
[Sponsors] 
May 15, 2009, 18:56 
Changing AoA

#21 
Member
Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 9 
I know two ways to set the AoA.
The cheap one is to modify the inlet velocity components. u=U*cos(AoA) v=U*sin(AoA) But, assuming you have a square/rectangular domain, if you do this, you have to make the lower (pos. AoA) or upper (neg. AoA) boundary an inlet, too, and the opposing boundary an opening or outlet (depending on whether you might get inflow there, if the boundary is close to the airfoil and the local flow deflection is larger than your AoA). So this the the easy but not very elegant way to do it. The better and more elegant way is two use two domains (meshes) with an interface. A circular domain around the airfoil, and a larger rectangular mesh around it, as farfield so to say, with a circular hole in it. You can rotate the inner domain by any desired angle. To do this, right click on the mesh in the outline menu of CFXPre > transform mesh > apply a rotation. Be sure to choose the right pivot axis and the right turning direction. You can even use a CEL expression for the angle for unsteady airfoil simulation. I've done that gefore and it works flawlessly. You should take care though to have decent mesh quality at the interface (uniform spacing, the same on either side) to avoid inconsistencies there. You could also try to use only one domain and mesh deformation, but I've never worked with this, so I'm not sure how it works. Good luck Jules 

May 15, 2009, 23:41 

#22 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
Thanks alot for the tip. It works great much better than setting the velocity direction using sin and cos.
Now to troubleshoot it. Not getting the values i want can seem to find a nice configuration to simulate all the AOA. Will start doing in reverse high AOA to low AOA. Is it advisable to use the high resolution advection scheme or upwind. Read the help files and it writes that the upwind advection scheme is recommended for turbulence modeling. But it is only 1 order accurrate right. Last edited by Arti; May 16, 2009 at 00:05. 

May 17, 2009, 13:46 

#23 
Member
Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 9 
Arti,
I am not sure about the advection scheme. By what means are you not getting the results you want? Drag? If you run your calculation with a turbulence model without transition model, you will have a turbulent boundary layer on the entire airfoil and then the drag will be much higher than in reality. In that case you should consider using the automatic transitional model in combination with the SST turbulence model. Also be aware that the flow around an airfoil at stalled condition will be unsteady, so you cannot get the right results with a steady state simulation. You should also note that the aerodynamic behaviour of an airfoil with AoA changing over time is different from that with constant AoA. If you want a resolved cL vs. AoA polar for steady airfoil condition, you can't simply sweep through the range of AoA in one transient simulation. You have to simulate at every AoA by itself. Jules 

May 18, 2009, 04:37 

#24 
Member
LSC
Join Date: May 2009
Posts: 58
Rep Power: 9 
Hi, I am actually simulating an incompressible flow..so I am wondering whether I need to set the Compressible Production under the Advanced control tab of Turbulence to "0" (default value is 3 as stated by manual)?? I have read the manual but it does not say anything about incompressible..please advice


May 18, 2009, 04:45 

#25 
Member
LSC
Join Date: May 2009
Posts: 58
Rep Power: 9 
I have set the Reference Pressure to 0[Pa] under the domain model..for the inlet, I have set cart. Vel and also turning off heat transfer to "None". For Outlet, I have set Static Pressure to 101325[Pa]..I use Air at 25degC as the fluid. Is there anything wrong with my boundary conditions for which I am simulating flow over airfoils which interest in lift and drag coefficient..


May 18, 2009, 05:10 

#26 
Member
Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 9 
If you do an incompressible simulation, the reference pressure doesn't really matter. I would just leave it at the default value: 1 [atm].
However, you set your back pressure wrong. The way you did it, the back pressure (pressure at exit) is 1 atm larger than your domain pressure, which is kind of like you had a compressor working against your flow. You probably get reversed flow. Put your outlet pressure to 0 Pa relative. Then you should get the right result. For the compressibility, I'm not exactly sure. AFAIK there used to be an option to set the fluid to "air incompressible" or something like that (CFX 10.0). In the new version I don't know where that option is, but I'm sure it's somewhere. Maybe it is "constant property gases > air at 25°". Please refer to the manual. Best wishes Jules 

May 18, 2009, 05:15 

#27 
Member
LSC
Join Date: May 2009
Posts: 58
Rep Power: 9 
Many thanks for your advice. One more thing is that since CFX only do 3D simulations, I have to sweep the mesh out. Usually, I sweep it out by 1[m] however I read that many advises to sweep with one cell thickness. So one cell thickness is the small grid spacing in my entire mesh?


May 18, 2009, 05:29 

#28 
Member
Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 9 
Pretty much.
I wouldn't really use the first BL cell height, because then the mesh would be ridiculously thin and a little hard to handle in Pre and Post, and also the aspect ratios of the cells in the far field would become very large. Use something like the average cell LENGTH on your airfoil surface. Jules 

May 18, 2009, 05:33 

#29 
Member
LSC
Join Date: May 2009
Posts: 58
Rep Power: 9 
yes..thats the problem i encountered while trying very hard to zoom in.. thanks for your advice!!


