CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Inlet BC for k-epsilon model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 6, 2012, 07:47
Default Inlet BC for k-epsilon model
  #1
Per
New Member
 
Per Christian Endresen
Join Date: Feb 2012
Location: Trondheim, Norway
Posts: 13
Rep Power: 5
Per is on a distinguished road
Hi

I am simulating pipe flow using simpleFoam. Instead of using a fixed value for k and epsilon at the inlet I am considering using for instance the turbulentIntensityKineticEnergyInlet condition for k.

Internal field and inlet conditions for k are:

//
internalField uniform 9.375e-4;

inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05; // Turbulent intensity
value $internalField;
}
//

Does (value $internalField) mean that it is calculated based on the initial internal field for k or the inlet BC for U, which is (0.5 0 0)? My (internalField uniform 9.375e-4) is calculated as k=1.5(Uavg*I)^2, where I=0.05. The turbulentIntensityKineticEnergyInlet condition is copied from an OpenFOAM tutorial case.

The k and epsilon file is renamed k.old and epsilon.old when I run simpleFoam. The new OpenFOAM generated k file has this inlet condition:

//
Inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
U U;
phi phi;
value uniform 0.0009375;
}
//

Regards
Per
Per is offline   Reply With Quote

Old   March 6, 2012, 21:34
Default
  #2
Senior Member
 
calim_cfd's Avatar
 
mauricio
Join Date: Jun 2011
Posts: 136
Rep Power: 8
calim_cfd is on a distinguished road
what you stated seems right

and the turbulentIntensityKineticEnergyInlet BC is inletoutlet type if im not mistaken.. which means it will fix the value for inflow and zerograd for outflow

and at line 146 of the respect *.C file you have it
Code:
    this->refValue() = 1.5*sqr(intensity_)*magSqr(Up);
and the renaming of files is nothing to worry about.. just more complete statements nothing rly new
__________________
Best Regards
/calim

"Elune will grant us the strength"
calim_cfd is offline   Reply With Quote

Old   March 7, 2012, 05:42
Default
  #3
Per
New Member
 
Per Christian Endresen
Join Date: Feb 2012
Location: Trondheim, Norway
Posts: 13
Rep Power: 5
Per is on a distinguished road
Thanks for the reply calim


I have actually not thought about that inlet condition as an inletOutlet (or outletInlet?) type. This certainly makes it more versatile. I found out (by experimenting with my initial conditions) that the inlet value for k (or epsilon for that matter) is calculated based on the intensity and initial magnitude of the velocity at the inlet (as you said) and is kept throughout the simulation, while the other fields are reference values used for startup of the simulation. Does anyone know why wall conditions (uniform value) not are kept for k and epsilon when using wall functions? Or more precise: are zeroGradient condition used (and appropriate) at walls for k and epsilon when using a wall function?


Regards
Per
Per is offline   Reply With Quote

Old   March 7, 2012, 14:03
Default
  #4
Senior Member
 
calim_cfd's Avatar
 
mauricio
Join Date: Jun 2011
Posts: 136
Rep Power: 8
calim_cfd is on a distinguished road
when you use wall functions, the value you set for k/epi at the wall patches is not rly used as result/input. It's just an initialization option and sort of requirement for paraview regarding time 0/

you specify the values for k/epis based at inlet/oultet based on you flow/geometry. These are fixed until the end of your simulation!

The value at the wall boundaries will change throughout the simulation. Constant values at the wall will be true only for, say a straight pipe with developed flow..... sth like that...
__________________
Best Regards
/calim

"Elune will grant us the strength"
calim_cfd is offline   Reply With Quote

Old   July 29, 2012, 02:20
Default tell me please???
  #5
Member
 
vahid
Join Date: Feb 2012
Location: Mashhad-Iran
Posts: 80
Rep Power: 4
vahid.najafi is an unknown quantity at this point
Hello Dear foamers.
I have a question???

I want to add k(kinetic turbulence energy) in solver interPhaseChangeFoam.
for this reason, added next line in this:

const volScalarField &k=U_.db().lookupObject<volScalarField>("k")
and wmake was Successfully .

but How can I Understand that this k is the same with k(kinetic turbulence energy)???Is it true?????
I replased M Instead k in Top Line :

const volScalarField &M=U_.db().lookupObject<volScalarField>("M")
but nothing error was not occured!!!!!!??????

Thanks alot.
vahid.najafi is offline   Reply With Quote

Reply

Tags
boundary, inlet, k-epsilon, turbulent

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
How to model a fan as inlet boundary condition? val46 OpenFOAM 2 October 11, 2010 10:07
Centrifugal Pump and Turbulence Model Michiel CFX 12 January 25, 2010 04:20
RANS-Sim. of airfoil: inlet condition of epsilon? Norman Cook Main CFD Forum 3 November 19, 2006 12:30
Velocity inlet K and Epsilon Daniel Bruno FLUENT 6 June 17, 2001 02:51
inlet boundary condition in k-e model Abhijit Tilak Main CFD Forum 1 June 2, 2000 09:42


All times are GMT -4. The time now is 02:57.