2. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-2
Chapter Overview
• In this chapter, performing steady-state thermal analyses in
Simulation will be covered:
– Geometry and Elements
– Contact and Types of Supported Assemblies
– Environment, including Loads and Supports
– Solving Models
– Results and Postprocessing
• The capabilities described in this section are generally
applicable to ANSYS DesignSpace Entra licenses and
above, except for an ANSYS Structural license.
– Some options discussed in this chapter may require more
advanced licenses, but these are noted accordingly.
– It is assumed that the user has reviewed Chapters 1-3 prior to
this chapter. (Chapters 4-5 are optional)
3. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-3
Basics of Steady-State Heat Transfer
• For a steady-state (static) thermal analysis in Simulation,
the temperatures {T} are solved for in the matrix below:
This results in the following assumptions:
– No transient effects are considered in a steady-state analysis
– [K] can be constant or a function of temperature
• Temperature-dependent thermal conductivity can be input for each
material property
– {Q} can be constant or a function of temperature
• Temperature-dependent film coefficients can be input for
convective boundary conditions
T
Q
T
T
K
4. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-4
Basics of Steady-State Heat Transfer
• Fourier’s Law provides the basis of the previous equation:
– This means that the thermal analysis Simulation solves for is a
conduction-based equation.
• Heat flow within a solid (Fourier’s Law) is the basis of [K]
• Heat flux, heat flow rate, and convection are treated as boundary
conditions on the system {Q}
• No radiation is currently considered
• No time-dependent effects are currently considered
– Heat transfer analysis is different from CFD (Computational
Fluid Dynamics)
• Convection is treated as a simple boundary condition, although
temperature-dependent film coefficients are possible.
• If a conjugate heat transfer/fluid problem needs to be analyzed,
one must use ANSYS CFD tools instead.
• It is important to remember these assumptions related to
performing thermal analyses in Simulation.
5. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-5
Physics Filters
• Before proceeding to a detailed discussion on performing
thermal analyses in Simulation, it is useful to point out that
if a thermal-only solution is to be performed, the Physics
Filter can be useful to filter the GUI.
– Under “View menu > Physics Filter,” unselect the “Structural”
option. Now, the available options in the Simulation GUI will
only reflect thermal analyses.
– This applies to options in the
“Environment” and “Solution”
levels only.
– If a thermal-stress simulation is to
be performed, do not turn off any
physics filters since both structural
and thermal options may be required.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
6. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-6
A. Geometry
• In thermal analyses, all types of bodies supported by
Simulation may be used.
– Solid, surface, and line bodies are supported by all products
which support thermal analyses.
• For surface bodies, thickness must be input in the Details view of
the Geometry branch
• The cross-section and orientation of line bodies is defined within
DesignModeler and is imported into Simulation automatically.
Although the cross-section and orientation is defined, this
information is meant for structural analyses, and the actual
thermal link element will have an ‘effective’ cross-section based on
the input properties.
• No heat flux or vector heat flux output is available with line bodies.
Only temperature results are available for line bodies.
– The “Point Mass” feature is not applicable in thermal analyses
• Point Mass is described in Chapter 4, Linear Structural Analysis.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
7. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-7
… Geometry
• It is important to understand assumptions related to using
shell and line bodies:
– For shell bodies, through-thickness temperature gradients are
not considered. A shell body should be used for thin
structures when it can be safe to assume temperatures on top
and bottom of surface are the same.
• Temperature variation will still be considered across the surface,
just not through the thickness, which is not explicitly modeled.
– For line bodies, thickness variation in the cross-section is not
considered. A line body should be used for beam- or truss-like
structures, where the temperature can be assumed to be
constant across the cross-section.
• Temperature variation will still be considered along the line body,
just not through the cross-section, which is not explicitly modeled.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
8. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-8
… Material Properties
• The only required material property is thermal conductivity.
– Material input is under the “Engineering Data” tab, and material
assignment is per part under the “Geometry” branch
– Thermal Conductivity is
input under the Engineering
Data tab.
Temperature-dependent
thermal conductivity can
be input as a table.
– Other material input
is not used in thermal.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
If any temperature-dependent material properties exist, this will
result in a nonlinear solution. This is because the temperatures are
solved for, but the materials are dependent on the temperatures, so
it is not linear.
9. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-9
B. Assemblies – Solid Body Contact
• When importing assemblies of solid parts, contact regions
are automatically created between the solid bodies.
– Surface-to-surface contact allows non-matching meshes at
boundaries between solid parts
– Contact enables heat transfer between parts in an assembly
Model shown is from a sample Inventor assembly.
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
10. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-10
… Assemblies – Contact Region
• In Simulation, the concept of contact and target surfaces
are used for each contact region.
– One side of the contact region is comprised of “contact”
face(s), the other side of the region is made of “target” face(s).
– Heat flow is allowed between contact and target faces (based
on the contact normal direction)
• When one side is the contact and the other side is the target, this
is called asymmetric contact. On the other hand, if both sides are
made to be contact & target, this is called symmetric contact.
However, the designation of which side is contact or target is
unimportant in thermal analysis.
• By default, Simulation uses symmetric
contact for solid assemblies.
• For ANSYS Professional licenses
and above, the user may change to
asymmetric contact, as desired.
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
11. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-11
… Assemblies – Contact Region
• As noted in the previous slide, heat flows within a contact
region in the contact normal direction
– No heat spreading is considered in the contact/target interface
• Heat spreading is considered within shell or solid elements at the
contact or target surfaces because of Fourier’s Law
• Heat flow within the contact region is in the contact normal
direction only
• This means that, regardless of the definition of the contact region,
heat flows only if a target element is present in the normal
direction
In the figure on the left, the solid
green double-arrows indicate
heat flow within the contact
region. Heat flow only occurs if a
target surface is normal to a
contact surface.
The light, dotted green arrows
indicate that no heat transfer will
occur between parts.
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
12. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-12
… Assemblies – Contact Region
• In Simulation, various contact behaviors exist
– The contact “Type” is meant for structural applications
– If the parts are initially in contact, heat transfer will occur
between the parts. If the parts are initially out of contact, the
parts will not transfer heat between each other.
– Based on the contact type, whether heat will be transferred
between contact and target surfaces is outlined below:
– The pinball region is automatically defined and set to a
relatively small value to accommodate small gaps which may
present in the model. The pinball region will be discussed
next.
Initially Touching Inside Pinball Region Outside Pinball Region
Bonded Yes Yes No
No Separation Yes Yes No
Rough Yes No No
Frictionless Yes No No
Contact Type
Heat Transfer Between Parts in Contact Region?
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
13. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-13
… Assemblies – Contact Region
• The pinball region may be input and
visualized in ANSYS Professional
licenses and above.
– If the target nodes lie within the pinball region
and the contact is bonded or no separation,
then heat transfer will occur (solid green lines)
– Otherwise, no heat transfer will occur between
nodes (dotted green lines)
In this figure on the right, the
gap between the two parts is
bigger than the pinball region,
so no heat transfer will occur
between the parts
Pinball Radius
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural
Mechanical/Multiphysics x
14. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-14
… Assemblies – Thermal Conductance
• By default, a high thermal contact conductance (TCC) is
defined between parts of an assembly
– The amount of heat flow between two parts is defined by the
contact heat flux q:
where Tcontact is the temperature of a contact “node” and Ttarget
is the temperature of the corresponding target “node” located
in the contact normal direction.
– By default, TCC is set to a relatively ‘high’ value, based on the
largest material conductivity defined in the model KXX and the
diagonal of the overall geometry bounding box ASMDIAG.
This essentially provides ‘perfect’ conductance between parts.
contact
target T
T
TCC
q
ASMDIAG
KXX
TCC /
000
,
10
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
15. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-15
… Assemblies – Thermal Conductance
• Perfect thermal contact conductance between parts means
that no temperature drop is assumed at the interface.
• One may want to include finite thermal conductance instead
– Two surfaces (at different temperatures) in contact experience
a temperature drop across the interface. The drop is due to
imperfect contact between the two surfaces. The imperfect
contact, and hence the finite contact conductance, can be
influenced by many factors such as:
• surface flatness
• surface finish
• oxides
• entrapped fluids
• contact pressure
• surface temperature
• use of conductive grease
DT
T
x
16. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-16
… Assemblies – Thermal Conductance
• In ANSYS Professional licenses and above, the user may
define a finite thermal contact conductance (TCC) if the
Pure Penalty or Augmented Lagrange Formulation is used.
