嵌套效果

目录

• 几何导入

• 区域处理

• 网格准备

• 攻角设置

• 嵌套区域融合

• 设置物理模型

• 设置材料特性

• 设置初始条件

• 设置边界条件

• 设置求解器

• 标量场（Scalar Scene）准备

• 收敛监控

• 运行仿真

• 结果可视化

• 攻角改变

• 清空并重运行仿真

• 结果可视化

• 总结

---

几何导入

• 加载一个模拟

  
  加载模拟

文件地址为安装目录下的doc/startutorialsdata/compressibleFlow/data/airfoil_oversetParts.sim

文件地址

另存到一个合适的地方

---

区域处理

• 复选Background和Overset
• 右击选择Assign Parts to Regions（分配零部件至区域）....

复选Background和Overset并分配区域

• 在对话框中选择Create a Region for Each Part（为每个零部件创建一个区域） for the Region Mode and Create a Boundary for Each Part Surface（为每个零部件表面创建一个边界） for the Boundary Mode.

将零部件分配给区域对话框

• 边界类型设置，Select the Regions > Background > Boundaries > Outside node and set the Type to Free Stream.

设置Outside的类型

• Repeat this procedure for the Symmetry boundary, but set its type to Symmetry Plane.

设置Symmetry的类型

• 设置Overset节点下的边界
  Airfoil->壁面
  Overset Boundary->重叠网格
  Symmetry->对称平面

Overset边界设置

---

网格准备

You create two Automated Mesh Operations to represent the Background and Overset regions.
The Automated Mesh Operations contain the same meshers, but use different mesh settings. It is important that, in the overlapping zone, which is defined by the Overset Boundary, mesh cells are of a comparable size in both meshes.
步骤：

• 设置Background网格
• 设置Overset网格
• 生成网格

设置Background网格

1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh.
   image.png
2. 网格生成器设置
   In the Create Automated Mesh Operation dialog:
   a. Select Background from the Partslist.
   b. Select the following meshers, in order:

Background Create Automated Mesh Set Background自动网格操作设置

3. Rename the Operations > Automated Mesh node to Background Mesh.

4. Edit the Operations（操作） > Background Mesh > Default Controls（默认控制） node and set the following properties:
   

   Default Controls
   Background Mesh 默认控制设置

5. Right-click the Operations > Background Mesh > Custom Controls（自定义控制） node and select New > Volumetric Control（体控制）.
   

   体控制

6. Edit the Volumetric Control node and set the following properties:
   

   Volumetric Control Set
   Volumetric Control Set

设置Overset网格

1. Copy and paste the Background Mesh node into the Operations node and rename the Copy of Background Mesh node to Overset Mesh.
   对Background Mesh [ctrl+c]选择操作 [ctrl+v],将新生成的副本重命名为Overset Mesh

2. Select the Operations > Overset Mesh node and set Input Parts（输入零部件） to Overset.

3. Select the Operations > Overset Mesh > Meshers（网格生成器） > Prism Layer Mesher（棱柱层网格单元生成器） node and set Distribution Mode（分布模式） to Wall Thickness（壁厚）.
   

   第2/3步设置

4. Edit the Operations > Overset Mesh > Default Controls（默认控制） node and set the following properties:
   

   操作-Overset Mesch-默认控制
   第4步设置

5. Rename the Operations > Overset Mesh > Custome Controls > Volumetric Control node to Overlap.
   You can reuse the volumetric control that you created for the background mesh.

6. Following the same procedure as for the background mesh, create three additional new volumetric controls and give them the following names:
   将第5步的Overlap复制三个副本，并重命名为
   Airfoil.
   Leading Edge.
   Trailing Edge.
   

   Overset Mesh下的4个自定义操作

（以下7/8步可以直接拉到后面的图示看）

7. In the Controls node of all four volumetric controls, set the following properties:
   

   volumetric controls set

8. For each volumetric control, select the following parts and the following values for Values > Custom Size:
   

   parts select
   第7/8步Overlap设置
   第7/8步Airfoil设置
   第7/8步Leading Edge设置
   第7/8步Trailing Edge设置

生成网格（Generating the Mesh）

With both Automated Mesh Operations for the background mesh and the overset mesh set up, you generate the volume mesh. You then convert the mesh from 3D to 2D to simplify the solution.

