Transcript Workshop 1 Basics

Workshop 6
Electronics Cooling with
Natural Convection and
Radiation
Introduction to CFX
Pardad Petrodanesh.Co
Lecturer: Ehsan Saadati
[email protected]
www.petrodanesh.ir
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-1
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Goals
Workshop Supplement
• This workshop models the heat dissipation from a hot electronics
component fitted to a printed circuit board (PCB) via a finned heat sink.
The PCB is fitted into a casing, which is open at the top and bottom.
• Initially only the heat transfer via convection and conduction will be
modelled. The effect of thermal radiation will then be included at a later
stage.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-2
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Loading Mesh (Workbench)
Workshop Supplement
1. Open a new Workbench project and save it
as HeatSink.wbpj
2. Look in the Component Systems section of
the toolbox and drag a CFX system onto
the Project Schematic
3. Double-click Setup to start CFX-Pre
4. In CFX-Pre, right-click Mesh and select
Import Mesh > ANSYS Meshing
5. Select HeatSink.cmdb and click Open
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-3
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Options
Workshop Supplement
1. In the tree expand Case Options, double-click General and ensure that
Automatic Default Domains is switched on and Automatic Default
Interfaces is active.
2. Set the Interface Method to One Per Domain Pair. Click OK.
Separate interfaces are required for each domain because
when radiation is added, emissivity will be set differently at
each domain interfaces
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-4
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Create Fluid Domains
Workshop Supplement
First add a domain for the fluid region. The effects of
buoyancy must be included, as the flow is driven by
natural convection. The buoyancy reference density
represents the density at the ambient conditions.
1.
2.
3.
4.
5.
6.
7.
8.
Right-click on Flow Analysis 1 and insert a new
domain named Fluid
Open the details for Fluid and set the Location to
Fluid
Set the Material to Air Ideal Gas
Switch the Buoyancy option to Buoyant and set
the directional components to (0, -g, 0)
–
Click on the expression button to enter –g
Set the Reference Density to 1.1093 [kg m^-3]
Click the Fluid Models tab
Set Heat Transfer to Thermal Energy and
Turbulence to None (Laminar)
Click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-5
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Creating Materials
Workshop Supplement
CFX contains a library of many materials, but for this case we will create user
materials for the component and Printed Circuit Board (PCB).
1. In the tree right-click on Materials and select
Insert > Material. Name it ComponentMat
2. Define the material as a Pure Substance in
the CHT Solids Material Group
3. Enable Thermodynamic State and select
Solid
–
This must be set to allow it to be used in a
solid domain
4. Click the Material Properties tab and set
Density to 1120 [kg m^-3]
5. Select Specific Heat Capacity and set it to
1400 [J kg^-1 K^-1]
6. Expand Transport Properties and set
Thermal Conductivity to 10 [W m^-1 K^-1]
7. Select OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-6
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Creating Materials
Workshop Supplement
8. Repeat steps 1-7 to create PCBMat using
–
–
–
Density = 1250 [kg m^-3]
Specific Heat Capacity = 1300 [J kg^-1 K^-1]
Thermal Conductivity = 0.35 [W m^-1 K^-1]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-7
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Create Solid Domains
Workshop Supplement
This case contains three different solid parts that use different materials.
Each part will be created as a different domain.
1. Insert a new domain called HeatSink
2. Set the Location to HeatSink
3. Set the Domain Type to Solid Domain with the Material set to
Aluminium
4. Click OK to create the domain
–
Note that an interface between the two domains is automatically created
5. Repeat steps 1-4 to create a solid domain called Component located
at IC using the Material ComponentMat, and a further solid domain
called PCB located at PCB using PCBMat
When all 4 domains are created the Default Domain will
automatically be removed from the tree. Separate interfaces
between each domain will have been automatically created,
rather than combined into a single interface.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-8
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Adding Energy Source
Workshop Supplement
The component is generating 75 [W] of heat which must be added to the
simulation. To add this energy source in CFX, a subdomain must be created.
1. In the tree right-click on the Component
domain and select Insert > Subdomain,
using the name Chip
2. Set the Location to IC so the subdomain
occupies the whole of the Component
domain
3. Switch to the Sources tab and check the
Sources box and the Energy box
4. Set the Option to Total Source, enter
75 [kg m^2 s^-3] then click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-9
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Boundary Conditions
Workshop Supplement
For this case all of the heat will be extracted by the air passing over the heat
exchanger so all solid walls will be defined using adiabatic settings. Within
the simulation heat can pass between all of the solid and fluid domains
because interfaces have been automatically created.
