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

Turbulators and boundary layer modelling

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 7, 2007, 16:32
Default Turbulators and boundary layer modelling
  #1
Keith
Guest
 
Posts: n/a
Hello to all

I am attempting to model the flow over a 2D aerofoil (120mm chord)with the addition of "turbulators" on the surfaces in different configurations. The turbulators are in fact simple pieces of tape (0.35mm thick) placed at various locations to trip the boundary layer to hopefully reduce bubble drag and delay separation at 0.3M Reynolds number. I'm using SST coupled with the Gamma Theta model for transitional turbulence. I'm hoping the boundary is resolved by setting y+, in CFX mesh, to 0.8 with 30 layers of inflation. My questions are as follows:

Do you think it is possible to model flow over 0.35mm trips and expect reasonable results?

Having seen posts containing pictures of transition modelling (Chebeba and PetrK) their surface plots were of transition onset Reynolds number or wall shear. If I understand correctly a turbulent boundary layer (BL) will have a higher wall shear value than a laminar BL but at what value (of wall shear or transition onset Reynolds number) can a turbulent BL be identified? The question I am trying to ask is how can I be sure that a BL has been tripped by use of turbulators in the models?

Any help would be greatly appreciated.

Keith

  Reply With Quote

Old   September 9, 2007, 18:33
Default Re: Turbulators and boundary layer modelling
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

If you use the Gamma Theta model and use some surface roughness to model the turbulators then I am not sure you will actually get transition where it is meant to be. If you forget the Gamma Theta model and explicitly define the transition at the turbulators then that should work - providing you do actually know where the transition occurs.

To identify turbulent regions look at the turbulence intermittency - 0=laminar, 1=turbulent.

Glenn Horrocks
  Reply With Quote

Old   September 10, 2007, 13:11
Default Re: Turbulators and boundary layer modelling
  #3
CycLone
Guest
 
Posts: n/a
Hi Keith,

If you are tripping the boundary layer you can specify the location at which transition occurs, rather than rely on the code to predict it. While the code probably will predict transition due to the presence of your strip, it will save you having to create a mesh that resolves the small change in height. You'll probably still want a region or a split in the surface where the change occurs so you can specify where the transition occurs, but nothing more. The documentation explains how to specify the transition location.

-CycLone
  Reply With Quote

Old   September 11, 2007, 18:37
Default Re: Turbulators and boundary layer modelling
  #4
Keith
Guest
 
Posts: n/a
Hi Glenn/Cyclone

Many thanks for your advice and suggestions. I would very much like to try out your recommendation of specifying the trip location and I think I have found the relevant area in the manual. Am I correct in assuming that you are prescibing the zero equation transition model to specify the intermittency with a user defined subroutine that is based on the x, y and z co-ordinates? I have had a quick look at how to do this and I'm a little stuck. Am I to create a CEL function that simply defines the co-ordinates (x=0.05, y=0.1 etc) and use this as the intermittency option? This then sets the intermittency at that point to 1 - i.e. turbulent?

Cyclone - if I'm way off could you direct me to the relevant area of the documentation please?

obliged in advance

Keith

  Reply With Quote

Old   September 12, 2007, 09:49
Default Re: Turbulators and boundary layer modelling
  #5
CycLone
Guest
 
Posts: n/a
Hi Keith,

The manual suggests a user defined function that would return 0 in the laminar surface region and 1 in the turbulent region, the boundary being at the trip location.

I would approach this differently now with some of the new CEL functions in version 11. The easiest way to delineate the tripped and laminar regions would be to identify them in your CAD model. With DesignModeler you could do this using the Imprint Face option of the Extrude, Sweep and Revolve operations or use the Imprint Face body operation. Imprint Face allows you break up a face. Alternatively, you could use your existing mesh and edit the regions to pick the faces that are in the laminar/turbulent zones. There are many other approaches, but I think you get the point.

Once you have a separate region, you can create a Composite Region which comprises all of the Laminar zones (or vice versa), and call it... I don't know... maybe "Laminar Regions" . You can then set the Intermittency as follows:

FLUIDS MODELS:
TURBULENCE MODEL:
Option = SST
TRANSITIONAL TURBULENCE:
Option = Specified Intermittency
Intermittency = 1 - inside()@REGION: Laminar Regions
END
END
END

The "inside()@location" function returns 1 if it is inside the location specified (which can be any 2D or 3D location and zero if not. REGION: This will give you the desired effect.

I've never tried it, so please let us know if this works.

-CycLone
  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



All times are GMT -4. The time now is 22:01.