ANSYS流固耦合计算实例

ANSYS

流固耦合计算实例

Oscillating Plate with Two-Way Fluid- Structure Interaction

Introduction

This tutorial includes:

, Features

, Overview of the Problem to Solve

, Setting up the Solid Physics in Simulation (ANSYS Workbench)

, Setting up the Fluid Physics and ANSYS Multi-field Settings in

ANSYS CFX-Pre

, Obtaining a Solution using ANSYS CFX-Solver Manager

, Viewing Results in ANSYS CFX-Post

If this is the first tutorial you are working with, it is important

to review the following topics

before beginning:

, Setting the Working Directory

, Changing the Display Colors

Unless you plan on running a session file, you should copy the

sample files used in this tutorial from the installation folder for your

software (/examples/) to your working directory. This prevents

you from overwriting source files provided with your installation. If

you

plan to use a session file, please refer to Playing a Session File.

Sample files referenced by this tutorial include:

,

,

,

,

1. Features

This tutorial addresses the following features of ANSYS CFX.

Component Feature Details

User Mode General Mode

ANSYS CFX-Pre Transient

Simulation Type

ANSYS Multi-field

Component Feature Details

Fluid Type General Fluid

Domain Type Single Domain

Turbulence Model Laminar

Heat Transfer None

Monitor Points Output Control

Transient Results File

Wall: Mesh Motion = ANSYS MultiField

Boundary Details Wall: No Slip

Wall: Adiabatic

Timestep Transient

Animation

ANSYS CFX-Post Plots Contour

Vector

In this tutorial you will learn about:

, Moving mesh

, Fluid-solid interaction (including modeling solid deformation

using ANSYS)

, Running an ANSYS Multi-field (MFX) simulation

, Post-processing two results files simultaneously.

2. Overview of the Problem to Solve

This tutorial uses a simple oscillating plate example to demonstrate

how to set up and run a simulation involving two-way Fluid-Structure

Interaction, where the fluid physics is solved in ANSYS CFX and the

solid physics is solved in the FEA package ANSYS. Coupling between the

two solvers is required throughout the solution to model the interaction

between fluid and solid as time progresses, and the framework for the

coupling is provided by the ANSYS Multi-field solver, using the MFX

setup.

The geometry consists of a 2D closed cavity. A thin plate is

anchored to the bottom of the cavity as shown below:

An initial pressure of 100 Pa is applied to one side of the thin

plate for 0.5 seconds in order to distort it. Once this pressure is

released, the plate oscillates backwards and forwards as it attempts to

regain its equilibrium (vertical) position. The surrounding fluid damps

the oscillations, which therefore have an amplitude that decreases in

time. The CFX Solver calculates how the fluid responds to the motion of

the plate, and the ANSYS Solver calculates how the plate deforms as a

result of both the initial applied pressure and the pressure resulting

from the presence of the fluid. Coupling between the two solvers is

required since the solid deformation affects the fluid solution, and the

fluid solution affects the solid deformation.

The tutorial describes the setup and execution of the calculation

including the setup of the solid physics in Simulation (within ANSYS

Workbench) and the setup of the fluid physics and ANSYS Multi-field

settings in ANSYS CFX-Pre. If you do not have ANSYS Workbench, then you

can use the provided ANSYS input file to avoid the need for Simulation.

3. Setting up the Solid Physics in Simulation (ANSYS Workbench)

This section describes the step-by-step definition of the solid

physics in Simulation within ANSYS Workbench that will result in the

creation of an ANSYS input file . If you prefer, you

can instead use the provided file and continue from

Setting up the Fluid Physics and ANSYS Multi-field Settings in ANSYS

CFX-Pre.

Creating a New Simulation

1. If required, launch ANSYS Workbench.

2. Click Empty Project. The Project page appears displaying an

unsaved project.

3. Select File > Save or click Save button.

4. If required, set the path location to a different folder. The

default location is your working

directory. However, if you have a specific folder that you want to

use to store files created

during this tutorial, change the path.

