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

Specify turbulent inlet

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 29, 2006, 02:49
Default I want to specify a inlet flow
  #1
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
I want to specify a inlet flow with backround turbulence. For this reason I have defined a inlet bc with fixed value for k and epsilon (I am using the k-e epsilon turbulence model). But the following error occurs:

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

I know I am using a high-Re turbulence model with wallfunctions and because of that I have to use zeroGradient at the walls.
But in my case I want to define a turbulent inlet.

Does anybody know what is going wrong or what I have to do?
chris1980 is offline   Reply With Quote

Old   August 29, 2006, 02:55
Default Yes. You have specified patch
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Yes. You have specified patch type wall for your inlet, which is not clever. You will find this either in your blockMeshDict or in the boundary file, depending where you got the mesh from.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 29, 2006, 03:03
Default Hrv, I have defined my inle
  #3
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
Hrv,

I have defined my inlet patch as type 'patch' not as wall?
chris1980 is offline   Reply With Quote

Old   August 29, 2006, 03:09
Default solved http://www.cfd-online.c
  #4
Member
 
chris book
Join Date: Mar 2009
Posts: 85
Rep Power: 8
chris1980 is on a distinguished road
solved

The problem was caused due an old boundary file in polymesh (blockmesh does not update it?).
chris1980 is offline   Reply With Quote

Old   August 29, 2006, 03:11
Default The code says: forAll(p
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
The code says:

forAll(patches, patchi)
{
const fvPatch& curPatch = patches[patchi];

if (isType<wallfvpatch>(curPatch))
{
# include "checkPatchFieldTypes.H"


and in checkPatchFieldTypes.H

if (!isType<zerogradientfvpatchscalarfield>(k_.bounda ryField()[patchi]))
{
FatalErrorIn("wall-function evaluation")
<< k_.boundaryField()[patchi].type()
<< " is the wrong k patchField type for wall-functions on patch "
<< curPatch.name() << nl
<< " should be zeroGradient"
<< exit(FatalError);

}

As you can see, you patch IS a wall.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Inlet turbulent boundary condition: external flows ROOZBEH FLUENT 2 February 8, 2009 08:02
Inlet turbulent boundary condition, external flows ROOZBEH Main CFD Forum 1 February 6, 2009 13:37
Turbulent inlet fluctuation scale christian OpenFOAM Running, Solving & CFD 1 April 2, 2008 06:08
turbulent inlet generation ricklee Main CFD Forum 0 July 2, 2006 11:46
inlet turbulent B.C. ROOZBEH FLUENT 3 September 25, 2003 07:07


All times are GMT -4. The time now is 19:06.