关于数值模拟离心泵过程中发散的一些问题
-
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; } -
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。
-
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 -
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 -
运算的log文件贴一下？simpleFoam的log
-
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 -
我换用linearUpwind后到200多步还是发散了，谢谢您！
-
调节一下你的k和epsilon初始的值，从log来看你的epsilon不可实现。
-
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。 -
我发现个问题，你那个同时调用GGI和MRF？
-
恩恩，是的，交界面处理使用的是GGI
-
我记得ggi和MRF不能同时用的。。
-
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
-
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。
-
明白了，谢谢前辈
论坛登录问题反馈可联系 li.dy@dyfluid.com