|
[Sponsors] |
cyclic boundary with same geometric size but different number of faces? (2018 ver.) |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Brent Shambaugh
Join Date: Nov 2018
Posts: 8
Rep Power: 7 ![]() |
I am having trouble with a boundary that involves a changing grid density. I think I need to use cyclicAMI instead of cyclic. There was a post with this question in 2012 about this linked to below.
The mesh looks like this: ![]() ![]() Observe that there are 20 faces on the left and 40 faces on the right of the boundary in the center. The error message is: Code:
For patch leftRightWallleft there are 20 face centres, for the neighbour patch leftRightWallsright there are 40 From function void Foam::cyclicPolyPatch::calcTransforms(const primitivePatch&, const pointField&, const vectorField&, const pointField&, const vectorField&) in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 156.--> FOAM FATAL ERROR: e.g. Code:
leftRightWallleft { type cyclic; neighbourPatch leftRightWallsright; nFaces 20; startFace 4720; } Code:
leftRightWallleft { type cyclicAMI; neighbourPatch leftRightWallsright; nFaces 20; startFace 4720; } For my Files, I replaced cyclic with cyclicAMI. (https://github.com/bshambaugh/openfo...lbow-twoFaces/) in constant/polyMesh/boundary Code:
leftRightWallleft { type cyclicAMI; neighbourPatch leftRightWallsright; nFaces 20; startFace 4720; } leftRightWallsright { type cyclicAMI; neighbourPatch leftRightWallleft; nFaces 40; startFace 4760; } Code:
leftRightWallleft { type cyclicAMI; nFaces 20; startFace 4720; } leftRightWallsright { type cyclicAMI; nFaces 40; startFace 4760; } Code:
leftRightWallleft { type cyclicAMI; nFaces 20; startFace 4720; } leftRightWallsright { type cyclicAMI; nFaces 40; startFace 4760; } Last edited by bshambaugh; November 5, 2018 at 09:36. Reason: adding error message |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Brent Shambaugh
Join Date: Nov 2018
Posts: 8
Rep Power: 7 ![]() |
This is a compound mesh that was created in Salome, and then modified to work with OpenFoam. A method similar to what I used is described here [1].
To solve this problem, I will look at Glue Faces in Salome [2], and MergeMesh and StitchMesh in OpenFoam [3]. Edit: Bookmarking this. It seems close. Problem using AMI [1] http://staff.um.edu.mt/__data/assets...o_OpenFOAM.pdf [2] http://www.salome-platform.org/forum/forum_10/818415930 [3] MergeMesh and stitchMesh Last edited by bshambaugh; November 5, 2018 at 20:17. Reason: Added a link to update progress, specifically pointing out edit |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Brent Shambaugh
Join Date: Nov 2018
Posts: 8
Rep Power: 7 ![]() |
I ran the code and I obtained in log.icoFoam: "
"ill defined primitiveEntry starting at keyword 'value' ..." Below is log.icoFoam followed by the constant/polyMesh/boundary, 0/p and 0/U configuration files. Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 4.1 Exec : icoFoam Date : Nov 10 2018 Time : 15:33:30 Host : "caelinux" PID : 30779 Case : /home/caelinux/OpenFOAM/caelinux-4.1/run/tutorials/incompressible/icoFoam/elbow-fchannel nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 PISO: Operating solver in PISO mode Reading transportProperties Reading field p AMI: Creating addressing and weights between 40 source faces and 20 target faces AMI: Patch source sum(weights) min/max/average = 1, 1, 1 AMI: Patch target sum(weights) min/max/average = 1, 1, 1 Reading field U --> FOAM FATAL IO ERROR: "ill defined primitiveEntry starting at keyword 'value' on line 63 and ending at line 69" file: /home/caelinux/OpenFOAM/caelinux-4.1/run/tutorials/incompressible/icoFoam/elbow-fchannel/0/U at line 69. From function void Foam::primitiveEntry::readEntry(const Foam::dictionary&, Foam::Istream&) in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 189. FOAM exiting Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 10 ( leftRightWallsright { type cyclicAMI; neighbourPatch leftRightWallleft; transform noOrdering; nFaces 40; startFace 3880; } outlet { type patch; nFaces 40; startFace 3920; } channelWallsright { type wall; nFaces 80; startFace 3960; } destinationFaceright { type wall; nFaces 1600; startFace 4040; } sourceFaceright { type wall; nFaces 1600; startFace 5640; } sourceFaceleft { type wall; nFaces 400; startFace 7240; } destinationFaceleft { type wall; nFaces 400; startFace 7640; } channelWallsleft { type wall; nFaces 40; startFace 8040; } leftRightWallleft { type cyclicAMI; neighbourPatch leftRightWallsright; transform noOrdering; nFaces 20; startFace 8080; } inlet { type patch; nFaces 20; startFace 8100; } ) // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { leftRightWallsright { type cyclicAMI; } outlet { type fixedValue; value uniform 0; } channelWallsright { type zeroGradient; } destinationFaceright { type zeroGradient; } sourceFaceright { type zeroGradient; } sourceFaceleft { type zeroGradient; } destinationFaceleft { type zeroGradient; } channelWallsleft { type zeroGradient; } leftRightWallleft { type cyclicAMI; } inlet { type zeroGradient; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { leftRightWallsright { type cyclicAMI; } outlet { type zeroGradient; } channelWallsright { type fixedValue; value uniform 0; } destinationFaceright { type noSlip; } sourceFaceright { type noSlip; } sourceFaceleft { type noSlip; } destinationFaceleft { type noSlip; } channelWallsleft { type noSlip; } leftRightWallleft { type cyclicAMI; } inlet { type fixedValue; value uniform(1 0 0); } } // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#4 | |
Senior Member
Robert
Join Date: May 2015
Location: Bremen, GER
Posts: 292
Rep Power: 12 ![]() |
Quote:
But on line 63 i find Code:
value uniform(1 0 0); Furthermore, on line 34 you have Code:
value uniform 0;
__________________
If you liked my answer to your question, please consider leaving a "Like" in return ![]() |
||
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[General] Extracting ParaView Data into Python Arrays | Jeffzda | ParaView | 30 | November 6, 2023 21:00 |
simpleFoam parallel | AndrewMortimer | OpenFOAM Running, Solving & CFD | 12 | August 7, 2015 18:45 |
SigFpe when running ANY application in parallel | Pj. | OpenFOAM Running, Solving & CFD | 3 | April 23, 2015 14:53 |
[snappyHexMesh] crash sHM | H25E | OpenFOAM Meshing & Mesh Conversion | 11 | November 10, 2014 11:27 |
Cluster ID's not contiguous in compute-nodes domain. ??? | Shogan | FLUENT | 1 | May 28, 2014 15:03 |