Transient Angle of Attack Simulation Not Displaying in Post
Hello 
Before I begin, I have read the manual and have done all of the tutorials. I am running a 2dimensional (2D Extruded Mesh) simulation of a NACA 0012 airfoil. I used the "Flow from a Circular Vent" tutorial to help model both a steady state and transient analysis. I created a fluid domain for the surrounding rectangular prism (15 m long, 4 m high, 1 m wide (but with symmetry and 2D mesh extrusion)) and a solid, steel domain for the airfoil (1 m long) itself. In the Transient Analysis, I configured CFXPre so that the Fluid Domain remains stationary while the Airfoil Domain rotates about the zaxis (the x and yaxes represent the 2dimensional Cartesian plane; hence a rotation about z changes the angle of attack) at some prescribed angular velocity (I have tried various, from 0.05 rad/s to 1 rad/s). The fluid domain has an axial velocity of 0.65 m/s. Although both the steady state and transient analyses run and converge successfully, I have the following problems in CFXPost:
Thanks for your help. 
Update
Hello 
I managed to run the airfoil simulation with a changing angle of attack. I changed the airfoil from a "Solid" to an "Immersed Solid". The animation now produces a moving airfoil. My problem now is this: Because I have 2 domains (immersed solid airfoil and fluid), the airfoil appears in both. In one, the airfoil is the domain and it is rotating. In the other (the fluid domain), the airfoil is just a boundary within the domain. In CFXPost, the airfoils from both domains are present (the rotating and stationary). This causes a problem because the results are treated as if there are 2 airfoils  1 rotating, 1 stationary at 0 degree AoA. How can I eliminate the stationary airfoil? 
Hi Josh,
Immersed solid is unlikely to be a good approach for airfoil modelling. It does not allow capturing of the airfoil boundary layer very well. What Re number is it running at? What Mach number? Any other physics of importance? If you could post an image of your geometry that would be good. I recommend you model this with the airfoil being a cut out section in a fluid domain. Then the easiest way of implementing the airfoil motion sounds like putting it is a rotating frame of reference and join it to the outer stationary frame of reference with a GGI on transient rotor/stator mode. You can do this with mesh motion but that is much more complicated and will be a far slower simulation. Also it sounds like your domain is quite close to the airfoil. If you are trying to get the infinite field results you will have significant error. Do a sensitivity analysis to find how far the outer boundaries need to be away from the airfoil. Glenn Horrocks 
first theres a few model the profile movement and these are described here http://www.cfdonline.com/Forums/cfx...sloshing.html
I'm not sure if you have made this error but if you use imersed solids the mesh for the fluid and imersed solid component must be separate and independant. 
Thanks for the replies.
Here are some details ... Geometry I did model the airfoil as a cutout from the fluid domain. I used "Point" to import my airfoil, created a spline of half the airfoil profile, extruded the halfprofile, and used a Body Operation to mirror the halfprofile to create a full, symmetrical profile. I then froze that full airfoil profile, created a second sketch of the fluid domain surrounding the airfoil, and extruded that. Finally, I used another Body Operation to cut the airfoil out of the fluid domain, which created 2 Parts, 2 Bodies. My geometry profile can be found below: http://picasaweb.google.com/counse/C...eat=directlink Mesh Pictures of my mesh scheme can be found in the same album: http://picasaweb.google.com/counse/C...eat=directlink I have 6 regions: Inlet, Outlet, Left, Right, Default 2D Region (the top and bottom), and Airfoil. My Default Body Spacing is 0.1 m. I used Line Control around the airfoil with a radius of 0.6 m, length scale 0.01 m, and expansion factor of 1.2. I used inflation on the airfoil with 40 layers, expansion factor 1.02, first layer thickness option with y+ = 1, Re = 10^4, and 1 m reference length. My meshing strategy in the options category was a 1 layer extruded 2D mesh. The extruded periodic pair was between the left and right sides (along the zaxis). Setup (Pre) The inlet velocity is 0.65 m/s, so the Reynolds number is Re = 10^4 The Mach number is M = 1.91 x 10^3 As per Tutorial 4 (?  whichever has flow through a circular vent with smoke), I created 2 analyses  a steady state and a transient. Really, the only difference is that the airfoil in the transient analysis is rotating (while the steady state airfoil remains stationary). The transient analysis type has no coupling, a 60 s total time, 48*1.25 timesteps, and initial time of 0 s. The domains are the airfoil and the fluid. The airfoil domain is solid (changed it for you, Glen), steel, and rotating about the zaxis at 0.001 rad/s with no mesh deformation. The only boundary is the default domain (the airfoil). The fluid domain has the following boundaries: symmetry on the top, bottom, left, and right; inlet with u = 0.65 m/s and medium intensity turbulence; outlet with 0 Pa average static pressure; smooth, noslip wall on the airfoil. komega turbulence is used. In the Solver Control, a second order backward Euler scheme is used with min. coeffs 1 and max. coeffs 2 and RMS 1E4 residuals for the convergence criteria. In the Output Control, pressure and velocity are output every 1 s. Solver Both the steady state and transient analyses complete and converge successfully. Post The stationary airfoil remains. When I click on various timesteps, I see both the stationary (0 degree AoA) and transient airfoil. The stationary one interferes with the transient one (i.e. the streamlines and pressure contours go around both). 
Quote:
Can someone please set me in the right direction? I'm struggling to figure this out. Thanks again for your help. 
1 Attachment(s)
this is what glenn meant for the rotating frame

