对旋转机械进行计算时的错误提示
-
大家好，最近在做旋转机械内流场的计算工作，使用了AMI动静交接面，采用MRF坐标系，可是当我开始计算时，却出现了以下错误提示。。。觉得很可能是边界条件设置有问题。。贴一下边界条件设置文件，如下。求大神指教！
lizehao@lizehao-Z97-HD3:~/openFoam/run/tubulence_model_test_on_centrifugal_pump/mesh5/merge_grid$ simpleFoam |tee simpleFoam.log /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 4.1 Exec : simpleFoam Date : Dec 08 2017 Time : 11:09:02 Host : "lizehao-Z97-HD3" PID : 30537 Case : /home/lizehao/openFoam/run/tubulence_model_test_on_centrifugal_pump/mesh5/merge_grid nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: convergence criteria field p tolerance 1e-05 field U tolerance 1e-05 field k tolerance 1e-05 field epsilon tolerance 1e-05 field nut tolerance 1e-05 Reading field p Reading field U Reading/calculating face flux field phi AMI: Creating addressing and weights between 18792 source faces and 2424 target faces AMI: Patch source sum(weights) min/max/average = 0.992729, 1.00082, 0.999897 AMI: Patch target sum(weights) min/max/average = 0, 1.00061, 0.580281 AMI: Creating addressing and weights between 7722 source faces and 3861 target faces AMI: Patch source sum(weights) min/max/average = 0.0916406, 1, 0.994738 AMI: Patch target sum(weights) min/max/average = 0, 1, 0.877149 AMI: Creating addressing and weights between 7722 source faces and 3861 target faces AMI: Patch source sum(weights) min/max/average = 0.0916406, 1, 0.994738 AMI: Patch target sum(weights) min/max/average = 0, 1, 0.877149 Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; C3 -0.33; sigmak 1; sigmaEps 1.3; } Creating MRF zone list from MRFProperties creating MRF zone: MRF1 No finite volume options present Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0389849, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0580972, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0935053, No Iterations 1 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:? #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:? #5 ? at ??:? #6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #7 ? at ??:?U文件，进口fixedValue，出口zeroGradient,壁面noslip，交接面cyclicAMI
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (2.744 0 0); boundaryField { wall1_runner { type noSlip; } wall2_runner { type noSlip; } wall3_runner { type noSlip; } wall4_runner { type noSlip; } interface_runner { type cyclicAMI; value uniform (2.744 0 0); } interface1_runner { type cyclicAMI; value uniform (2.744 0 0); } interface2_runner { type cyclicAMI; value uniform (2.744 0 0); } wall2_suction { type noSlip; } outflow_suction { type noSlip; } wall1_suction { type noSlip; } inlet { type fixedValue; value uniform (2.744 0 0); } interFace1_suction { type cyclicAMI; value uniform (2.744 0 0); } interFace2_suction { type cyclicAMI; value uniform (2.744 0 0); } wall1_volute { type noSlip; } interface_volute { type cyclicAMI; value uniform (2.744 0 0); } wall2_volute { type noSlip; } outlet_volute { type zeroGradient; } }P文件，进口及壁面zeroGradient,出口fixedValue，交接面cyclicAMI
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { wall1_runner { type zeroGradient; } wall2_runner { type zeroGradient; } wall3_runner { type zeroGradient; } wall4_runner { type zeroGradient; } interface_runner { type cyclicAMI; value uniform 0; } interface1_runner { type cyclicAMI; value uniform 0; } interface2_runner { type cyclicAMI; value uniform 0; } wall2_suction { type zeroGradient; } outflow_suction { type zeroGradient; } wall1_suction { type zeroGradient; } inlet { type zeroGradient; } interFace1_suction { type cyclicAMI; value uniform 0; } interFace2_suction { type cyclicAMI; value uniform 0; } wall1_volute { type zeroGradient; } interface_volute { type cyclicAMI; value uniform 0; } wall2_volute { type zeroGradient; } outlet_volute { type fixedValue; value uniform 0; } }k文件，进口fixedValue,出口inletoutlet，壁面kqRWallFunction，交接面cyclicAMI
