Áramlások numerikus szimulációja (BMEGEÁTAG26)

Computational Fluid
Dynamics
(BMEGEÁTAG26, BMEGEÁTAM05)
2016. spring, 2nd practice
Based on the learning material of Dr. Gergely Kristóf (link), created by:
• Tamás Benedek
• E-mail: benedek [at] ara.bme.hu
• Web: www.ara.bme.hu/~benedek/CFD/workbench
• If you have any problem, please don’t hesitate to ask your course
leader or me!
Agenda:
• 1st week: simulation of the flow in an orifice meter
• 2nd week: simulation of a centrifugal pump
• 3rd week: simulation of an exhaust
• 4th week: simulation of an transsonic airfoil
• 5th week: simulation of the buoyancy in a kitchen
• 6th week: individual problem solving
• 7th week: midterm exam
Main rules:
• Don’t use any special character or space! (in the file names,
folder names, names of the zones and boundaries, …) The
ANSYS can’t handle it.
• Working folder: C:/Work/Neptun_code (Neptun_code =
your code)
• The saved files will be deleted when you turn off the
computers of the CFD lab  if you want to continue your
work, please save it on a flash drive or send it to yourself
attached to an e-mail
Course leaders:
• László Nagy (nagy [at] ara.bme.hu)
• Bendegúz Bak (bak [at] ara.bme.hu)
• Esztella Balla (balla [at] ara.bme.hu)
• Balázs Farkas (farkas [at] ara.bme.hu)
• Péter Füle (fule [at] ara.bme.hu)
• András Tomor (tomor [at] ara.bme.hu)
• Bence Tóth (tothbence [at] ara.bme.hu)
Solving a problem with CFD
CAD model
(Design Modeler)
Mesh generation
(Mesher)
Solver
(FLUENT)
WORKBENCH
Postprocessing
(FLUENT/CFD post)
Aim of Exercise 2
– Pump (2D, periodic boundary conditions)
1. Chapter: The geometry
Download of base construction point set
http://www.ara.bme.hu/oktatas/tantargy/NEPTUN/BMEGEATAG26/ENGLISH_course/2015-2016-II/ea_lecture/
Right click on basic construction points, select :
„Hivatkozás mentése más néven…” , this means „Save target
in different name…” (or „Save as”) in hungarian.
Save the javascript for example in the:
C:/Work/yourneptuncode/orifice/filename.js
!Dont use space or any specific characters!
Start Screen of ANSYS Workbench
Drag and drop the element
Fluid Flow(Fluent)
Into the Project Schematic
area
Starting Design Modeler
1) Click on Advanced
Geometry Options
Change Analysis type to 2D
2) Double-click on Geometry
to start Design Modeler
Setting units
Select Millimeter unit in
Units menu
Workplane selection
Select XYPlane, right click,
then select Look At to align
plane to forntal view
Reading construction points
To generate basic construction
points onto the plane,
Use File/Run Script
Find and select the
downloaded script file
Constraints
2) At Constraints group, find
Auto Constarints and check
the Cursor box
1) After the appearance of
points, change to Sketching
panel
Drawing circular arcs
Use Draw/Arc by 3 points
command to draw the
pressure (upper) side of
blade (first select endpoints,
then middle point)
Drawing circular arcs
Do the same with leading
edge and suction (lower)
side
Drawing circular arcs
Trailing edge is an Origincentered arc (use Arc by
center)
Constraints
Fix endpoints of leading
edge and leading edge arc
using Constraints/Fixed
command
Drawing a Spline
Connect with a spline the
endpoints of computational
domain (you may have to
roll down in menu) – After
endpoint, right click and
select Open End in the
context menu
Copy/Paste the periodic boundary
1
1) Modify/Copy
2) Select spline
3) Right click:End/Use
plane origin as handle –
(you close the selection
and set the Origin as the
basepoint of Paste
command
3
2
Copy/Paste the periodic boundary
2
1
Automatic change to Paste
command
1) Cahnge r value to 60°
2) Right click: Rotate by –r
Copy/Paste the periodic boundary
Click on Origin with the
cursor: Copy/Paste finished
Drawing in let and aoutlet boundaries
Inlet/Outlet boundaries are
Origin centered arcs (Arc by
center)
Publication of input parameters
1
3
2
1) Select
Dimensions/Radius
command
2) Set (type) trailing edge
radius to 125 mm
3) By checking the box,
Publish parameter and
name it as R_out
2
Creating Surface
2
1
3
1)Go to Modelling panel
2) Select Sketch1
3) Select Concept/Surface
from sketches
Contd.
Apply
Contd.
