The equation for conservation of energy equates the increase in internal energy per unit mass, , to the rate at which work is being done by the stresses and the rate at which heat is being added. In the absence of heat conduction the energy equation can be written as

The equation of state is assumed for the pressure as a function of the current density, , and the internal energy per unit mass, :

An equation of state is said to be linear in energy when it can be written in the form

A Mie-Grüneisen equation of state is linear in energy. The most common form is

The Hugoniot energy, , is related to the Hugoniot pressure by

The equation of state and the energy equation represent coupled equations for pressure and internal energy. Abaqus/Explicit solves these equations simultaneously at each material point.

Linear U_s – U_p Hugoniot form

A common fit to the Hugoniot data is given by

where and s define the linear relationship between the shock velocity, , and the particle velocity, , as follows:

With the above assumptions the linear Hugoniot form is written as

where is equivalent to the elastic bulk modulus at small nominal strains.

There is a limiting compression given by the denominator of this form of the equation of state

or

At this limit there is a tensile minimum; thereafter, negative sound speeds are calculated for the material.

Input File Usage:	Use both of the following options:
	*DENSITY (to specify the reference density ) *EOS, TYPE=USUP (to specify the variables , s, and )

Abaqus/CAE Usage:

Property module: material editor: GeneralDensity (to specify the reference density ) MechanicalEos: Type: Us - Up (to specify the variables , s, and )

Initial state

The initial state of the material is determined by the initial values of specific energy, , and pressure stress, p. Abaqus/Explicit will automatically compute the initial density, , that satisfies the equation of state, . You can define the initial specific energy and initial stress state (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). The initial pressure used by the equation of state is inferred from the specified stress states. If no initial conditions are specified, Abaqus/Explicit will assume that the material is at its reference state:

Input File Usage:	Use either or both of the following options, as required:
	*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY *INITIAL CONDITIONS, TYPE=STRESS

Abaqus/CAE Usage:	Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step
	Initial specific energy is not supported in Abaqus/CAE.

The tabulated equation of state provides flexibility in modeling the hydrodynamic response of materials that exhibit sharp transitions in the pressure-density relationship, such as those induced by phase transformations. The tabulated equation of state is linear in energy and assumes the form

You can specify the functions and directly in tabular form. The tabular entries must be given in descending values of the volumetric strain (that is, from the most tensile to the most compressive states). Abaqus/Explicit will use a piecewise linear relationship between data points. Outside the range of specified values of volumetric strains, the functions are extrapolated based on the last slope computed from the data.

*DENSITY (to specify the reference density )
*EOS, TYPE=TABULAR (to specify  and  as functions of )

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY
*INITIAL CONDITIONS, TYPE=STRESS

The user-defined equation of state provides a general capability for modeling the volumetric response of materials through user subroutine VUEOS (see “VUEOS,” Section 1.2.15 of the Abaqus User Subroutines Reference Guide). The equation of state defines the pressure as a function of the current density, , and the internal energy per unit mass, : . Abaqus/Explicit solves the energy equation together with the equation of state using an iterative method. The pressure stress, , and the derivatives of the pressure with respect to the internal energy and to the density, and , must be provided by user subroutine VUEOS. The latter is needed for the evaluation of the effective bulk modulus of the material, which is necessary for the stable time increment calculation.

Optionally, you can also specify the number of property values needed as data in the user subroutine as well as the number of solution-dependent variables (see “User subroutines: overview,” Section 18.1.1).

*EOS, TYPE=USER, PROPERTIES=n

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY
*INITIAL CONDITIONS, TYPE=STRESS

*DENSITY

The equation of state is designed for modeling the compaction of ductile porous materials. The implementation in Abaqus/Explicit is based on the model proposed by Hermann (1968) and Carroll and Holt (1972). The constitutive model provides a detailed description of the irreversible compaction behavior at low stresses and predicts the correct thermodynamic behavior at high pressures for the fully compacted solid material. In Abaqus/Explicit the solid phase is assumed to be governed by either the Mie-Grüneisen equation of state or the tabulated equation of state. The relevant properties of the porous material in the virgin state, to be discussed later, and the material properties of the solid phase are specified separately.

The porosity of the material, n, is defined as the ratio of pore volume, , to total volume, , where is the solid volume. The porosity remains in the range , with 0 indicating full compaction. It is convenient to introduce a scalar variable , sometimes referred to as “distension,” defined as the ratio of the density of the solid material, , to the density of the porous material, , both evaluated at the same temperature and pressure:

An equation of state is assumed for the pressure of the porous material as a function of ; current density, ; and internal energy per unit mass, , in the form

The equation of state must be supplemented by an equation that describes the behavior of as a function of the thermodynamic state. This equation takes the form

