1. Chapter Six
Thermal Analysis

2. Chapter Overview
In this chapter, performing steady-state and transient thermal analyses in Simulation will be covered:
Geometry
Assemblies – Solid Body Contact
Heat Loads
Solution Options
Results and Postprocessing
Workshop 6.1
Thermal Transient Setup
Transient Settings
Transient Loads
Transient Results
Workshop 6.2
The capabilities described in this section are generally applicable to ANSYS DesignSpace Entra licenses and above, except for an ANSYS Structural license.
August 26, 2005
Inventory #002265
6-2

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: Assumptions:
No transient effects are considered in a steady-state analysis
[K] can be constant or a function of temperature
{Q} can be constant or a function of temperature
August 26, 2005
Inventory #002265
6-3

4. Basics of Steady-State Heat Transfer
Fourier’s Law provides the basis of the previous 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}
Convection is treated as a boundary condition although temperature-dependent film coefficients are possible
It is important to remember these assumptions related to performing thermal analyses in Simulation.
August 26, 2005
Inventory #002265
6-4

5. Physics Filters
If a thermal-only solution is to be performed the Physics Filter can be used to filter the GUI
Under “View menu > Physics Filter,” unselect the “Structural” and “Electromagnetic” options
This applies to options in the “Environment” and “Solution” levels only
If a thermal-stress simulation is to be performed, do not turn off the structural physics filter
August 26, 2005
Inventory #002265
6-5

6. A. Geometry
In thermal analyses, all types of bodies supported by Simulation may be used.
Solid, surface, and line bodies are supported
For surface bodies, thickness must be input in the Details view of the Geometry branch
Line bodie cross-section and orientation is defined within DesignModeler
Cross-section and orientation information results in an ‘effective’ thermal cross-section
Only temperature results are available for line bodies
The “Point Mass” feature is not available in thermal analyses
LINK33 support in DS later
August 26, 2005
Inventory #002265
6-6

7. … Geometry Shell and line body assumptions:
For shell bodies through-thickness temperature gradients are not available. Shells assume temperatures on top and bottom of surface are the same
For line bodies through thickness variation in the temperature is not available. Line bodies assume the temperature is constant across the cross-section
Temperature variation will still be considered along the line body
LINK33 support in DS later
August 26, 2005
Inventory #002265
6-7

8. … Material Properties
The only required material property is thermal conductivity
Thermal Conductivity is input in the Engineering Data application
Temperature-dependent thermal conductivity is input as a table
If any temperature-dependent material properties exist, this will result in a nonlinear solution.
August 26, 2005
Inventory #002265
6-8

9. B. Assemblies – Solid Body Contact
When importing assemblies of solid parts, contact regions are automatically created between the solid bodies enabling heat transfer between parts in an assembly
August 26, 2005
Inventory #002265
6-9
Model shown is from a sample Inventor assembly.

10. … Assemblies – Contact Region
No heat spreading is considered in the contact/target interface
Heat flow within the contact region is in the contact normal direction only
Heat flows only if a target element is present in the normal direction of a contact element
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.
August 26, 2005
Inventory #002265
6-10

11. … Assemblies – Contact Region
If the parts are initially in contact heat transfer will occur between the parts.
If the parts are initially out of contact no heat transfer takes place
Summary:
The pinball region determines when contact occurs and is automatically defined and set to a relatively small value to accommodate small gaps in the model
August 26, 2005
Inventory #002265
6-11

12. … Assemblies – Contact Region
If the contact is bonded or no separation, then heat transfer will occur (solid green lines) when the surfaces are within the pinball radius
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
August 26, 2005
Inventory #002265
6-12

13. … Assemblies – Thermal Conductance
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”
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.
August 26, 2005
Inventory #002265
6-13

14. … 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
The contact conductance can be influenced by many factors:
surface flatness
surface finish
oxides
entrapped fluids
contact pressure
surface temperature
use of conductive grease DT T x
August 26, 2005
Inventory #002265
6-14

15. … 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
If thermal contact resistance is known invert this value and divide by the contacting area to obtain TCC value
If “Thermal Conductance” is left at “Program Chosen,” near-perfect thermal contact conductance will be defined.
thermal contact conductance can be input which is the same as including thermal contact resistance at a contact interface.
August 26, 2005
Inventory #002265
6-15

16. … Assemblies – Thermal Conductance
Thermal Contact Notes:
For symmetric contact the user does not need to account for a ‘double’ thermal contact resistance
MPC bonded contact allows for perfect thermal contact conductance
August 26, 2005
Inventory #002265
6-16

17. … 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:
The user can set the search direction as either the target normal or pinball region.
If a gap exists the pinball region can be used for the search direction to detect contact beyond a gap
August 26, 2005
Inventory #002265
6-17