To allow air to enter or leave the simulation domain, the top and bottom face
of the fluid domain are defined as openings.
1. Right-click on the Fluid domain and insert a new boundary called Walls
and set the Boundary Type to Wall
2. Set the Location to Wall
3. Switch to the Boundary Details tab and check that Heat Transfer is set
to Adiabatic then click OK
4. In the PCB domain rename PCB Default to PCBwalls and check that
Heat Transfer is set to Adiabatic
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-10
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Boundary Conditions
Workshop Supplement
1. In the Fluid domain rename Fluid Default to Openings and check that
the Location is set to be the two ends of the fluid domain
2. In the Basic Settings tab change the Boundary Type to Opening
3. In the Boundary Details tab set the Mass and Momentum option to
Opening Pres. and Dirn with a relative pressure of 0 [Pa]
4. Set Heat Transfer to Opening Temperature at 45 [C]
The Opening Pressure and Opening Temperature options
set Total values when flow is entering the domain and
Static values when flow is leaving.
This is appropriate when the flow outside the domain is
accelerated from rest before entering the domain but will
have a velocity when leaving.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-11
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Solver Control
Workshop Supplement
1. From the tree right-click Solver Control
and select Edit
2. Increase the Max. Iterations to 500
3. Leave the Fluid Timescale Control set to
Auto Timescale
4. Leave Solid Timescale set to Auto
Timescale
–
Note that solid regions will use a much
larger timescale than fluid regions
because only the energy equation is
being calculated within the solid
5. Click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-12
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Radiation Setup
Workshop Supplement
The next step is to redefine the model to include radiation effects. This will
be set up as a second analysis that can be run after the convection only
case using results from the initial simulation as starting conditions. This
reduces the overall computational time, as the convection only case will be
much closer to the end solution.
Most of the settings will be the same as the original analysis so the first step
will be to make a duplicate analysis.
1. Right-click on Flow Analysis 1 and rename it to Convection
2. Right-click on Convection and select Duplicate
3. Rename Copy of Convection to Radiation
–
This will form the basis of the radiation case
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-13
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Adding Radiation to the Air Domains
Workshop Supplement
The effects of radiation need to be included in the new analysis. In
this case, the surface-to-surface model will be used so radiation is only
passed from wall to wall and the fluid does not participate in any way.
This saves computational time and is appropriate since air will not
absorb or emit significant thermal radiation on these length scales.
1. In the Radiation analysis, edit the
Fluid domain
2. Switch to the Fluid Models tab
3. Under Thermal Radiation set the
Option to Discrete Transfer
4. Set Transfer Mode to Surface to Surface
5. Click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-14
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Updating the Boundary Conditions.
Workshop Supplement
Adding radiation will produce an error because additional information is now
required at the Openings boundary.
1. Edit the boundary Openings. Make sure that it is the copy from the
Radiation Flow Analysis that is being edited
2. Click the Boundary Details tab and see that Thermal Radiation has been
added and is set to Local Temperature
3. Click OK to accept this addition to the boundary condition
As the default value was all that was required in this case an
alternative method of correcting this error would have been to
right-click on the error message and select Auto Fix Physics.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-15
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Radiation Emissivity
Workshop Supplement
Different materials will have different radiation emissivity values. These can
be set at each of the boundaries around the Fluid domain within the
Radiation analysis. The emissivity of a surface is a function of the material,
surface finish and any coatings that may have been applied as well as local
temperature and the radiation wavelength.
1.In the Fluid domain find the
interface boundary that
connects the HeatSink to the
fluid
–
Hint: boundaries are
highlighted in the viewer
when selected
2.Open up that boundary and
in the Boundary Details tab
change Emissivity to 0.3
then click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-16
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Radiation Emissivity
Workshop Supplement
Note that each interface object is shown at the
flow analysis level. There are two interface
boundaries (at the domain level) associated with
each interface object. Here we are editing the
emissivity values for the interface boundaries in
the fluid domain. The interface boundaries in the
solid domains do not have an emissivity, because
there is no radiation in the solid domain (they are
opaque!).
3.Find the interface boundary in the Fluid domain
connecting the Component and Fluid domains and
set Emissivity to 0.9
4.Find the interface connecting the PCB to the
Fluid domain and set Emissivity to 0.9
5.Open the boundary Walls and set Emissivity to
0.9
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-17
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Defining Configurations
Workshop Supplement
CFX-Pre now contains two separate setups for this project. It is necessary to
indicate the order in which they run and how they are linked. This is
achieved by setting up configurations. (Note that you could run each case
separately, manually starting the radiation case from the convection
solution.)