May 18, 2009, 13:06 

#30 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
LSC
I suggest u look at the help files for the reference pressure. Its under "Setting a Reference Pressure". That will help u determine your pressure datum. Try to make the first height as thin as possible it helps. Y+ of 1 should be good enough and easier to mesh. About the one cell thickness, Its actually trying to simulate 2D effect. So if u want to do 2D u sweep by the smallest grid xlength in the mesh. I did it by sweeping a length of 1 so that i do not need to worry about the Area when calculating Cl and Cd The negative drag problem was removed after i used the method of rotating my mesh suggested by Jules. Hi Jules. I understand what you mean about the drag. The advection scheme and SST together does not pose much of a problem to me now. Im getting alright results for the AOA that im interested in now. After SST i will be switching to the Ke model which is slightly hard to work with without a good mesh. Thanks for the tip on making the grid but i wasnt successful in trying to create it ended using a Cgrid like the one used in the cornell airfoil tutorial. Which works fine. Last edited by Arti; May 18, 2009 at 13:38. 

May 19, 2009, 00:34 

#31 
Member
LSC
Join Date: May 2009
Posts: 58
Rep Power: 9 
Hi Arti, hows your CL and CD error like? I used SST for turbulence and it is much better than kepsilon but CD error was still large.


May 19, 2009, 05:17 

#32  
Member
Jules Bell
Join Date: May 2009
Posts: 31
Rep Power: 9 
Quote:
like I said, if you want the correct cD, you have to use a transitional model. Otherwise the BL on the entire airfoil will be turbulent and your cD will be around factor 23 higher than in reality, of course depending on the type of airfoil and the AoA. Be aware that for the transitional model to work properly, a Y+ of approx. 1 is required. (no wall function applicable in the laminar / transitional portion of the BL). Best wishes, Jules 

May 19, 2009, 06:18 

#33 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
My values for drag has reduced alot after i applied the method of rotation you told me. The Y+ is still at 1, hope its good enough for ke models. Guess i will try the transitional model after the kw and ke model if the end results are not satisfactory. As i do not want to complicate things. So far its working well.Thanks.
Last edited by Arti; May 19, 2009 at 06:49. 

May 19, 2009, 11:55 

#34 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
Is there a way to adject the Under relaxation factor for continuity and momentum in Cfx 11? Have a slight problem with one AOA. Angles from all the way 10 degrees were ok but at 3 degree it fails to converge with the settings i have. I want to try tune the relaxation factors.


May 19, 2009, 22:02 

#35 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,955
Rep Power: 100 
Hi,
Forget about adjusting underrelaxation factors. In CFX if you are thinking of adjusting an underrelaxation factor then 99% of the time something else is wrong. In the olden days of SIMPLE based solvers you had to tweak the URF all the time but not now. Have you done a mesh refinement study? A convergence tolerance study? A boundary proximity study? Investigated turbulence transition and inlet turbulence levels? These are fundamental issues which need to be addressed before you fiddle with the solver settings. Glenn Horrocks 

May 20, 2009, 07:43 

#36 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
I did a mesh test for 50K 60K and 80K plus cells of my setup. Am now using the 80K cell as my choice. Am trying to do the lift and drag curves to confirm it with the experimental results i have. I think im getting it. Some settings were slightly off. Will try again. Thanks for the advice.


May 20, 2009, 08:10 
Cfx

#37 
New Member
Chirag Shah
Join Date: May 2009
Posts: 3
Rep Power: 9 
How to find Axial and tangential velocity in CFX Post???


May 20, 2009, 08:56 

#38 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
U can use the function calculator to find those values around the airfoil.


May 20, 2009, 09:13 
Cfx

#39 
New Member
Chirag Shah
Join Date: May 2009
Posts: 3
Rep Power: 9 
how can i find axial and tangial velcoity in general problem not in airfoil in CFX Post?


May 20, 2009, 11:11 

#40 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
Same way. You can
(1) use the function calculator to find the average velocity on any wall, (2) plot a chart of x and any velocity(u need to draw a line or poly line around the wall to do that). (3) Or u can choose to monitor a point in CFX Pre. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pros and Cons for CFX, CFdesign, COMSOL  Val  Main CFD Forum  3  June 10, 2011 02:20 
nucleate boiling simulation in CFX  Anil  CFX  3  August 25, 2010 14:18 
PhD using CFX  Rui  CFX  9  May 28, 2007 05:59 
2D simulation  ICEM meshing for CFX question  Ben Makhal  CFX  5  April 11, 2007 08:44 
Simulation of turbine cascade in CFX.  Jonas Pedro Caumo  CFX  0  December 9, 2006 14:54 