blockMesh划分网格，在v2112和v6均测试可以，v8报错

尚善若水

请教一下大家，我用 of 的 blockMesh 划分一个带圆形喷孔几何体的六面体网格。blockMesh 在 v2112 和 v6 均测试可以运行，但是 v8 报错。我刚学习 of，自己没排查出错误，请教下大家。
错误提示如下：

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

Creating block mesh from
    "system/blockMeshDict"
Using #calcEntry at line 46 in file "/home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/system/blockMeshDict"
Using #codeStream with "/home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_b7af15ef665f94aa93a235a5e34750b6bd3e16a1.so"
Invoking "wmake -s libso /home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/dynamicCode/_b7af15ef665f94aa93a235a5e34750b6bd3e16a1"
wmake libso /home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/dynamicCode/_b7af15ef665f94aa93a235a5e34750b6bd3e16a1
    Ctoo: codeStreamTemplate.C
/home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/system/blockMeshDict: In function 'void Foam::codeStream_b7af15ef665f94aa93a235a5e34750b6bd3e16a1(Foam::Ostream&, const Foam::dictionary&)':
/home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/system/blockMeshDict:1:8: error: '$D' was not declared in this scope
 /*--------------------------------*- C++ -*----------------------------------*\
        ^
make: *** [Make/linux64GccDPInt32Opt/codeStreamTemplate.o] Error 1


--> FOAM FATAL IO ERROR: 
Failed wmake "dynamicCode/_b7af15ef665f94aa93a235a5e34750b6bd3e16a1/platforms/linux64GccDPInt32Opt/lib/libcodeStream_b7af15ef665f94aa93a235a5e34750b6bd3e16a1.so"


file: /home/users/nus/e0944146/OpenFOAM/e0944146-8/run/JISCF/system/blockMeshDict from line 17 to line 45.

    From function static void (* Foam::functionEntries::codeStream::getFunction(const Foam::dictionary&, const Foam::dictionary&))(Foam::Ostream&, const Foam::dictionary&)
    in file db/dictionary/functionEntries/codeStream/codeStream.C at line 214.

FOAM exiting

网格如下：

测试文件 blockMesh.zip

coolhhh

@尚善若水
我用OpenFOAM-8试了下，提示‘$D’ was not declared，尝试找到$D，在后面加个空格，如下所示。

alpha 45.0;                   // o-block degree
// s     #calc "$D/4.0";         // Inner square side half
// sc    #calc "$D/4.0 + 0.1";   // Inner square side curvature
// R     #calc "$D/2.0";         // Radius of the jet nozzle

s     #calc "$D /4.0";         // Inner square side half
sc    #calc "$D /4.0 + 0.1";   // Inner square side curvature
R     #calc "$D /2.0";         // Radius of the jet nozzle

接着能运行一会，又出现error: ‘$lx’ was not declared，也是类似在后面加个空格，就可继续运行。

// round 函数表示四舍五入取整数

// xCells #calc "round($lx/$deltax)"; // 310  
// yCells #calc "round($ly/$deltay)"; // 110
// zCells #calc "round($lz/$deltaz)"; // 200

xCells #calc "round($lx /$deltax)"; // 310  
yCells #calc "round($ly /$deltay)"; // 110
zCells #calc "round($lz /$deltaz)"; // 200

以此方式后续还有好几个类似的参数都这个问题，当基本改完后，运行还是有如下错误。这块也不清楚什么问题了

    ln: ./lnInclude
    wmkdep: codeStreamTemplate.C
    Ctoo: codeStreamTemplate.C
    ld: /home/user1/OpenFOAM/user1-8/run/blockmesh/dynamicCode/_d585a44b91ff1f499e2e3d99401445beaf8aa06c/../platforms/linux64GccDPInt32Opt/lib/libcodeStream_d585a44b91ff1f499e2e3d99401445beaf8aa06c.so
Creating block edges
No non-planar block faces defined
Creating topology blocks


--> FOAM FATAL IO ERROR: 
wrong token type - expected int32_t, found on line 184 the doubleScalar 10

file: /home/user1/OpenFOAM/user1-8/run/blockmesh/system/blockMeshDict/blocks at line 184.

    From function Foam::Istream& Foam::operator>>(Foam::Istream&, int32_t&)
    in file primitives/ints/int32/int32IO.C at line 62.

FOAM exiting

coolhhh

@尚善若水刚再试了OpenFOAM-2012，可以运行没有任何报错。如果你需要用OpenFOAM-8计算，看是否可以用其他版本的先生成网格，然后再用OpenFOAM-8计算？

coolhhh

@尚善若水除了加空格，再把rsCells改为10，就可以在OpenFOAM-8 运行了。上面提示的错误是指划分网格数量应该是int类型数值

//rsCells 10.0; // Number of cells between inner square and circle 

rsCells 10; // Number of cells between inner square and circle

李东岳

尚善若水

@coolhhh 厉害厉害，我就觉着是变量定义格式问题，但是自己不太懂。感谢～