Fixed transition airfoil
 

Hi all
I am gonna run a 2D transonic airfoil but the transition is fixed, is there any way that I can do this in CFX?
And one more question, for mach number 0.76 may I use steady state simulation?

If you mean the laminar/turbulent transition is fixed - then use the turbulence transition model with the defined intermittency model. Then you can define the transition location.

If you mean the location of a shock wave or something like that - you cannot really fix that, it is an output of the simulation.

The Mach number does not affect the decision to choose steady or transient. If the flow is steady then use a steady state model. If transient - well, it's obvious. A Mach 0.76 flow could be steady or transient.

Thank you Glenn
I ran the simulation with air at 25 as the fluid and it converged very well ( but no accurate result) however when I changed it to Air ideal gas it got diverged after 70 iterations, have any idea?

Air at 25 is an incompressible fluid, so this simulation did not model compressible effects. The Air ideal gas model probably had some compressible flow effects occuring - these are always difficult to converge, especially at transonic flows. Try using local timescale factor to start convergence along, then switch back to physical time scale in the final run to full convergence.

Thanks again Glenn.
The convergency problem was because of the poor quality mesh around the foil and it got solved. I changed the mesh from C to O to keep the boundary layer elements refined while avoiding sudden jumps in the mesh at the blunt trailing edge, and it did works fine.Now I have CL with 7% error but CD with more than 90% error comparing to experimental values. Free stream flow conditions are: Re=30e6 and M=0.78 (also AOA=0). I 'v tried different types of mesh and domain size and I am almost sure that those are not the source of error. Also maximum Y+ on the airfoil doesn 't exceed 0.05. In the experiments they fixed transition point at 0.3Chord but I used gamma-theta model to find the onset of transition. What else should I do to get accurate results specially about CD? I think the problem backs to viscous parts of lift and drag since the pressure distribution on the airfoil is similar to that of the experimental work.

Getting lift about right but a significant error in drag is common in airfoil simulations. There are some posts on the forum and lots of published literature about what is required to get more accurate from there.

To progress from here you need to do careful sensitivity analysis on mesh, proximity of the boundaries and convergence tolerance. Also you might do better with a purely turbulent model rather than the transition model - unless you have a foil with a large amount of laminar flow.

This FAQ discusses accuracy in general: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Dear all

I am simulating 2-D transonic NACA-0012 airfoil in cfx5 solver.
I am trying to validated my results with experimental results given in the literature,on that inlet B.C.conditon is well described(velocity=265 m/sec),but outlet B.C. is not given properly.

If I am specify outlet B.C. as supersonic my resluts are matching in laminar and transitional region,but differ in turbulence region.

If subsonic outlet B.C. is specify so we need to give vel or pr information,therefore what it should be the values in don't know.

Inlet-
velocity=265 m/s
relative pr=0 pa(i.e. atm pr)
M no.=0.779

please help me.

The supersonic outlet is not a proper BC as you have just a small supersonic region around the airfoil but not through whole domain. Outet is the best, but you may be able to use opening, as well. For the validation purpose you need to know the flow condition from the literature.