Epsilon BC at wall and Inflow for High-Re Model

ArathoN · October 22, 2014, 20:59

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.

RodriguezFatz · October 23, 2014, 03:27

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

ArathoN · October 23, 2014, 08:15

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) .

RodriguezFatz · October 23, 2014, 08:23

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.

ArathoN · October 23, 2014, 08:33

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.

RodriguezFatz · October 23, 2014, 08:56

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...

ArathoN · October 23, 2014, 12:00

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.

jherb · November 10, 2014, 09:47

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

ArathoN · November 10, 2014, 19:12

Quote:

Originally Posted by jherb

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)".

jherb · November 10, 2014, 19:52

Look for convection in http://www.foamcfd.org/Nabla/guides/ProgrammersGuidese9.html

October 22, 2014, 20:59	Epsilon BC at wall and Inflow for High-Re Model	#1
ArathoN Senior Member ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 16	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.

October 23, 2014, 03:27		#2
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	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.

October 23, 2014, 08:23		#4
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	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.

October 23, 2014, 08:56		#6
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	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.

November 10, 2014, 09:47		#8
jherb Senior Member Joachim Herb Join Date: Sep 2010 Posts: 650 Rep Power: 22	In an incompressible flow, shouldn't div(phi) == 0? Code: div(phi,k) = phidiv(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

October 23, 2014, 08:15		#3
ArathoN Senior Member ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 16	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) .

October 23, 2014, 08:33		#5
ArathoN Senior Member ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 16	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.

October 23, 2014, 12:00		#7
ArathoN Senior Member ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 16	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.

November 10, 2014, 19:52		#10
jherb Senior Member Joachim Herb Join Date: Sep 2010 Posts: 650 Rep Power: 22	Look for convection in http://www.foamcfd.org/Nabla/guides/ProgrammersGuidese9.html

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 07:03
Wall functions	tutlhino	OpenFOAM Pre-Processing	0	July 2, 2007 06:04
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 12:11