ANSYS CFX Tutorial Laminar Flow in a Rectangular Duct

Transcription

ANSYS CFX Tutorial
Laminar Flow in a Rectangular Duct
22 January 2013
V4.00
ANSYS CFX Tutorial
Scott J. Ormiston
Jeffrey R. Berg
Department of Mechanical Engineering
University of Manitoba
Winnipeg, Manitoba
Canada
V4.00
22 January 2013
Page 1 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Introduction
This tutorial has been adapted from a tutorial created by Jeff Berg (M.Sc. student) in 2004. That tutorial was based
on running the CFX-TASCflow (V2.11) rct.lam tutorial in CFX-5 (v5.7).
Geometry Nomenclature
The duct has a length Lx , a height L y , and a depth
Lz .The duct length is aligned with the x axis, the depth with
the y axis, and the height with the z axis. The flow is assumed to be symmetric about an x-z plane that bisects the
duct in the y direction and therefore only half the duct is modelled. One corner of the duct is assumed to lie at the
origin. Figure 1 below shows the duct geometry. When the geometry was defined in the creation of the
computational mesh, all faces of the domain were assigned names. The names of the inlet and outlet planes (at
x  0 and x  L x ) are RCT_W and RCT_E, respectively. The names of the planes at y  0 and y  L y are RCT_S
and RCT_N, respectively. The names of the planes at z  0 and z  Lz are RCT_B and RCT_T, respectively.
Figure 1: Rectangular Duct Geometry
Problem Definition
The problem is a laminar, incompressible, constant property flow of water in a rectangular duct. The code will be
run with the heat transfer model turned off (even though an alternative approach would be to run the code with the
heat transfer model as “isothermal” and specify the desired temperature for an isothermal flow). The flow is
modelled with a rectilinear uniform grid for half the domain using symmetry in the y direction.
The problem parameters are:
 Mass flow = 3.962 x 10-2 [kg / s] for the full duct. The mass flow rate at the inlet of the half duct is therefore
1.981 x 10-2 [kg / s].
 Density = 997.0 [kg / m3].
 Viscosity = 8.899 x 10-4 [kg / m s].
 Duct length = 2.00 m ( Lx ).
 Duct height = 0.40 m ( Ly ). The actual grid height is 0.20 m due to symmetry.
 Duct depth = 0.30 m ( L z ).
 Hydraulic diameter of the duct, Dh , is 0.34286 m.
 Reynolds number based on the hydraulic diameter is 127.2.
Features
This tutorial demonstrates how to:
Page 2 of 25
ANSYS CFX Tutorial