18. … Assemblies – Spot Weld
Spot welds provide discreet heat transfer points:
Spotweld definition is done in the CAD software (currently only DesignModeler and Unigraphics)
Spotwelds can be created in Simulation manually at vertices
LINK33 support in DS later
August 26, 2005
Inventory #002265
6-18

19. C. Heat Loads Heat Flow: Heat Flux: Internal Heat Generation:
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
Heat Flux:
A heat flux can be applied to surfaces only
Heat flux has units of energy/time/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.
August 26, 2005
Inventory #002265
6-19

20. … Adiabatic Conditions
Perfectly Insulated:
Perfectly insulated condition is applied to surfaces
This is the default condition in thermal analyses when no load is applied:
This load type is 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 an entire part, then use the perfectly insulated condition to selectively ‘remove’ the loading on some surfaces
August 26, 2005
Inventory #002265
6-20

21. … Thermal Boundary Conditions
Temperature, Convection and Radiation:
At least one type of thermal boundary condition must be present to prevent the thermal equivalent of rigid body motion
Given Temperature or Convection load should not be applied on surfaces that already have another heat load or thermal boundary condition applied to it
Perfect insulation will override thermal boundary conditions
Given Temperature:
Imposes a temperature on vertices, edges, surfaces or bodies
Temperature is the degree of freedom solved for
August 26, 2005
Inventory #002265
6-21

22. … Thermal Boundary Conditions
Convection:
Applied to surfaces only (edges in 2D analyses)
Convection q is related to a film coefficient h, the surface area A, and the difference in the surface temperature Tsurface & ambient temperature Tbulk
“h” and “Tbulk” are user-input values
The film coefficient h can be constant or temperature dependent
August 26, 2005
Inventory #002265
6-22

23. … Thermal Boundary Conditions
Temperature-Dependent Convection:
Select “New Convection…” for the Correlation
The “Engineering Data” tab will open and the Coefficient Type can then be defined for the convection load
Determine what temperature is used for h(T):
Average film temperature T=(Tsurface+Tbulk)/2
Surface temperature T= Tsurface
Bulk temperature T= Tbulk
Difference of surface and bulk temperatures T=(Tsurface-Tbulk)
Select the temperature-dependency from the pull-down menu
August 26, 2005
Inventory #002265
6-23

24. … Thermal Boundary Conditions
Temperature-Dependent Convection (continued):
The user inputs the film coefficients and temperatures in a table. The values are plotted on a graph, as shown below
Temperature-dependent convection will result in a nonlinear solution.
The only exception is if the film coefficient h is based on a function of the bulk temperature only.
Right mouse click on the table to add or delete values.
August 26, 2005
Inventory #002265
6-24

25. … Thermal Boundary Conditions
Temperature-Dependent Convection (continued):
The convection data can also be imported from a file
August 26, 2005
Inventory #002265
6-25

26. … Thermal Boundary Conditions
Radiation:
Applied to surfaces (edges in 2D analyses)
Where:
σ = Stefan-Boltzman constant
ε = Emmisivity
A = Area of radiating surface
F = Form factor (1)
Provides for radiation to ambient only (not between surfaces)
Form factor assumed to be 1
Stefan Boltzman constant is determined and set automatically based on the active working unit system
August 26, 2005
Inventory #002265
6-26

27. D. Solution Options
Solution options are set under the “Solutions” branch:
The ANSYS database can be saved
Two solvers are available in Simulation:
Default = Program Chosen
Iterative = PCG solver
Direct = sparse solver
The “Weak Springs” and “Large Deflection” options are meant for structural analyses only, so they can be ignored for a thermal analysis
August 26, 2005
Inventory #002265
6-27

28. … Solution Options
Informative settings show the user the status of the analysis:
“Analysis Type”
Nonlinear solution
Solver working directory
Any solver messages which appear after solution can be checked afterwards under “Solver Messages”
August 26, 2005
Inventory #002265
6-28

29. … Solving the Model To solve the model, request results and “Solve”
If a “Solution Information” branch is requested, the details of the solution output can be examined
August 26, 2005
Inventory #002265
6-29

30. … Solving the Model
To perform a thermal-stress solution add structural supports and/or loads and request structural results, then solve the model
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
Simulation automates this type of coupled-field solution
August 26, 2005
Inventory #002265
6-30

31. 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.
A new solution is not required for retrieving output of a solved model.
August 26, 2005
Inventory #002265
6-31

32. … Temperature Temperature:
Temperature is a scalar quantity and has no direction associated with it.
August 26, 2005
Inventory #002265
6-32

33. … Heat Flux Heat flux contour or vector plots are available:
Heat flux q is defined as
“Total Heat Flux” and “Directional Heat Flux” can be requested
The magnitude & direction can be plotted as vectors by activating vector mode
August 26, 2005
Inventory #002265
6-33

