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

About empty patch in parallel run

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 30, 2009, 00:51
Default About empty patch in parallel run
  #1
New Member
 
Zheng.Zhi
Join Date: Jul 2009
Location: LanZhou China
Posts: 10
Rep Power: 8
Zheng.Zhi is on a distinguished road
For chtMultiRegionFoam parallel run , I have written a small modification to decomposePar that works on regions' mesh after splitMeshRegion .
After decomposition , maybe regionI's mesh all distribute in processor0 and none distribute in processor1 .

when I use symmetry plane for a 2D case , it works well , but empty patch does not work .

I found empty patch's updateCoeffs() does not allow zero mesh number:

template<class Type>
void emptyFvPatchField<Type>::updateCoeffs()
{
if
(
this->patch().patch().size()
% this->dimensionedInternalField().mesh().nCells()
)
{
FatalErrorIn("emptyFvPatchField<Type>::updateCoeff s()")
<< "This mesh contains patches of type empty but is not 1D or 2D\n"
" by virtue of the fact that the number of faces of this\n"
" empty patch is not divisible by the number of cells."
<< exit(FatalError);
}


}

When I modify updateCoeffs() , let it does nothing :

template<class Type>
void emptyFvPatchField<Type>::updateCoeffs()
{
}

Then when regionI is a solid region, it works , but when regionI is a fluid region , still have problem :

[ff02:29082] *** An error occurred in MPI_Recv
[ff02:29082] *** on communicator MPI_COMM_WORLD
[ff02:29082] *** MPI_ERR_TRUNCATE: message truncated
[ff02:29082] *** MPI_ERRORS_ARE_FATAL (goodbye)

it occurs when solve(U equation) in UEqn.H of chtMultiRegionFoam :

fEqnResidual = solve
(
UEqn() == -fvc::grad(pf[i])
).initialResidual();

So I don't know why empty patch can't work when regionI have Zero mesh number in processor1 , but symmetry plane can work well .

Can anybody help me with this problem? Thanks.


Zheng.Zhi is offline   Reply With Quote

Old   July 30, 2009, 07:55
Default
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
I've pushed a fix for the division by zero (cells) to 1.6.x.

2) if you are running chtMultiRegionFoam, the 1.6 version allows independent decomposition of all regions so you're highly unlikely to get zero cells. Look at the Allrun script in the tutorial.
mattijs is offline   Reply With Quote

Old   August 2, 2009, 22:01
Default
  #3
New Member
 
Zheng.Zhi
Join Date: Jul 2009
Location: LanZhou China
Posts: 10
Rep Power: 8
Zheng.Zhi is on a distinguished road
HiMr.Mattijs :

I've run the multiRegionHeater tutorial of OpenFoam version 1.6 , yes the chtMultiRegionFoam can run in parallel well . That's great , Thank you very much Mattijs .
Zheng.Zhi 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
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51
Cyclic patch in parallel calculations didomenico OpenFOAM Running, Solving & CFD 4 March 7, 2007 06:46
Run in parallel a 2mesh case cosimobianchini OpenFOAM Running, Solving & CFD 2 January 11, 2007 07:33
Minimum number of nodes to run CFX in parallel Rui CFX 3 April 11, 2005 20:46
How to run parallel in ICEM_CFD? Kiddo Main CFD Forum 2 January 24, 2005 09:53


All times are GMT -4. The time now is 00:47.