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

SStkOmega Initial Condition problem??

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

Like Tree1Likes
  • 1 Post By ArathoN

Reply
 
LinkBack Thread Tools Display Modes
Old   January 5, 2014, 09:44
Default SStkOmega Initial Condition problem??
  #1
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
ArathoN is on a distinguished road
Hi I really hope some kind soul will help me After 2 months i couldn't find the solution by my self and i decided to ask the community (Hoping that this time some one will answer me).

I'm studying the Backward facing step and i'm using the Makiola Data to validate the code. Here the checkMesh output:
Code:
Checking geometry...
    Overall domain bounding box (-1 -0.1 -0.0600333) (5 0.1 0.0600333)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-9.79501e-18 6.68689e-16 9.46468e-20) OK.
    Max cell openness = 2.42701e-16 OK.
    Max aspect ratio = 180.003 OK.
    Minimum face area = 5.27601e-07. Maximum face area = 0.00749943.  Face area magnitudes OK.
    Min volume = 6.33473e-08. Max volume = 1.33007e-05.  Total volume = 0.130418.  Cell volumes OK.
    Mesh non-orthogonality Max: 20.1903 average: 6.51521
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.444594 OK.
    Coupled point location match (average 0) OK.
My data are:
Code:
Reynold numbers: 15000, 64000
Aspect Ratio:2
Hinlet=Hstep=0.1 m
I%= sqrt(0.1) * 100 (as in the makiola paper)
nu=1.45e-5
U(Re1)=2.175
U(Re2)=9.28
l (mixing-length)= 10% Hstep
K, Omega calculated with the formulas in the wiki (the ones with the mixing length)
Omegawall= 60*nu/[ deltay^2 * Cmu]      (i found this relation in the wilcox)
I decided to use the SSTKomega model, after some problems with setting up the case (it's my first case using OpenFoam) i could run it and obtain some physically accepted results, but they were not experimentally correct. In particular the adimensionalised reattachment distance (Xr/Hstep) is higher than the experimental value (7.5 vs 6 more or less).

To solve i searched a lot in the forum and changed in every aspect the boundary condition and also the schemes with no effect, i tried using the KEpsilon and it gives as expected a lesser value.

Here some BC setting i've chosen for Re=15000:

Code:
Omega
Inlet: fixedValue 153.84
Outlet: zeroGradient
upperWall: fixedValue 9700
lowerWall: fixedValue 9700

K
Inlet: fixedValue 0.71
Outlet: zeroGradient
upperWall: fixedValue 1e-16
lowerWall: fixedValue 1e-16
Code:
Omega
Inlet: fixedValue 153.84
Outlet: zeroGradient
upperWall: omegaWallFunction
lowerWall: omegaWallFunction

K
Inlet: fixedValue 0.71
Outlet: zeroGradient
upperWall: kqRWallFunction
lowerWall: kqRWallFunction
And the last one with the zerogradient setting for the wall but from what i understood it is the same as the wall function.

If it is needed i can also upload my scheme file and everything that is needed.

P.S: I used the yPlusRAS to check the "yPlus" value and It is always less than the unit for the case Re=15000

Finally sorry for my bad English, i tried to write as correctly as i could.

Damn i didn't notice the mistake in the title sorry for that.

Last edited by ArathoN; January 7, 2014 at 21:02. Reason: some problemi were solved
ArathoN is offline   Reply With Quote

Old   January 7, 2014, 20:58
Default
  #2
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
ArathoN is on a distinguished road
Please someone help me!!!! I changed again the mesh but i didn't get the Desired results, i even changed the geometry dimensions to the ones in the Makiola paper.
Right now I'm with no idea how to proceed.

I noticed that if i use the zerogradient BC on the wall for the variables omega and k it will give some really strange results. If i plot the wallshearstress against the distance from the step the shearstress is always negative as if there is no recirculatinge zone. Does anyone know why?

PS. The yplus is under 1 for both the walls.
ArathoN is offline   Reply With Quote

Old   January 9, 2014, 18:03
Default
  #3
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
ArathoN is on a distinguished road
I've done more tests but with no success. I made even a fiber mesh but the results didn't change.

Now I have a doubt what if the turbolent length length was wrong? I considered it as 10% H, then I lowered it until 3% H. However the biggest turbolent scale length is is in the same order of the step height. I'll try this new setting then I'll comment hoping in some help meanwhile.
ArathoN is offline   Reply With Quote

Old   January 9, 2014, 21:16
Default
  #4
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
ArathoN is on a distinguished road
Finally I have some good results, I choose there BC on the walls:
K-----> fixed value at 1e-16
Omega------->zerogradient

Now I have a better reattachment length, xr/h=6.3 against the experimental value 5.8; at this point I decided to change the turbolent length scale and I considered it as 20℅ of Hstep giving me a xr/h=5.9 really close to the desired value. So I'll change again the turbulence length then I'll consider the other configurations; until now I focused one the 20 step; to validate my observation.


P.S funny how this thread is turning into a monologue. I hope that my findings may help someone in the future :P
msuaeronautics likes this.
ArathoN 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
rhoSimplecFoam Mach0.8 no pressure values CFDnewbie147 OpenFOAM Running, Solving & CFD 16 November 23, 2013 06:58
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Extremely slow simulation with interDyMFoam jrrygg OpenFOAM Running, Solving & CFD 9 April 23, 2013 10:14
pisoFoam - unstable pressure residual Industrial_CFD OpenFOAM Running, Solving & CFD 21 February 24, 2013 16:39
Error while running rhoPisoFoam.. nileshjrane OpenFOAM Running, Solving & CFD 8 August 26, 2010 12:50


All times are GMT -4. The time now is 07:39.