Reference:  ANSYS Thermal Analysis Guide

Chapter 2: Steady-State Thermal Analysis

Reference:  ANSYS Coupled-Field Analysis Guide

Chapter 2: Sequentially Coupled Physics Analysis

We use steady state thermal analysis when the heat flow does not vary with time (not for start-up or shut-down conditions).

Objectives:

• Determine operating temperature distribution
• Determine heat flow rates (to size heating/cooling systems)

Thermal Analysis variables: temperature DOF, heat

Linear vs. Nonlinear Heat Transfer

Nonlinear FEA model behaviors:

• material properties vary significantly with temperature
• loads that vary with temperature
• convection film coefficients (H) that vary significantly with temperature
• radiation heat transfer (absolute T⁴)
• special elements: thermostat, coupled-field or multi-field

ELEMENTS

1D (thermal network):

• LINK33 for conduction
• LINK34 for convection
• LINK31 for radiation
• MASS71 lumped thermal mass
• COMBIN37 control element (thermostat)

2D:

• PLANE55 lower-order, quad. or triangle, planar or axisymmetric
• PLANE77 higher-order, quad. or triangle, planar or axisymmetric

3D solid:

• SOLID70 lower-order, brick - tetrahedral
• SOLID90 higher-order, brick - pyramid - tetrahedral
• SOLID87, higher-order, tetrahedral

3D shell:

• SHELL57 lower-order, in-plane conduction shell
• SHELL131 lower-order, in-plane & through thickness conduction shell (may have layers)
• SHELL132 higher-order, in-plane & through thickness conduction shell (may have layers)

MATERIAL PROPERTIES

• KXX is the thermal conductivity
• DENS is the density (necessary for transient heat transfer)
• C is the specific heat (necessary for transient heat transfer)
• HF may be used for temperature dependent film coefficients

LOADING

• Temperature: specified (DOF) temperature at points, if known
• Heat Flow: specified heat flow at points, if knows
• Convection: edge or face b.c. representing fluid (not modeled)
• Heat Flux: specified edge or face distribution of heat
• Heat Generation:  specified internal heating (volumetric)

POSTPROCESSING

• Contour plots of temperature
• Total Heat Flow: Reaction Solution, Element Table
• Vectors of Heat Flux (TF) to visualize flow of energy
• Evaluate Mesh Error (TEPC)

THERMAL STRESS ANALYSIS

Reference: Building Better Products with Finite Element Analysis, Vince Adams and Abraham Askenazi, Onword Press, 1st edition, 1999.  ISBN 1-56690-160X, Chapter 14, pp. 411-23.

Thermal-stress analysis variables: displacement DOF, stress, strain, force

Expansion/Shrinkage occurs according to: e_TH = a_TH (T - T_REF)

• e_TH = thermal strain
• a_TH = coefficient of thermal expansion (material property)
• T_REF = reference (strain-free) temperature

Stress is produced in cases of restrained thermal expansion, e.g., from constraint which may be from the boundary conditions, but also can come from different materials in an assembly.

Examples:

• Weld stress/distortion
• Molded/Cast part shrinkage
• Press-fit analysis
• create desired interference by imposing an artificial thermal environment condition
• Preload in spring or bolt

SIMPLE CASE: 

Sequential FEA solutions, thermal then structural (indirectly coupled), to determine stress/strain, deflection, and forces caused by differential expansion/shrinkage

"indirectly coupled" = thermal conditions effect the structural analysis, but the structural response does NOT effect the heat transfer behavior.

Procedure:

• after solving the thermal model,
• resume the thermal database
• change the 'jobname'
• delete all thermal analysis loads
• Switch element types: thermal to structural (ETCHG,TTS)
• add structural material properties (EX, NUXY, and ALPX)
• define the reference temperature for thermal strain calculations (TREF)
• define proper structural constraints on the model
• define any other structural loads that act on the model
• read the temperature results from the thermal analysis results file (RTH) and apply them as loads to the structural analysis (LDREAD, assumes the same mesh for both runs)
• verify the temperature distribution on the structural model (/PBF,TEMP,,1 then EPLOT)
• solve and postprocess

More Complicated Case (not covered in FEA-2):

When the mesh is NOT the same for the thermal and structural models, additional postprocessing steps allow interpolation of temperature data from the thermal model solution to the structural model loading.

Why ?  Often a finer mesh, with small features restored (i.e., fillets in sharp corners) is needed for the structural analysis.

Most Complicated Case (not covered in FEA-2):

Coupled-field/Multifield elements (directly coupled solutions) are needed when the deformations cause changes in the heat transfer behavior (e.g., contact between parts)

In this case, a single analysis with multiple "field" substep loops solves for each case of "physics" for the model.