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

r^{p l} = η σ : {\dot{ε}}^{p l},

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

ρ c (θ) \dot{θ} = r^{p l},

where $ρ$ is the material density and $c (θ)$ is the specific heat (see Density and Specific Heat).

Subsequent Thermal Diffusion Analysis in Abaqus/Standard

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.

Example

The following input options could be used to perform a heat transfer analysis using the temperatures from an adiabatic analysis and then continue the stress analysis:

**Static adiabatic analysis
 …
STEP
STATIC, ADIABATIC
 …
**Write the temperatures to the results file as element 
**variables averaged at the nodes
EL FILE, POSITION=AVERAGED AT NODES
 TEMP
END STEP
**Heat transfer analysis using the temperatures from the 
**static analysis as initial conditions
 …
INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=new results file,
 STEP=step, INC=increment
STEP
HEAT TRANSFER
 …
NODE FILE
 NT
END STEP
**Restart from the adiabatic analysis using temperatures 
**obtained from the heat transfer analysis
RESTART, WRITE, READ, STEP=k, INC=i, END STEP
 …
STEP
STATIC 
 … 
TEMPERATURE, FILE=heat_transfer_results_file
 … 
END STEP

Fully Coupled Temperature-Displacement Analysis

If the continuation of the analysis into thermal diffusion requires a fully coupled temperature-displacement analysis (see Fully Coupled Thermal-Stress Analysis), the simplest (but more expensive) approach is to use coupled temperature-displacement elements throughout the adiabatic analysis. At the end of the static or the dynamic adiabatic calculations, the temperatures must be written to the results file as element variables averaged at the nodes. In addition, you must constrain all temperature degrees of freedom since they are not used in the adiabatic analysis. The adiabatic analysis can then be restarted to apply the correct temperature distribution obtained from the adiabatic analysis to the temperature degree of freedom of each node in the model. To create the input for the boundary conditions, you must postprocess the results file obtained from the adiabatic analysis and extract the value of TEMP at each node in the model (see Accessing the Results File Information). The temperature boundary conditions can be released as needed in subsequent coupled temperature-displacement analysis steps.

Example

The following input options could be used to perform a coupled temperature-displacement analysis using the temperatures from an adiabatic analysis:

**Static adiabatic analysis, coupled temperature-displacement
**plane stress elements
 …
ELEMENT, TYPE=CPS4T, ELSET=EALL
 …
BOUNDARY
nodes, 11, 11, 0.0
STEP
STATIC, ADIABATIC
 …
**Write the temperatures to the results file as element 
**variables averaged at the nodes
EL FILE, POSITION=AVERAGED AT NODES
 TEMP
END STEP
**Restart from the adiabatic analysis
RESTART, WRITE, READ, STEP=k, INC=i, END STEP
 …
STEP
STATIC
**Dummy step to associate the temperature variable TEMP with 
**the temperature degree of freedom at each node
 1.0, 1.0
 …
BOUNDARY, OP=NEW
 node, 11, 11, temperature
 …
END STEP
**Coupled temperature displacement run for cool down of 
**structure: continuation of the restart analysis
 …
STEP
COUPLED TEMPERATURE-DISPLACEMENT
 0.1, 1.0
 …
BOUNDARY, OP=NEW
**no temperature boundary condition specified
END STEP

Initial Conditions

Initial temperatures can be prescribed at nodes as initial conditions. Initial values of stresses, field variables, solution-dependent state variables, etc. can also be specified (see Initial Conditions).

Boundary Conditions

Boundary conditions can be applied to displacement degrees of freedom in an adiabatic analysis in the same way that they are applied in nonadiabatic dynamic, explicit dynamic, or static analysis steps (see Boundary Conditions). Temperature is not a degree of freedom in an adiabatic analysis.

Loads

The loading options available for an adiabatic analysis are the same as those available for nonadiabatic dynamic, explicit dynamic, or static analysis steps (see About Loads).