34. … Reaction Heat Flow Rate
Reaction heat flow rates is available for Given Temperature or Convection boundary conditions:
Reaction heat flow rate is printed in the Details view after a solution.
August 26, 2005
Inventory #002265
6-34

35. … Reaction Heat Flow Rate
The “Worksheet” tab for the “Environment” branch has a tabular summary of reaction heat flow rates
Note: 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. The solution will still be valid, but the reported values may not be accurate
August 26, 2005
Inventory #002265
6-35

36. F. Workshop 6.1 – Steady State Thermal Analysis
Goal:
Analyze the pump housing shown below for its heat transfer characteristics.
August 26, 2005
Inventory #002265
6-36

37. Transient Thermal Analysis
The previous discussion related to steady state analyses only. The following section introduces the ability to apply time dependent boundary conditions on thermal models
The previous sections are equally applicable in steady state or transient analyses
Three additional areas will be addressed concerning transient analysis:
Input time dependent boundary conditions
Set up transient solution options
Access results over time
August 26, 2005
Inventory #002265
6-37

38. G: Thermal Transient Setup
A thermal transient analysis is specified from the Environment branch
An “End Time” must then be entered to indicate the duration of the analysis
Supported transient loads:
Temperature
Heat flux
Heat generation rate
Heat flow
Convection film coefficient
Ambient temperature for radiation or convection
August 26, 2005
Inventory #002265
6-38

39. . . . Thermal Transient Setup
When a transient analysis is requested the GUI will update with new information sections:
Environment will contain an “Initial Condition” branch
Solution will contain a “Transient Settings” branch
A timeline and table will be inserted below the graphics screen
August 26, 2005
Inventory #002265
6-39

40. . . . Initial Conditions Initial conditions can be handled in 2 ways:
Uniform specified temperature
Non uniform temperature distribution based on a previously solved Environment
Choose the steady state result to be used as an initial condition then, RMB > “Generate Transient Environment with Initial Condition”
August 26, 2005
Inventory #002265
6-40

41. H. Transient Settings Transient settings and details:
August 26, 2005
Inventory #002265
6-41
The next several pages contain descriptions of individual areas

42. . . . Transient Settings Transient Details: Curve Type Column
Time stepping controls
Visibility of transient information
Tabular Data
Curve Type Column
DT (Delta Time) Legend
Chart Legend
August 26, 2005
Inventory #002265
6-42

43. . . . Transient Settings Automatic Step Resets:
Automatic time step reset places resets at extreme inflection points in the load history
The slider controls the reset frequency
Manual resets can be added by RMB in the transient settings graph and at the desired time point
Manual reset points can be moved by dragging with the cursor
Move reset point
August 26, 2005
Inventory #002265
6-43

44. . . . Transient Settings
Time reset points are indicated by the triangular markers at the top of the chart
Automatic resets: solid
Manual resets: wire frame
August 26, 2005
Inventory #002265
6-44

45. . . . Transient Settings
The “visible” column in the time line legend controls specific information to be plotted
Notice here the heat flux is applied as a step function with solution resets at each inflection point
Heat flux history
Time step reset points
August 26, 2005
Inventory #002265
6-45

46. I. Transient Loads
Transient loads are applied using the same techniques discussed earlier. The only difference will be the setup in the details for the load
Instead of choosing “Constant” (default), choose “Load History”
The history data can be imported from a previously saved file or created using the Engineering Data application
August 26, 2005
Inventory #002265
6-46

47. . . . Transient Loads
After choosing “New Load History”, time and load data is entered in the Engineering Data application
The plot builds as the data is entered
Project load histories are managed the same way as materials and convections
August 26, 2005
Inventory #002265
6-47

48. Check boxes control timeline display
J. Transient Results
Transient results are plotted like steady state, by highlighting the branch, however additional information and controls are available
The details view and graphics legend include the “display time”
Timeline and tabular data are available for each result time solved for
Check boxes control timeline display
August 26, 2005
Inventory #002265
6-48

49. New time point selected
. . . Transient Results
To view results from different time points:
Click on the time point of interest in the timeline
The details will indicate a red background until the results are retrieved for the selected time point
To complete the operation, in the timeline “RMB > Retrieve Results”
Results not updated
New time point selected
August 26, 2005
Inventory #002265
6-49

50. . . . Transient Results
Transient animations are controlled using the same controller as steady state animations
To animate a specific range use the mouse to drag over the desired times
The resulting animation will span the highlighted region
August 26, 2005
Inventory #002265
6-50

51. K. Workshop 6.2 – Transient Thermal Analysis
Goal:
Analyze the heating base on a steam iron like the ones shown here for steady state and cyclic loading conditions
August 26, 2005
Inventory #002265
6-51