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

decompose with wallfunctions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 14, 2009, 04:06
Default decompose with wallfunctions
  #1
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

I'm having some problems decomposing a case with wallfunctions.
If I run it in serial there are no problems but when trying to decompose I get this error (below).

If I add the "value uniform 0;" below the kqRWallFunction line I can decompose but I don't see why this should be required when using high Re turb model in parallel.

My k and epsilon entry for the wall

propeller
{
type kqRWallFunction;
}

propeller
{
type epsilonWallFunction;
}

Cannot find 'value' entry on patch propeller of field k in file "/home/nini/OpenFOAM/nini-1.6/run/Full3d/P1410_4/0/k"
which is required to set the values of the generic patch field.
(Actual type kqRWallFunction)

Please add the 'value' entry to the write function of the user-defined boundary-condition
or link the boundary-condition into libfoamUtil.so

file: /home/nini/OpenFOAM/nini-1.6/run/Full3d/P1410_4/0/k:ropeller from line 55 to line 55.
From function genericFvPatchField<Type>::genericFvPatchField(con st fvPatch&, const Field<Type>&, const dictionary&)
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 72.
linnemann is offline   Reply With Quote

Old   September 14, 2009, 10:23
Default
  #2
Member
 
santhosh
Join Date: Apr 2009
Location: pune, India
Posts: 67
Rep Power: 8
santoo_cfd is on a distinguished road
I also faced this problem. One trickier solution would be to run in serial till the openFOAM creates new k and epsilon files and moves old files as k.old and epsilon.old, try decomposepar then.

But It would be nice if decomposePar utility changed to consider keqWallfunction boundary too.

Santosh..
santoo_cfd is offline   Reply With Quote

Old   September 14, 2009, 11:22
Default
  #3
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
I did something similar.

I just decomposed and then deleted the "value" line in each of the k/epsilon files under each processor folder, not a nice approach but it works :-)
linnemann is offline   Reply With Quote

Old   October 16, 2009, 05:03
Default
  #4
Member
 
John Wang
Join Date: Mar 2009
Location: Singapore
Posts: 71
Rep Power: 8
cwang5 is on a distinguished road
Humm... I've read some post that uses
value $internalField;
not sure what it does, but seems to be working.
cwang5 is offline   Reply With Quote

Old   October 16, 2009, 06:41
Default
  #5
New Member
 
Matteo Carpentieri
Join Date: Mar 2009
Posts: 28
Rep Power: 8
mcarpe is on a distinguished road
Hi,
as far as I understand the behaviour of the wall function routines in OpenFOAM, I believe that the values in the BC are just placeholders. They are not used by the solvers and are re-calculated for the wall patches. However, some of the utilities will complain if a value is not provided (decomposePar and paraFoam, for example). I believe this is a bug, and the only solution, for now, is to provide 'dummy' values (for example the same value as the internal field, or 0).

This is just my opinion, maybe someone more expert than me will deliver a better answer

@cwang5: I think that statement is just another way of using the internal field values; as I was saying above, it should not have any effect on the calculations.
mcarpe 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
CGNS converters available mbeaudoin OpenFOAM Meshing & Mesh Conversion 125 July 1, 2015 21:09
Wallfunctions onoff gjesing OpenFOAM Running, Solving & CFD 5 February 11, 2010 00:55
Regarding wallFunctions Hectux OpenFOAM Running, Solving & CFD 0 May 29, 2009 03:23
Serial OK parallel failsmesh conversion problem r2d2 OpenFOAM Running, Solving & CFD 15 July 31, 2008 15:04
Bug in twoPhaseEulerFoam wallfunctions alberto OpenFOAM Bugs 1 February 9, 2007 15:15


All times are GMT -4. The time now is 01:56.