 |
 |
 |
|
|
|
[Sponsors] | ||||
CyclicAMI: Unable to find initial target face |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 28, 2017, 23:31
|
CyclicAMI: Unable to find initial target face
|
#1 |
|
Member
Anders Utnes
Join Date: May 2017
Location: Norway
Posts: 34
Rep Power: 8  |
Hi
Im having a channel flow with a repeating geometry inside. To simplify this I'm using a LES model where I try to use the cyclic BC. Im using FreeCAD and SnappyHexMesh to generate the mesh, thus causing the iunlet and outlet to have a slight difference in faces. I try to compensate by using cyclicAMI. However, I keep getting the error "Unable to find initial target face". Does anyone know what this means? Code:
Boundary:
inlet
{
type cyclicAMI;
nFaces 3128;
startFace 400334;
matchTolerance 0.01;
transform noOrdering;
neighbourPatch outlet;
}
outlet
{
type cyclicAMI;
nFaces 3172;
startFace 403462;
matchTolerance 0.01;
transform noOrdering;
neighbourPatch inlet;
U:
inlet
{
type fixedValue;
value uniform (0.01 0 0);
}
outlet
{
type inletOutlet;
inletValue uniform (0 0 0);
value uniform (0.01 0 0);
}
P:
inlet
{
type cyclicAMI;
}
outlet
{
type cyclicAMI;
}
|
|
|
|
|
|
September 29, 2017, 00:03
|
|
#2 |
|
Member
Anders Utnes
Join Date: May 2017
Location: Norway
Posts: 34
Rep Power: 8 |
Resolved.
Turns out that my error was using noOrdering when I should use translational. Code:
Boundary:
inlet
{
type cyclicAMI;
nFaces 3128;
startFace 400334;
matchTolerance 0.001;
transform translational;
neighbourPatch outlet;
separationVector (0.000480 0 0);
}
outlet
{
type cyclicAMI;
nFaces 3172;
startFace 403462;
matchTolerance 0.001;
transform translational;
neighbourPatch inlet;
separationVector (-0.000480 0 0);
P:
inlet
{
type cyclicAMI;
}
outlet
{
type cyclicAMI;
}
|
|
|
|
|
|
|
March 6, 2019, 10:51
|
|
#3 |
|
Member
Min Zhang
Join Date: Mar 2017
Posts: 81
Rep Power: 9 |
Hello Alasir,
I am having similar issues with the implementation of cyclicAMI boundary condition. Your kind help would be greatly appreciated! My questions are as follows: (1) My patch2 and patch3 are quite different, does it matter? (2) What does "translational" mean here? (3) How to set the "separationVector" value? My patch2 position in y-direction is y=0 and patch3 position is y=2.19. Thanks in advance!! My CFD/constant/polyMesh/boundary file is attached below: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.x | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/cellZone_0/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 5 ( patch2 { type cyclicAMI;//symmetry; physicalType cyclicAMI;//symmetry; neighbourPatch patch3; nFaces 406; startFace 91945; transform translational; separationVector (0 -2.19 0); } patch3 { type cyclicAMI;//symmetry; physicalType cyclicAMI;//symmetry; neighbourPatch patch2; nFaces 351; startFace 92351; transform translational; separationVector (0 2.19 0); } inlet { type patch; physicalType patch; nFaces 316; startFace 92702; } outlet { type patch; physicalType patch; nFaces 160; startFace 93018; } walls { type wall; nFaces 42871; startFace 93178; } ) My errors are here: Number of processor faces = 3643 Max number of cells = 1156 (46.0249% above average 791.646) Max number of processor patches = 5 (41.1765% above average 3.54167) Max number of faces between processors = 229 (50.8647% above average 151.792) Time = 0 AMI: Creating addressing and weights between 406 source faces and 351 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 : (3.718 0 0.1752) target box span : (3.9 0 0.219) source box : (0 0 0.0219) (3.718 0 0.1971) target box : (0 4.38 0.0219) (3.9 4.38 0.2409) inflated target box : (-0.195307 4.18469 -0.173407) (4.09531 4.57531 0.436207) --> FOAM FATAL ERROR: Unable to find initial target face From function void Foam::AMIMethod<SourcePatch, TargetPatch>::initialise(labelListList&, scalarListList&, labelListList&, scalar\ ListList&, label&, label&) in file lnInclude/AMIMethod.C at line 149. FOAM aborting #0 Foam::error:  rintStack(Foam::Ostream&) at ??:?#1 Foam::error::abort() at ??:? #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(F\ oam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, int\ &, int&) at ??:? |
