OpenFOAM槽道流动怎么添加初始湍流脉动

Posted on Edited on In Views:
本文主要介绍一下OpenFOAM槽道流DNS和LES计算中，如何初始激发湍流状态。How to initialize turbulence about channel flow in OpenFOAM.

OpenFOAM槽道流动怎么添加初始湍流脉动

   在槽道流动计算中，湍流状态是很难发生的，因为计算中扰动比较难发生，一般都是人工进行添加来进行计算，但是由于人工添加脉动可能在计算过程逐渐被耗散，因此需要一些专门方式来进行添加脉动。

boxTurb

  boxturb前处理工具1：不支持非均匀化网格，需要网格进行均匀化处理，最后mapFields到其他网格上去，进行继续计算。
  具体也可以参考A boxTurb16 and dnsFoam tutorial2简单的介绍。
  具体例子见此贴子3。

Codestream

  EugeneDeVilliers博士论文提到的方法4，见章节5.1.2。
  代码解析：

1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
internalField   #codeStream
{
    code
    #{
        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const objectRegistry& db = d.db();

        const fvMesh& mesh = refCast<const fvMesh>(d.db());

        volVectorField& fld =
        const_cast<volVectorField&>(db.lookupObject<volVectorField>("U"));

        // settings need modified start
        // direction
        direction streamDir = 0;
        direction spanDir = 2;
        direction heightDir = 1;
        // half height
        const scalar h = 1.0;
        const scalar Um = 0.4;
        const scalar Retau = 1000;
        const scalar nu = 2e-5;
        const scalar utau = Retau*nu/h;
        // settings need modified end

        // spanwise wavenumber: spacing z+ = 200
        const scalar betaPlus = 2.0*constant::mathematical::pi*(1.0/200.0);
        // streamwise wave number: spacing x+ = 500
        const scalar alphaPlus = 2.0*constant::mathematical::pi*(1.0/500.0);
        const scalar sigma = 0.00055;
        const scalar epsilon = Um/200.0;
        const scalar duplus = Um*0.25/utau; //具体见Eugene De Villiers的博士论文

        const bool setBulk = true;
        const bool perturb = true;

        // Random number generator
        Random perturbation(1234567);

        const vectorField& centres = mesh.C();

        forAll(centres, celli)
        {
            // add a small (+/-20%) random component to enhance symetry breaking
            scalar deviation=1.0 + 0.2*perturbation.GaussNormal<scalar>();

            const vector& cCentre = centres[celli];

            scalar zplus = cCentre[spanDir]*Retau/h;
            scalar y = min(cCentre[heightDir], 2*h-cCentre[heightDir]);
            scalar yplus = y*Retau/h;
            scalar xplus = cCentre[streamDir]*Retau/h;

            if (setBulk)
            {
                // laminar parabolic profile
                fld[celli] = vector::zero;

                fld[celli][streamDir] =
                    3.0*Um * (y/h - 0.5*sqr(y/h));
                    // Blasius Um*( 5/4*(1-pow(zloc-1,4)));
            }

            if (perturb)
            {
                // streak streamwise velocity
                fld[celli][streamDir] +=
                    (utau * duplus/2.0) * (yplus/40.0)
                    * Foam::exp(-sigma * Foam::sqr(yplus) + 0.5)
                    * Foam::cos(betaPlus*zplus)*deviation;

                // streak spanwise perturbation
                fld[celli][spanDir] =
                    epsilon
                * Foam::sin(alphaPlus*xplus)
                * yplus
                * Foam::exp(-sigma*Foam::sqr(yplus))
                * deviation;
            }
        }
        fld.writeEntry("", os);
        // os << fld.internalField();

    #};

    codeInclude
    #{
        #include "fvCFD.H"
    #};
 
    codeOptions
    #{
        -I$(LIB_SRC)/finiteVolume/lnInclude \
        -I$(LIB_SRC)/meshTools/lnInclude
    #};

    codeLibs
    #{
        -lfiniteVolume \
        -lmeshTools
    #};

};

  按照代码说明把需要改的参数改好，将上述代码写入算例/0/U文件中，即可计算，具体效果如下图。

利用CodeStream生成的湍流

mapFields

  The mapFields function object maps input fields from local mesh to secondary mesh at runtime. mapFields 可以使得之前的湍流流场(速度场和压力场)插值到新算例中，从来进行计算，这样计算大大增加了计算速度，可以很快地出现湍流现象。
  格式如下：
  Usage: mapFields [OPTIONS] <sourceCase>7
  Options的选项:

1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
-case <dir>       Specify case directory to use (instead of cwd)
-consistent       Source and target geometry and boundary conditions identical
-mapMethod <word>
                Specify the mapping method
-parallelSource   The source is decomposed
-parallelTarget   The target is decomposed
-sourceDecomposeParDict <file>  Read decomposePar dictionary from specified location
-sourceRegion <word>
                Specify the source region
-sourceTime <scalar|'latestTime'>
                Specify the source time
-subtract         Subtract mapped source from target
-targetDecomposeParDict <file>
                Read decomposePar dictionary from specified location
-targetRegion <word>
                Specify the target region
-doc              Display documentation in browser
-help             Display short help and exit
-help-full        Display full help and exit

Map volume fields from one mesh to another

Using: OpenFOAM-v2206 (2206) - visit www.openfoam.com

  其中需要注意的是：consistent代表的是几何条件和边界条件都相同的时候使用，当不相同的时候(比如在使用光滑算例插值到有结构的算例中去的时候，就不能使用consistent Options)8。

参考链接

Buy me a coffee
OYYO WeChat Pay WeChat Pay