© Written by J.Y. WANG

数值风洞模拟范例——

仅CFX前处理及求解定义部分

CFD数值模拟过程

 

CFX前处理及求解定义：

1.导入网格（Import Mesh）

2.定义模拟类型（Simulation Type）

3.创建计算域（Domain）

4.指定边界条件（Boundary Condition）

5.给出初始条件（Initial Conditions）

6.定义求解控制（Solver Control）

7.定义输出数据（Output File & Monitor Points）

8.写入定义文件（.def File）并求解

Starting CFX-Pre

1.  Prepare the working directory using the following files in the examples directory:

• WindProfile.ccl
• BluntBodyMesh.gtm

2.  Set the working directory and start CFX-Pre.

Defining a Case in CFX-Pre

1.  In CFX-Pre, select File > New Case.

2.  Select General and click OK.

3.  Select File > Save Case As.

4.  Under File name, type BluntBody.

5.  Click Save.

Importing the Mesh

1. Edit Case Options > General in the Outline tree view and ensure that Automatic Default Domain is turned off.

Default Domain generation should be turned off because you will create a new domain manually, later in this tutorial.

1. Right-click Mesh and select Import Mesh > Other. The Import Mesh dialog box appears.
2. Apply the following settings:

Setting	Value
File name	BluntBodyMesh.gtm

1. Click Open.

Importing CEL Expressions

1.  Select File > Import > CCL.

2.  Ensure that Import Method is set to Append.

3.  Select WindProfile.ccl, which should be in your working directory.

4.  Click Open.

LIBRARY:

CEL:

EXPRESSIONS:

zb = 10 [m]

ub = 29.2 [m s^-1]

Ht = 350 [m]

Lu = 30 [m]

alpha = 0.16 []

uz = if( z>zb, ub*((z+0.00001[m])/zb)^alpha, ub )

Iz = if( z>zb, 0.1*(Ht/(z+0.00001[m]))^(alpha+0.05), 0.31 )

kz = 1.5*(Iz*uz)^2

ez = 0.09^0.75*(kz^1.5)/Lu

END

END

END

Setting the Analysis Type

1. Click Analysis Type.
2. Apply the following settings:

Tab	Setting	Value
Basic Settings	Analysis Type > Option	Steady State

1. Click OK.

Creating the Domain

1. Ensure that Flow Analysis 1 > Default Domain is deleted. If not, right-click Default Domain and select Delete.
2. Click Domain, and set the name to BluntBody.
3. Apply the following settings to BluntBody:

Tab	Setting	Value
Basic Settings	Location and Type > Location	Fluid
	Fluid and Particle Definitions	Fluid 1
	Fluid and Particle Definitions > Fluid 1 > Material	Air Ideal Gas
	Domain Models > Pressure > Reference Pressure	1 [atm]
Fluid Models	Heat Transfer > Option	Isothermal
	Heat Transfer > Fluid Temperature	20 [C]
	Turbulence > Option	Shear Stress Transport

Creating the Boundaries

Inlet Boundary

1.  Click Boundary.

2.  Under Name, type Inlet.

3.  Apply the following settings:

Tab	Setting	Value
Basic Settings	Boundary Type	Inlet
	Location	Inlet
Boundary Details	Flow Regime > Option	Subsonic
	Mass and Momentum > Option	Cart. Vel. Components
	Mass and Momentum > U	uz
	Mass and Momentum > V	0 [m s^-1]
	Mass and Momentum > W	0 [m s^-1]
	Turbulence > Option	k and Epsilon
	Turbulence > Turb. Kinetic Energy	kz
	Turbulence > Turb. Eddy Dissipation	ez

4.  Click OK.

Outlet Boundary

1.  Create a new boundary named Outlet.

2.  Apply the following settings:

Tab	Setting	Value
Basic Settings	Boundary Type	Outlet
	Location	Outlet
Boundary Details	Mass and Momentum > Option	Opening Pres. And Dirn
	Mass and Momentum > Relative Pressure	0 [Pa]
	Flow Direction > Option	Normal to Boundary Condition
	Turbulence > Option	Zero Gradient

