a 1unit extrusion as i mentioned above.
The meshing for that 2D model was using a couple featuers (that we oultine in the Help documentation).
Thre was a coarser surface mesh on the full domain to capture the bulk of the physics.
There was Edge mesh assignments used to ensure the airfoils shape was prperly represented
Then lastly a Mesh Refinement Region used to refine the mesh closer to the airfoil and to capture the more detailed aspect of what is going on around (and in the wake of) the airfoil.
All of those edges were what you had in your ipt for defining the Airfoil contour. Some of them are somewhat small and require zooming in to see them
The UCS is turned on/off under the View tab with the "Axes" button.
sir, thank's for your help i have been able to calculate the lift coefficient for my own model..
after that, my question is, how i can determined the center of force for 2d model ?, is it possible to locating the aerodynamic center through 2d model ??