generally, the default setting is
choosing for solver：
FLUENT provides three di erent solver formulations:
 segregated
 coupled implicit
 coupled explicit(显式格式主要用于激波等波动解的捕捉问题)

The segregated solver traditionally has been used for incompressible and mildly compressible flows. The coupled approach, on the other hand, was originally designed for high-speed compressible flows.

By default, FLUENT uses the segregated solver, for high-speed compressible flows (as discussed above), highly coupled flows with strong body forces (e.g., buoyancy or rotational forces), or flows being solved on very fine meshes, you may want to consider the coupled implicit solver instead.

For cases where the use of the coupled implicit solver is desirable, but your machine does not have sufficient memory, you can use the segregated solver or the coupled explicit solver instead.(explicit save memory use,but need more iterations for converged solution.

Choosing the Discretization Scheme

1)first-order upwind vs second-order upwind
When the flow is aligned with the grid the first-order upwind discretization may be acceptable. For triangular and tetrahedral grids, since the flow is never aligned with the grid, you will generally obtain more accurate results by using the second-order discretization. For quad/hex grids, you will also obtain better results using the second-order discretization, especially for complex flows. For most cases, you will be able to use the second-order scheme from the start of the calculation. In some cases, however, you may need to start with the first-order scheme and then switch to the second-order scheme after a few iterations. For example, if you are running a high-Mach-number flow calculation that has an initial solution much different than the expected final solution, Finally, if you run into convergence diffculties with the second-order scheme, you should try the first-order scheme instead.

2)Quick vs upwind(Quick适用于结构网格，流动方向与网格一致，对于非结构网格推荐用2阶迎风)
The QUICK discretization scheme may provide better accuracy than the second-order scheme for rotating or swirling flows solved on quadrilateral or hexahedral meshes. For compressible flows with shocks, using the QUICK scheme for all variables, including density, is highly recommended for quadrilateral, hexahedral, or hybrid meshes.

3)central-differencing scheme vs upwind
The central-differencing scheme is available only when you are using the LES turbulence model, and it should be used only when the mesh spacing(网格间距）is fine enough so that the magnitude of the local Peclet number (Equation 26.2-5) is less than 1.

4)power law vs upwind
A power law scheme is also available, but it will generally yield the same accuracy as the first-order scheme.

Choosing the Pressure Interpolation Scheme(压力离散格式）

a number of pressure interpolation schemes are available when the segregated solver is used in FLUENT. For most cases the standard(default) scheme is acceptable, but some types of models may benenit from one of the other schemes:
 For problems involving large body forces, the body-force-weighted scheme is recommended.
 For flows with high swirl numbers, high-Rayleigh-number natural convection, highspeed rotating flows, flows involving porous media, and flows in strongly curved domains, use the PRESTO! scheme.
 对于可压流，应该使用二阶格式
 Use the second-order scheme for improved accuracy when one of the other schemes is not applicable.

Choosing the Density Interpolation Scheme which is available at solve a single-phase compressible flow.

If you are calculating a compressible flow with shocks, the first-order upwind scheme may tend to smooth the shocks; you should use the second-order-upwind or QUICK scheme for such flows.

Choosing the Pressure-Velocity Coupling Method(压力－速度方程耦合方法）

SIMPLE vs. SIMPLEC
SIMPLE is the default, but many problems will benenit from the use of SIMPLEC, For relatively uncomplicated problems (laminar
ows with no additional models activated) in which convergence is limited by the pressure-velocity coupling, you can often obtain a converged solution more quickly using SIMPLEC. With SIMPLEC, the pressurecorrection under-relaxation factor is generally set to 1.0, which aids in convergence speedup. In some problems, however, increasing the pressure-correction under-relaxation to 1.0 can lead to instability due to high grid skewness. For such cases, you will need to use one or more skewness correction schemes, use a slightly more conservative under-relaxation value (up to 0.7), or use the SIMPLE algorithm. The SIMPLEC skewness correction allows FLUENT to obtain a solution on a highly skewed mesh in approximately the same number of iterations as required for a more orthogonal mesh.