3.  Click OK.

Free-Slip Wall Boundary

1.  Create a new boundary named FreeWalls.

2.  Apply the following settings:

Tab	Setting	Value
Basic Settings	Boundary Type	Wall
	Location	FreeWalls
Boundary Details	Mass and Momentum > Option	Free Slip Wall

3.  Click OK.

Wall Boundary on the Blunt Body Surface

1.  Create a new boundary named Body.

2.  Apply the following settings:

Tab	Setting	Value
Basic Settings	Boundary Type	Wall
	Location	Body
Boundary Details	Mass and Momentum > Option	No Slip Wall

3.  Click OK.

Setting Initial Values

The initial conditions are consistent with inlet boundaries.

1. Click Global Initialization .
2. Apply the following settings:

Tab	Setting	Value
	Initial Conditions > Cartesian Velocity Components > Option	Automatic with Value
	Initial Conditions > Cartesian Velocity Components > U	uz
	Initial Conditions > Cartesian Velocity Components > V	0 [m s^-1]
	Initial Conditions > Cartesian Velocity Components > W	0 [m s^-1]
	Initial Conditions > Static Pressure > Option	Automatic with Value
	Initial Conditions > Static Pressure > Relative Pressure	0 [Pa]
	Initial Conditions > Turbulence > Option	k and Epsilon
Global Settings	Initial Conditions > Turbulence > Turbulence Kinetic Energy > Option	Automatic with Value
	Initial Conditions > Turbulence > Turbulence Kinetic Energy > Value	kz
	Initial Conditions > Turbulence > Turbulence Eddy Dissipation > Option	Automatic with Value
	Initial Conditions > Turbulence > Turbulence Eddy Dissipation > Value	ez

1. Click OK.

Setting Solver Control

1. Click Solver Control .
2. Apply the following settings:

Tab	Setting	Value
	Advection Scheme > Option	Specified Blend Factor
	Advection Scheme > Blend Factor	0.75
	Turbulence Numerics > Option	High Resolution
Basic Settings	Convergence Control > Max. Iterations	100
	Convergence Control > Fluid Timescale Control > Timescale Control	Physical Timescale
	Convergence Control > Fluid Timescale Control > Physical Timescale	2 [s]
	Convergence Criteria > Residual Target	1e-05

1. Click OK.

Obtaining a Solution in Serial

1.  Click Start Run.

2.  When CFX-Solver is finished, select the check box next to Post-Process Results.

3.  If using Standalone Mode, select the check box next to Shut down CFX-Solver Manager.

4.  Click OK.

Obtaining a Solution with Local Parallel

To run in local parallel mode, the machine you are on must have more than one processor.

In CFX-Solver Manager, the Define Run dialog box should already be open.

1.  Leave Type of Run set to Full.

If Type of Run was instead set to Partitioner Only, your mesh would be split into a number of partitions but would not be run in the CFX-Solver afterwards.

2.  Set Run Mode to a parallel mode suitable for your configuration; for example, HP MPI Local Parallel.

This is the recommended method for most applications.

3.  If required, click Add Partition to add more partitions.

By default, 2 partitions are assigned.

4.  Select Show Advanced Controls.

5.  Click the Partitioner tab at the top of the dialog box.

6.  Use the default MeTiS partitioner.

Your model will be divided into two sections, with each section running in its own CFX-Solver process. The default is the MeTiS partitioner because it produces more efficient partitions than either Recursive Coordinate Bisection or User Specified Direction.

7.  Click Start Run.

8.  When CFX-Solver is finished, select the check box next to Post-Process Results.

9.  If using Standalone Mode, select the check box next to Shut down CFX-Solver Manager.

10. Click OK.