FLUENT求解器设置主要包括：1、压力-速度耦合方程格式选择2、对流插值 3、梯度插值 4、压力插值
下面对这几种设置做详细说明。 一、压力-速度耦合方程求解算法
FLUENT中主要有四种算法：SIMPLE，SIMPLEC，PISO，FSM
(1)SIMPLE(semi-implicit method for pressure-linked equations)半隐式连接压力方程方法，是FLUENT的默认格式。
(2)SIMPLEC(SIMPLE-consistent)。对于简单的问题收敛非常快速，不对压力进行修正，所以压力松弛因子可以设置为1
(3)Pressure-Implicit with Splitting of Operators (PISO)。对非定常流动问题或者包含比平均网格倾斜度更高的网格适用
(4)Fractional Step Method (FSM)对非定常流的分步方法。用于NITA格式，与PISO具有相同的特性。
二、对流插值（动量方程）
FLUENT有五种方法：一阶迎风格式、幂率格式、二阶迎风格式、MUSL三阶格式、QUICK格式
（1）FLUENT默认采用一阶格式。容易收敛，但精度较差，主要用于初值计算。 （2）Power Lar.幂率格式，当雷诺数低于5时，计算精度比一阶格式要高。
（3）二阶迎风格式。二阶迎风格式相对于一阶格式来说，使用更小的截断误差，适用于三角形、四面体网格或流动与网格不在同一直线上；二阶格式收敛可能比较慢。
（4）MUSL(monotone upstream-centered schemes for conservation laws).当地3阶离散格式。主要用于非结构网格，在预测二次流，漩涡，力等时更精确。
（5）QUICK（Quadratic upwind interpolation）格式。此格式用于四边形/六面体时具有三阶精度，用于杂交网格或三角形/四面体时只具有二阶精度。
三、梯度插值梯度插值主要是针对扩散项。
FLUENT有三种梯度插值方案：green-gauss cell-based，Green-gauss node-based，least-quares cell based.
（1）格林-高斯基于单元体。求解方法可能会出现伪扩散。
（2）格林-高斯基于节点。求解更精确，最小化伪扩散，推荐用于三角形网格上
（3）基于单元体的最小二乘法插值。推荐用于多面体网格，与基于节点的格林-高斯格式具有相同的精度和格式。
四、压力插值压力基分离求解器主要有五种压力插值算法。
（1）标准格式（Standard)。为FLUENT缺省格式，对大表妹边界层附近的曲线发现压力梯度流动求解精度会降低（但不能用于流动中压力急剧变化的地方——此时应该使用PRESTO!格式代替）
（2）PRESTO!主要用于高旋流，压力急剧变化流（如多孔介质、风扇模型等），或剧烈弯曲的区域。
（3）Linear（线性格式）。当其他选项导致收敛困难或出现非物理解时使用此格式。 （4）second order（二阶格式）。用于可压缩流动，不能用于多孔介质、阶跃、风扇、VOF/MIXTURE多相流。
（5）Body Force Weighted体积力。当体积力很大时，如高雷诺数自然对流或高回旋流动中采用此格式。
++========== 首先，所谓的steady和unsteady就表述了流动状态是否随时间变化的含义，这是定性的问题，你自己建立模型一定要明确的。这在计算过程中就是体现在方程不同，unsteady流多了时间变量，那么unsteady流就要进行时间离散。
其次，两种求解的结果对比而言：
一种情况是你要求解的物理问题是steady的，从理论上来说那么两种求解方式收敛之后的结果都是一样或者近似的。只不过需要注意的是，在unsteady的求解中dt的选取会影响你的计算结果，有可能会计算发散，而且还必须要足够的计算步达到收敛才能和steady的结果进行比较。换句话说，如果你用unsteady的方法去求解steady流，如果计算本身就没收敛，就取结果进行比较，那么肯定是不行的。一般而言，在进行unsteady求解的时候，前面一段时间的计算结果基本上是不予采用的，因为有一个数值收敛的过程。
另一种是你要求解的物理问题是unsteady的，那么你用steady的求解方法得出的结果就是一堆垃圾了，没有任何价值。
看你的帖子里面说有物体的移动，我不清楚具体的物理模型，但估计应该是unsteady流。
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