Thanks for the drawing, George. I do understand the theory, just not the method. I'm not sure how to rotate the area around the airfoil.

you need to create two meshes, one is the outside (preferable hex) and one surrounding the wing profile (easiest is tetra with inflation but you could put some more effort and create a nice mesh to capture the flow).
in cfx you can define the mesh movement in many ways: for steady state use one domain and rotate the inner mesh in cfx pre according to your requirements. for transient you can do this in a few ways: one is mentioned in the sloshing link I posted above another way is to use two domains the outer mesh is the stationary frame and the inner mesh is the rotating frame ( this is what glenn was on about) another uses subdomain to define the motion but distorts the mesh 
I tried Glenn's method (2 Domains  the solid airfoil and the fluid surroundings). In Post, I only saw rotation if the airfoil domain was treated as an immersed solid. Even then, as the airfoil rotated (it was colored blue), another stationary airfoil was present. Hence there were 2 airfoils whose streamlines and pressure contours were intertwined.
I think the reason for this is that although I have a solid airfoil domain, the airfoil is also a boundary in the fluid domain, so the solver treats the simulation as if there are 2 airfoils. How do I properly define the 2 domains to avoid this? Or is this caused by something else? I would do the moving mesh method, but Glenn said it's complicated and causes long simulation times. Since my summer student contract expires soon, I don't know if I have time to learn and implement something that complicated. Thanks for any help! 
i think your problem is the way you created the mesh. as I said if you use imersed solids the mesh for the fluid and imersed solid component must be separate and independant (in simple terms if you used workbench to create the geomerty the wing and the fluid space are two independant parts.
all other cases require all bodies need be in the same part and share the same topology 
Quote:

Quote:
Thanks again! I really appreciate your help. 
Quote:
This is very low because I am modeling a low Reynolds UAV. Despite the likelihood of laminar flow, the professor and client requested komega turbulence modeling. They are interested in Reynolds numbers of 10^4 and 5x10^4 at angles of 0, 5, 10, and 15 degrees. Quote:
Quote:
Quote:
Quote:
My main problem still persists. I cannot model an airfoil with changing angle with a transient analysis. I tried: 1) Using 1 Domain, which was then rotated at a certain angular velocity. This, however, did not produce results that displayed a changing angle. In other words, I could not animate the airfoil changing in angle. 2) Using 2 Domains, 1 stationary (fluid surroundings) and 1 rotating (solid airfoil). This, just as before, did not produce results that displayed a changing angle. 3) Using 2 Domains, 1 stationary (fluid surroundings) and 1 rotating (immersed solid airfoil). Although this did display an airfoil with changing angle, the original solid airfoil at 0 degrees remained, as well, causing interference (in other words, there were 2 airfoils  1 rotating, 1 stationary at 0 degrees). If I model the geometry as 1 Part, 1 Solid (like you suggested with merged topology and with the airfoil acting as a cutout from the fluid domain), how can I make the airfoil, and not the whole fluid domain, rotate? I really appreciate your help. I've tried reading the manual for 2 weeks now and have done all the available tutorials, but to no avail. 
Quote:
I never said you need to use the immersed solid, I'm just telling you whats wrong with your problem definition and your mesh when you used the immersed solids option to use the stationery/rotating frame reference you obviously need to use two fluid domains. purely for informational purposes if while creating your mesh you have a shared topology (thats the default option in workbench) which basically means you use the same nodes at the mesh interface, you can use more than one mesh in a domain. 
Quote:

Quote:
If you insist on using a turbulence model then the only model which makes sense is SST with the turbulence transition model  and I bet it never trips to turbulence anyway! Quote:
As for your difficulties in getting the thing to move, have a look at any of the rotor/stator tutorials in the CFX examples. All we are suggesting here is to make the rotational speed a CEL expression rather than a constant and make it sweep out the motion you intend. Glenn Horrocks 
Quote:
Quote:
Quote:
Thanks for all the help. Joshua 
Quote:
Quote:
Glenn 
Quote:

All times are GMT 4. The time now is 00:30. 