22 January 2013
V4.00
Import a grid (created using ICEM CFD)
Specify boundary conditions
Solve the flow problem
Do some post-processing of the results
Setup
First, create a new directory called cfx-tutorial. Make sure that the path to this directory does not contain
any space characters. Spaces in a directory name or path will cause an error message in CFX (in addition, a
hyphen cannot be used in the simulation name). Make this new directory your current directory (i.e., “cd” to that
directory).
The grid for this tutorial has been pre-generated. It was created in software called ICEM CFD. For the purposes of
this tutorial, the completed grid will be imported into CFX. The completed grid is in a file called duct.cfx5
that can be copied to your current directory using:
cp -p ~engsjo/pub/mech-4822/cfx-tutorial/duct.cfx5 ./
or it can be downloaded (it is inside a zip file called cfxtutorial_duct_cfx5.zip) from a link in the
following web page:
http://home.cc.umanitoba.ca/~engsjo/teaching/Tutorials/index.htm#cfxtutorial
You can also use the grid that you created if you did the ICEM CFD tutorial: Simple Duct Grid.
This grid has uniform mesh spacing and 41, 11, and 16 nodes in each of the x, y, and z directions, respectively.
Assumptions about Running CFX
These instructions assume that:
1. The user has modified (customised) his/her Unix account as specified in the Linux/Unix Hands On tutorial
notes used in MECH 4822.
2. The user is connected to a Linux-based server or workstation using VNCviewer. Examples of suitable
Linux machines (with suffix .cc.umanitoba.ca) are mars, venus, jupiter, cc01, cc02,
cc03, cc04, and moon.
3. The version of the software is ANSYS CFX v14.0.
The CFX launcher can be started by typing:
cfx5 &
and then using the buttons for CFX-Pre, CFX-Solver, and CFD-Post.
In the past, two synonyms were used for running the pre-processor (cfx5pre) and the post-processor
(cfx5post) in a VNCviewer environment:
 vnc-cfxpre (which is equivalent to cfx5pre -gr mesa& )
 vnc-cfxpost (which is equivalent to cfx5post -gr mesa& )
to obtain correct graphical images when using VNCviewer. These can still be used as an alternative to the
launcher.
Page 3 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Defining the Simulation in CFX-Pre
To begin using CFX-Pre, start the program by typing
vnc-cfxpre
1. Creating a New Simulation
Select File > New Simulation
Simulation Type default is General (click on General in the window and then click OK)
Also click on OK in the following window:
To name the simulation: Select File > Save Case
In the window, set File name to rct_lam.cfx and click Save.
Page 4 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
2. Importing the Mesh
Select File > Import > Mesh
Files of type: Select ICEM CFD
File name: Enter (or browse for) duct.cfx5
Click Open
3. Domain Specification
Select Insert > Domain
Name: enter duct
Click OK
Page 5 of 25
ANSYS CFX Tutorial
Under the Domain: duct tab in the Basic Settings tab, click on
that appears, click on DUCT and then Click OK
22 January 2013
V4.00
and then in the Selection Dialog box
Still under the Basic Settings tab:
Location: this should be DUCT
Domain Type: this should be Fluid Domain
Coordinate Frame: this should be Coord 0
Fluid and Particle Definitions… this should be Fluid 1
Fluid 1:
Option: this should be Material Library
Material: select Water
Morphology:
Option: this should be Continuous Fluid
Do not click Minimum Volume Fraction.
Domain Models
Pressure:
Reference Pressure: this should be 1 [atm]
Buoyancy Model: Option: this should be Non Buoyant
Domain Motion:
Option: this should be Stationary
Mesh Deformation: Option: this should be None
Page 6 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Click Apply
Under the Fluid Models tab:
Heat Transfer:
Option: select None
Turbulence Model: Option: select None (Laminar)
Combustion:
Option: this should be None
Thermal Radiation:
Option: this should be None
Do not click Electromagnetic Model.
Click Apply
Under the Initialization tab:
Click Domain Initialization box
Click Initial Conditions box
Page 7 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Leave all the values as the default values.
Now, Click OK
4. Defining the Inlet Boundary Condition
Select Insert > Boundary
Name: enter inlet
Click OK
Under Boundary: inlet tab:
Basic Settings tab:
Boundary Type: select Inlet
Location: select RCT_W
Page 8 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Boundary Details tab:
Flow Regime: Option: Subsonic
Mass and Momentum: Option: select Mass Flow Rate
Click on space beside Mass Flow Rate and enter: 0.01981
Flow Direction: Option: Normal to Boundary Condition
Click OK
5. Defining the Outlet Boundary Condition
Select Insert > Boundary Condition
Name: enter outlet
Click OK
Page 9 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Under Boundary: outlet tab:
Basic Settings tab:
Boundary Type: select Outlet
Location: select RCT_E
Flow Regime: Option: Subsonic
Mass and Momentum: Option: Average Static Pressure
Click on space beside Relative Pressure and enter: 0.0
Leave Pres. Profile Blend at 0.05
Pressure Averaging: Option: Average Over Whole Outlet
Click OK
Page 10 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
6. Defining the Symmetry Plane Boundary Condition
Name: enter symmetry
Click OK
Under Boundary: symmetry tab:
Basic Settings tab:
Boundary Type: select Symmetry
Location: select RCT_S
Click OK
7. Defining the Walls Boundary Condition
Name: enter walls
Click OK
Under Boundary: walls tab:
Basic Settings tab:
Boundary Type: select Wall
Location: click on the
icon. In the Selection Dialog window, click on RCT_B, then, while
holding down the Ctrl key, click on RCT_N and RCT_T. Click OK.
Page 11 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Mass And Momentum: Option: select No Slip Wall
Do not check the box by Wall Velocity
Click OK
The overall image of the domain should now appear as:
Page 12 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Note that there is no duct domain “default” in the list. This means that all surfaces have been assigned a
boundary condition.
8. Setting the Solver Controls
Select Insert > Solver > Solver Control
Under Solver Control tab:
Details of Solver Control in Flow Analysis 1 tab:
Basic Settings tab:
Advection Scheme: Option: High Resolution
Convergence Control:
Min. Iterations: 1
Max. Iterations: 100
Fluid Timescale Control:
Timescale Control: select Physical Timescale
Length Scale Option: select Physical Timescale
Physical Timescale: click in the box and enter 6000
Convergence Criteria:
Residual Type: RMS
Residual Target: 1.E-4
Leave the boxes unchecked for Conservation Target, Elapsed Wall Clock Time Control, and Interrupt
Control.
Click OK
Page 13 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
9. Writing the Solver Definition File
Select Tools > Solve > Write Solver Input File
Alternatively, you can click on the icon:
In the window that appears:
File name: rct_lam.def
Files of type: CFX-Solver Input Files (*.def)
Click Save
Page 14 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
10. Saving the Simulation
Select File > Save Case
11. Ending the CFX-Pre Session
Select File > Quit
Obtaining a Solution Using the CFX-Solver
To start the solver, at the command line, type:
cfx5solve &
When the solver window comes up, if it is narrow, widen it by dragging the right edge of the window.
1. Defining the Run
Select File > Define Run
In the Define Run Window:
Solver Input File: browse for and select rct_lam.def
Run Definition tab:
Leave the box unchecked for Initial Values Specification
Type of Run: Full
Click the box by Double Precision
Parallel Environment:
Run Mode: select Platform MPI Local Parallel
You should see your host name appear in a table of Host Name and Partitions. Click the
right to set the number of partitions to 4:
on the
Page 15 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Click Start Run
The calculation should proceed with text information in one window and the residuals of the equations in
a second window. In this case there should be a print-out of 12 outer loop iterations and then some
summary information, followed by a Solver Run Finished Normally window that pops up. In this
window there is some run information. Click OK.
This solver run created the textual record of the run: rct_lam_001.out and the results file that can be postprocessed: rct_lam_001.res.
Page 16 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
2. Ending the Solver Session
Select File > Quit
Viewing the Results using CFD-Post
As simple examples of post-processing, this tutorial illustrates how to create a graph of a velocity profile at the
duct exit and a velocity vector plot on the plane of symmetry. There are many other features available in CFDPost. For more details on these features, consult the course instructor and teaching assistant, as well as the on-line
CFD-Post help.
To begin using CFD-Post type:
vnc-cfxpost
1. Loading the Results File
Select File > Load Results
In the file browser window, click on rct_lam_001.res and then click Open.
2. Creating a Line at the Exit Plane
Select Insert > Location > Line
Name: enter Exit Line
Click OK
Page 17 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
A sidebar entitled “Details of Exit Line” should appear.
Geometry tab:
Domains: All Domains
Definition:
Method: Two Points
Point 1: enter 2, 0, 0
Point 2: enter 2, 0, 0.3
Line Type: click on circle for Cut
Click on Apply
(Aside: In the future, we will use Line Type Sample and specify a number of points to sample.)
A yellow line will appear at the end of the duct image in the 3D viewer.
After zooming, it should appear like:
Page 18 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
In order to zoom in, you can use some of the icons at the top of the 3D viewer window:
To zoom click the
(zoom) or
(zoom box) icons. You can also use the pan icon:
to move
the image around and a scroll wheel on a mouse to zoom. You can also change the view by right
clicking on the 3D viewer window and choosing a Predefined Camera. If you want to see the entire duct
again, click on the fit view icon:
.
3. Creating a Graph (Chart) of a Velocity Profile at the Exit
Select Insert > Chart
Name: U Velocity versus z
Click OK
Under Details of U Velocity versus z:
General tab:
Type: XY
Title: U Velocity at the Exit
Caption: Exit Velocity Graph
Data Series tab:
For Series 1:
Name: click in the box and enter Exit Line Profile
Location: select Exit Line
X Axis tab:
Page 19 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Variable: select Z