– The thermal contact conductance per unit area is input for
each contact region in the Details view, as shown below.
– If thermal contact resistance is known, invert this value and
divide by the contacting area to obtain TCC value.
– When this is done, there will now be a temperature drop
between the contact and target surfaces for a contact region.
If “Thermal Conductance” is left
at “Program Chosen,” near-
perfect thermal contact
conductance will be defined.
The user can change this to
“Manual” to input finite thermal
contact conductance instead,
which is the same as including
thermal contact resistance at a
contact interface.
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural
Mechanical/Multiphysics x
17. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-17
… Assemblies – Thermal Conductance
• If using symmetric contact, the user does
not need to account for a ‘double’
thermal contact resistance.
– Input values as normal
• MPC bonded contact allows for perfect
thermal contact conductance.
– In this case, no thermal contact
conductance is used nor defined because
‘contact’ is related via constraint
equations.
– The contact “node” and corresponding
target “node” will have the same
temperature because of perfect contact
conductance.
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural
Mechanical/Multiphysics x
Do not use “Normal Lagrange”
formulation for thermal analyses. If
selected, the ANSYS solver will actually
use “Augmented Lagrange” with a
‘perfect’ thermal contact conductance.
18. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-18
… Assemblies – Surface Body Contact
• For ANSYS Professional licenses and above, mixed
assemblies of shells and solids are supported
– Allows for more complex modeling of assemblies, taking
advantage of the benefits of shells, when applicable
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural
Mechanical/Multiphysics x
19. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-19
… Assemblies – Surface Body Contact
• Edge contact is a subset of general contact
– For contact including shell faces or solid
edges, only bonded or no separation
behavior is allowed.
– For contact involving shell edges, only
bonded behavior using MPC formulation is
allowed.
• For MPC-based bonded contact, user can set
the search direction (the way in which the
multi-point constraints are written) as either
the target normal or pinball region.
• If a gap exists (as is often the case with
shell assemblies), the pinball region can be
used for the search direction to detect
contact beyond a gap.
• MPC results in perfect contact conductance
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural
Mechanical/Multiphysics x
20. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-20
… Assemblies – Spot Weld
• Spot welds provide a means of connecting shell assemblies
at discrete points for heat transfer
– Spotweld definition is done in the CAD software. Currently,
only DesignModeler and Unigraphics define spotwelds in a
manner that Simulation supports.
– Spotwelds can also be created in Simulation manually, but
only at discrete vertices.
ANSYS License Availability
DesignSpace Entra
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
DesignModeler x
Pro/ENGINEER
Unigraphics x
SolidWorks
Inventor
Solid Edge
Mechanical Desktop
CATIA V4
CATIA V5
ACIS (SAT)
Parasolid
IGES
21. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-21
C. Loads
• There are three types of loads in thermal analyses:
– Heat Loads:
• These loads pump heat into the system.
• Heat loads can be input as a known heat flow rate or heat flow rate
per unit area or unit volume.
– Adiabatic Condition:
• This is the naturally-occurring boundary condition, where there is
not heat flow through the surface.
– Thermal Boundary Conditions:
• These boundary conditions act as heat sources or heat sinks with
a known temperature condition.
• These can be either a prescribed temperature or a convection
boundary condition with a known bulk temperature.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
22. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-22
… Heat Loads
• Heat Flow:
– A heat flow rate can be applied to a vertex, edge, or surface.
The load gets distributed for multiple selections.
– Heat flow has units of energy/time (i.e., power).
• Heat Flux:
– A heat flux can be applied to surfaces only.
– Heat flux has units of energy/time/area (i.e., power/area)
• Internal Heat Generation:
– An internal heat generation rate can be applied to bodies only.
– Heat generation has units of energy/time/volume
A positive value for heat load will add energy to the system.
Also, if multiple loads are present, the effect is cumulative.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
23. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-23
… Adiabatic Conditions
• Perfectly Insulated:
– Perfectly insulated condition is applied to surfaces
– Can be thought of as a zero heat flow rate loading
– This is actually the naturally-occurring condition in thermal
analyses, when no load is applied.
