|
[Sponsors] |
November 28, 2023, 18:48 |
Cannot find patchField entry for motorBike
|
#1 |
New Member
Alejandro Vargas
Join Date: Nov 2023
Posts: 4
Rep Power: 3 |
Greetings OpenFOAM community,I've encountered an error that's left me a bit stumped. I've been working on adapting a simulation from a motorBike case to a new geometry, specifically an F1 rear wing, for simplicity's sake. However, I only changed the name of the new geometry while keeping the internal structure the same as motorBike.
Despite only renaming the new geometry without altering the internal structure, I'm facing the persistent error message "Cannot find patchField entry for motorBike" when running the simulation. Is there a specific file or setting within OpenFOAM where the reference to the motorBike case might still be lingering, causing this error? I haven't modified any other settings except for the name change of the new geometry, the blockMeshDict and some things of the snappyHexMeshDict. I'd greatly appreciate any insights or suggestions on how to resolve this issue. Thank you! This is the error message: [3] --> FOAM FATAL IO ERROR: [3] Cannot find patchField entry for motorBike [3] [3] file: /root/OpenFOAM/root-11/run/alerondrs/motorBike/motorBike/processor3/0/p/boundaryField from line [4] [4] [4] --> FOAM FATAL IO ERROR: [4] Cannot find patchField entry for motorBike [4] [4] file: /root/OpenFOAM/root-11/run/alerondrs/motorBike/motorBike/processor4/0/p/boundaryField from line 25[0] [0] [0] --> FOAM FATAL IO ERROR: [0] Cannot find patchField entry for motorBike [0] [0] file: /root/OpenFOAM/root-11/run/alerondrs/motorBike/motorBike/processor0/0/p/boundaryField from line 25 to line 54. [0] [0] From function void Foam::GeometricBoundaryField<Type, PatchField, GeoMesh>::readField(const Foam:imensionedField<TypeR, GeoMesh>&, const Foam::dictionary&) [with Type = double; PatchField = Foam::fvPatchField; GeoMesh = Foam::volMesh][1] [1] And this is the 0/p file: Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 11 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { format ascii; class volScalarField; location "0"; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } lowerWall { type symmetryPlane; } "motorBike_.*" { type zeroGradient; } upperWall { type symmetryPlane; } front { type symmetryPlane; } back { type symmetryPlane; } "proc.*" { type processor; } } // ************************************************************************* // Last edited by Alejandro VR; November 28, 2023 at 21:39. |
|
November 29, 2023, 04:11 |
|
#2 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,223
Rep Power: 28 |
Hello,
What do you see in your constant/polyMesh/boundary file? (or processor*/constant/polyMesh/boundary if you're running in parallel) Yann |
|
November 29, 2023, 11:34 |
|
#3 | |
New Member
Alejandro Vargas
Join Date: Nov 2023
Posts: 4
Rep Power: 3 |
Quote:
Yes, this is it the processor*/constatn/polyMesh/boundary: Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 11 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { format binary; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 11 ( front { type symmetryPlane; inGroups List<word> 1(symmetryPlane); nFaces 0; startFace 405332; } back { type symmetryPlane; inGroups List<word> 1(symmetryPlane); nFaces 0; startFace 405332; } inlet { type patch; nFaces 0; startFace 405332; } outlet { type patch; nFaces 0; startFace 405332; } lowerWall { type symmetryPlane; inGroups List<word> 1(symmetryPlane); nFaces 0; startFace 405332; } upperWall { type symmetryPlane; inGroups List<word> 1(symmetryPlane); nFaces 0; startFace 405332; } motorBike { type wall; inGroups List<word> 1(wall); nFaces 41312; startFace 405332; } procBoundary0to1 { type processor; inGroups List<word> 1(processor); nFaces 1427; startFace 446644; matchTolerance 0.0001; myProcNo 0; neighbProcNo 1; } procBoundary0to2 { type processor; inGroups List<word> 1(processor); nFaces 658; startFace 448071; matchTolerance 0.0001; myProcNo 0; neighbProcNo 2; } procBoundary0to3 { type processor; inGroups List<word> 1(processor); nFaces 1; startFace 448729; matchTolerance 0.0001; myProcNo 0; neighbProcNo 3; } procBoundary0to5 { type processor; inGroups List<word> 1(processor); nFaces 1536; startFace 448730; matchTolerance 0.0001; myProcNo 0; neighbProcNo 5; } ) // ************************************************************************* // And i forgot to write it, but the step im following are the same (without the importing part), of the Allrun file: Code:
#!/bin/sh cd ${0%/*} || exit 1 # Run from this directory # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions runApplication blockMesh runApplication decomposePar -copyZero runParallel snappyHexMesh -overwrite find . -type f -iname "*level*" -exec rm {} \; runParallel renumberMesh -overwrite runParallel potentialFoam -initialiseUBCs runParallel $(getApplication) #------------------------------------------------------------------------------ |
||
November 29, 2023, 11:42 |
|
#4 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,223
Rep Power: 28 |
Alright, in the boundary file you have a patch named motorBike but in your boundary conditions you are defining conditions for every patches starting with motorBike_
So the solver complains because it cannot find a boundary condition for the patch motorBike Update your files in 0 directory with motorBike (match only the patch named motorBike) or "motorBike.*" (matches any patches starting with motorBike) instead of "motorBike_.*" Cheers, Yann |
|
November 29, 2023, 12:17 |
|
#5 | |
New Member
Alejandro Vargas
Join Date: Nov 2023
Posts: 4
Rep Power: 3 |
Quote:
Omg, that worked, you helped me a lot, thanks |
||
Tags |
error, running, simulation |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Cannot find patchField entry for *** | mbox97 | OpenFOAM Meshing & Mesh Conversion | 2 | November 25, 2021 11:06 |
Cannot find patchField entry for InletWall | range_rover | OpenFOAM Running, Solving & CFD | 5 | November 18, 2020 22:21 |
Parallel snappyHexMesh problem: Cannot find patchField entry for procBoundary2to7 | hconel | OpenFOAM Pre-Processing | 0 | October 5, 2018 18:22 |
OpenFOAM 1.6-ext git installation on Ubuntu 11.10 x64 | Attesz | OpenFOAM Installation | 45 | January 13, 2012 13:38 |
Problem Building OF on Centos cluster (no admin rights) | CKH | OpenFOAM Installation | 5 | November 13, 2011 07:32 |