Click on the circle for Hybrid
Leave the box checked for Determine ranges automatically
Y Axis tab:
Variable: select Velocity u
Click on the circle for Hybrid
Leave the box checked for Determine ranges automatically
Click on Apply
You should see the chart shown below in the right window (Chart Viewer).
The data used in this chart can also be exported to a spreadsheet program by using the export feature.
To do this:
Click Export
File name: enter u_exit_profile.csv
File Type: Comma Separated Values (*.csv)
Click on Save
Page 20 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
The file created, when loaded into Excel (and formatted with more decimals for column A and
scientific notation for column B), looks like:
These data can also be exported in a text file format for plotting with gnuplot or other plotting software.
4. Creating a Velocity Vector Plot
Click on the 3D Viewer tab.
Select Insert > Vector
Name: enter Symm Plane Vectors
Click OK
A sidebar entitled “Details of Symm Plane Vectors” should appear.
Page 21 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
Geometry tab:
Domains: All Domains
Definition:
Locations: select symmetry
Sampling: Vertex
Reduction: Reduction Factor
Factor: select 1.0
Variable: Velocity
Boundary Data: Click on the circle for Hybrid
Projection: None
Click on Apply
The vector plot below should appear in the 3D Viewer window. The domain was zoomed in for the
image.
Page 22 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
3. Ending the CFD-Post Session
Select File > Quit
Click on Save & Quit
File name: enter rct_lam.cst
Files of type: CFD-Post State (*.cst)
Click on Save
Page 23 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
The state file that was saved (rct_lam.cst) has saved the new objects created in the previous CFD-Post
session. When examining the same results file another time in Post, those setting can be re-loaded using File >
Load State. Another powerful feature is that the same state file can be loaded when viewing a different set of
results on the same geometry and all plots (charts, vectors, etc.) are re-computed automatically for the new results.
Further Exploration
In order to get more experience using ANSYS CFX, you can try the following additional tasks.
1. Restart the flow calculation and converge to a tighter tolerance.
a) Re-start CFX-Pre and re-load rct_lam.cfx.
b) Go to the solution controls and change:
 Maximum iterations to 500
 Residual type to maxium
 Residual target to 0.000001 (1.E-6)
c) Save the case file
d) Write a new rct_lam.def file.
e) Start the Solver and define a new run
 Select the rct_lam.def file just created
 Click on the box for Initial Values Specification
 For Initial Values 1: for File Name, browse for rct_lam_001.res
 Set up a Platform MPI Local Parallel run again with 4 partitions
 Start the run and then close the solver after it is finished.
f) Start CFD-Post and load the new results file.
g) Load the rct_lam.cst file and examine the results.
Page 24 of 25
ANSYS CFX Tutorial
22 January 2013
V4.00
2. Add energy equation calculation and thermal boundary conditions.
a) Re-start CFX-Pre and re-load rct_lam.cfx.
b) In the Outline below Analysis Type, double click on “duct”. Under “Domain: duct”, click on the
Fluid Models tab. Change the “Heat Transfer” Option to “Thermal Energy”. Click OK.
You will see an error message appear that refers to boundary conditions. This means you need to
add thermal boundary conditions. You will add an inlet temperature and a wall temperature. The
symmetry and outlet conditions do not need to be changed.
c) Double click on “inlet” below duct under Analysis Type.
 Click on the Boundary Details tab. Under Heat Transfer Option, select Static Temperature.
Then, click in the box beside Static Temperature and enter 300 (the units should be K).
Click OK.
d) Double click on “walls” below duct under Analysis Type.
 Click on the Boundary Details tab. Under Heat Transfer Option, select Heat Flux. Then,
click in the box beside Heat Flux in and enter 2000 (the units should be W/m2). Click OK.
e) Use File > Save Case As to save the current setup as rct_lam_thermal.cfx.
f) Write a Solver Input File: rct_lam_thermal.def.
g) Start the Solver and define a new run
 Select the rct_lam_thermal.def file just created
 Do not use Initial Values Specification
 Use double precision
 Set up a Platform MPI Local Parallel run again with 4 partitions
 Start the run and then close the solver after it is finished.
h) Start CFD-Post and load the new results file.
i) Load the rct_lam.cst file and examine the results.
j) Try creating a contour plot of Temperature at the outlet face.
k) Save the modified state as rct_lam_thermal.cst.
l) Examine the temperature results. Create a new chart that is the temperature profile at the Exit Line
created earlier.
m) Create a new line that goes down the centre of the duct. Create a chart that plots the temperature
along this line.
Page 25 of 25

ANSYS CFX Tutorial Laminar Flow in a Rectangular Duct

Transcription

Similar documents

THE STATION YOU LISTEN TO MOST!

WHY RE-LEVEL - Superior Mobile Home

FAST TUBE

residential venting application

How to Wrap a Horse`s Foot

ELUCID Decision Support System and Field

specification sheet - Aprilaire Partners