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

simpleFooUnable to find initial target face

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 29, 2017, 19:04
Default simpleFooUnable to find initial target face
  #1
Member
 
Vedamt Chittlangia
Join Date: Feb 2016
Posts: 64
Rep Power: 6
vcvedant is an unknown quantity at this point
Hello,

I am simulating flow past an airfoil in OpenFOAM. I have created the mesh in Pointwise and then exported it as CAE from Pointwise. I have the following boundary conditions:

INLET -> fixedValue
OUTLET -> zeroGradient;
Periodic_1 -> cyclicAMI, neighbourPatch Periodic_2;
Periodic_2 -> cyclicAMI , neighbourPatch Periodic_1;
frontAndBack -> Empty;
CS -> wall;

I checked the mesh using checkMesh and found it to be OK.
But when I run the simulation using
Code:
simpleFoam
I get the following error: unable to find initial target face
Code:
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

AMI: Creating addressing and weights between 453 source faces and 387 target faces
--> FOAM Warning : 
    From function AMIMethod<SourcePatch, TargetPatch>::checkPatches()
    in file lnInclude/AMIMethod.C at line 57
    Source and target patch bounding boxes are not similar
    source box span     : (1.552 0.796554 0.0388)
    target box span     : (1.552 0.796554 0.0388)
    source box          : (-0.430502 -0.0584186 0) (1.1215 0.738135 0.0388)
    target box          : (-0.430502 -0.515211 0) (1.1215 0.281343 0.0388)
    inflated target box : (-0.517747 -0.602456 -0.0872454) (1.20874 0.368588 0.126045)


--> FOAM FATAL ERROR: 
Unable to find initial target face

    From function void Foam::AMIMethod<SourcePatch, TargetPatch>::initialise(labelListList&, scalarListList&, labelListList&, scalarListList&, label&, label&)
    in file lnInclude/AMIMethod.C at line 149.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::AMIMethod<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::initialise(Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, int&, int&) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#3  Foam::faceAreaWeightAMI<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::calculate(Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, int, int) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#4  Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::update(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#5  Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::constructFromSurface(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::autoPtr<Foam::searchableSurface> const&) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#6  Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::AMIInterpolation(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::autoPtr<Foam::searchableSurface> const&, Foam::faceAreaIntersect::triangulationMode const&, bool, Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::interpolationMethod const&, double, bool) in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#7  Foam::cyclicAMIPolyPatch::resetAMI(Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::interpolationMethod const&) const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#8  Foam::cyclicAMIPolyPatch::AMI() const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#9  Foam::cyclicAMIPolyPatch::applyLowWeightCorrection() const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#10  Foam::cyclicAMIFvPatch::makeWeights(Foam::Field<double>&) const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#11  Foam::surfaceInterpolation::makeWeights() const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::surfaceInterpolation::weights() const in "/gpfs/home/vjc5126/work//OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#13  Foam::tmp<Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::linearInterpolate<Foam::Vector<double> >(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/gpfs/home/vjc5126/work/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/simpleFoam"
#14  ? in "/gpfs/home/vjc5126/work/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/simpleFoam"
#15  __libc_start_main in "/lib64/libc.so.6"
#16  ? in "/gpfs/home/vjc5126/work/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/simpleFoam"
Aborted (core dumped)
I think it has to do something with cyclicAMI but I cannot understand what is the problem. I am attaching my case folder. I will be really grateful if somebody can help me resolve this.

Here is the link to the case: case

Thanks,

Vedant


Update: I re-checked the geometry and the periodic BCs have the same area and shape

Last edited by vcvedant; August 29, 2017 at 21:58. Reason: update
vcvedant is offline   Reply With Quote

Old   August 29, 2017, 22:34
Default
  #2
Member
 
Vedamt Chittlangia
Join Date: Feb 2016
Posts: 64
Rep Power: 6
vcvedant is an unknown quantity at this point
I am able to get resolve this issue by adding in the constant/polyMesh/boundary:
Code:
Periodic_1
{
   type    cyclicAMI;
   :
   :
   transform  translational;
   separationVector   (0 0.4567923 0);
}
Same was added to Periodic_2 but with negative value of y-component of the vector.


But now the when I run the simpleFoam, I get 'nan' in the first iteration for p.
vcvedant is offline   Reply With Quote

Old   August 30, 2017, 09:48
Default
  #3
Member
 
Vedamt Chittlangia
Join Date: Feb 2016
Posts: 64
Rep Power: 6
vcvedant is an unknown quantity at this point
Another update: I changed the solver type for p and the simulation proceeds further but got very high continuity errors, 10^28. Then I ran the case in laminar and let the velocity field develop. Thereafter I turned on the turbulence and the continuity errors decreased.
I will update this post if I am able to solve this post and get results as per some previous studies in FLUENT and CFX.