• Usually, one does not need to apply a perfectly insulated condition
on surfaces since that is the natural behavior for a regular surface.
• Hence, this loading is meant to be used as a way to remove
loading on specified surfaces. For example, it may be easier for a
user to apply heat flux or convection on all surfaces, then use the
perfectly insulated condition to selectively ‘remove’ the loading on
some surfaces (such as those in contact with other parts).
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
24. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-24
… Thermal Boundary Conditions
Thermal boundary conditions present a known local or
‘remote’ temperature condition.
• At least one type of thermal boundary condition must be present.
Otherwise, the steady-state temperature will be infinite if only heat
is pumped into a system!
• Also, Given Temperature or Convection load should not be applied
on surfaces that already have another heat load or thermal
boundary condition applied to it.
– If applied on an entity which also has a heat load, the
temperature boundary condition will override.
– Perfect insulation will override thermal boundary conditions.
• Given Temperature:
– This imposes a temperature on vertices, edges, or surfaces.
– Temperature is the degree of freedom solved for, but this fixes
the temperature on selected entities to a given value.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
25. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-25
… Thermal Boundary Conditions
• Convection:
– Applied to surfaces only.
– Convection relates a ‘ambient temperature’ with the surface
temperature:
where the convective heat flux q is related to a film coefficient
h, the surface area A, and the difference in the surface
temperature Tsurface & ambient temperature Tbulk.
– Meant to provide a simplified way of accounting for heat
transport from a fluid. “h” and “Tbulk” are user-input values.
– The film coefficient h can be constant or input from a file (next)
ambient
surface T
T
hA
q
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
26. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-26
… Thermal Boundary Conditions
• Temperature-Dependent Convection (continued):
– If film coefficient h is input from a file, this can be a constant
or temperature-dependent value h(T).
• Define a convection boundary condition under the Environment
branch and define the Type to be “Temperature-Dependent”. Next,
select “New Convection…” for the Correlation. The “Engineering
Data” tab will open and the Coefficient Type can then be defined
for the new convection load.
• Determine what temperature is used for h(T) first, for temperature-
dependent film coefficients. Temperature can be:
– Average film temperature
T=(Tsurface+Tbulk)/2
– Surface temperature
T= Tsurface
– Bulk temperature
T= Tbulk
– Difference of surface and
bulk temperatures
T=(Tsurface-Tbulk)
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
Select the temperature-
dependency from the
pull-down menu
27. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-27
… Thermal Boundary Conditions
• Temperature-Dependent Convection (continued):
• After the type of temperature-dependency is selected, the user
may input the film coefficients and temperatures in a table. The
values are plotted on a graph, as shown below.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
If any temperature-dependent
convection load is applied, this
will result in a nonlinear solution
since the surface temperature is
solved for, but the film coefficient
h is based on a function of the
surface temperature.
The only exception is if the film
coefficient h is based on a
function of the bulk temperature
only. In Simulation, the bulk
temperature is constant and input
by the user, so this load will not
be nonlinear.
Right mouse click on the table
to add or delete values.
28. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-28
… Thermal Boundary Conditions
• Temperature-Dependent Convection (continued):
• The convection data can also be imported from a file.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
29. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-29
… Thermal Loads Summary
• For some structural users, it may be useful to provide an
analogy of structural and thermal analyses:
– There are some types of loads that do not have any analogy
• There is no thermal equivalent for inertial loads such as rotational
velocity or acceleration
• The analogy of convective boundary condition is a ‘foundation
stiffness’ support in structural terms, similar to a grounded spring
Structural Thermal
Natural Condition No external force Perfectly Insulated
(No heat flow rate)
Direct Given Displacement Given Temperature
Indirect Convection
Direct Force Heat Flow
Per Area Pressure Heat Flux
Per Volume Thermal Expansion Internal Heat Generation
Inertial Loads Acceleration
Boundary
Conditions
Load
30. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-30
D. Solution Options
• Solution options can be set under the “Solutions” branch:
– The ANSYS database can be saved if “Save
ANSYS db” is set
• Useful if you want to open a database in ANSYS
– Two solvers are available in Simulation
• The default solver is automatically chosen and
does not usually need to be changed.
