OpenFOAM简单blockMesh浮点异常

Question

我正在一步一步地学习OpenFOAM，目前正在尝试用blockMesh工具创建一个非常简单的网格，但始终获得浮点异常。我的blockMeshDict与用户手册第4.3.1节中的啮合教程几乎完全一致。

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

scale 1.0;

vertices
(
    (0 0 0) //0
    (0 0 1) //1
    (0 1 1) //2
    (0 1 0) //3
    (1 0 0) //4
    (1 0 1) //5
    (1 1 1) //6
    (1 1 0) //7
);

edges
(
);

blocks
(
    hex (0 1 2 3 7 6 5 4)
    (2 1 1)               // 2 blocks in the x direction
    simpleGrading (1 1 1) // default expansion ratios
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 1 2 3) 
        );
    }

    outlet
    {
        type patch;
        faces
        (
            (4 5 6 7)
        );
    }

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

这只是一个单位长度的“空气管”立方体，沿x轴有两个部分，另一边和墙壁上有一个入口和出口：

​

​

此配置立即因以下错误而中断：

$ blockMesh
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 9-c8374a4890ad
Exec   : blockMesh
Date   : Nov 02 2021
Time   : 11:50:35
Host   : "artixlinux"
PID    : 10555
I/O    : uncollated
Case   : /home/andrii/foamtest
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

Reading "blockMeshDict"

Creating block mesh from
    "system/blockMeshDict"
Creating block edges
No non-planar block faces defined
Creating topology blocks
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/usr/lib/libc.so.6"
#3  Foam::face::centre(Foam::Field<Foam::Vector<double> > const&) const at ??:?
#4  Foam::blockDescriptor::check(Foam::Istream const&) at ??:?
#5  Foam::blockDescriptor::blockDescriptor(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:?
#6  Foam::block::block(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:?
#7  Foam::block::New(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:?
#8  void Foam::PtrList<Foam::block>::read<Foam::block::iNew>(Foam::Istream&, Foam::block::iNew const&) at ??:?
#9  Foam::blockMesh::createTopology(Foam::IOdictionary const&, Foam::word const&) at ??:?
#10  Foam::blockMesh::blockMesh(Foam::IOdictionary const&, Foam::word const&) at ??:?
#11  ? in "/opt/OpenFOAM/OpenFOAM-9/platforms/linux64GccDPInt32Opt/bin/blockMesh"
#12  __libc_start_main in "/usr/lib/libc.so.6"
#13  ? in "/opt/OpenFOAM/OpenFOAM-9/platforms/linux64GccDPInt32Opt/bin/blockMesh"
zsh: floating point exception  blockMesh

我相当肯定，这不仅仅是一个坏掉的OpenFOAM安装(我特别使用的是archive的组织版本)，因为复制的一个不同的网格数据集取代了本教程中给出的归档文件，工作得非常完美。

我对此失去了理智，我多次检查顶点和面部描述，没有发现任何问题，但错误仍然存在。我错过了什么错误吗？

Answer 1

blockMeshDict文件的问题在于您没有遵循以下规则：

局部坐标系由在块定义中表示顶点的顺序来定义，该顺序如下：

• 轴原点是块定义中的第一个条目，顶点0。
• x方向由顶点0移动到顶点1；
• y方向由顶点1移动到顶点2；
• 顶点0，1，2，3定义平面z= 0。
• 顶点4是通过在z方向上从顶点0移动而得到的。
• 顶点5,6和7分别由顶点1,2和3沿z方向移动得到。
• 当您指定faces时，您必须遵循右手规则。

下面是一个正确工作的blockMesh版本：

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

scale 1.0;

vertices
(
    (0 0 0) //0
    (0 0 1) //1
    (0 1 1) //2
    (0 1 0) //3
    (1 0 0) //4
    (1 0 1) //5
    (1 1 1) //6
    (1 1 0) //7
);

edges
(
);

blocks
(
    hex (0 4 7 3 1 5 6 2) //>>>> Follow the rules above <<<<
    (2 1 1)               // 2 blocks in the x direction
    simpleGrading (1 1 1) // default expansion ratios
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 1 2 3) 
        );
    }

    outlet
    {
        type patch;
        faces
        (
            (4 7 6 5)
        );
    }

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

使用：

blockMesh
paraFoam -block

你会得到：

​

​

侧注：在使用OpenFOAM基金会版本(openfoam.org)时，您指的是openfoam.com文档。要小心，因为它们不一定是兼容的。

Answer 2

在大多数情况下，您可以直接从blockMesh -help命令行获得最快的帮助。您将获得这类ASCII艺术：

...
Block mesh generator.
  The ordering of vertex and face labels within a block as shown below.
  For the local vertex numbering in the sequence 0 to 7:
    Faces 0, 1 (x-direction) are left, right.
    Faces 2, 3 (y-direction) are front, back.
    Faces 4, 5 (z-direction) are bottom, top.
                        7 ---- 6
                 f5     |\     |\     f3
                 |      | 4 ---- 5     \
                 |      3 |--- 2 |      \
                 |       \|     \|      f2
                 f4       0 ---- 1
    Y  Z
     \ |                f0 ------ f1
      \|
       O--- X

Using: OpenFOAM-v2106 (2106) - visit www.openfoam.com
Build: f815a12bba-20210902
Arch:  LSB;label=32;scalar=64

这是记忆顶点排序的最快的备忘单。

请注意，blockMesh还有一个非常快速的-write-vtk选项。它以.vtu格式写出基本块，您可以在任何版本的截视图中显示它(不需要额外的插件)。我通常使用截视范围内的点悬停函数来询问顶点数。

一旦您像这样定义了您的块，您可能很高兴知道您也可以用块id和本地faces id来定义边界面。因此，您的边界可能如下所示：

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 0)  // x-min
        );
    }
    outlet
    {
        type patch;
        faces
        (
            (0 1)  // x-max
        );
    }
...
);