Thermo-mechanics J. Cugnoni, LMAF / EPFL 2012

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)

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

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

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.

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

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

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