前两天在丫总的微信群问了关于这两个选项的问题，后来查看了ANSYS 帮助文档，有了一个大概了解，分享给大家，方便大家以后在泵小丫网站查看此类问题的相关介绍，以下文献均参考至ANSYS Help 2020R1.(有问题看帮助文档挺有用的)
从“压力-速度耦合”下拉列表中选择“Coupled (耦合算法)”表示您正在使用基于压力的耦合算法，该算法在理论指南的“耦合算法”中有描述。与基于压力的分离算法相比，该算法具有一定的优越性。基于压力的耦合算法对稳态单相流的实现具有更强的鲁棒性和有效性。但它不适用于使用非迭代时间推进选项(NITA)的情况。
注意：在某些使用多孔跳跃边界条件的情况下，Coupled 耦合算法方案可能会遇到收敛问题，不响应耦合求解器设置的变化。这种行为取决于特定的流动构型和多孔跳跃边界条件值。如果在使用多孔跳跃边界条件和耦合格式的情况下观察到收敛不稳定，建议将压力-速度耦合算法 Coupled 改为分离格式算法中的某个算法。（ 作者：雨丘原 出处：bilibili）
- Coupled with Volume Fractions选项
The Coupled with Volume Fractions option (also known as Full Multiphase Coupled in previous ANSYS Fluent versions) couples velocity corrections, shared pressure corrections, and the correction for volume fraction simultaneously. Theoretically, it should be more efficient, however it may have some drawbacks in robustness and CPU time usage. The robustness issue stems from the lack of control of the solution of the volume fraction equation. The continuity constraint (sum of all volume fractions equals 1, and individual values limited between zero and one) cannot be enforced exactly during inner solver iterations, and slight variations from the physical limits may lead to divergence. Research is ongoing in this area to improve the method. The method is advantageous for heterogeneous mass transfer when a low Courant number is given; it also works well in dilute situations.
The Volume Fraction Coupling Method aims to achieve a faster steady-state solution compared to the segregated method of solving equations. It may not be a suitable option for transient applications due to the significant overhead in CPU time compared to the segregated method, unless it is run with a larger time step size.
与体积分数耦合选项（在以前的 ANSYS Fluent 版本中也称为全多相耦合）同时耦合速度校正、共享压力校正和体积分数校正。理论上，它应该更高效，但是它在鲁棒性和 CPU 时间使用方面可能存在一些缺点。鲁棒性问题源于对体积分数方程的解缺乏控制。连续性约束（所有体积分数的总和等于 1，并且单个值限制在 0 和 1 之间）在内部求解器迭代期间无法准确执行，物理限制的轻微变化可能会导致发散。该领域正在进行研究以改进该方法。当给定较低的库朗数时，该方法有利于非均相传质；它在稀释的情况下也能很好地工作。
与求解方程的分离方法相比，体积分数耦合方法旨在实现更快的稳态解。与隔离方法相比，由于 CPU 时间的显着开销，它可能不适用于瞬态应用程序，除非它以更大的时间步长运行。
- Note: The Coupled with Volume Fractions option is available in the interface after you have selected Coupled from the Scheme drop-down list for Pressure-Velocity Coupling. For steady-state cases, the Pseudo Transient option will be enabled automatically when you enable the Coupled with Volume Fractions option for the VOF and mixture models.
- 注意：从压力-速度耦合的方案下拉列表中选择耦合后，界面中的耦合体积分数选项可用。 对于稳态情况，当您为 VOF 和混合模型启用耦合体积分数选项时，将自动启用伪瞬态选项。
- Limitations and Recommendations of the Coupled with Volume Fraction Options for the VOF and Mixture Models
The coupled with volume fractions option has the following limitations:
- It is not available when Slip Velocity is enabled for the Mixture multiphase model.
- It is not supported when using the Singhal-Et-Al cavitation model.
- It is not supported when the Explicit formulation for volume fraction is selected.
Recommended uses of the coupled with volume fractions option:
- The Pseudo-transient solver is recommended for steady-state calculations.
- It is recommended that you use lower under-relaxation factors for momentum for higher order schemes.VOF 和混合模型的耦合体积分数选项的限制和建议
与体积分数耦合选项有以下限制：
当为 Mixture 多相模型启用 Slip Velocity （速度滑移）时，它不可用。
使用 Singhal-Et-Al 空化模型时不支持。
选择体积分数的显式公式时不支持。
耦合体积分数选项的推荐用途：
建议使用伪瞬态求解器进行稳态计算。
对于高阶方案，建议您使用较低的欠松弛因子作为动量。
-
Solving N-Phase Volume Fraction Equations选项
For a multiphase flow, the sum of the phase volume fractions must always equal 1. By default, Fluent enforces this constraint by solving the volume fraction equations for each of the secondary phases and then setting the volume fraction of the primary phase to the complement.
In certain cases, where poor convergence and/or mass imbalance are observed, enabling Solve N-Phase Volume Fraction Equations may improve solutions, although in practice the results obtained from using this option are case dependent. If selected, this option will solve all volume fraction equations, including both primary and secondary phases. The resulting phase volume fractions are then scaled in order to satisfy the requirement of summing to 1. This approach is more computationally expensive than the default approach and, in general, should not be necessary for the simulation.
Note: The Solve N-Phase Volume Fraction Equations option is not available for the Volume of Fluid model or Eulerian with Multi-Fluid VOF Model enabled.
对于多相流，相体积分数的总和必须始终等于 1。默认情况下，Fluent 通过求解每个次级相的体积分数方程，然后将初相的体积分数设置为互补相来强制执行此约束。
在某些情况下，如果观察到收敛性差或质量不平衡，启用求解 N 相体积分数方程可能会改进解决方案，尽管在实践中使用此选项获得的结果取决于具体情况。如果选中，此选项将求解所有体积分数方程，包括初级和次级相。然后缩放得到的相体积分数以满足求和为 1 的要求。这种方法比默认方法在计算上更昂贵，并且通常不需要模拟。
注意：求解 N 相体积分数方程选项不适用于流体体积模型或启用多相流 VOF欧拉模型。
（图文无关）大多数均为谷歌翻译，仅做部分修改。如有错误敬请指正。