Pressure-Implicit with Splitting of Operators (PISO)
The PISO algorithm with neighbor correction is highly recommended for all transient flow calculations, especially when you want to use a large time step. (For problems that use the LES turbulence model, which usually requires small time steps, using PISO may result in increased computational expense, so SIMPLE or SIMPLEC should be considered instead.) PISO can maintain a stable calculation with a larger time step and an under-relaxation factor of 1.0 for both momentum and pressure.
For steady-state problems, PISO with neighbor correction does not provide any noticeable advantage over SIMPLE or SIMPLEC with optimal under-relaxation factors.
When you use PISO neighbor correction, under-relaxation factors of 1.0 or near 1.0 are recommended for all equations.If you use just the PISO skewness correction for highly-distorted meshes (without neighbor correction), set the under-relaxation factors for momentum and pressure so that they sum to 1 (e.g., 0.3 for pressure and 0.7 for momentum). If you use both PISO methods, follow the under-relaxation recommendations for PISO neighbor correction, above.

Fractional Step Method
The Fractional Step method (FSM) is available when you choose to use the NITA scheme, the FSM is slightly less computationally expensive compared to the PISO algorithm. For some problems (e.g., simulations that use VOF), FSM could be less stable than PISO.
In most cases, the default values for the solution controls are enough to set a robust convergence of the internal pressure correction sub-iterations due to skewness. Only very complex problems (e.g., moving deforming meshes, sliding interfaces, the VOF model) could require a reduction of relaxation for pressure up to a value of 0.7 or 0.8.

Setting Under-Relaxation Factors---the most important is pressure and momentum Under-Relaxation Factors

Under-Relaxation Factors control the change of variable value produced during each iteration.
the smaller value of Under-Relaxation Factors is set, the more stable iteration is got, but the harder convergence.
It is good practice to begin a calculation using the default under-relaxation factors. If the residuals continue to increase after the first 4 or 5 iterations, you should reduce the under-relaxation factors.
For most flows, the default under-relaxation factors do not usually require modification. If unstable or divergent behavior is observed, however, you need to reduce the underrelaxation factors for pressure, momentum, k, and εfrom their default values to about 0.2, 0.5, 0.5, and 0.5.
In problems where density is strongly coupled with temperature, as in very-high-Rayleigh-number natural- or mixed-convection flows, it is wise to also underrelax the temperature equation and/or density (i.e., use an under-relaxation factor less than 1.0).Conversely, when temperature is not coupled with the momentum equations (or when it is weakly coupled), as in flows with constant density, the under-relaxation factor for temperature can be set to 1.0.
For other scalar equations (e.g., swirl, species, mixture fraction and variance) the default Setting Solution Controls for the Non-Iterative Solver under-relaxation may be too aggressive for some problems, especially at the start of the calculation. You may wish to reduce the factors to 0.8 to facilitate convergence.

other uses

Changing the Courant Number
1)Courant Numbers for the Coupled Explicit Solver:in general, you can assume that the multi-stage scheme is stable for Courant numbers up to 2.5. The default CFL for the coupled explicit solver is 1.0, but you may be able to increase it for some 2D problems. You should generally not use a value higher than 2.0. If your solution is diverging, and your problem
is properly set up and initialized, this is usually a good sign that the Courant number needs to be lowered. Depending on the severity of the startup conditions, you may need to decrease the CFL to a value as low as 0.1 to 0.5 to get started.
2)Courant Numbers for the Coupled Implicit Solver:The default CFL for the coupled implicit solver is 5.0. It is often possible to increase the CFL to 10, 20, 100, or even higher, depending on the complexity of your problem.

多重网格
基本原理：微分方程的误差分量可以分为两大类，一类是频率变化较缓慢的低频分量；另一类是频率高，摆动快的高频分量。一般的迭代方法可以迅速地将摆动误差衰减，但对那些低频分量，迭代法的效果不是很显著。高频分量和低频分量是相对的，与网格尺度有关，在细网格上被
视为低频的分量，在粗网格上可能为高频分量。
多重网格方法作为一种快速计算方法，迭代求解由偏微分方程组离散以后组成的代数方程组，其基本原理在于一定的网格最容易消除波长与网格步长相对应的误差分量。该方法采用不同尺度的网格，不同疏密的网格消除不同波长的误差分量，首先在细网格上采用迭代法，当收敛速度变缓慢时暗示误差已经光滑，则转移到较粗的网格上消除与该层网格上相对应的较易消除的那些误差分量，这样逐层进行下去直到消除各种误差分量，再逐层返回到细网格上。
。FLUENT 中有四种多重网格循环：V，W，F 以及灵活("flex")循环。V 和W 循环可以用在AMG 和FAS 中，F 和灵活循环只限用于AMG 方法。（W 和灵活AMG 循环由于要花费大量的计算而不可用于解耦合方程组。），F 循环比V 循环需要更多的计算，但是比W 循环花费要少一些。但是它的收敛性比V 循环要好，大致和W 循环的收敛性差不多。对于耦合求解器设置来说，F 循环是默认的AMG 循环类型。
灵活循环和V，W 循环之间的主要区别是：灵活循环会通过残差减小的公差和终止判据的满足情况来确定什么时候，按什么样的频率来处理每一层网格，而V 和W 循环则明确定义了各个层面之间的转换模式。
灵活循环：当当前层面的误差减小速度不够快时，多重网格程序就会调用下一个网格层面的计算（restriction），。B 的值控制了处理的粗化
网格层面的频率。默认值是0.7。如果b 的值较大，就会处理较小的频率，反之亦然。当校正解的误差减小到该网格层初始误差的某一分数a（在0 和1 之间）时，当前网格层上的校正方程就可以被认为是充分收敛了。参数a 被称为终止判据（termination）。默认值是0.1。