|
|
|
|
|
|
May 23, 2019, 06:13
|
|
#4 | |
|
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 6 |
Quote:
Anyone ? Thankyou in advance Vishsel |
||
|
|
|
||
|
April 4, 2020, 10:22
|
|
#5 |
|
New Member
Join Date: Jan 2015
Location: Berlin
Posts: 5
Rep Power: 11 |
For the sake of completeness and because I had the same question:
As far as I understood (and it seems to work in my case) the separationVector (x y z) is just the offset-vector (or translation vector) between your 2 patches - as seen from the patch where it is defined (as in the example above you have to specify it for both patches, so the second separationVector has the opposite dir. as the first one) |
|
|
|
|
|
|
September 18, 2020, 20:07
|
|
#6 | |
|
Member
Uttam
Join Date: May 2020
Location: Southampton, United Kingdom
Posts: 34
Rep Power: 5 |
Quote:
Did you find a solution to this? I am facing a similar problem. |
||
|
|
|
||
|
May 12, 2021, 16:42
|
|
#7 | |
|
Member
Gang Wang
Join Date: Oct 2019
Location: China
Posts: 64
Rep Power: 7 |
Dear Mr. Zhang,
Have you solved this issue? I've met the same error with urs for several days but I cannot find the solution. Best regards, Gang Quote:
|
||
|
|
|
||
|
May 26, 2023, 22:32
|
Unable to set source and target faces
|
#8 |
|
New Member
Helloy
Join Date: Jul 2012
Posts: 4
Rep Power: 13 |
Hello everyone,
I'm trying to simulate a fan by using sliding Mesh and cyclicAMI but I'm having the next error when I wanted to run with pimpleDyMFoam (v1712): [101] --> FOAM FATAL ERROR: [101] Unable to set source and target faces [101] [101] From function void Foam::faceAreaWeightAMI<SourcePatch, TargetPatch>::setNextFaces(Foam::label&, Foam::label&, Foam::label&, const boolList&, Foam::labelList&, const Foam:  ynamicList<int>&, bool) 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> >&>; Foam::label = int; Foam::boolList = Foam::List<bool>; Foam::labelList = Foam::List<int>][101] in file lnInclude/faceAreaWeightAMI.C at line 287. [101] FOAM parallel run aborting and this is my createPatchDict: FoamFile { version 2.0; format ascii; class dictionary; location system; object createPatchDict; } pointSync false; patches ( { name cm_fan_region_00_940w_brose_interface_ami; patchInfo { type cyclicAMI; matchTolerance 1.0E-4; neighbourPatch cm_fan_region_00_940w_brose_interface_slave_ami; transform noOrdering; } constructFrom patches; patches (cm_fan_region_00_940w_brose_interface); } { name cm_fan_region_00_940w_brose_interface_slave_ami; patchInfo { type cyclicAMI; matchTolerance 1.0E-4; neighbourPatch cm_fan_region_00_940w_brose_interface_ami; transform noOrdering; } constructFrom patches; patches (cm_fan_region_00_940w_brose_interface_slave); } ); the problem involves a rotational movement. If someone has an idea or suggestion, I will appreciate. |
|
|
|
|
|
|
|
|
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 with chtMultiregionFoam radiation boundary condition | baran_foam | OpenFOAM Running, Solving & CFD | 10 | December 17, 2019 17:36 |
| chtMultiRegionSimpleFoam: maximum number of iterations excedeed. | Nkl | OpenFOAM Running, Solving & CFD | 19 | October 10, 2019 02:42 |
| simpleFoam error - "Floating point exception" | mbcx4jc2 | OpenFOAM Running, Solving & CFD | 12 | August 4, 2015 02:20 |
| calculation stops after few time steps | sivakumar | OpenFOAM Running, Solving & CFD | 7 | March 17, 2013 06:37 |
10Likes
Linear Mode
