CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Backward facing step (http://www.cfd-online.com/Forums/openfoam-solving/58259-backward-facing-step.html)

sega December 2, 2008 11:32

Hello. I'm trying so simula
 
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

ngj December 2, 2008 13:39

Hi Sebastian The separation
 
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.

maysmech February 27, 2011 03:53

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.

francescomarra February 28, 2011 09:59

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

tcarrigan February 28, 2011 10:33

Quote:

Originally Posted by maysmech (Post 297160)
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.

maysmech March 4, 2011 05:38

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.:confused:

Any suggestion will be appreciated.

Tarak June 1, 2011 18:46

Inlet BC for Backstep
 
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

maysmech June 2, 2011 00:05

Hi,

Inlet profile was same as Driver & Seegmiller's paper profile.

Tarak June 2, 2011 00:07

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


All times are GMT -4. The time now is 21:48.