FAS 优于AMG 方法的地方在于，对于非线性问题前者可以做得更好，这是因为系统的非线性可以通过重新离散传到粗糙层面；当使用AMG 时，一旦系统被线化，直到细化层面算子被更新，求解器才会“感觉到”非线性。

Turning On FAS Multigrid
FAS multigrid is an optional component of the coupled explicit solver. For most problems, you can start out with 4 or 5 levels. For large 3D problems, you may want to add more levels. If you believe that multigrid is causing convergence trouble, you can decrease the number of levels.

Initializing the Solution
you can initialize the entire flow domain, also you can Patching Values in Selected Cells.

 

Special Treatment for Strong Body Forces in Multiphase Flows：1）The Frozen Flux Formulation－－－This option is only available for single-phase transient problems that use the segregated iterative solver and do not use a moving/deforming mesh model.2）Time-Advancement Schemes contain two types：Iterative Time-Advancement Scheme－－－The iterative scheme is the default in FLUENT and Non-Iterative Time-Advancement Scheme－－－ FLUENT offers two versions of NITA schemes; the non-iterative fractional step method and the non-iterative PISO method .

 

用残差光顺的方法增加库朗数
在Solution Controls（求解过程控制）面板中，残差光顺的迭代值在缺省设置中被设定为0，即在缺省设置中没有使用残差光顺技术。如果将Iterations（迭代计数器）增加为1或更大的数，则可以进一步设置Smoothing Factor（光顺因子）。将光顺因子设定为0.5 可以将库朗数增加为原数值的两倍。

改变多步格式
首先启动Multi-Stage Parameters（多步格式参数）面板：Solve->Controls->Multi-Stage...
在缺省设置中，FLUENT 使用5 步格式，每步的系数分别为0.25、0.166666、0.375、0.5 和1.0。在对多步格式非常熟悉的情况下可以增加多步格式的步数，同时修改每步的系数。修改系数的一般要求是：
（1）系数为介于0 和1 之间的实数。
（2）最后一步的系数必须为1。

使用无反射边界条件
如果要采用无反射边界条件，最好先在不使用这类边界条件时将问题计算一遍，在获得收敛解之后，再加入无反射边界条件，继续进行计算并再度获得收敛解。使用无反射边界条件的步骤如下：
（1）加入无反射边界条件的文本命令如下：define->boundary-conditions->non-reflecting->enable? 如果不知道无反射边界条件是否已经加入计算可以用文本命令show-status 进行查看。
（2）无反射边界条件初始化的文本命令如下：define->boundary-conditions->non-reflecting->initialize 初始化成功后，系统会显示相应的系统信息。
（3）如果有必要，可以修改相关参数，相关的文本命令如下：define->boundary-conditions->non-reflecting->set 相关参数的含义为：
  under-relaxation：设定亚松弛因子，缺省值为0.75。
  discretization：设定离散格式，缺省为高阶格式。
  verbosity：设定信息长度，0 为不显示，1 为显示基本信息，2 为显示详细信息。
1. 在混合平面模型中使用无反射边界条件
如果计划在计算中同时采用无反射边界条件和混合平面模型，则首先要将混合平面定义为压强
2. 在并行版FLUENT 中使用无反射边界条件
在无反射边界条件与并行求解器共同使用时，采用无反射边界条件的网格单元必须处于同一个分区中。为保证所有单元在同一个分区中，可以用人工方式进行网格分区。

 

标签： 点击： 评论: