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

Epsilon BC at wall and Inflow for High-Re Model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 22, 2014, 19:59
Default Epsilon BC at wall and Inflow for High-Re Model
  #1
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 8
ArathoN is on a distinguished road
Hi,

I know that for commercial cfd application it is generally accepted the use of High-Re models for low-Re Meshes (especially for low-speed flows tipical of automotive related cases).

The dissipation energy as defined in High-Re Meshes doesn't tend to zero at the wall but it depends on the viscosity and the second derivative of the turbulent energy (or the first derivative of the squared turbulent energy multiplied by a factor 2), hence what type of BC do you consider?

It's better a fixedValue with either a value that tends to zero or an epsilon defined by the relation found considering the log law and a local equilibrium (Production=Dissipation)
Code:
epsilon= Cmu075 * kp^1.5 / (kappa * yp)
Or it is more advisable the use of a zeroGradient BC.


Moreover digging into the code I've found that there are two relation that define epsilon, the first is present in "epsilonWallFuction"
Code:
epsilon= Cmu075 * kp^1.5 / (kappa * yp)
and the second is derived from nut in the turbulenceModels files and it is for internalMesh:
Code:
epsilon=Cmu * sqr(k)/nu *(nut/nu)^-1
Until now I've found that here they recommend the use of the first relation to define epsilon at the inflow however isn't it more appropriate to use the second one? I tried calculating bot and they differ almost by one order of magnitude and I don't know what to use, I usually try both and see which gives better results.
ArathoN is offline   Reply With Quote

Old   October 23, 2014, 02:27
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Hey Arathon,

What you are looking for is called:
"CFD of Air Flow in Hydro Power Generators by Pirooz Moradnia".
Google for the pdf. He discusses all the OpenFOAM models with their correct b.c.s
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 23, 2014, 07:15
Default
  #3
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 8
ArathoN is on a distinguished road
I read it and for high-re models he choose zero-gradient for the theoretical definition however this is true for k only in log layer/equilibrium region (while it is null at the wall). In that thesis he use high-re models only on high-re meshes, what I want to know is what if I wanted to use the model on low-re mesh.

Maybe it is just a dumb question considering that the differences between low-re and high-re models lies on how epsilon is defined at wall. For high-re it shouldn't be zero but almost a fixed value so maybe in this point of view a zero-gradient may give better results, while on low-re epsilon is modified into epsilon.tilda which is null at the wall (this is the dumping needed to resolve the model near the wall) .
ArathoN is offline   Reply With Quote

Old   October 23, 2014, 07:23
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
I am not sure if I get you right. Do you want to use a high-Re model on low-Re meshes? This doesn't work. You need a low-Re model for that. Low-Re models have integrated damping functions that allow for resolving the layer. You can not just adopt the boundary conditions of the high-Re model to get a low-Re model.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 23, 2014, 07:33
Default
  #5
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 8
ArathoN is on a distinguished road
This was a curiosity because a friend working on a "cfd company" said that for studying flow over cars they usually use k-epsilon, so I thought what Bc did they use for epsilon.
Moreover reading some threads here most people suggest an epsilon null at wall for y+<1, this is totally wrong imo. It's better a zero-gradient? But this can be plausible only if the flow remain simple.
ArathoN is offline   Reply With Quote

Old   October 23, 2014, 07:56
Default
  #6
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
As far as I know epsilon=0 only holds for the Launder Sharma k-epsilon model, because it uses a transformed epsilon variable in a way that e=0. This is not the "real" epsilon but just an "epsilon tilde". Other models don't work like that...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 23, 2014, 11:00
Default
  #7
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 8
ArathoN is on a distinguished road
Yeah you're right. It's been a while since I used fluent does it have a k-epsilon with near wall treatment because they are using it with y+ less the unit. Dunno why but they don't care to use a more appropriate model like komegasst.

OT: how the hell is div operator calculated in the turbulence models, does it take into account the continuity conservation? I've just compared the OF formulation with the theoretical equations and they differ on how it is written the div(phi, k) :

Of1.6-------->div(phi,k)-k div(phi)
Of2.3-------->div(phi, K)
Theory---------->phi div(k)
For Incomprensibile k-epsilon.
ArathoN is offline   Reply With Quote

Old   November 10, 2014, 09:47
Default
  #8
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 391
Rep Power: 11
jherb is on a distinguished road
In an incompressible flow, shouldn't div(phi) == 0?
Code:
div(phi,k) = phi*div(k) + k *div(phi) = phi*div(k)
I think in OpenFOAM a certain implementation was chosen because of its numerical stability.

Regarding wall functions for the turbulence quantities:
http://www.cfd-online.com/Forums/ope...omega-sst.html
http://www.cfd-online.com/Forums/ope...tml#post306339
http://www.openfoam.org/mantisbt/view.php?id=179
jherb is offline   Reply With Quote

Old   November 10, 2014, 19:12
Default
  #9
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 8
ArathoN is on a distinguished road
Quote:
Originally Posted by jherb View Post
In an incompressible flow, shouldn't div(phi) == 0?
Code:
div(phi,k) = phi*div(k) + k *div(phi) = phi*div(k)
I think in OpenFOAM a certain implementation was chosen because of its numerical stability.

Regarding wall functions for the turbulence quantities:
http://www.cfd-online.com/Forums/ope...omega-sst.html
http://www.cfd-online.com/Forums/ope...tml#post306339
http://www.openfoam.org/mantisbt/view.php?id=179
Sure in incompressible flow the velocity divergence should be null because of the conservation law however i didn't find how openfoam recognize that. I searched how the divergence operator is formulated and all related files but still no clue on how OF resolve "div(phi,k)".
ArathoN is offline   Reply With Quote

Old   November 10, 2014, 19:52
Default
  #10
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 391
Rep Power: 11
jherb is on a distinguished road
Look for convection in http://www.foamcfd.org/Nabla/guides/ProgrammersGuidese9.html
jherb 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
CFX13 Post Periodic interface EtaEta CFX 7 December 8, 2011 18:15
k-w turbulent model and inflow boundary conditions vaina74 Main CFD Forum 6 April 26, 2010 06:03
Wall functions tutlhino OpenFOAM Pre-Processing 0 July 2, 2007 05:04
SST model Autometic wall function parameters? David CFX 0 November 24, 2005 05:47
Wall functions or low-Re models? J. P. Main CFD Forum 7 July 9, 1998 11:11


All times are GMT -4. The time now is 19:08.