1. Thermo-mechanics
J. Cugnoni, LMAF / EPFL 2012

2. Three kind of « thermo-mechanics »
Un-coupled: Known temperature field => mechanical model (linear statics + th. expansion)
One way coupling: solve thermal problem => temperature field => solve mechanical problem
Fully coupled: solve at the same time temperature & displacement field (includes mechanical dissipation)

3. Thermal problem Variables Material Boundary conditions:
Essential variable: Temperature field T
Natural variable: heat flux q
Material
Conductivity l
Density r & specific heat cp if transient
Boundary conditions:
Temperature: Tsurf = f(t) if transient
Surface heat fluxes:
Imposed heat flux qsurf=f(t)
Convection: qsurf = h (T –Text(t))
Volume heat source: s = f(t) q
T, l, r, cp, s
Text

4. Thermal problem in Abaqus
Select Step = Heat transfer
Choose steady state or transient
If transient: set time period, set small initial increment, set max DT per increment (<1/10 of max DT)
In Mesh:
select element type: Heat transfer, linear
Loading:
Need to impose at least one temp. (rigid body)
Adiabatic interface: leave free = no flux!
Flux = load, Temperature = BC
Convection: in interaction module, create Surface Film condition, enter h and Text
If transient: define an amplitude curve (tool => amplitude), need to start at zero for t=0, smooth step is a good choice

5. Un-coupled thermo-mechanics model (thermal stress calculation for a know temperature field)
Select Step = Static General
Keep standard options
In Mesh:
select element type: Stress , Quadratic (standard option)
Loading:
Need to impose a temperature field. Either manually (constant by region) or by importing thermal analysis results. This is done in Load module by creating a predefined field of “Temperature”.
If temperature is imposed manually, pick the regions and assign a temperature and amplitude curve.
If temperature is imported from thermal analysis: pick a region, choose a file and define the time range of the temperature results to import.

6. Coupled Thermo mechanics in Abaqus
Select Step = Coupled Temp-Displacement
Choose steady state or transient
If transient: set time period, set small initial increment, set max DT per increment (<1/10 of max DT)
In Mesh:
select element type: Coupled Temp.-Displacement, quadratic
Loading:
Need to impose at least one temp. & block 6 rigid body motions
Adiabatic interface: leave free = no flux!
Flux = load, Temperature = BC
Convection: in interaction module, create Surface Film condition, enter h and Text
If transient: define an amplitude curve (tool => amplitude), need to start at zero for t=0

7. Démos Bi-material beam: Thermal switch
Coupled Thermo-mechanical problem
Transient analysis
Heat transfer & expansion properties
Heat transfer BC:
Temperature
Convection
Heat Flux
Time dependent boundary conditions

8. Demo: thermal switch Beam dimensions 60 x 5 x 1 mm Invar, 0.5 mm
Block: clamped, T= 0°C
Convection: q=h (T-Text), h = 100 W/m2/K
Water
Prop.
Steel
Invar
Young’s modulus
210 GPa
141 GPa
Poisson ratio
0.3
Th. Expansion
1e-5
1e-6
Density
7800 kg/m3
8000 kg/m3
Conductivity
30 W/m/K
10 W/m/K
Specific heat
1000 J/kg/K
500 J/kg/K
Steel, 0.5 mm
T water = f(time)
T=100°C
T=0°C 1
Time (s) 60