PS: Please feel free if anyone wants to give their inputs.

Thanks
vcvedant is offline   Reply With Quote

Old   September 6, 2018, 10:43
Default
  #4
New Member
 
Thomas M
Join Date: Aug 2018
Posts: 13
Rep Power: 4
tmik is on a distinguished road
Any more details on this? I have the same error:


Code:
Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.0001
    field Ux     tolerance 0.0001
    field Uy     tolerance 0.0001
    field k      tolerance 0.0001
    field epsilon        tolerance 0.0001

Reading field p

AMI: Creating addressing and weights between 76 source faces and 76 target faces
--> FOAM Warning :
    From function void Foam::AMIMethod<SourcePatch, TargetPatch>::checkPatches() const [with SourcePatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>; TargetPatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>]
    in file lnInclude/AMIMethod.C at line 57
    Source and target patch bounding boxes are not similar
    source box span     : (0.164987 0.0569055 0.0005)
    target box span     : (0.164987 0.0569055 0.0005)
    source box          : (-0.186475 0.0302639 0) (-0.0214882 0.0871693 0.0005)
    target box          : (-0.186475 -0.141037 0) (-0.0214882 -0.0841312 0.0005)
    inflated target box : (-0.195201 -0.149763 -0.00872627) (-0.0127619 -0.0754049 0.00922627)


--> FOAM FATAL ERROR:
Unable to find initial target face

    From function bool Foam::AMIMethod<SourcePatch, TargetPatch>::initialise(Foam::labelListList&, Foam::scalarListList&, Foam::labelListList&, Foam::scalarListList&, Foam::label&, Foam::label&) [with SourcePatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>; TargetPatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>; Foam::labelListList = Foam::List<Foam::List<int> >; Foam::scalarListList = Foam::List<Foam::List<double> >; Foam::label = int]
    in file lnInclude/AMIMethod.C at line 127.

FOAM aborting
using type cyclicAMI in both boundary and constraint files. Somehow it works fine with type cyclic as long as my tolerance is 0.11 (large tolerance).

Last edited by tmik; September 10, 2018 at 08:16.
tmik is offline   Reply With Quote

Old   May 13, 2019, 03:29
Default separationVector
  #5
Member
 
Vishsel
Join Date: May 2019
Posts: 54
Rep Power: 3
Vishsel is on a distinguished road
Hi all,

May i know how to define value for separationVector in createPatchDict ?

Thanks in advance,
Vishsel.
Vishsel is offline   Reply With Quote

Old   July 11, 2019, 21:07
Default
  #6
Member
 
Neilson Whit
Join Date: Aug 2011
Posts: 72
Rep Power: 11
wolfindark is on a distinguished road
Quote:
Originally Posted by Vishsel View Post
Hi all,

May i know how to define value for separationVector in createPatchDict ?

Thanks in advance,
Vishsel.
the vectors are not referencing the origin of global coordinates. instead, you should write the vectors by taking the origin of the surface coordinates.

surface1 surface2
at (-2 0 0) at (2 0 0)
| ---------------------> |

the separation vector for your surface1 will be (4 0 0) which shows that your neighbour surface surface2 separated from your reference surface1 with that vector.
wolfindark is offline   Reply With Quote

Old   July 12, 2019, 09:33
Default Thanks
  #7
New Member
 
Thomas M
Join Date: Aug 2018
Posts: 13
Rep Power: 4
tmik is on a distinguished road
Thanks Wolfinthedark! I had no idea, but you are correct.
I was using the vector from the origin instead of between surfaces (or in my case edges)

Code:
Wrong way:
                             |<--------------------.------------------->|
[vector: (0 -2 0)]   surface1                 origin                 surface2  [vector: (0 2 0)]
 
_________________________________________________________
 
Correct way:
     |--------------------------------------->|
surface1                                       surface2  [vector: (0 4 0)]
 
     |<---------------------------------------|
surface1                                       surface2 [vector: (0 -4 0)]
tmik is offline   Reply With Quote

Reply

Tags
airfoil 2d, cyclic boundary, cyclicami, periodic bc

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Maximum number of iterations exceeded chtmultiregionsimpleFoam Moncef OpenFOAM Running, Solving & CFD 28 July 13, 2020 14:26
Problem Building OF on Centos cluster (no admin rights) CKH OpenFOAM Installation 5 November 13, 2011 06:32
Error while running rhoPisoFoam.. nileshjrane OpenFOAM Running, Solving & CFD 8 August 26, 2010 12:50
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16
[blockMesh] BlockMeshmergePatchPairs hjasak OpenFOAM Meshing & Mesh Conversion 11 August 15, 2008 07:36


All times are GMT -4. The time now is 22:25.