[brophya2013]

Hi All,

I am trying to model a 2D Airfoil in Star-CCM+ with little success. The Airfoil is a NACA0025 that was created in ProEngineer Creo and save as a .x_t file.

When I create the structured mesh and convert to 2D, the mesh is coming out as "botchy" around the airfoil. It does not look as good as mesh from GridPro but we can not use this.

I imported the airfoil and created a block around the airfoil to simulate the wind tunnel. The surface size of the airfoil is smaller than the surface size of the wind tunnel.

Is there something that I am missing, the Cl values are double what I am expecting.

Thanks for reading,
Andrew

[abdul099]

How do you create a structured mesh? Or do you mean a trimmed mesh? Can you please post some pictures of the mesh?

[brophya2013]

Thanks abdul for your reply,

Yes, by structured mesh I mean trimmer, apologies for not being clear.

See attached pics.

Andrew

[abdul099]

Sorry when I'm a little direct, but your prism layers are... crap.
First, make sure your last prism layer is not thicker than the first trimmed mesh cell. The transition from the prism layers to the bulk mesh is pretty important. Maybe you also need to increase the growth rate a bit.

I also would add an at least small trimmer wake refinement to capture flow details of the air leaving the airfoil. And make sure, the prism layers at the trailing edge are not so thick, they will not be so important there.

And when the first picture should be your whole domain: That's too small. There will be a pressure and velocity field around the airfoil which should NOT be affected by the boundary conditions, which are usually a fixed velocity or something similar. In general, the airfoil should be far enough from the boundary, that the velocity field (e.g. a slower velocity in the stagnation point) does not reach to the boundary condition. So make sure, your box around the airfoil is far enough to not affect he airfoil. This might be a bit hard since you might need huge domain, but you can have pretty big cells far away from the airfoil. Even when it's more than 20 times the airfoil chord length: That's nothing special.

Please try to improve the points I've mentioned, and keep us informed about the success.

[brophya2013]

Originally Posted by abdul099

Sorry when I'm a little direct, but your prism layers are... crap.
First, make sure your last prism layer is not thicker than the first trimmed mesh cell. The transition from the prism layers to the bulk mesh is pretty important. Maybe you also need to increase the growth rate a bit.

I also would add an at least small trimmer wake refinement to capture flow details of the air leaving the airfoil. And make sure, the prism layers at the trailing edge are not so thick, they will not be so important there.

And when the first picture should be your whole domain: That's too small. There will be a pressure and velocity field around the airfoil which should NOT be affected by the boundary conditions, which are usually a fixed velocity or something similar. In general, the airfoil should be far enough from the boundary, that the velocity field (e.g. a slower velocity in the stagnation point) does not reach to the boundary condition. So make sure, your box around the airfoil is far enough to not affect he airfoil. This might be a bit hard since you might need huge domain, but you can have pretty big cells far away from the airfoil. Even when it's more than 20 times the airfoil chord length: That's nothing special.

Please try to improve the points I've mentioned, and keep us informed about the success.

Thanks abdul for the reply and appreciate the bluntness. I'm a new user and first time using this software.

Attached is my updated mesh - now I have four blocks as volumetric controls and I've added a wake refinement and made the inlet 30 times the chord lenth away and also the outlet.

For 10 deg AOA I expect Cl to be 1.0, im getting in the region of 1.5-1.6. The Re is approximately 270000.

All feedback welcome.

[brophya2013]

Two more attachments.

Andrew

[brophya2013]

Any ideas about my mesh please?

[Chris2337]

Hey Andrew,

Your mesh away from the body looks way finer than it needs to be so you could coarsen that to make it easier.
Your prism layer looks pretty thin compared to what it needs to be, use the turbulent Blasius flat plate approximation to get a rough idea how thick it needs to be.
Are you calculating for the first layer to be a Y+ of 1? If not look up a calculator online. You only need about 25 prism layers too (cant see how many you have).
Lastly be sure to use K-omega with the gamma transition model or your answers will be double the drag at that Re number.

Thanks,
Chris