Does anyone know about any Cfd software capable of dealing with wall boundaries with suction or injection? Has anyone ever tried to simulate any kind of boundary layer control in any commercial CFD? Seems to me that it is a pretty old problem and, therefore these modern CFD should be able to predict... Is there any free code to simulate at least the boundary layer zone for these cases?

Best Regards, Luiz

hello, can u pl explain more what r u asking or inother word looking for

I would like to set a non-slipping wall in the surface of an airfoil and then allow suction/injection over there as a means to control flow separation.

Thanks, Luiz

hello, still ur question is ot clear. pl expalin what do u mean by non slipping wall.

A no-slipping wall boundary condition is simply a wall over which the velocity of the fluid is zero.

Therefore, in a common situation, the speed of the fluid layers adjacent to the surface of an airfoil would have null tangencial component and null normal component. This is an easy problem. Most CFD would do this.

What I would like to do is to simulate the same airfoil but with a different boundary condition: tangencial velocity equals to zero, but normal velocity (I mean, normal to the airfoil surface) not equal to zero. This normal velocity is supposed to simulate a suction or injection (depending on its sign) throught the airfoil walls. This is a classic way of controlling boundary layer separation, but I do not know how to do it in Fluent, and dont even know if there is any CFD capable of doing this...

Thank you, Luiz

What about setting a boundary condition of an "inlet" type, i.e. specifying all 3 components of the velocity? Most CFD would do this.

I tought about that, but if I set it as vel inlet, the CFD will not calculate the wall functions (wall law) which is done only with wall bound. cond.. Therefore I would need to build a very refined mesh around the airfoil. Also I would have to set the boundary condition in every face, since they belong to a curved surface. Do you think that is the way to go?

Thank you , Luiz

Are you sure that wall functions can be applied to walls with blowing/suction? At least you'll need some special wall functions which are not embedded in most CFD codes.

And yes, you'll need to set boundary conditions on every face.

The only other way I see is treating such wall as permeable surface and specifying high (for blowing) or low (for suction) pressure inside the airfoil.

luiz,

I had solved such a blowing BC problem quite a long time ago using another CFD package. It allowed prescriprion of wall function in the tangential direction (with an appropriate grid to maintain y+ in the 30-150 range) and prescribed normal velocity. However, the actual settings may be different in other packages. It might be better if you post your querry in the FLUENT forum.

how to define the suction/injectin boundary conditions? velocity component normal to surface, exit pressure, and exit density or temperature. in most cases, momentum ratio is presented.

Hi,

I would not advise setting the blowing wall as an inlet. The physics of a blowing/suction boundary layer is in fact mostly a no-slip boundary layer that is perturbed slightly by the addition/extraction of a small ammount of fluid. One of the main problems with setting the boundary as an inlet is the appropriate specification of the closure for momentum flux. The issue of a wall function has already been mentioned. Further, even if one were to integrate to the wall, the wall shear stress will not be applied correctly.

Wilcox discusses the near-wall treatment under section 4.7.3, Surface Mass Injection of "Turbulence Modeling for CFD", first edition.

There also exists the possibility to introduce a small mass and momentum source in a thin 3-D region near the wall using volumetric sources. In this case I would suggest a grid that resolves the viscous sub-layer and integrate to the wall. Additionally some tuning would be required to select the thickness of the region from/to which to remove/add the mass. This can very nicely be tuned by running several detailed model cases with all of the details resolved for the holes or slots.

Best of Luck,

Bak_Flow