C-Grid around an airfoil
I just started using Star CCM+. I'd like to run a simulation around an airfoil. During my literature research i found out that a C-Grid ist widely considered as the most suitabel mesh for my kind of problem. I've tried to create a mesh in Star CCM+ similar to the one in the picture below but like I said I'm a beginner and i've failed yet to create such a mesh so it would be nice if someone could give me some advice :).
This is a structured mesh. Commercial CFD software works with unstructured meshes.
Although unnecessary, if you really want to, you can set up different domains over the upstream and downstream halves of the airfoil and use primarily prism layers with low stretching within the upstream domain, and add a wake refinement for the downstream domain.
I'm doing simulation on the foils by using Star-CCM+. Unfortunately, I still have not got the expected resutls yet. I think the most important is how to generate a fine mesh in Star-CCM+. In order to obtain the good mesh, as nomad mentioned, I apply prims layer and volumetric control to refine the mesh near the wall as long as in the wake. But the results are still not close to the experimental data (NACA series). All lift coefficient and drag coefficient are higher than exp. So I hope some ones can help me how to solve for this problem! is there any tutorials about the mesh generation for the foils in Star-CCM+ ? many thanks! Trieu
You need to use the Gamma Re Theta correlation that is part of the k-omega solver. This has been recently published and has been implemented in starccm+. It predicts transition more accurately. This is the paper if you can find it:
Transition Modeling for General CFD Applications in Aeronautics , R.B.Langtry and F.R.Menter
Select the Gamma Re Theta model within the k-omega solver, then write a simple field function to define the location of the free stream in terms of the wall distance or centroid of the cell closest to the wall. Also, make sure that your wall Y+ values are really low (<1). This should give you a very accurate drag prediction to within 5% (at least for angles of attack of up to 6-8 degrees).
Firstly, I would say thanks you so much for your useful information!
Then I would ask you for more helps. Because I've tried to download the paper which you mentioned, but I can not. The other problem is I have not studied about how to define a new field function in Star-CCM.
Could you send me that paper as long as teach me about the field function in Star-CCM?
Thanks you in advance!
You need to turn on the Gamma Re Theta transition model through the k-omega solver.
Create a field function where you define the position of the freestream. There's an example in the help file which I'm repeating here:
$WallDistance > 0.005?1:0
This is saying that the free stream edge is at 0.005m from the boundary where you're measuring the forces. This number will change depending on the type of flow taking place over the wing, but for now you can approximate the entire freestream edge over the whole wing as a single iso surface.
Select this field function in the Physics-Model-GaReTheta-Free Stream Edge.
Lastly, and most important, make sure your wall y+ over the entire boundary is less than 1. Ensure a fine leading and trailing edge mesh, add a control volume if you have to. You will have to run the simulation, monitor the Wall y+, and remesh accordingly so that wall y+ is less than 1.
This should give you a drag prediction that's within 5% of experiment for angle of attack less than 8 degrees, and within 10% otherwise.
|All times are GMT -4. The time now is 05:48.|