To generate the mesh:

1.To build the volume mesh, click the Generate Volume Mesh button in the toolbar. This process can take a few minutes.
点击工具栏中的生成体网格按钮

生成体网格

2.To view the mesh, create a mesh scene.
生成一个网格场景以查看网格

网格场景

3.Zoom in on the Overset boundary to compare the cell size of the overset mesh to the background mesh at this boundary.
中键缩放，右键平移查看结果

生成的网格结果

You can convert the mesh from 3D to 2D to simplify the solution.
将3D网格转换到2D网格

4. In the menu bar, select Mesh（网格） > Convert to 2D（转换为二维）
   

   转换为二维按钮

5. In the Convert Regions to 2D dialog, tick the Delete 3D regions after conversion option and click OK.
   在将区域转换为2D对话框中勾选转换后删除3D区域
   

   勾选转换后删除3D区域

6. Save the simulation.

   
   生成的结果

---

设置攻角Specifying Angle of Attack

Rotate the Overset region to correspond to a 2.54° angle of attack of the airfoil.
将嵌套网格区域旋转到2.54°攻角。

The steps presented here demonstrate how using overset meshes allows you to change the relative position of bodies without the need to generate a mesh.

1. Right-click the Regions > Overset 2D node and select Transform > Rotate
   右击区域>Overset 2D选择变换>旋转

旋转Overset 2D

2. In the Rotate Regions dialog, set the Angle to -2.54 deg（注意这个deg）.
   

   角度设置

3. Click Apply, and then click Close.
   

   网格旋转的结果

---

嵌套区域融合Coupling the Overset Region

Overset regions are coupled to the background region using the Overset Mesh interface.
Normally, this interface can be created before generating the background and overset meshes. To activate this interface feature, you must create a physics continuum. Current implementation requires that the background and overset regions use the same physics continuum. In this tutorial, you are creating the Overset Mesh interface after converting the mesh to 2D as this step deletes all previously created interfaces.
To create the interface:

1. Multi-select the Background 2D and Overset 2D regions.
   复选Background 2D和Overset 2D
2. Right-click the selected regions and choose Create Interface > Overset Mesh.
   右击依次选择创建界面>重叠网格
   创建界面>重叠网格

An Overset Mesh 1 node appears under the Interfaces. Use the default Distance Weighted Interpolation Option for the mesh coupling.

节点中自动新增一个重叠网格 1

When you initialize the Overset Mesh interface, STAR-CCM+ chooses acceptor cells on the overset region. Cells in the background region that are overlapped by the overset region are deactivated.

分析嵌套网格Analyzing Overset Mesh

Display cell status in a scalar scene.
To analyze the mesh before running the simulation, initialize the Overset Mesh interface:

1. Right-click the Interfaces node and select Initialize.
   右击界面选择初始化
   初始化网格界面

Notice that the background mesh within the airfoil part has been removed in Mesh Scene 1.

生成结果

Analyze the overset mesh using the Overset Cell Status field function.

2. Create a scalar scene.
   The Scalar Scene 1 display appears.
   生成一个新场景>标量
   

   新场景>标量

3. Right-click the scalar bar at the bottom of the display and select Overset Cell Status from the pop-up menu.
   

   select Overset Cell Status

4. Select the Scalar Scene 1 > Displayers > Scalar 1node and set Representation to Overset Mesh.
   选择标量场景 1>显示器>标量 1节点，讲表示设置为Overset Mesh
   

   标量 1>表示

First look at the cell status in the overset region.

5. Select the Scalar Scene 1 > Displayers > Scalar 1 > Parts node and tick the Overset 2D region in the Parts property.
   选择标量场景 1>显示器>标量 1>零部件节点，只选择Overset 2D零件
   选择零部件

6. Select the Scalar Scene 1 > Displayers > Scalar 1 > Scalar Field node and set the Min to -2.0 and the Max to 1.0.
   标量场设置

Acceptor cells outline the overset region in blue.

嵌套区域显示

7. To see the background region cell status, change the Parts to Background 2D within the Scalar Scene 1 > Displayers > Scalar 1 > Parts node.
   The red cells in the background mesh are inactive.
   嵌套区域显示

设置物理模型Setting up Physics Models

Models define the spatial and temporal solution methods and the physical properties of the flow.
In this example, the flow is steady, turbulent, and compressible. Use the default Spalart-Allmaras Turbulence model and the ideal gas model. The analysis also uses the coupled solver, which is recommended for all supersonic and transonic compressible flows.
By default, a continuum called Physics 1 is created when the three-dimensional mesh is generated and a Physics 1 2D continuum is created when the mesh is converted to two-dimensional. You can delete the Physics 1 continuum, as only one is used in this simulation.

1. Delete the Continua > Physics 1 node.
   To use a more appropriate name for the Physics 1 2D continuum:
   删除Physics 1
   

   删除Physics 1

2. Rename the Continua > Physics 1 2D node to Airfoil
   将Physics 1 2D重命名为Airfoil
   You can now choose the physics models for the continuum.
   

   将Physics 1 2D重命名为Airfoil

3. For the Airfoil continuum, select the following models, in order:
   双击连续体>Airfoil>模型进行设置
   

   Airfoil continuum Set

模型设置

4. Click Close.

---

设置材料特性Setting Material Properties

Set the Reynolds number to 6.5e6, changing the dynamic viscosity
Use the following steps:

1. Open the Continua > Airfoil > Models > Gas > Air node.
   双击打开连续体>Airfoil>模型>气体
2. Edit the Material Properties node and set the following properties:
   Material Properties Set
   气体模型设置

---

设置初始条件Setting Initial Conditions

As in the Transonic Flow tutorial, initialize the velocity field to 250.0 m/s.

1. Edit the Continua > Airfoil > Initial Conditions node and set the following properties:
   双击打开连续体>Airfoil>初始条件
   Initial Conditions

初始条件设置

The default values for the remaining initial conditions are suitable for this tutorial.

---

设置边界条件Setting Boundary Conditions

Set the conditions at the boundaries of the airfoil and the domain.

The geometry used for this tutorial has only two boundaries for the physics:

• A wall boundary representing the surface of the airfoil and defined in the Overset region.

• A freestream boundary at the external edge of the entire solution domain defined in the Background region.

Set the freestream conditions on the outer perimeter of the Background region.

1.Edit the Regions > Background 2D > Boundaries > Outside > Physics Values node and set the following properties:
双击设置区域>Background 2D>边界>Outside>物理值

Physics Values
设置物理值

All other conditions for the freestream boundary and the default wall are suitable for this problem.

---

设置求解器Setting Solver Parameters

The simplicity of this problem allows a rapidly converging solution to be obtained using a larger Courant number.
In problems involving more complex geometries or physics, attempting to shorten the run time in this way may cause the solution to diverge.
To increase the Courant number:

1. Select the Solvers > Coupled Implicit node and set Courant Number to 20.0.
   求解器>耦合隐式设置库朗数为20.0
   

   求解器>耦合隐式

2. Save the simulation.

---

准备标量场Preparing a Scalar Scene

View the Mach number profile during the run to monitor the supersonic flow region above the airfoil.

Use the following steps:

1.Create a scalar scene.
A new Scalar Scene display appears.
右击并选择生成场景>新场景>标量

2.Right-click the scalar bar at the bottom of the display and select Mach Number > Lab Reference Frame from the pop-up menu.

以马赫数为标量

3.Initialize the run by clicking Initialize Solution in the toolbar, then use the middle mouse button to zoom in on the airfoil in the center of the scalar scene.
在工具栏中点击初始化求解

初始化求解

4.To change the style of the Mach number contours, select the Scalar Scene 2 > Displayers > Scalar 1node and set Contour Style to Smooth Filled.
选择场景>标量场景2>标量1，将轮廓样式设置为平滑填充

---

收敛监控Monitoring Convergence

To determine when the problem has converged, plot the lift and drag coefficients.
Use the following steps:

1. Right-click the Reports node and select New Report > Force Coefficient.
   New Report > Force Coefficient

右击报告选择新报告>力系数

生成力系数报告

A new report node named Force Coefficient 1 is created.

2. Rename this node Drag Coefficient
   重命名为Drag Coefficient

3. Select the Drag Coefficient node and set the following properties:
   

   Drag Coefficient Properties
   Drag Coefficient Set
   Drag Coefficient属性

4. Right-click the Drag Coefficient node and select Create Monitor and Plot from Report.
   右击Drag Coefficient选择根据报告创建监视器和绘图
   A new plot node appears named Drag Coefficient Monitor Plot.
   

   根据报告创建监视器和绘图

5. Repeat the steps described above to create and display a plot for the lift coefficient. Use the same settings as for the drag coefficient except rename the report node Lift Coefficient and set its Direction property to [0.0, 1.0, 0.0]
   重复前述步骤（可以直接复制粘贴）创建一个Lift Coefficient ，注意改方向
   Lift Coefficient属性

6. Save the simulation.

---

运行仿真Running the Simulation

You are now ready to run the simulation.

Use the following steps:

1.Click Run in the toolbar.
点击工具栏中的运行

The Residuals display is created automatically and shows the progress of the solver.

During the run, it is possible to stop the analysis by clicking Stop in the toolbar. If you do halt the simulation, it can be continued later by clicking Run. If left alone, the simulation continues until 1000 iterations have been completed.
可以在停止标准>Maximum Steps中设置最大步数

2.Save the simulation after the solver has finished

---

结果可视化Visualizing the Results

The Scalar Scene display shows the Mach number profile at the end of the run.
The profile shows the transonic flow around the airfoil, including the shock wave produced behind the supersonic region on the upper surface.

马赫数分布

The lift and drag coefficient plots provide a check for convergence. As there is little variation in both monitors, it is reasonable to conclude that the solution has converged.

阻力系数收敛曲线
升力系数收敛曲线

---

改变攻角Changing Angle of Attack

Rotate the overset mesh.
One advantage of using an overset mesh is being able to transform regions without having to remesh. If, for instance, you want to study the airfoil at a different angle of attack, you can rotate the Overset region by a different angle and rerun the simulation.

1. Right-click the Regions > Overset 2D node and select Transform > Rotate... .
   右击区域>Overset 2D，选择转换>旋转
   

   旋转操作

2. In the Rotate Regions dialog, set Angle to -10 deg（注意deg->°）.
   

   设置攻角
   旋转结果

3. Click Apply.

The transformed overset region must be completely within that refined part of the background region where the background mesh is of the same size as the overset mesh.

---

清空并重运行仿真Clearing and Rerunning the Simulation

Clear the solution and rerun the simulation using the same physics setup.

Use the following steps:

1.In the menu bar, select Solution > Clear Solution.

清除求解

2.Click Run in the toolbar.

---

结果可视化Visualizing the Results

Re-examine the scalar scene.
The scalar scene solution is shown below. You can see that if the angle of attack is increased further, the steep adverse pressure gradient on the upper surface of the airfoil causes the flow to separate close to the leading edge, resulting in a large wake.

马赫数分布图
阻力系数收敛曲线
升力系数收敛曲线

---

总结Summary

This Transonic Flow tutorial demonstrated how to use overset mesh to simulate transonic flow over an airfoil

This tutorial introduced the following features of STAR-CCM+:

• Creating and analyzing an overset mesh for an airfoil problem.

• Defining models for a compressible flow problem.

• Defining the material properties required for the selected models.

• Setting solver parameters for a steady-state run.

• Analyzing results and convergence.

• Modifying angle of attack.