• To save only the data files, use the following TUI option:

  file → auto-save → case-frequency → if-mesh-is-modified

  This will result in the options in the When the Data File is Saved, Save the Case group box being disabled in the Autosave dialog box. In essence, this TUI command forces ANSYS Fluent to the save case file only when the mesh is modified. It does not disable case file saving, but reduces it to an absolute minimum. This is necessary to do so since you cannot read a data file without a case file containing a matching mesh.

• First-to-Higher Order Blending While the higher-order scheme may result in greater accuracy，it can also result in convergence diflcultes and instabilties at certain flow conditions.On the other hand，using a first-order scheme may not provide the desired accuracy.One approach to achieving improved accuracy while maintaining good stability is to use a discretization blending factor.This feature is available for both density-based and pressure-based solvers and can be invoked using the fllowing text command：

solve-→ set-→numerics 

Enter a value between 0 and 1 when asked for the blending factor:

1st-order to higher-order blending factor[min=0.0 一max=1.0]

A blending factor of 0 reduces the gradient reconstruction to a first-order discretization scheme，whereas 1 will recover high-order discretization A blending factor of less than 1（typically 0.75 or 0.5）will make the convective fluxes more difusive，which in some flow conditions can stabilie a solution that is otherwise unstable when the full higher-order discretization scheme is employed.

Important：Note that in order to use this feature effectively，make sure that one of the allowed higher order discretization schemes is selected for the desired variables in the Solution Methods task page.

• 有时候为了提高收敛速度和计算精度，可以使用求解数据的插值(先用稀疏网格进行计算导出数据，相当于对之后计算密网格的初始化)：

利用FLUENT计算计算经常会出现这样的情况：有时候要研究几何模型对流场的影响，常常需要固定边界条件，变化的是几何模型与网格。这事就存在msh文件的导入、边界设定的问题。若需要计算的模型很多，一个个文件的设置则显得相当的麻烦与耗时。

事实上，FLUENT提供了很多方式为我们解决这一问题。最主要有两种方式：

方式一：利用TUI命令写出边界条件

首先创建原始网格，注意命名规范。

导入fluent进行各项边界条件设置后，利用下面的TUI命令。

file/write-settings

该命令执行之后会出现如图1所示的命令，输入保存的文件名，这里输入的是bc，这样会将边界数据保存到bc文件中，存储在工作目录下。

边界文件的读入：导入网格文件后，可以利用TUI命令读入边界数据。TUI命令为：

file/read-settings

如图2所示。这样既可将文件读入。

注意：采用此方式进行边界条件的替换的时候，需要保证边界名称一致。即所设置的边界名称一致。不一致的名称会被忽略。

方式二：利用GUI方式

导入初始网格进行所有设置完毕后，保存case与data文件。

【File】>【Read】>【mesh】弹出图3所示的面板。

注意图中的选择，千万别用默认的第一个，否则如果你没有保存的话就悲催了。

选择Replace mesh之后，点击Continue即可导入新msh文件，这样边界数据会自动写入到新模型文件上。

此种方法与第一种方法注意事项相同。

对于复杂模型，肉眼不可见就需要通过软件来标记（mark）负体积的位置，这样操作：19.2 的版本中，GUI 找到这样的设置：Setting updomain>Adapt>Mark/Adapt cells>Iso value adaption，打开如下窗口，在 Iso-values of 中找到 Mesh，下面选择 Cell Volume，然后点 Compute，看看当前的网格体积都是什么范围，这里显示的是一个负数到正数的范围，说明有负体积的网格，然后在 Iso–Min 中输入负体积最小值，Iso-Max 输入 0，点击 Mark 就可以标记负体积的网格了。

然后在 Adapt 的窗口下面选择 ManageAdaption Registers，出来的窗口中选择刚刚的 Isovalue0 点击 Display 就出来了。当然，如果再看不清楚，那就点击右下角的 Options 把你需要的网格也 Draw 出来。图 9 为被标记的负体积网格单元。

这个小技巧可以避免因为忘记，计算卡死，闪退之类的问题而丢失你宝贵的案例文件，以下是官方文档原文：
When not using tools such as LSF or SGE, a different checkpointing mechanism can be used when running an ANSYS FLUENT simulation. You can checkpoint an ANSYS FLUENT simulation while iterating/time-stepping, so that ANSYS FLUENT saves the case and data files and then continues the calculation, or so that ANSYS FLUENT saves the case and data files and then exits.

• Saving case and data files and continuing the calculation:
  On Windows, create a file called check-fluent.txt, i.e.,

C:\temp\check-fluent.txt

• Saving case and data files and exiting ANSYS FLUENT:
  On Windows, create a file called exit-fluent.txt, i.e.,

temp\exit-fluent.txt

The saved case and data files will have the current iteration number appended to their file names.

ANSYS FLUENT offers an alternate way to checkpoint an unsteady simulation. While the default behavior is to checkpoint the simulation at the end of the current iteration, for unsteady simulations you have the option of completing all of the iterations in the current time-step before checkpointing. This can be set by entering the following Scheme command prior to running the unsteady simulation:

(ckpt/time-step?#t)

Now when you save the checkpoint file (as described previously), the case and data file will be saved at the end of the current time-step and named accordingly. To switch back to the default checkpointing mechanism at the end of the current iteration, use the following Scheme command:

(ckpt/time-step?#f)

To change the default location of the saved case and data files, you can use the following Scheme commands:

(set! checkpoint/check-filename pathname)

and

(set! checkpoint/exit-filename pathname)

where pathname is the path you wish to set as the new default location of the saved case and data files.

• 在TUI界面输入mesh/modify-zones/extrude-face-zone-delta，根据提示输入需延长的边界面的ID或名称并回车，然后根据提示输入每一段拉伸长度（单位m），每输入一个长度回车一次（不需再拉伸时不输长度直接回车），最终拉伸长度为每段之和。
  
  
  变为：
  
• 在TUI界面输入mesh/modify-zones/extrude-face-zone-para，根据提示输入需延长的边界面的ID或名称并回车，然后输入需拉伸的总长度，回车后依次输入每一段的比例参数（比例参数从0一直到1，如0、0.1、0.2、……1，各段数字表示分别表示各段起点与拉伸起始面的距离占总长度的比例）。