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0.01; boundaryField { wall1_runner { type kqRWallFunction; value uniform 0.01; } wall2_runner { type kqRWallFunction; value uniform 0.01; } wall3_runner { type kqRWallFunction; value uniform 0.01; } wall4_runner { type kqRWallFunction; value uniform 0.01; } interface_runner { type cyclicAMI; value $internalField; } interface1_runner { type cyclicAMI; value $internalField; } interface2_runner { type cyclicAMI; value $internalField; } wall2_suction { type kqRWallFunction; value uniform 0.01; } outflow_suction { type kqRWallFunction; value uniform 0.01; } wall1_suction { type kqRWallFunction; value uniform 0.01; } inlet { type fixedValue; value uniform 0.01; } interFace1_suction { type cyclicAMI; value $internalField; } interFace2_suction { type cyclicAMI; value $internalField; } wall1_volute { type kqRWallFunction; value uniform 0.01; } interface_volute { type cyclicAMI; value $internalField; } wall2_volute { type kqRWallFunction; value uniform 0.01; } outlet_volute { type inletOutlet; inletValue $internalField; value $internalField; } }epsilon文件，进口fixedValue,出口inletoutlet，壁面epsilonWallFunction，交接面cyclicAMI
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object epsilon; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -3 0 0 0 0]; internalField uniform 0.0095; boundaryField { wall1_runner { type epsilonWallFunction; value uniform 0.0095; } wall2_runner { type epsilonWallFunction; value uniform 0.0095; } wall3_runner { type epsilonWallFunction; value uniform 0.0095; } wall4_runner { type epsilonWallFunction; value uniform 0.0095; } interface_runner { type cyclicAMI; value $internalField; } interface1_runner { type cyclicAMI; value $internalField; } interface2_runner { type cyclicAMI; value $internalField; } wall2_suction { type epsilonWallFunction; value uniform 0.0095; } outflow_suction { type epsilonWallFunction; value uniform 0.0095; } wall1_suction { type epsilonWallFunction; value uniform 0.0095; } inlet { type fixedValue; value uniform 0.0095; } interFace1_suction { type cyclicAMI; value $internalField; } interFace2_suction { type cyclicAMI; value $internalField; } wall1_volute { type epsilonWallFunction; value uniform 0.0095; } interface_volute { type cyclicAMI; value $internalField; } wall2_volute { type epsilonWallFunction; value uniform 0.0095; } outlet_volute { type inletOutlet; inletValue $internalField; value $internalField; } } -
只能看出来
Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:?可能除以0了，但是并不知道是哪里出去了，需要更深度的debug
-
嗯嗯:crying: 我看到CFD-online上一些前辈们也是这样说，然后我就懵圈了，完全不知道应该怎样去debug，不知道应该遵循一个怎样的流程或原则。。:crying:
-
使用了AMI动静交接面，采用MRF坐标系
为什么同时使用AMI和MRF？
-
嗯。。因为网格划分时把动静部件分开划分，然后合并的时候有交接面，所以用了AMI。。然后我是采用多重参考系定义速度。。难道它们之间是有矛盾的？:big_mouth:
-
这样的话你用AMI就不需要用MRF了 :big_mouth:
-
嗯。。可我目前算的是稳态，不用MRF的话怎么处理内部的旋转部件呢:surprised:
-
估计你之前用过Fluent，OpenFOAM里面MRF也可以瞬态，拟瞬态。
-
@lllwonderliquid 你可以不用设定AMI边界条件。这个和fluent可能不一样，也就是说动静网格可以是一个整体，但是把其中的一部分网格设定为rotater。至少我这样算是成功了。
-
@lllwonderliquid 或者另一个思路去理解。你分别生成了动、静区域，但是这两个区域的交界面必须一致。这是和fluent里不同的地方。我也一直试图理解AMI边界的用法，按理说和fluent一样是可行的，但是实际使用的时候并不行。
-
@李东岳 你好！之前看过你在cfd-online的回复(https://www.cfd-online.com/Forums/openfoam-programming-development/153989-modified-pimplefoam-solver-mrfpimplefoam-solver.html)，我想知道pimpleFoam(2.3.x)能否可以直接使用MRF吗？只需要添加fvOptions即可？
-
只需要添加fvOptions即可？
是的。主要是多相那面代码处理有点甚至超过了Weller的高度。单相这面容易。
-
@李东岳 也就是说MRF通过fvOptions(U)对动量方程产生作用？若在pimpleFOAM中添加温度T方程，需要考虑MRF作用吗，是否得添加fvOptions(T)？
-
要的，简单添加
fvOptions(T); fvOptions.constrain(TEqn); fvOptions.correct(T);即可，这就是面向对象的方便之处。是不是要比Fluent简单点？我不清楚Fluent..没准Fluent那面更简单，哈哈。
-
@李东岳 非常感谢！
-
@李东岳 有很多帖子(尤其与Fluent相关)都表明MRF只适用于稳态求解，不知道在Openfoam中能否实现MRF瞬态求解? 是否有相关的求解器(已验证其准确性)？
-
目前OpenFOAM这面采用MRF做计算已经发表的文章有很多，包括我用OpenFOAM计算的旋转搅拌器。在这里贴一个其他课题组的：http://www.sciencedirect.com/science/article/pii/S0892687516301789
有关Fluent，我的理解只局限于理论，你可以参考英文版的理论指南里面的论述。使用MRF进行瞬态模拟是可能的。
但同时我也注意到很多用Fluent的用户告诉我说Fluent中的MRF不能用于瞬态计算。由于我没有用过Fluent，我自己也有点迷惑Fluent那面具体怎么个情况。
不过可以确定的是，理论上是可以的
-
@lllwonderliquid 请问你的问题目前解决了吗？
我目前也在使用MRF以及AMI边界条件进行计算，但是碰到了与你类似的问题
