Navigation

    CFD中文网

    CFD中文网

    • Login
    • Search
    • 最新

    用simpleFoam求解器时出现的错误,求教如何解决

    OpenFOAM
    5
    13
    7879
    Loading More Posts
    • Oldest to Newest
    • Newest to Oldest
    • Most Votes
    Reply
    • Reply as topic
    Log in to reply
    This topic has been deleted. Only users with topic management privileges can see it.
    • 温
      温宝霖 last edited by CFD中文网

      /*---------------------------------------------------------------------------*\
      | =========                 |                                                 |
      | \\      /  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   : Apr 10 2017
      Time   : 15:01:18
      Host   : "11"
      PID    : 9444
      Case   : /home/w11/OpenFOAM/w11-4.1/run/ASBM2-Da
      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-06
          field U	 tolerance 1e-06
      
      Reading field p
      
      Reading field U
      
      Reading/calculating face flux field phi
      
      Selecting incompressible transport model Newtonian
      Selecting turbulence model type laminar
      No MRF models present
      
      No finite volume options present
      
      
      Starting time loop
      
      Time = 1
      
      smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 9.33846e-13, No Iterations 136
      smoothSolver:  Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
      GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0975624, No Iterations 26
      time step continuity errors : sum local = 0.00312299, global = -0.000382393, cumulative = -0.000382393
      ExecutionTime = 11.95 s  ClockTime = 12 s
      
      .........
      
      Time = 80
      
      smoothSolver:  Solving for Ux, Initial residual = 0.564078, Final residual = 8.76275e-13, No Iterations 103
      smoothSolver:  Solving for Uy, Initial residual = 0.391492, Final residual = 9.39228e-13, No Iterations 97
      GAMG:  Solving for p, Initial residual = 0.990623, Final residual = 0.617109, No Iterations 1000
      time step continuity errors : sum local = 1.38438e+20, global = 5.64087e+19, cumulative = 5.64087e+19
      ExecutionTime = 1160.33 s  ClockTime = 1164 s
      
      Time = 81
      
      smoothSolver:  Solving for Ux, Initial residual = 0.414375, Final residual = 3.94608e-10, No Iterations 1000
      smoothSolver:  Solving for Uy, Initial residual = 0.468273, Final residual = 2.39705e-10, No Iterations 1000
      #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::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:?
      #4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
      #5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
      #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
      #7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
      #8  Foam::fvMatrix<double>::solve() at ??:?
      #9  ? at ??:?
      #10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
      #11  ? at ??:?
      浮点数例外 (核心已转储)
      
      
      这是我的fvSolution文件
      solvers 
      {
      
          U
          {
              solver           smoothSolver;
              smoother         GaussSeidel;
              tolerance        1e-12;
              relTol           0;
              nSweeps          1;
          }
      
          p
          {
              solver           GAMG;
              tolerance        1e-9;
              relTol           0.1;
              smoother         GaussSeidel;
              nPreSweeps       0;
              nPostSweeps      2;
              cacheAgglomeration on;
              agglomerator     faceAreaPair;
              nCellsInCoarsestLevel 10;
              mergeLevels      1;
          }
      
      }
      
      
      SIMPLE
      {
          nNonOrthogonalCorrectors 0;
      
          residualControl
          {
              p               1e-6;
              U               1e-6;
          }
      
      	pRefCell 0;
      	pRefValue 0;
      }
      
      relaxationFactors
      {
          p               0.2;
          U               0.9;
      }
      
      

      这个问题困扰了我好几天,本人小白一枚,年初刚接触OpenFOAM,之前做过几次小的模拟没遇到过这种情况,请教各位大神如何解决,感激不尽。

      1 Reply Last reply Reply Quote
      • 赵
        赵一铭 last edited by

        你的质量不守恒。你的网格质量如何?确定不需要开湍流?

        温 1 Reply Last reply Reply Quote
        • 温
          温宝霖 last edited by CFD中文网

          Create time
          
          Create polyMesh for time = 0
          
          Time = 0
          
          Mesh stats
              points:           972441
              faces:            2653016
              internal faces:   2348082
              cells:            841637
              faces per cell:   5.94211
              boundary patches: 6
              point zones:      0
              face zones:       0
              cell zones:       0
          
          Overall number of cells of each type:
              hexahedra:     792917
              prisms:        44780
              wedges:        0
              pyramids:      0
              tet wedges:    0
              tetrahedra:    0
              polyhedra:     3940
              Breakdown of polyhedra by number of faces:
                  faces   number of cells
                      4   4
                      5   3936
          
          Checking topology...
              Boundary definition OK.
           ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
              Cell to face addressing OK.
              Point usage OK.
              Upper triangular ordering OK.
              Face vertices OK.
              Number of regions: 1 (OK).
          