5. Under File name, type OscillatingPlate.

6. Click Save.

7. Under Link to Geometry File on the left hand task bar click

Browse. Select the provided

file and click Open.

8. Make sure that is highlighted and click New

simulation from the

left-hand taskbar.

Creating the Solid Material

1. When Simulation opens, expand Geometry in the project tree at the

left hand side of the

Simulation window.

2. Select Solid, and in the Details view below, select Material.

3. Use the arrow that appears next to the material name Structural

Steel to select New

Material.

4. When the Engineering Data window opens, right-click New Material

from the tree view

and rename it to Plate.

5. Enter 2.5e06 for Young's Modulus, 0.35 for Poisson's Ratio and

2550 for Density.

Note that the other properties are not used for this simulation, and

that the units for these

values are implied by the global units in Simulation.

6. Click the Simulation tab near the top of the Workbench window to

return to the

simulation.

Basic Analysis Settings

The ANSYS Multi-field simulation is a transient mechanical analysis,

with a timestep of 0.1 s

and a time duration of 5 s.

1. Select New Analysis > Flexible Dynamic from the toolbar.

2. Select Analysis Settings from the tree view and in the Details

view below, set Auto Time

Stepping to Off.

3. Set Time Step to 0.1.

4. Under Tabular Data at the bottom right of the window, set End

Time to 5.0 for the

Steps = 1 setting.

Inserting Loads

Loads are applied to an FEA analysis as the equivalent of boundary

conditions in ANSYS CFX. In this section, you will set a fixed support,

a fluid-solid interface, and a pressure load. Fixed Support

The fixed support is required to hold the bottom of the thin plate

in place.

1. Right-click Flexible Dynamic in the tree and select Insert >

Fixed Support from the

shortcut menu.

2. Rotate the geometry using the Rotate button so that the bottom

(low-y) face of the

solid is visible, then select Face and click the low-y face.

That face should be highlighted to indicate selection.

3. Ensure Fixed Support is selected in the Outline view, then, in

the Details view, select

Geometry and click 1 Face to make the Apply button appear (if

necessary). Click Apply

to set the fixed support.

Fluid-Solid Interface

It is necessary to define the region in the solid that defines the

interface between the fluid in CFX and the solid in ANSYS. Data is

exchanged across this interface during the execution of the simulation.

1. Right-click Flexible Dynamic in the tree and select Insert >

Fluid Solid Interface from

the shortcut menu.

2. Using the same face-selection procedure described earlier, select

the three faces of the

geometry that form the interface between the solid and the fluid

(low-x, high-y and high-x

faces) by holding down to select multiple faces. Note that

this load is

automatically given an interface number of 1.

Pressure Load

The pressure load provides the initial additional pressure of 100

[Pa] for the first 0.5 seconds of the simulation. It is defined using a

step function.

1. Right- click Flexible Dynamic in the tree and select Insert >

Pressure from the shortcut

menu.

2. Select the low-x face for Geometry.

3. In the Details view, select Magnitude, and using the arrow that

appears, select Tabular

(Time).

4. Under Tabular Data, set a pressure of 100 in the table row

corresponding to a time of 0.

[s] and [Pa], Note: The units for time and pressure in this table

are the global units of respectively.

5. You now need to add two new rows to the table. This can be done

by typing the new time

and pressure data into the empty row at the bottom of the table, and

Simulation will

automatically re-order the table in order of time value. Enter a

pressure of 100 for a time

value of 0.499, and a pressure of 0 for a time value of 0.5.

This gives a step function for pressure that can be seen in the

chart to the left of the table. Writing the ANSYS Input File

The Simulation settings are now complete. An ANSYS Multi-field run

cannot be launched from within Simulation, so the Solve buttons cannot

be used to obtain a solution.

1. Instead, highlight Solution in the tree, select Tools > Write

ANSYS Input File and

choose to write the solution setup to the file .

2. The mesh is automatically generated as part of this process. If

you want to examine it,

select Mesh from the tree.

