CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Wall suction/injection

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 23, 2003, 20:34
Default Wall suction/injection
  #1
luiz
Guest
 
Posts: n/a
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

  Reply With Quote

Old   September 24, 2003, 19:25
Default Re: Wall suction/injection
  #2
professor
Guest
 
Posts: n/a
hello, can u pl explain more what r u asking or inother word looking for
  Reply With Quote

Old   September 25, 2003, 07:25
Default Re: Wall suction/injection
  #3
luiz
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 25, 2003, 16:32
Default Re: Wall suction/injection
  #4
professor
Guest
 
Posts: n/a
hello, still ur question is ot clear. pl expalin what do u mean by non slipping wall.
  Reply With Quote

Old   September 25, 2003, 21:04
Default Re: Wall suction/injection
  #5
luiz
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 26, 2003, 08:20
Default Re: Wall suction/injection
  #6
Anton Lyaskin
Guest
 
Posts: n/a
What about setting a boundary condition of an "inlet" type, i.e. specifying all 3 components of the velocity? Most CFD would do this.
  Reply With Quote

Old   September 26, 2003, 14:53
Default Re: Wall suction/injection
  #7
luiz
Guest
 
Posts: n/a
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
  Reply With Quote

Old   September 29, 2003, 02:31
Default Re: Wall suction/injection
  #8
Anton Lyaskin
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   September 29, 2003, 06:49
Default Re: Wall suction/injection
  #9
Rami
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   October 30, 2003, 04:50
Default Re: Wall suction/injection
  #10
autofly
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   November 3, 2003, 14:27
Default Re: Wall suction/injection
  #11
BAK_FLOW
Guest
 
Posts: n/a
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
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug unoder OpenFOAM Installation 11 January 30, 2008 21:30
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 16:38.