Adiabatic analysis

Adiabatic thermal-stress analysis is typically used to simulate high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation is an important effect because of temperature-dependent material properties. The temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increases caused by inelastic deformation; temperature is not a degree of freedom in the problem. No allowance is made for conduction of heat in an adiabatic analysis. For problems where both inelastic heating and conduction of the heat are important, a fully coupled temperature-displacement analysis must be performed (Fully coupled thermal-stress analysis).

In an adiabatic analysis plastic straining gives rise to a heat flux per unit volume of

where $r^{pl}$ is the heat flux that is added into the thermal energy balance, $\eta$ is the user-specified inelastic heat fraction (assumed constant; discussed below), $\mathit{\sigma }$ is the stress, and ${\dot{\mathit{\epsilon }}}^{pl}$ is the rate of plastic straining. The heat equation solved at each integration point is

where $\rho$ is the material density and $c\left(\theta \right)$ is the specific heat (see Density and Specific heat).

DYNAMIC, ADIABATIC
DYNAMIC, EXPLICIT, ADIABATIC
STATIC, ADIABATIC

Step module:
Create Step: Dynamic, Implicit: Basic: Include adiabatic heating effects
Create Step: Dynamic, Explicit: Basic: Include adiabatic heating effects
Create Step: Static, General: Basic: Include adiabatic heating effects

In Abaqus/Standard thermal diffusion analysis can be performed after the adiabatic calculation (for example, to study the cool-down of a component after sudden deformation). In this case the temperatures at the end of the adiabatic analysis must be written to the Abaqus/Standard results file as element variables averaged at the nodes. Since temperature values in an adiabatic analysis can be written to the results file as element quantities only by using the TEMP output variable identifier, they cannot be read directly into a subsequent thermal diffusion analysis as initial conditions. However, if you postprocess the results file to produce a second results file in which the temperature data are provided as nodal quantities, a subsequent heat transfer analysis can be performed with these temperatures as initial conditions. See Predefined Fields and Accessing the results file information for details. Alternatively, you could postprocess the results file to produce a data list containing data pairs consisting of nodes and temperatures.

The temperatures, NT, obtained from the heat transfer analysis can then be used to drive a continuation of the previous stress analysis. This stress analysis should be restarted from the end of the adiabatic analysis and will provide the response to the change of the temperature field obtained during the heat transfer analysis. In this case Abaqus/Standard will automatically read the temperatures from the results file that was obtained from the heat transfer analysis and apply them in the restarted analysis.