3. Save the Simulation database, use the tab near the top of the

Workbench window to return

to the Oscillating Plate [Project] tab, and save the project itself.

4. Setting up the Fluid Physics and ANSYS Multi-field Settings in

ANSYS CFX-Pre

This section describes the step-by-step definition of the flow

physics and ANSYS Multi-field settings in ANSYS CFX-Pre.

Playing a Session File

If you want to skip past these instructions and to have ANSYS CFX-

Pre set up the simulation automatically, you can select Session > Play

Tutorial from the menu in ANSYS CFX-Pre, then

run the session file: . After you have played

the session file as described in earlier tutorials under Playing the

Session File and Starting ANSYS CFX- Solver Manager, proceed to Obtaining

a Solution using ANSYS CFX-Solver Manager.

Creating a New Simulation

1. Start ANSYS CFX-Pre.

2. Select File > New Simulation.

3. Select General and click OK.

4. Select File > Save Simulation As.

5. Under File name, type OscillatingPlate.

6. Click Save.

Importing the Mesh

1. Right-click Mesh and select Import Mesh.

2. Select the provided mesh file, and click

Open.

Note:The file that was just created in Simulation,

, will be used as an input file for the ANSYS Solver.

Setting the Simulation Type

A transient ANSYS Multi-field run executes as a series of timesteps.

The Simulation Type

tab is used both to enable an ANSYS Multi-field run and to specify

the time-related settings for it (in the External Solver Coupling

settings). The ANSYS input file is read by ANSYS CFX-Pre so

that it knows which Fluid Solid Interfaces are available.

Once the timesteps and time duration are specified for the ANSYS

Multi-field run (coupling run), ANSYS CFX automatically picks up these

settings and it is not possible to set the timestep and time duration

independently. Hence the only option available for Time Duration is

Coupling

Time Duration, and similarly for the related settings Time Step and

Initial Time.

1. Click Simulation Type .

2. Apply the following settings

Tab Setting Value

External Solver Coupling > Option ANSYS MultiField

External Solver Coupling > ANSYS Input File

[a]

Coupling Time Control > Coupling Time Duration > Total 5 [s] Time

Basic

Coupling Time Control > Coupling Time Steps > Option Timesteps

Settings

Coupling Time Control > Coupling Time Steps > Timesteps 0.1 [s]

Simulation Type > Option Transient

Simulation Type > Time Duration > Option Coupling Time Duration

Simulation Type > Time Steps > Option Coupling Time Steps

Simulation Type > Initial Time > Option Coupling Initial Time

[a] This file is located in your working directory.

3. Click OK.

Note:You may see a physics validation message related to the

difference in the units used in

ANSYS CFX-Pre and the units contained within the ANSYS input file.

While it is important to

review the units used in any simulation, you should be aware that,

in this specific case, the

message is not crucial as it is related to temperature units and

there is no heat transfer in this case.

Therefore, this specific tutorial will not be affected by the

physics message.

Creating the Fluid

A custom fluid is created with user-specified properties. 1. Click

Material .

2. Set the name of the new material to Fluid. 3. Apply the following

settings

Tab Setting Value

Option Pure Substance

Basic Settings Thermodynamic State (Selected)

Thermodynamic State > Thermodynamic State Liquid

Material Properties Equation of State > Molar Mass 1 [kg kmol^-1]

Tab Setting Value

Equation of State > Density 1 [kg m^-3]

Transport Properties > Dynamic Viscosity (Selected)

Transport Properties > Dynamic Viscosity > Dynamic 0.2 [Pa s]

Viscosity

4. Click OK.

Creating the Domain

In order to allow the ANSYS Solver to communicate mesh displacements

to the CFX Solver, mesh motion must be activated in CFX.

1. Right click Simulation in the Outline tree view and ensure that

Automatic Default

Domain is selected. A domain named Default Domain should now appear

under the

Simulation branch.

2. Double click Default Domain and apply the following settings