how to evaluate seperation in 3D flow problem?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 12, 2005, 08:31 how to evaluate seperation in 3D flow problem? #1 justCFD Guest   Posts: n/a I normally use the diminishing shear stress as an indication for flow separation. However, I learnt some where that this is not the best method for 3D problem. I wonder how you all decide if the flow separation will occur in your problem.... I think there should be a couple of other ways to analyse the flow separation in CFD.....Please kindly share with me. Thank you.

 July 12, 2005, 10:53 Re: how to evaluate seperation in 3D flow problem? #2 ramp Guest   Posts: n/a You cam find out by looking at the vorticity profile over the body surface... The negative magnitude on the profile shows there is a separation from the body. The point at which the vorticity is zero is the separation point.

 July 12, 2005, 12:10 Re: how to evaluate seperation in 3D flow problem? #3 justCFD Guest   Posts: n/a Ramp: Thanks for your suggestion. Have you heard anything about skin friction line? I have some journal papers that make use of this concept to visualise the 3D flow separation but I can't find any details of how the authors define the skin friction lines etc...

 July 12, 2005, 13:38 Re: how to evaluate seperation in 3D flow problem? #4 ramp Guest   Posts: n/a Skin friction line is a shear-stress (non-dimensional) profile over the surface of the body. You can get it in any basic fluid mechanics and boundary layer flow related books. I think the skin friction and vorticity profile both are good to find the separation information for constant viscosity flows. In case of variable viscosity flows, the surface vorticity profile will provide the exact information.

 July 12, 2005, 16:16 Re: how to evaluate seperation in 3D flow problem? #5 Jim_Park Guest   Posts: n/a For a flat plate, they're the same, give or take a sign and a viscosity. Consider that vorticity = du/dy - dv/dx, where x is the primary flow direction, y is the direction normal to the plate. Since the boundary condition on v is v(x) = 0 (no slip at the plate), dv/dx = 0 at the wall. This leaves the vorticity at the wall = du/dy. The shear at the wall is viscosity x du/dy, just the vorticity multiplied by the viscosity. At least the 0's in vorticity and shear along the wall should occur at the same place. Clear this simple analysis needs to be reconsidered for an inclined or curved boundary in 2 or 3 dimensions.

 July 12, 2005, 17:28 Re: how to evaluate seperation in 3D flow problem? #6 ramp Guest   Posts: n/a Yes Jim_Park, the same analysis can be considered for curved geometries. Thanks

 July 13, 2005, 04:26 Re: how to evaluate seperation in 3D flow problem? #7 Tom Guest   Posts: n/a As a minor point - in 3D boundary layer flow the point of separation is not necessarily a point of zero surface stress. That is if you have a point of zero stress (both u_y and w_y zero on the surface) then you have separation/attachmet but the converse is not true! The flow can separate without both u_y=w_y=0 at the same point. This is the case of a limiting streamline (a line onto which neighbouring streamlines converge). To my knowledge(*) there is no simple way to identify this case from the full Navier-Stokes equations (in the boundary-layer equations it corresponds to the formation of singularity in the flow where the vertical velocity becomes infinite), Tom. (*) but see "A vorticity dynamics theory of three-dimensional flow separation" by Wu et al.(2000) in Physics of Fluids vol 12 no 8.

 July 14, 2005, 08:49 Re: how to evaluate separation in 3D flow problem? #8 Axel Rohde Guest   Posts: n/a Separation of flow over a 3-D surface can easily be detected by plotting 'tufts'. You multiply the surface stress tensor with the surface outward unit normal which gives you the (surface) traction. You normalize this traction vector and then scale it so you can actually see it when plotted. This traction vector acts like a tuft attached to the body surface in an actual windtunnel. Unless the flow is compressible and highly unsteady, the traction is tangential to the surface. For further study, download my dissertation and take a look at pages 70 (traction), 75 (surface forces), 106 (tufts on non-spinning disk) and 144 (tufts on spinning disk). http://www.microcfd.com/download/pdf/dissertation.pdf Also, my website's home page, www.microcfd.com, shows the tufts on a spinning disk. Again, where these tufts suddenly change direction is where the flow separates. For a spinning disc, the line of separation is along the side rather than the aft body.

 July 14, 2005, 17:40 Re: how to evaluate separation in 3D flow problem? #9 justCFD Guest   Posts: n/a Cool.... I never thought that I can plot my CFD result this way. Thank you for your input here. I'll read thru your thesis carefully and see if that can be apply on my case too...

 July 14, 2005, 17:51 Re: how to evaluate seperation in 3D flow problem? #10 justCFD Guest   Posts: n/a Thank you for all the valuable inputs here. Tom's comments are very similar to what I read from the paper so far. The authors claim that the location of separation on a 3D curved surface can be identified through a plot of converging skin friction lines. Anyone know if the plot of surface streamline can be used to determine the separation as well?

 July 19, 2005, 07:53 Re: how to evaluate separation in 3D flow problem? #11 krish Guest   Posts: n/a U can see further details regarding surface streamlines here... basically plot stream traces at the surface using (x,z,dudy,dwdy) ... http://www.aerodyn.org/Wings/3dsepar.html#example

 March 13, 2013, 11:35 flow separation #12 New Member   Join Date: Feb 2013 Posts: 18 Rep Power: 5 Hi everybody, I've to evaluate if there is flow separation and eventual reattachment points on the roof of a building , which is sourronded by a huge parallelepiped of air (to simulate wind driven natural ventilation in buildings). How could I do? Thanks a lot for any suggestion Bests

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ziemowitzima OpenFOAM Running, Solving & CFD 0 April 5, 2010 13:30 nikhil FLUENT 0 March 29, 2010 23:52 Markus CFX 5 February 19, 2005 18:30 jehanzeb FLUENT 5 August 3, 2004 08:04 ram Main CFD Forum 5 June 17, 2000 21:31

All times are GMT -4. The time now is 16:33.

 Contact Us - CFD Online - Top