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

Inlet BC OpenFOAM 12

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 30, 2005, 04:04
Default It looks like in ver 1.2, tota
  #1
ghanshyam
Guest
 
Posts: n/a
It looks like in ver 1.2, totalPressureInlet and inletOutlet bcs have been removed. In ver 1.1 at the inlet, three options were there, i.e. totalPressureInlet, inletOutlet, and pressureInlet. Now only pressureIlnet is available. Am I correct or something is wrong with my installation?

Regards
GS
  Reply With Quote

Old   August 30, 2005, 04:14
Default No boundary conditions have be
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
No boundary conditions have been removed and some have been added. You will find the BC implementations in sub-directories of OpenFOAM-1.2/src/OpenFOAM/fields/fvPatchFields or in OpenFOAM-1.2/src/cfdTools/general/derivedFvPatchFields.
henry is offline   Reply With Quote

Old   August 30, 2005, 04:24
Default Thanks Henry. I am just going
  #3
ghanshyam
Guest
 
Posts: n/a
Thanks Henry. I am just going through the new version. Now at the "outlet" many more options are available and an extra "inletOutlet" category has been added in ver 1.2. This will be very usefull for external flows.

Thanks and regards
GS
  Reply With Quote

Old   August 30, 2005, 06:35
Default For k and epsilon wall BCs in
  #4
ghanshyam
Guest
 
Posts: n/a
For k and epsilon wall BCs in ver 1.1 we had two options (a) k -> fixedValue, epsilon -> zeroGradient
(b) wall function (i.e. zero gradient for k and epsilon)

These two options are still available in 1.2, but when I use option (a) I get following message:

------------------------------------------
--> FOAM FATAL ERROR : fixedValue is the wrong k patchField type for wall-functi
ons on patch plate_wall
should be zeroGradient

From function wall-function evaluation
in file /data/OpenFOAM/OpenFOAM-1.2/src/cfdTools/general/lnInclude/checkPatc
hFieldTypes.H at line 3.

FOAM exiting
------------------------------------------

It looks like it is forcing to use wall function. In case I do not want to use wall function what do I do?

Regards
GS
  Reply With Quote

Old   August 30, 2005, 06:45
Default All high-Re turbulence models
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
All high-Re turbulence models use wall-function of some kind because that is a requirement. For wall functions to work properly you must choose appropriate boundary conditions for the form of the implementation which in the case of OpenFOAM is zeroGradient on both k and epsilon. If you have been choosing otherwise your results will be wrong. To stop people making this error I have put in a check in 1.2.

If you don't want to use wall-functions choose a low-Re model with special near-wall modelling and run with a mesh fine enough in the near-wall region for it to be stable. There are several low-Re turbulence models to choose from.

If you don't like either of these options there are two others, either run with slip walls or implement the model and boundary conditions you think is best for your purpose.
henry is offline   Reply With Quote

Old   August 30, 2005, 07:16
Default Thanks Henry for the clarifica
  #6
ghanshyam
Guest
 
Posts: n/a
Thanks Henry for the clarification. I will prefer to go for realizable k epsilon model with a two layer approach near the wall. Which you know I have already implemented. I will test and see how it works with this version.

Regards
GS
  Reply With Quote

Old   August 30, 2005, 07:20
Default ... and you should choose the
  #7
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
... and you should choose the k-epsilon BCs that are appropriate for your implementation of the two layer approach which may not be a standard option in FoamX so you might have to either edit the k-epsilon files by hand and specify the BCs that way or add the options you require to the FoamX configuration files.
henry is offline   Reply With Quote

Old   August 30, 2005, 07:44
Default Thats right. Basically it will
  #8
ghanshyam
Guest
 
Posts: n/a
Thats right. Basically it will be same as the one for low Re models.

Regards
GS
  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
OpenFoam vs CFX5 mass balance in OpenFoam tangd OpenFOAM Running, Solving & CFD 33 May 23, 2010 16:36
CheckMesh error using a tutorial from OpenFOAM 114 with openFOAM 13 martapajon OpenFOAM Native Meshers: blockMesh 7 January 21, 2008 13:52
OpenFOAM users in Munich OpenFOAM benutzer in M%c3%bcnchen jaswi OpenFOAM 0 August 3, 2007 13:11
A new Howto on the OpenFOAM Wiki Compiling OpenFOAM under Unix mbeaudoin OpenFOAM Installation 2 April 28, 2006 08:54
How to set smoke inlet speed on inlet Adam FLUENT 0 October 4, 2005 08:18


All times are GMT -4. The time now is 02:43.