# Backward facing step

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

 December 2, 2008, 11:32 Hello. I'm trying so simula #1 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 11 Hello. I'm trying so simulate the flow over a backward facing step from this publication: Barton (1995) - A numerical study of flow over a confined backward-facing step (International Journal for Numerical Methods in Fluids, Vol. 21, 653-665). The simulation is running but I'm not sure how to compare the reattachment and separation points in the flow field. How are these point defined? I think is has to do something about the pressure distribution alongside the walls? Does anybody have an idea? Greetings Sebastian __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 December 2, 2008, 13:39 Hi Sebastian The separation #2 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,608 Rep Power: 25 Hi Sebastian The separation zone is defined by the part of the boundary along which the time averaged bed shear stress is negative ([1]). As the time averaged bed shear stress reflects the velocity in the cell next to the boundary, then the reattachment point is defined as the point at which the near-wall velocity is zero. Best regards, Niels [1]: It should be noted that the separation zone in itself might consists of consecutive cells, which are rotating in opposite directions, thus it is the largest value of x at which u_bed = 0 which defines the reattachment point. __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 February 27, 2011, 03:53 #3 Senior Member     Join Date: Jan 2010 Posts: 347 Blog Entries: 2 Rep Power: 8 Hi, i want use Driver & Seegmiller paper to validate OpenFOAM pisoFoam solver. The problem is, reattachment point of paper is about 6H, which H is step height. But, in my simulation it is 4.5h for k-e, and near 8H for LRR and LES. I have used OF pitzDaily setting and set geometry also inlet k and U from Driver's paper. i have examined coarse and dense meshes. i checked it with high yPlus with wall function also with yPlus=2 whith zeroGradient near wall treatment. I am confused why can't i reach to correct reattachment point. Any help will be appreciated. Regards.

 February 28, 2011, 09:59 #4 Member   Franco Marra Join Date: Mar 2009 Location: Napoli - Italy Posts: 52 Rep Power: 8 Dear maysmech, I am trying to do similar validation, up to now directly using the Pitz & Daily geometry for separated flows and just for the LES approach. Similarly, I got very long reattachment length. I noticed that the inlet profile does not change so rapidly going downstream as experimental results reports. Therefore I suspect that the computation of the eddy viscosity is under-estimated. I got extensive comparisons in the periodic channel flow geometry with many other solvers (under a joint initiative of several research groups working in Italy), confirming that OpenFoam compute very low value of eddy viscosity in comparison with other flow solvers. Let me know if your simulations confirm these trends. Regards, Franco

February 28, 2011, 10:33
#5
Senior Member

Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 127
Rep Power: 7
Quote:
 Originally Posted by maysmech Hi, i want use Driver & Seegmiller paper to validate OpenFOAM pisoFoam solver. The problem is, reattachment point of paper is about 6H, which H is step height. But, in my simulation it is 4.5h for k-e, and near 8H for LRR and LES. I have used OF pitzDaily setting and set geometry also inlet k and U from Driver's paper. i have examined coarse and dense meshes. i checked it with high yPlus with wall function also with yPlus=2 whith zeroGradient near wall treatment. I am confused why can't i reach to correct reattachment point. Any help will be appreciated. Regards.

I've run this simulation before. Granted it was in FLUENT, but I found kOmegaSST works the best in this case for predicting the location of reattachment.

In this case, because it's a rather simple geometry, you may want to resolve the boundary layer and better predict the location of reattachment. For this your y+ should be less than 1.

March 4, 2011, 05:38
#6
Senior Member

Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
Thanks Franco and Travis,

I used Driver & Seegmiller geometry exactly.
As i heard yPlus should be less than 5 to use zeroGradient instead of wall function. i don't know about y+ less than 1.

Quote:
 Similarly, I got very long reattachment length. I noticed that the inlet profile does not change so rapidly going downstream as experimental results reports. Therefore I suspect that the computation of the eddy viscosity is under-estimated. I got extensive comparisons in the periodic channel flow geometry with many other solvers (under a joint initiative of several research groups working in Italy), confirming that OpenFoam compute very low value of eddy viscosity in comparison with other flow solvers.
So what do you think about what i should do?
inlet of Driver's paper is 4H before step. I set inlet U and K same as Driver test case. For LRR model, i calculated epsilon by ( epsilon=(0.09^0.75)*(K^1.5)/l which "l" is 0.05 of inlet height for this case) and set it as inlet.
I also run the case with 10 times of above epsilon also set inlet turbulence intensity from 0 to 20% of U but not possible to reach 6H reattachment. LES has same problem.

Any suggestion will be appreciated.

 June 1, 2011, 18:46 Inlet BC for Backstep #7 Senior Member   Tarak Join Date: Aug 2010 Location: State College, PA Posts: 105 Rep Power: 6 Hii, can you please tell how did you give the inlet BC for the backward facing step, i.e an inlet boundary layer profile or something like that; or did you just give an uniform inlet velocity profile? Thanks, Tarak

 June 2, 2011, 00:05 #8 Senior Member     Join Date: Jan 2010 Posts: 347 Blog Entries: 2 Rep Power: 8 Hi, Inlet profile was same as Driver & Seegmiller's paper profile.

 June 2, 2011, 00:07 #9 Senior Member   Tarak Join Date: Aug 2010 Location: State College, PA Posts: 105 Rep Power: 6 Hii, Thanks for the reply. Can you please tell me how you got the inlet profile generated, means how do i get such a boundary layer profile matching that of the experiment? Thanks, Tarak

 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 erni FLUENT 3 November 23, 2011 14:49 Sungho Yoon CFX 10 August 4, 2008 05:32 Jimmy Main CFD Forum 3 July 25, 2004 22:37 Chris De Langhe FLUENT 1 March 5, 2000 17:04 Chris De Langhe FLUENT 0 February 28, 2000 11:20

All times are GMT -4. The time now is 22:11.