2) Click on Generate to apply
command and make surface
1) Select Add frozen
3) Close Design Modeler
2. Chapter: The Mesh
Mesher start
Save Project (NO spaces and
$pecial chäracters
WHATSOEVER)
Double click on Mesh
Mesher is started
Initial mesh
In Project Tree, Click on
Mesh then on Update to see
current mesh
Setting boundaries as Named Selections
1
1) Select Line Selection Tool
2) Select inlet boundary
3) Right click on line, select
Create Named Selection
command form the
context menu
2
3
Setting boundaries as Named Selections
Name it as velocity_inlet
Setting boundaries as Named Selections
2
4
Similarly create:
1) Pressure_outlet
2) Per1
3) Per2
4) Leading_edge
5) Trailing_edge
6) Pressure_side
7) Suction_side
6
1
3
7
5
Setting mesh sizing
Open (explore) Sizing menu
- Set Min size: 1 mm
- Set Max Face Size: 2 mm
- Set Max Size larger than
both if conflict appears
Publish Max Face Size by
checking box
Refining boundary layer mesh
Update mesh
Right click on Mesh
InsertInflation
Refining boundary layer mesh
1
2
2,3
1) Select Surface Selection
Tool
2) Geometry: whole
surface
3) Apply
Refining boundary layer mesh
1
2
2,3
1) Select Line Selection Tool
2) Boundary: 4 edges of
blade (hold ctrl to select
multiple lines)
3) Apply
Refining boundary layer mesh
Transition ratio: 0.6
Maximum layers: 4
Growth rate: 1.5
Refining boundary layer mesh
Update
Refining boundary layer mesh – transition
ratio
Use transition ratio to set relative thickness of boundary layer mesh. Range: 0-1
transition ratio: 0.6
transition ratio: 0.2
Refining boundary layer mesh – # of layers
Use # of layers to… set… number of layers?! (number of cell layers generated by the
Inflation, belonging to the Boundary layer mesh)
Numb. of layers: 4
Numb. of layers: 10
Refining boundary layer mesh – growth rate
Use Growth rate to set the thicknes ratio of two consecutive cell layers
Growth rate: 1.5
Growth rate: 1.1
Close Mesher
Close Mesher
3. Chapter: Physical model Setup, Running
simulation
FLUENT start
Double click on Setup
FLUENT starts
FLUENT start
Launcher Window of FLUENT
Possible input:
- Number of Processors
- Number Precision
- Color Scheme of GUI
Leave as it is, just click OK
now
Definiton of periodicity
1
In Boundary Conditions
menu, Type of per1 and
per2 Zones must be set from
wall to interface
2
Definiton of periodicity
2
Set periodicity of
computational domain by
using Mesh
Interfaces/Create command:
- Mesh Interface: per
- interface zone1: per1
- interface zone2: per2
- interterface options:
periodic boundary
condition
- Type: rotational
- Check Auto Compute
Offset
- Click Create
- (Click Close if needed)
Turbulence model
Set turbulence model in
Models/Viscosus menu:
- k-epsilon
- Realizable
- Enhanced wall treatment
Material properties
3
1
2
4
In Materials menu, we obtain water material properties by:
1) Double click on Fluid: air
2) Click on Fluent Database….
3) Search and select water-liquid (<h2o <l>)
4) Copy
5) Close both windows
Fluid Zones
1
2
3
In Cell Zones menu,
Set the properties of our
single zone
1) Material name: water
liquid
2) Frame motion: check
3) Rotational velocity: 62.8
rad/s
Velocity inlet
1
2
In Boundary Conditions
slecet velocity_inlet and
click on Edit:
1) Velocity magnitude 3.5
m/s, Absolute refernce
frame
2) Turbulence
• Intesity, 10%
• Hydr. Diam, 0.01 m
Solution methods
A Solution Methods menu:
Set Schemes:
- Pressure-velocity coupling:
Coupled
- Second Order upwind
wherever possible
Convergence Monitors
1
2
In Monitors menu,
Turn off automatic
convergence detection by
given residual values
1) Double click on
Monitors/Residuals
2) Convergence criterion:
none
Convergence Monitors
Let’s create a New convergence
monitor: Torque on the blade:
- Monitors/Residuals, Statistic and
Force monitors
- Create/Moment…
Convergence Monitors
1) Plot
2) Select Wall Zones belonging to
the blade
3) Moment axis: z=1, Center: 0,0
1
2
3
Initialize
Initialize simulation by
- Selecting Hybrid
Initialization and
- clicking on Inizialize
Runing the simulation
1
3
2
4
1) Set the screen layout to
be 2-divided
2) Go to Run Calculataion
menu
3) Change Number of
Iterations to 500
4) Hit Calculate
Calculation complete
Reports for surface integrals
2
1
5
4
3
In Reports menu, select Surface integrals, and
click Set Up:
1) Field variable: Pressure / Static Pressure
2) Report type: area weighted average
3) Surfaces: select ONLY velocity-inlet
4) Click on Save output Parameter….
5) Name it as Pressure-in
Do one single iteration step (or a few)
by running the simulation again
Close FLUENT
4. Chapter: Results
Postprocessing
Double click on Results
CFD-post starts
Displaying varibale distributions
1
2
3
4
5
1)
2)
3)
4)
5)
Volume rendering
Name: ex. pressure
Domains: all
Variable: pressure
Apply
Displaying the pressure distribution
Displaying the streamlines
2
3
1
1) Hide Volume rendering 1 by
turning off checkbox in model
tree
2) Streamlines
3) Name: stramline1
Displaying the streamlines
1
2
3
1) Start from: velocity inlet
2) Number of points: as you like
3) Apply
Displaying velocity vektors
1
2
3
1) Vectors
2) Domains: surface body
3) Location: surface body
Changing the published parameters
3
Double click on Parameters
Run the case with different published
parameters
Fill up input parameters of Table of Design points
as in Excel to set parametric runs
(above image is illustration)
Click Update All Design Points to start parametric
runs and obtain output parameters
Actual simulation starts, it takes time
Two recommended variations:
Change mesh size to 0.0015 m
Radius to 110 mm
(Disproportional values will result in impossible geometry and kill the simulation)
Bruce Willis