toposet之后出现空集。。。

16c

toposet之后polymesh下set文件夹的文件内全部显示是空集，终端显示识别了你的范围是XXX但是这个范围内狗der没有，我是真不到哪里出问题了。
toposetdric代码是这样的：

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
   {
        name    porous;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box     (0 0 10) (2000 500 15);
        }
    }

   
   /* 
   {
        name    porousZone;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set porous;
        }
    }
        */

   
    {
        name    inletA;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0 0 15) (0.1 500 25);
        }
    }

    {
        name    inletB;
        type    faceSet;
        action  new;
        source  cellToFace;
        sourceInfo
        {
            set     inletA;
            option  all;
        }
    } 

    {
        name    inletB;
        type    faceSet;
        action  subset;
        source  patchToFace;
        sourceInfo
        {
            name walls;
        }
    }

    {
        name    outletA;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (1999.9 0 15) (2000 500 50);
        }
    }

    {
        name    outletB;
        type    faceSet;
        action  new;
        source  cellToFace;
        sourceInfo
        {
            set     outletA;
            option  all;
        }
    } 

    {
        name    outletB;
        type    faceSet;
        action  subset;
        source  patchToFace;
        sourceInfo
        {
            name walls;
        }
    }
        
);

// ************************************************************************* //

终端是这样说的：

openfoam@openfoam-virtual-machine:~/OpenFOAM/openfoam-5.x/run/1$ topoSet
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 5.x-7f7d351b741b
Exec   : topoSet
Date   : Nov 25 2024
Time   : 09:45:57
Host   : "openfoam-virtual-machine"
PID    : 181025
I/O    : uncollated
Case   : /home/openfoam/OpenFOAM/openfoam-5.x/run/1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Reading topoSetDict

Time = 0
    mesh not changed.
Created cellZoneSet porous
    Applying source boxToCell
    Adding cells with center within boxes 1((0 0 10) (2000 500 15))
    cellZoneSet porous now size 0
Created cellSet inletA
    Applying source boxToCell
    Adding cells with center within boxes 1((0 0 15) (0.1 500 25))
    cellSet inletA now size 0
Created faceSet inletB
    Applying source cellToFace
    Adding faces according to cellSet inletA ...
    faceSet inletB now size 0
Read set faceSet inletB with size 0
    Applying source patchToFace
    Adding all faces of patch walls ...
    Found matching patch walls with 31250 faces.
    faceSet inletB now size 0
Created cellSet outletA
    Applying source boxToCell
    Adding cells with center within boxes 1((1999.9 0 15) (2000 500 50))
    cellSet outletA now size 0
Created faceSet outletB
    Applying source cellToFace
    Adding faces according to cellSet outletA ...
    faceSet outletB now size 0
Read set faceSet outletB with size 0
    Applying source patchToFace
    Adding all faces of patch walls ...
    Found matching patch walls with 31250 faces.
    faceSet outletB now size 0
End

blockMesh是这样的：

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
convertToMeters 0.001;
vertices
(
    (0 0 0)                 // 0
    (2000 0 0)               // 1
    (2000 500 0)            // 2
    (0 500 0)              // 3

   /* 
    (0 0 15)                // 4
    (2000 0 15)              // 5
    (2000 500 15)           // 6
    (0 500 15)             // 7
    */

    (0 0 50)                // 4
    (2000 0 50)              // 5
    (2000 500 50)            // 6
    (0 500 50)             // 7   

    // (0 0 25)                // 12
    // (0 500 25)              // 13
);
blocks
(
    hex (0 1 2 3 4 5 6 7) (500 125 25) simpleGrading (1 1 1)
    // hex (4 5 6 7 8 9 10 11) (500 125 35) simpleGrading (1 1 1) 
    
);

edges
(
);

boundary
(

    walls
    {
        type wall;
        faces
        (
            (0 1 5 4)
            (2 3 7 6)
            (0 4 7 3)
            (1 2 6 5)
        );
    }
   
    atmosphere
    {
        type patch;
        faces
        (
            (4 5 6 7)
            (0 1 2 3)
        );
    }
mergePatchPairs
(
);

我搞这个破玩意好几天了，一点头绪没有，还得求着各位大佬帮帮忙瞅一眼。。。。

学流体的小明

你blockMesh文件convertToMeters 0.001;
实际就是把下面的坐标乘以0.001画网格，画出来的计算域是(0,0,0)到(2,0.5,0.05)。
而你toposet直接从(0,0,10)开始画box，当然找不到了。

16c

@学流体的小明在 toposet之后出现空集。。。中说：

你blockMesh文件convertToMeters 0.001;
实际就是把下面的坐标乘以0.001画网格，画出来的计算域是(0,0,0)到(2,0.5,0.05)。
而你toposet直接从(0,0,10)开始画box，当然找不到了。

大哥按你说的改了topoSetDric , box的坐标和网格尺寸我也确定了是能对应上的，但是createPatch并ParaFoam之后出现了inlet这个面变成了豁牙子。。。

改之后的topoSet是这样的：

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
   {
        name    porous;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box     (0 0 10e-3) (2000e-3 500e-3 12e-3);
        }
    }

   
   
   {
        name    porousZone;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set porous;
        }
    }
        

   
    {
        name    inletA;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0 0 12e-3) (4e-3 500e-3 22e-3);
        }
    }

    {
        name    inletB;
        type    faceSet;
        action  new;
        source  cellToFace;
        sourceInfo
        {
            set     inletA;
            option  all;
        }
    } 

    {
        name    inletB;
        type    faceSet;
        action  subset;
        source  patchToFace;
        sourceInfo
        {
            name walls;
        }
    }

    {
        name    outletA;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (1.996 0 12e-3) (2 500e-3 50e-3);
        }
    }

    {
        name    outletB;
        type    faceSet;
        action  new;
        source  cellToFace;
        sourceInfo
        {
            set     outletA;
            option  all;
        }
    } 

    {
        name    outletB;
        type    faceSet;
        action  subset;
        source  patchToFace;
        sourceInfo
        {
            name walls;
        }
    }
        
);

// ************************************************************************* //

createPatch是这样的：

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
//       with transformations (i.e. cyclics).
pointSync false;
// writeCyclicMatch  false;
// Patches to create.
patches
(
    {
        name inlet;
        patchInfo
        {
            type            patch;
        }
        constructFrom set;
        set inletB;
    }

    {
        name outlet;
        patchInfo
        {
            type            patch;
        }
        constructFrom set;
        set outletB;
    }
);

// ************************************************************************* //

这个豁牙子问题我之前跟着阿B上田东的视频做案例的时候也出现了不知道是什么玩意而且case跑完之后他明显是个实际存在的数值上的豁牙子，不是paraview显示问题

学流体的小明

感觉是topoSet选择网格，提取各种面的时候有些问题了，我没用过这方面的功能，不太了解。
你如果只是想把边界面提取出来的话，在blockMesh当中就可以设置吧。

李东岳

豁牙子注意一下toposet点位置的精度。

16c

@学流体的小明在 toposet之后出现空集。。。中说：

感觉是topoSet选择网格，提取各种面的时候有些问题了，我没用过这方面的功能，不太了解。
你如果只是想把边界面提取出来的话，在blockMesh当中就可以设置吧。

@李东岳在 toposet之后出现空集。。。中说：

豁牙子注意一下toposet点位置的精度。

感谢两位大佬提点，豁牙子问题解决了...

CFD中文网

toposet之后出现空集。。。