|
[Sponsors] |
February 26, 2016, 09:20 |
patch problem with chtMultiRegionSimpleFoam
|
#1 |
New Member
Join Date: Feb 2016
Posts: 2
Rep Power: 0 |
Hi,
I am learning to use chtMultiRegionSimpleFoam by creating a 2D case with a solid box (called wall) on the floor encircled by air. The bottom of the wall has a temperature higher than the rest of the domain (500K for bottom wall and 300K for the rest). I am using the tutorial planeWall2D to realize my case. I have two domains: domain0 air and domain1 wall. The interface between solid region and fluid region is defined by: - wall_to_air for domain1 - air_to_wall for domain0 When I run the case I obtained this fatal error : /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.x | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ /* Windows port by CFD support (www.cfdsupport.com) [based on Symscape] *\ \*---------------------------------------------------------------------------*/ Build : 2.3.x-819030ed51bd Exec : C:\OpenFOAM\*** fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region domain0 for time = 0 Create solid mesh for region domain1 for time = 0 *** Reading fluid mesh thermophysical properties for region domain0 Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to turbulence Selecting turbulence model type laminar Adding to ghFluid Adding to ghfFluid Selecting radiationModel none Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region domain1 Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Selecting radiationModel opaqueSolid Selecting absorptionEmissionModel constantAbsorptionEmission Selecting scatterModel none Adding fvOptions No finite volume options present Time = 1 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.001204138, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0115684, No Iterations 1 --> FOAM FATAL ERROR: Cannot find patch wall_to_air in region domain0 Valid patches are 6 ( leftlet rightlet topair bottom_air air_to_wall frontAndBackPlanes ) From function mappedPatchBase::samplePolyPatch() in file mappedPatches/mappedPolyPatch/mappedPatchBase.C at line 1259. FOAM exiting I don't understand because the patch wall_to_air doesn't need to be in the domain0, it is the interface of domain1. Does anybody know where this problem comes from? |
|
February 26, 2016, 10:57 |
|
#2 |
Member
Joćo Ferreira
Join Date: Nov 2014
Location: Braga, Portugal
Posts: 53
Rep Power: 11 |
From the error it appears that the error is in the boundary (polyMesh folder) file, where you define the wall_to_air.
Perhaps you could post that file here to see if there's any error. Regards |
|
February 27, 2016, 02:52 |
|
#3 |
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 20 |
The error message tells you that the region you specified only has these patches available
Code:
Cannot find patch wall_to_air in region domain0 ( leftlet rightlet topair bottom_air air_to_wall frontAndBackPlanes ) |
|
February 29, 2016, 03:08 |
|
#4 |
New Member
Join Date: Feb 2016
Posts: 2
Rep Power: 0 |
Thank you for your responses. You can find, in the following, the "PolyMesh" boundary:
FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 8 ( leftlet { type patch; inGroups 1(patch); nFaces 28; startFace 1484; } rightlet { type patch; inGroups 1(patch); nFaces 28; startFace 1512; } topair { type symmetryPlane; inGroups 1(symmetryPlane); nFaces 28; startFace 1540; } bottomair { type wall; inGroups 1(wall); nFaces 14; startFace 1568; } bottomwall { type wall; inGroups 1(wall); nFaces 14; startFace 1582; } air_to_wall { type mappedWall; inGroups 1(wall); nFaces 28; startFace 1596; sampleMode nearestPatchFace; sampleRegion domain0; samplePatch wall_to_air; } wall_to_air { type mappedWall; inGroups 1(wall); nFaces 28; startFace 1624; sampleMode nearestPatchFace; sampleRegion domain1; samplePatch air_to_wall; } frontAndBackPlanes { type empty; inGroups 1(empty); nFaces 1568; startFace 1652; } ) |
|
February 29, 2016, 04:50 |
|
#5 |
Member
Joćo Ferreira
Join Date: Nov 2014
Location: Braga, Portugal
Posts: 53
Rep Power: 11 |
As Bloerb said, the sampleRegion of the mappedWall boundaries is wrongly defined.
The "domain0" and "domain1" regions does not exist. In this entry you have to insert an existent region, one of the regions you have on your regionProperties file. The sampleRegion refers to the neighbour region you want to couple with. |
|
March 3, 2016, 15:32 |
Similar issue
|
#6 |
New Member
Shahil
Join Date: Jan 2016
Posts: 5
Rep Power: 10 |
Hi Philibert,
Were you able to overcome your error? Because I am exactly facing the same problem. If you have solved your problems, please help me to a solution to this error. Shahil. |
|
March 3, 2016, 16:33 |
|
#7 |
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 20 |
As i have said the sampleRegion keyword or patch definition was ill defined. Open the boundary files in each region and check if it contains the patches of that region.
Code:
patchinregion0_to_patchinregion1 // your patch in this region { type mappedWall; nFaces ...; startFace ...; sampleMode nearestPatchFace; // mapping method. sampleRegion domain1; // the domain the adjacent patch is in samplePatch patchinregion1_to_patchinregion0; the adjacent patch } In the polyMesh boundary file of your fluid region you have to define Code:
fluid_to_solid// your patch in this region { type mappedWall; nFaces ...; startFace ...; sampleMode nearestPatchFace; // mapping method. sampleRegion solid; // the domain the adjacent patch is in samplePatch solid_to_fluid; the adjacent patch } Code:
solid_to_fluid// your patch in this region { type mappedWall; nFaces ...; startFace ...; sampleMode nearestPatchFace; // mapping method. sampleRegion fluid; // the domain the adjacent patch is in samplePatch fluid_to_solid; the adjacent patch } |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Problem with cyclic boundaries in Openfoam 1.5 | fs82 | OpenFOAM | 36 | January 7, 2015 00:31 |
[Gmsh] Single volume Mesh gmsh | PeteH | OpenFOAM Meshing & Mesh Conversion | 9 | August 6, 2013 08:54 |
Cyclic Boundary Condition | Luiz Eduardo Bittencourt Sampaio (Sampaio) | OpenFOAM Running, Solving & CFD | 36 | July 2, 2012 12:23 |
[Gmsh] Import gmsh msh to Foam | adorean | OpenFOAM Meshing & Mesh Conversion | 24 | April 27, 2005 08:19 |
Multicomponent fluid | Andrea | CFX | 2 | October 11, 2004 05:12 |