The following types of mechanical loads can be prescribed:

Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see Concentrated Loads.
Distributed pressure forces or body forces can be applied; see Distributed Loads. The distributed load types available with particular elements are described in Abaqus Elements Guide.

Predefined Fields

Predefined temperature fields cannot be used during an adiabatic analysis step.

The values of user-defined field variables can be specified; these values affect only field-variable-dependent material properties, if any. See Predefined Fields.

Material Options

In Abaqus/Standard only Mises plasticity with isotropic elasticity and isotropic hardening (Inelastic Behavior) is allowed in adiabatic stress analysis. Kinematic or combined hardening is not available, but rate effects can be included. However, portions of the model can include only elastic material; no change in temperature occurs in the elastic regions, since there is no source of heat generation. In Abaqus/Explicit both Mises and Hill plasticity are allowed in adiabatic stress analysis.

You must specify the density, the inelastic heat fraction, and the specific heat as part of the material definition for the material in which heat will be generated by plastic dissipation. You can also specify latent heat if necessary (Latent Heat).

The inelastic heat fraction is the amount of inelastic dissipation used to calculate the increase in temperature. The default value of the inelastic heat fraction is 0.9. If the inelastic heat fraction is not included in the material definition, the heat generated by inelastic deformation is not included in the analysis.

In Abaqus/Standard adiabatic analyses can also be carried out with user subroutine UMAT. In this case the temperature must be defined as a solution-dependent state variable, and all coupling terms must be included in the user subroutine. If conductivity (Conductivity) is defined for the material, it will be ignored during adiabatic analysis steps.

Temperature-Dependent Material Properties

Material properties can be temperature dependent. Since the only source of temperature change in adiabatic analysis is inelastic deformation, the temperature can only rise. This temperature rise may cause thermal expansion (usually a small effect) and localization of the deformation if the flow stress is reduced by the temperature rise. Since the adiabatic assumption applies only in rapid events and inelastic deformation usually causes significant temperature rises only if the deformation is substantial, the strain rates are often large in adiabatic analysis. The softening of the material caused by the temperature rise may, thus, be offset somewhat by strengthening associated with rate dependence if the material is rate sensitive.

Elements

Any of the stress/displacement or coupled temperature-displacement elements in Abaqus can be used in an adiabatic analysis (see Choosing the Appropriate Element for an Analysis Type). Mass or spring elements will not contribute to the heating of the material since they cannot generate plastic strains.

If coupled temperature-displacement elements are used in an adiabatic analysis, the temperature degrees of freedom will be ignored.

Output

Since temperatures are updated at the material calculation points, output of temperature is available with output variable TEMP, not with output variable NT.

The element output available for an adiabatic analysis includes stress; strain; energies; the values of state, field, and user-defined variables; and composite failure measures. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in Abaqus/Standard Output Variable Identifiers and Abaqus/Explicit Output Variable Identifiers.

Input File Template

HEADING
…
MATERIAL, NAME=name
ELASTIC, TYPE=ISOTROPIC
Data lines to define isotropic linear elasticity
PLASTIC
Data lines to define metal plasticity
DENSITY
Data lines to define density
INELASTIC HEAT FRACTION
Data line to define inelastic heat fraction
SPECIFIC HEAT
Data lines to define specific heat
… 
BOUNDARY
Data lines to specify zero-valued boundary conditions
INITIAL CONDITIONS, TYPE=type
Data lines to specify initial conditions
AMPLITUDE, NAME=name
Data lines to define amplitude variations
**


STEP, NLGEOM
The NLGEOM parameter is used in Abaqus/Standard to include geometric nonlinearity
DYNAMIC, ADIABATIC or DYNAMIC, EXPLICIT, ADIABATIC or 
STATIC, ADIABATIC
Data line to control time incrementation or to specify the time period of the step
BOUNDARY, AMPLITUDE=name
Data lines to describe nonzero or zero-valued boundary conditions
CLOAD and/or DLOAD and/or DSLOAD
Data lines to specify loads
FIELD
Data lines to specify field variable values
END STEP