• The “Iterative” solver can be efficient for solving
large models whereas the “Direct” solver is a
robust solver and handles any situation.
• The ability to change the default solver is under
“Tools > Options… > Simulation: Solution
> Solver Type”
– The “Weak Springs” and “Large Deflection”
options are meant for structural analyses only,
so they can be ignored for a thermal analysis.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
31. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-31
… Solution Options
– Informative settings show the user the status of the analysis:
• For a regular thermal analysis, the “Analysis Type”
will be set to “Static Thermal.” If structural
supports and results are present, then the
analysis type will be “Thermal Stress.”
• A nonlinear solution will be required if
temperature-dependent (a) material properties or
(b) convection film coefficients are present. This
means that several internal iterations will be run
to achieve heat equilibrium.
• The solver working directory is where scratch files
are saved during the solution of the equations.
By default, the TEMP directory of your Windows
system environment variable is used, although this
can be changed in “Tools > Options… >
Simulation: Solution > Solver Working Directory”.
– Any solver messages which appear after
solution can be checked afterwards under
“Solver Messages”
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
32. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-32
… Solving the Model
• To solve the model, request results first (covered next) and
click on the “Solve” button on the Standard Toolbar
– By default, two processors (if present) will be used for parallel
processing. To change this, use “Tools > Options… >
Simulation: Solution > Number of Processors to Use”
– Recall that if a “Solution Information” branch is requested, the
details of the solution output can be examined.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
33. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-33
… Solving the Model
• To perform a thermal-stress solution, simply add structural
support(s) and request structural results, then solve the
model.
– Structural loads are optional but can also be added.
– Simulation will know that a thermal-stress analysis is to be
performed (under Details view of the Solution branch). The
following will be performed automatically:
• A steady-state thermal analysis will be performed
• The temperature field will be mapped back onto the structural
model
• A structural analysis will be performed
– See Chapter 4 for details on Structural Analyses
– Simulation automates this type of coupled-field solution, so
the user does not have to worry about the above details.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
34. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-34
E. Results and Postprocessing
• Various results are available for postprocessing:
– Temperature
– Heat Flux
– “Reaction” Heat Flow Rate
• In Simulation, results are usually requested before solving,
but they can be requested afterwards, too.
– If you solve a model then request results afterwards, click on
the “Solve” button , and the results will be retrieved. A
new solution is not required for retrieving output of a solved
model.
35. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-35
… Temperature
• Temperature contour plots can be requested:
– Temperature is the degree of freedom solved for,
and it is the most basic output request.
– Temperature is a scalar quantity and, therefore,
has no direction associated with it.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
36. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-36
… Heat Flux
• Heat flux contour or vector plots are available:
– Heat flux q is defined as
and is related to the thermal gradient T. The heat flux output
has three components and can aid the user in seeing how the
heat is flowing.
– The magnitude plotted as contours: “Total Heat Flux”
– The magnitude & direction as vectors: “Vector Heat Flux”
• Recall that wireframe is best for viewing vectors
– Components of heat flux
can be requested with
“Directional Heat Flux”
and can be mapped on
any coordinate system.
T
KXX
q
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
37. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-37
… Reaction Heat Flow Rate
• Reaction heat flow rates is available for any Given
Temperature or Convection boundary condition
– Recall that both given temperature and convection supply a
known temperature, either directly or indirectly. Hence, this
acts as a heat source/sink, and the amount of heat flowing in
(positive) or out (negative) of the support can be output.
– For each individual Given Temperature or
Convection load, the Reaction heat flow rate
is printed in the Details view after a solution.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
38. ANSYS
Workbench
–
Simulation
Training Manual
Steady-State Thermal Analysis
March 29, 2005
Inventory #002215
6-38
… Reaction Heat Flow Rate
• The “Worksheet” tab for “Environment” branch has a
tabular summary of reaction heat flow rates.
– If a thermal support shares a vertex, edge, or surface with
another thermal support or load, the reported reaction heat
flow rate may be incorrect. This is due to the fact that the
underlying mesh will have multiple supports applied to the
same nodes. The solution will still be valid, but the reported
values may not be accurate because of this.
ANSYS License Availability
DesignSpace Entra x
DesignSpace x
Professional x
Structural
Mechanical/Multiphysics x
