CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Backward facing step

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2008, 11:32
Default Hello. I'm trying so simula
  #1
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
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!"
sega is offline   Reply With Quote

Old   December 2, 2008, 13:39
Default Hi Sebastian The separation
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,608
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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.
ngj is offline   Reply With Quote

Old   February 27, 2011, 03:53
Lightbulb
  #3
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
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.
maysmech is offline   Reply With Quote

Old   February 28, 2011, 09:59
Default
  #4
Member
 
Franco Marra
Join Date: Mar 2009
Location: Napoli - Italy
Posts: 52
Rep Power: 8
francescomarra is on a distinguished road
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
francescomarra is offline   Reply With Quote

Old   February 28, 2011, 10:33
Default
  #5
Senior Member
 
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 127
Rep Power: 7
tcarrigan is on a distinguished road
Quote:
Originally Posted by maysmech View Post
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.
tcarrigan is offline   Reply With Quote

Old   March 4, 2011, 05:38
Default
  #6
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
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.
maysmech is offline   Reply With Quote

Old   June 1, 2011, 18:46
Default Inlet BC for Backstep
  #7
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
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
Tarak is offline   Reply With Quote

Old   June 2, 2011, 00:05
Default
  #8
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Hi,

Inlet profile was same as Driver & Seegmiller's paper profile.
maysmech is offline   Reply With Quote

Old   June 2, 2011, 00:07
Default
  #9
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
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
Tarak is offline   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
backward facing step erni FLUENT 3 November 23, 2011 14:49
DNS for backward-facing step using CFX Sungho Yoon CFX 10 August 4, 2008 05:32
Backward Facing Step Jimmy Main CFD Forum 3 July 25, 2004 22:37
Backward facing step Chris De Langhe FLUENT 1 March 5, 2000 17:04
Backward facing step 2 Chris De Langhe FLUENT 0 February 28, 2000 11:20


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