Navigation

    CFD中文网

    CFD中文网
    • Login
    • Search
    • 最新

    关于数值模拟离心泵过程中发散的一些问题

    OpenFOAM
    3
    15
    5140
    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.
    • C
      cfd-cxb last edited by

      在用MRFSimpleFoam求解离心泵过程中当divSchemes采用一阶的upwind时计算可以收敛，没问题，但是采用如下的高阶格式时计算基本不能进行下去，只能算一两步，这个问题出在哪里? 请帮忙解决，谢谢

      divSchemes
{
    default         none;
    div(phi,U)      Gauss limitedLinearV 1;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,epsilon) Gauss limitedLinear 1;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}
fvSolution 文件如下
solvers
{
    p
    {
        solver           GAMG;
        tolerance        1e-6;
        relTol           0.05;
       smoother         GaussSeidel;
       cacheAgglomeration true;
        nCellsInCoarsestLevel 800;
        agglomerator     faceAreaPair;
        mergeLevels      1;
    }

    U
    {
        solver           smoothSolver;
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-5;
        relTol           0.1;
    }

    k
    {
        solver           smoothSolver;
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-5;
        relTol           0.1;
    }

    epsilon
    {
        solver           smoothSolver;
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-5;
        relTol           0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 1;
    pRefCell 0;
    pRefValue 0;
}
relaxationFactors
{
    p               0.3;
    U               0.5;
    k               0.5;
    epsilon         0.5;
}
      1 Reply Last reply Reply Quote
      • 李东岳
        李东岳 管理员 last edited by

        很难判断，和网格，边界关系很大，simpleFoam是一个很简单的求解器，发散只能是设置的问题肯定不是求解器的问题。有的时候离心泵计算要使用并不是太稳定的边界条件组合。只能说检查下边界条件和网格质量。或许可以贴log文件看看。

        2021年CFD/OpenFOAM课程 https://www.cfd-china.com/topic/2397

        1 Reply Last reply Reply Quote
        • C
          cfd-cxb last edited by

          谢谢前辈，下面是网格质量检查的log文件，用的是非结构网格

          Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    all points:           249875
    live points:          249875
    all faces:            2796614
    live faces:           2796614
    internal faces:       2718602
    cells:                1378804
    boundary patches:     10
    point zones:          0
    face zones:           3
    cell zones:           3

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    1378804
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 3
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
Nuumber of cells per region: 
	0	192712
	1	282795
	2	903297


Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Area [m^2]  Surface topology                  
    GUIDE-INLET         1454     777      0.00621397  ok (non-closed singly connected)  
    GUIDE-OUTLET        1444     771      0.00621367  ok (non-closed singly connected)  
    GUIDE-BIMIAN        5252     2723     0.0167709   ok (non-closed singly connected)  
    IMPELLER-INLET      1866     985      0.00621398  ok (non-closed singly connected)  
    IMPELLER-OUTLET     3747     2037     0.0122964   ok (non-closed singly connected)  
    IMPELLER-BIMIAN     9398     5365     0.0300004   ok (non-closed singly connected)  
    IMPELLER-BLADE      11873    6399     0.0358377   ok (non-closed singly connected)  
    VOLUTE-OUTLET       1238     665      0.00502107  ok (non-closed singly connected)  
    VOLUTE-INLET        3708     2041     0.0122965   ok (non-closed singly connected)  
    VOLUTE-BIMIAN       38032    19247    0.110309    ok (non-closed singly connected)  

Checking geometry...
    This is a 3-D mesh
    Overall domain bounding box (-0.0994947 -0.12194 -0.105381) (0.0399865 0.18 0.134736)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Mesh (non-empty, non-wedge) dimensions 3
    Boundary openness (1.39036e-16 7.89536e-17 1.26213e-17) Threshold = 1e-06 OK.
    Max cell openness = 3.12848e-16 OK.
    Max aspect ratio = 4.28896 OK.
    Minumum face area = 7.24618e-07. Maximum face area = 7.48018e-06.  Face area magnitudes OK.
    Min volume = 3.60661e-10. Max volume = 5.62725e-09.  Total volume = 0.00266114.  Cell volumes OK.
    Mesh non-orthogonality Max: 50.7974 average: 7.4258 Threshold = 70
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.52081 OK.

Mesh OK.