          Checking patch topology for multiply connected surfaces...
                             Patch    Faces   Points                  Surface topology
                      frontAndBack    33720    37963  ok (non-closed singly connected)
                              left    10000    10251  ok (non-closed singly connected)
                             right    10000    10251  ok (non-closed singly connected)
                            bottom     3026     3561  ok (non-closed singly connected)
                               top     4712     5452  ok (non-closed singly connected)
                        fixedWalls   243476   249736  multiply connected (shared edge)
            <<Writing 2 conflicting points to set nonManifoldPoints
          
          Checking geometry...
              Overall domain bounding box (-0.17 -0.0604041 -0.001) (0.17 0.0601678 0.001)
              Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
              Mesh has 2 solution (non-empty) directions (1 1 0)
           ***Number of edges not aligned with or perpendicular to non-empty directions: 928948
            <<Writing 951037 points on non-aligned edges to set nonAlignedEdges
              Boundary openness (-2.86088e-16 1.1772e-16 -1.21395e-15) OK.
              Max cell openness = 7.07551e-16 OK.
              Max aspect ratio = 12.3976 OK.
              Minimum face area = 1.35674e-09. Maximum face area = 2.45047e-06.  Face area magnitudes OK.
              Min volume = 6.42698e-13. Max volume = 9.79806e-11.  Total volume = 3.44166e-05.  Cell volumes OK.
              Mesh non-orthogonality Max: 77.2055 average: 16.6713
             *Number of severely non-orthogonal (> 70 degrees) faces: 28.
              Non-orthogonality check OK.
            <<Writing 28 non-orthogonal faces to set nonOrthoFaces
           ***Error in face pyramids: 1 faces are incorrectly oriented.
            <<Writing 1 faces with incorrect orientation to set wrongOrientedFaces
           ***Max skewness = 7.85662, 2557 highly skew faces detected which may impair the quality of the results
            <<Writing 2557 skew faces to set skewFaces
              Coupled point location match (average 0) OK.
          
          Failed 3 mesh checks.
          
          X 1 Reply Last reply Reply Quote
          • 温
            温宝霖 @赵一铭 last edited by

            @赵一铭 之前的模拟一直用的层流,没出过这种问题。是哪个参数大小需要修改么?

            C 1 Reply Last reply Reply Quote
            • X
              xpqiu 教授 @温宝霖 last edited by

              @温宝霖 这个网格有问题,不能算

              1 Reply Last reply Reply Quote
              • C
                CFD中文网 @温宝霖 last edited by CFD中文网

                @温宝霖
                你出错的那个例子也是用层流模拟的:upset: 网格snappyHexMesh做的?上来就79万啊。

                CFD中国标准用户测试帐号
                目前由徐笑笑登录

                温 1 Reply Last reply Reply Quote
                • 温
                  温宝霖 @CFD中文网 last edited by

                  @cfd-china 是的,用的snappyHexMesh做的网格。老师跟我说网格数多一点模拟的值更准确,我就用的100×100×100网格做的。我是照着一个案例自己取的值,案例做的是2维模拟,网格数400×100×1。我取的是一个立方体,之前模拟的都是2维,第一次做3维就懵了

                  赵 W 2 Replies Last reply Reply Quote
                  • 赵
                    赵一铭 @温宝霖 last edited by

                    @温宝霖
                    snappyHexMesh生成的网格有时候质量不是特别高会影响收敛,如果几何简单的话最好生成六面体网格,simpleFoam非常稳健,设置正确很难出现收敛问题。

                    1 Reply Last reply Reply Quote
                    • W
                      wwzhao 教授 @温宝霖 last edited by

                      @温宝霖 检查边界条件,3D模拟不应该包含empty边界

                      温 2 Replies Last reply Reply Quote
                      • 温
                        温宝霖 @wwzhao last edited by

                        @wwzhao 好的,谢谢您

                        1 Reply Last reply Reply Quote
                        • 温
                          温宝霖 @wwzhao last edited by

                          @wwzhao 我改了边界条件之后重生成了网格,果然模拟出来了。太谢谢您了,解决了困扰我的问题

                          1 Reply Last reply Reply Quote
                          • 温
                            温宝霖 last edited by

                            这个问题现在已经解决了,是数值单位的错误。因为我的初始边界条件中入口处的p=1e-3,出口处的p=0,将网格的数值缩小了一千倍以后,使他们在同一数量级上再运行simpleFoam就不会出现“浮点数例外,核心已转储”的错误了。
                            我还发现在用snappyHexMesh画三维网格的时候,如果将blockMeshDict中frontAndBack设为empty,在进行snap步骤之后依然得不到很优美的平滑的网格连接。而我听从了@wwzhao 的建议之后,将frontAndBack设置成与除了出口和入口之外的其他四个面的边界条件一致,也就是patch之后,再进行snappyHexMesh,就能得到平滑的网格了。
                            这三天我失败了上百次,终于在昨天晚上凌晨的时候解决了这个问题,谢谢各位大神的指导,谢谢你们。

                            C 1 Reply Last reply Reply Quote
                            • C
                              CFD中文网 @温宝霖 last edited by

                              @温宝霖 恭喜。
                              你模拟的是什么问题?能否发个网格截图出来看看?听起来挺有意思。

                              CFD中国标准用户测试帐号
                              目前由徐笑笑登录

                              1 Reply Last reply Reply Quote
                              • First post
                                Last post

                              CFD中文网 | 东岳流体 | 京ICP备15017992号-2
                              论坛登录问题反馈可联系 li.dy@dyfluid.com