1. In the main tree expand Simulation Control then right-click on
Configurations and select Insert > Configuration, accepting the default
name
2. In the General Settings tab set the Flow Analysis to Convection and
Activation Condition 1 to Start of Simulation
3. Click OK
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-18
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Defining Configurations
Workshop Supplement
4. Insert a second configuration and set the
Flow Analysis to Radiation. Set the
Activation Condition to End of
Configuration, and set Configuration
Names to Configuration 1
5. Switch to the Run Definition tab, select
Configuration Execution Control then
Initial Values Specification. Set the
option to Configuration Results, using
Configuration 1
6. Click OK
The convection case will run first, then
when it finishes the .res file it created will
be used to initialise the radiation
simulation.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-19
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Running the Simulation
Workshop Supplement
1. Select File > Quit to exit CFX-Pre
2. Save the Project
3. In the Project Schematic, right-click on
Solution and select Update
4. While the solver is running right-click on
Solution again and select Display Monitors
to check on progress
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-20
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Running the Simulation
Workshop Supplement
This case uses a multi-configuration setup so the first screen will show
the global progress by showing which configuration is being run.
1. Change the Workspace from the current run to Configuration1_001
–
The standard out file and residuals are displayed
2. This run will take a while to run so after a few iterations stop the run and
the results provided will be used
3. Close the Solver Manager
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-21
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Open CFD-Post
Workshop Supplement
The results field in the existing CFX module is associated with the
partially calculated results from your setup. To analyse the existing
results you will add a new results field to the project.
1.
From the Component Systems
section of the Toolbox drag a
Results system onto the
Project Schematic
2.
Right-click on the Results cell
(B2) and select Edit
3.
When CFD-Post opens, select
File > Load Results and select
HeatSink.mres. Use the
option Load complete history
as: Separate cases
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-22
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Case Comparison
Workshop Supplement
The case comparison tool allows two
different setups to be shown side by side
and any differences between the two cases
identified.
1. In the tree edit Case Comparison
2. Enable the check-box Case
Comparison Active and check that Case
1 is set to Configuration 1 and Case 2 is
set to Configuration 2
–
In the viewer a new view is created to
display the difference between the
convection only case and the case
including radiation
3. Click Apply to enter comparison mode
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-23
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Temperature
Workshop Supplement
Temperature will be a key variable for any electronics
cooling application so it will be displayed in several
locations, such as within the flow, on the surfaces of
the solid region and by extracting the maximum
temperature within the component. When these
plots are created they appear in the User Locations
and Plots section of the tree.
1.
Create a YZ plane using Location > Plane.
Name it Centre, set X to 0 [m] and colour using
the variable Temperature.
2.
Create a contour plot using Insert > Contour or
by clicking on . Use the fluid-solid interfaces
as the location (use the ‘…’ icon and Ctrl key to
select multiple locations from both
configurations). Set the Variable to Temperature
using the Global Range.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-24
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Temperature
Workshop Supplement
1. Move to the function calculator using the
icon on the toolbar. Set the options to:
Function = maxVal
Location = Component
Case = All Cases
Variable = Temperature
2. Click Calculate
–
Note that with radiation (Configuration 2) the
temperature in the solid is significantly lower
than when radiation was not included. The
cooling of the component is mirrored with an
increase in the temperature of the walls
around the fluid zone. This can be seen if
you plot the temperature on the walls or use
the Function Calculator with the areaAve
function.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-25
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Flow Displays
Workshop Supplement
To show the flow patterns a range of methods can be used including
streamlines, vector plots and isosurfaces.
1. Switch off the visibility of the existing plots
2. Insert an isosurface using Location > Isosurface and set the Variable to
Velocity with a value of 0.5 [m s^-1]
3. Gradually reduce the isosurface value to 0.2 [m s^-1] and notice that for
the radiation case higher speed flow can be observed close to the fluid
walls as well as the PCB
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-26
April 28, 2009
Inventory #002599
WS6: Electronics Cooling
Flow Displays
Workshop Supplement
1. Insert a vector plot using Insert > Vector or click on
2. Set the location to Centre. Change the sampling to Equally Spaced
with 1000 points
–
If you wish to see the pattern in the slow speed sections try going to the
Symbol tab and select Normalize Symbols
1. Insert streamlines using Insert > Streamlines or by clicking on
2. Set Start From to Openings
3. Apply 100 equally spaced points and set the Direction to Forward
and Backward
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS6-27
April 28, 2009
Inventory #002599