End
          1 Reply Last reply Reply Quote
          • C
            cfd-cxb last edited by

            边界条件：
            进口：速度进口，压力零梯度
            出口：速度零梯度，压力固定值0
            壁面：速度固定值（0 0 0），压力零梯度

            1 Reply Last reply Reply Quote
            • 李东岳
              李东岳 管理员 last edited by

              运算的log文件贴一下？simpleFoam的log

              2021年CFD/OpenFOAM课程 https://www.cfd-china.com/topic/2397

              1 Reply Last reply Reply Quote
              • C
                cfd-cxb last edited by

                您好，算例运行不起来，只能跑一步

                Create time

Create mesh for time = 0

Initializing the GGI interpolator between master/shadow patches: GUIDE-OUTLET/IMPELLER-INLET
Initializing the GGI interpolator between master/shadow patches: IMPELLER-OUTLET/VOLUTE-INLET

SIMPLE: no convergence criteria found. Calculations will run for 1400 steps.

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model RNGkEpsilon
RNGkEpsilonCoeffs
{
    Cmu             0.0845;
    C1              1.42;
    C2              1.68;
    alphak          1.39;
    alphaEps        1.39;
    eta0            4.38;
    beta            0.012;
    sigmak          0.71942;
    sigmaEps        0.71942;
}

Creating MRF for cell zone IMPELLER. rpm = 2900
Excluded patches: 2(3 4)

Starting time loop

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0108375, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0104409, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.0104084, No Iterations 2
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.027634, No Iterations 6
GAMG:  Solving for p, Initial residual = 0.0357851, Final residual = 0.000575861, No Iterations 2
time step continuity errors : sum local = 7.76946, global = 0.352411, cumulative = 0.352411
smoothSolver:  Solving for epsilon, Initial residual = 0.13384, Final residual = 0.00135303, No Iterations 2
bounding epsilon, min: -2.55034 max: 52.4243 average: 2.34921
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0250789, No Iterations 2
ExecutionTime = 12.85 s  ClockTime = 13 s

Time = 2

smoothSolver:  Solving for Ux, Initial residual = 0.20708, Final residual = 0.00402441, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.249236, Final residual = 0.0056065, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 0.222885, Final residual = 0.00479877, No Iterations 2
                1 Reply Last reply Reply Quote
                • C
                  cfd-cxb last edited by

                  我换用linearUpwind后到200多步还是发散了，谢谢您！

                  1 Reply Last reply Reply Quote
                  • 李东岳
                    李东岳 管理员 last edited by

                    调节一下你的k和epsilon初始的值，从log来看你的epsilon不可实现。

                    2021年CFD/OpenFOAM课程 https://www.cfd-china.com/topic/2397

                    1 Reply Last reply Reply Quote
                    • C
                      cfd-cxb last edited by

                      首先，非常感谢您的回复
                      我调整了k以及epsilon，但是还是不可以，当我将div(phi,U)调为upwind或者linearUpwind Gauss时，div(phi,k)与div(phi,epsilon)不管是那种格式都能算，但是若是我将div(phi,U)设为limitedlinearV 1格式，div(phi,k)与div(phi,epsilon)不管那种格式都不行，算例都只算一步。

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

                        我发现个问题，你那个同时调用GGI和MRF？

                        1 Reply Last reply Reply Quote
                        • C
                          cfd-cxb last edited by

                          恩恩，是的，交界面处理使用的是GGI

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

                            我记得ggi和MRF不能同时用的。。

                            1 Reply Last reply Reply Quote
                            • C
                              cfd-cxb last edited by

                              谢谢您的回复，我用的是foam-extend版本，里面有同时调用的例子的

                              1 Reply Last reply Reply Quote
                              • 李东岳
                                李东岳 管理员 last edited by

                                我调整了k以及epsilon，但是还是不可以，当我将div(phi,U)调为upwind或者linearUpwind Gauss时，div(phi,k)与div(phi,epsilon)不管是那种格式都能算，但是若是我将div(phi,U)设为limitedlinearV 1格式，div(phi,k)与div(phi,epsilon)不管那种格式都不行，算例都只算一步。

                                如果是用稳态算例，可以先迎风算出来流场之后，再加阶数，SIMPLEFoam很稳健，一般不会出现问题。我觉得还是设置的问题。

                                2021年CFD/OpenFOAM课程 https://www.cfd-china.com/topic/2397

                                1 Reply Last reply Reply Quote
                                • C
                                  cfd-cxb last edited by

                                  明白了，谢谢前辈

                                  1 Reply Last reply Reply Quote
                                  • First post
                                    Last post

                                  CFD中文网 | 东岳流体 | 京ICP备15017992号-2