Hello, I'm predicting the flow physics around a NACA0012 airfoil section with CFX-4.2. The computational domain consists of a C-Grid (200*50cells) around the airfoil and an H-Structure in the wake region (50*50). The domain extents 10*chord in all directions. Using higher-order upwind differencing and standard k-epsilon TM, showed best convergens. However, integration of all forces (pressure & shear) at the wall patch yield a drag coefficient around .03 at 4 degree angle of incidence, respectively. This is around three times higher than expected.

Does anyone know a solution to the problem.

Oliver

P.S.: YPLUS is well above 11.6. The lift coef. is o.k.

Hi, Oliver.

Not enough information. Did you check for grid independence? If not, do it.

What is Re value? Is it the same as in experiment? Is it large enough for the boundary layer to be fully turbulent? If not, the transition might occur at the wrong position depending on the k and epsilon upstream: this model often gives transition too far upstream, and this leads to overestimating the drag.

Did you try a flat plate at zero incidence first? I cannot tell at the moment if the flow past that wing is separated at 4 degrees of incidence. If yes, you cannot expect to predict the drag reliably with any TM, I am afraid.

Regards, Sergei.

(1). I don't see any problem at all. (2). As long as you are running CFD codes, a new version of the code will arrive in the future with improved accuracy! So, you must be honest and follow the exact instruction to run the code to make sure that an improved version will arrive. (3). As I said before, to succeed you must first fail, and fail many times. My suggestion is: keep running the code and try to get different solutions for your airfoil problem. The solution will improve in time. At least, solve the same problem one hundred times from now on to develope some kind of feeling first.

Dear Sergei,

The model was run at 10^5<Re<10^6, .1<Ma<.3. The calcualtion in all cases was checked for grid independency. For the Re-No. calculated no transition occurs. Might it be that the standard wall roughness pararmater (9.8) for the wall function is not appropriate for simulation of airfoil sections?

Oliver

Hi there,Well i'm glad i found someone who has found exactly the same problem as i have been having the last few months.I am also running CFX 4.2 and getting very poor drag extimates for a naca0012 airofoil. I've been using HYBRID differencing on all equations.Y+ is between 30-500. Even at zero incidence the drag is miles out !! I've have however, done lots of research into the drag and grid on flat plates which can be found on my web site www.soton.ac.uk/~shipsci (just click on my name under researchers) the results might be of some use to you. Do you know of any good references for creating C-Grids around airofoils ? Look forward to hearing from you soon. Do let me know how you get on.I'll do the same. If i manage to get a grid that solves well i'll sen dit to you. Regards James Date.

(1). If you can get both the lift and the drag right, then you have the exact solution. (2). It is unlikely that this will happen for turbulent flows. (3). For laminar flows, there is a possibility. But, then, you still have to work very very hard.

Hi, Have you checked your stagnation pressure? It is known to be overpredicted using a linear k-epsilon turbulence model. We have seen values of Cp_stag up to 1.1 sometimes. Anders

(1). I have briefly visited the web site and the paper on flat plate drag prediction. It is nice to see the systematic approach taken in the validation. But the case was on the integrated total drag on a finite flat plate, which is different from the validation of the local skin friction distribution. (2). In order to obtain the correct integrated drag force, the skin friction distribution from the leading edge must be accurately predicted. (3). To achieve this , the laminar flow portion and the transitional flow region of the flat plate must be modelled correctly also. This is also true for the flow over an airfoil, where laminar flow and transitional region also exist in the airfoil leading edge area. ( this is nothing new.) In a similar case, the heat transfer around a cooled HP blade also presents the same laminar-to-turbulent flow region around the leading edge. (4). So, to be fair to the code, one can only say that the actual flow field was not modelled accurately to include the laminar-to-turbulent flow region. And as the Reynolds number changes the location of the transition also changes. (5). The best way to do is to match the skin friction at some point, and see whether the skin friction development will match the data or not. (6). So, in the validation of the drag on an airfoil, it is necessary to use tripped boundary layer test data for comparison with the all turbulent flow computation. (7). Most turbulence models were fine tuned for the flat plate data, so, in the case of an airfoil with curved surface, one can not expect to get very good results. (8). In the case of the finite flat plate data, it would be ideal to have a long one to reduce the impact of the laminar-to-turbulent transition. At the same time, the boundary layer could also be tripped to give turulent boundary layer flow, which should be easier for validation purposes.

I have actually addressed the problem of the laminar-transition problem in my report by modelling long flat plates, and shown that the contribution to the over all drag from the small laminar leading edge region is small as expected. How can one model laminar-turbulent transition on a flat plate, when the turbulence model in CFX is either on or off ? Has any body managed to achieve good lift/drag prediction using CFX4.2 ? Surely AEA Tech would have used the naca0012 section as a validation case at some time or other !! Any idea's much appreciated.

Regards James Date

(1). The modelling of the the laminar-transitional-turbulent boundary layer has been around since the days of boundary layer era of 60's. That's why I always say that a code is a dead thing, it can not even read the history. (2). Back in 60's, people had already incorporated laminar-transitional-turbulent flow model into their boundary layer computer codes. (3). Still thinking that the modern CFD codes are advanced technology? It is far less efficient and less accurate than the old boundary layer codes. If you don't find the option in the code, it is 30 years behind, in this area. This is not a joke.