The function captures the general behavior to be expected in a ductile porous material. The unloaded virgin state corresponds to the value , where is the reference porosity of the material. Initial compression of the porous material is assumed to be elastic. Recall that decreasing porosity corresponds to a reduction in . As the pressure increases beyond the elastic limit, , the pores in the material start to crush, leading to irreversible compaction and permanent (plastic) volume change. Unloading from a partially compacted state follows a new elastic curve that depends on the maximum compaction (or, alternatively, the minimum value of ) ever attained during the deformation history of the material. The absolute value of the slope of the elastic curve decreases as decreases, as will be quantified later. The material becomes fully compacted when the pressure reaches the compaction pressure ; at that point , a value that is retained forever. The function therefore has multiple branches: a plastic branch, , and multiple elastic branches, , corresponding to elastic unloading from partially compacted states. The appropriate branch of A is selected according to the following rule:

If the solid phase is modeled using the Mie-Grüneisen equation of state, is given directly by the reference sound speed, . On the other hand, if the solid phase is modeled using the tabulated equation of state, is computed from the initial bulk modulus and reference density of the solid material, . In this case the reference density is required to be constant; it cannot be a function of temperature or field variables.

Following Wardlaw et al. (1996), the above equation for the elastic curve in Abaqus/Explicit is simplified and replaced by the linear relations

Input File Usage:

Use the following option to specify the reference density of the solid phase, :

*DENSITY Use one of the following options to specify additional material properties for the solid phase: *EOS, TYPE=USUP (if the solid phase is modeled using the Mie-Grüneisen equation of state) *EOS, TYPE=TABULAR (if the solid phase is modeled using the tabulated equation of state) Use the following option to specify the properties of the porous material (the reference sound speed, ; the reference porosity, ; the elastic limit, ; and the compaction pressure, ): *EOS COMPACTION

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY
*INITIAL CONDITIONS, TYPE=STRESS
*INITIAL CONDITIONS, TYPE=POROSITY

The Jones-Wilkins-Lee (or JWL) equation of state models the pressure generated by the release of chemical energy in an explosive. This model is implemented in a form referred to as a programmed burn, which means that the reaction and initiation of the explosive is not determined by shock in the material. Instead, the initiation time is determined by a geometric construction using the detonation wave speed and the distance of the material point from the detonation points.

The JWL equation of state can be written in terms of the internal energy per unit mass, , as

*DENSITY (to specify the density of the explosive )
*EOS, TYPE=JWL (to specify the material constants  and )

Arrival time of detonation wave

Abaqus/Explicit calculates the arrival time of the detonation wave at a material point as the distance from the material point to the nearest detonation point divided by the detonation wave speed:

where is the position of the material point, is the position of the Nth detonation point, is the detonation delay time of the Nth detonation point, and is the detonation wave speed of the explosive material. The minimum in the above formula is over the N detonation points that apply to the material point.

Burn fraction

To spread the burn wave over several elements, a burn fraction, , is computed as

where is a constant that controls the width of the burn wave (set to a value of 2.5) and is the characteristic length of the element. If the time is less than , the pressure is zero in the explosive; otherwise, the pressure is given by the product of and the pressure determined from the JWL equation above.

*EOS, TYPE=JWL
*DETONATION POINT

*INITIAL CONDITIONS, TYPE=STRESS

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY

The ignition and growth equation of state models shock initiation and detonation wave propagation of solid high explosives. The heterogeneous explosive is modeled as a homogeneous mixture of two phases: the unreacted solid explosive and the reacted gas products. Separate JWL equations of state are prescribed for each phase:

*DENSITY(to specify the density of the explosive )
*EOS, TYPE=IGNITION AND GROWTH, DETONATION ENERGY=
(to specify the material constants   and 
 of the unreacted solid explosive and the reacted gas product)

The mass fraction

The mixture of unreacted solid explosive and reacted gas products is defined by the mass fraction

where is the mass of the unreacted explosive, and is the mass of the reacted products. It is assumed that the two phases are in thermomechanical equilibrium:

It is also assumed that the volumes are additive:

Similarly, the internal energy is assumed to be additive:

where

Hence, the specific heat of the mixture is given by

Input File Usage:	Use the following options to define the specific heat of the unreacted solid explosive:
	*EOS, TYPE=IGNITION AND GROWTH *SPECIFIC HEAT, DEPENDENCIES=n Use the following options to define the specific heat of the reacted gas product: *EOS, TYPE=IGNITION AND GROWTH *GAS SPECIFIC HEAT, DEPENDENCIES=n

Abaqus/CAE Usage:

Use the following options to define the specific heat of the unreacted solid explosive:

Property module: material editor: MechanicalEos: Type: Ignition and GrowthThermalSpecific Heat Use the following options to define the specific heat of the reacted gas product: Property module: material editor: MechanicalEos: Type: Ignition and growth: Gas Specific tabbed page: Specific Heat You can toggle on Use temperature-dependent data to define the specific heat as a function of temperature and/or select the Number of field variables to define the specific heat as a function of field variables.

The reaction rate

The conversion of unreacted solid explosive to reacted gas products is governed by the reaction rate. The reaction rate equation in the ignition and growth model is a pressure-driven rule, which includes three terms:

These three terms are defined as follows:

where , and z are reaction rate constants.

The first term, , describes hot spot ignition by igniting some of the material relatively quickly but limiting it to a small proportion of the total solid . The second term, , represents the growth of reaction from the hot spot sites into the material and describes the inward and outward grain burning phenomena; this term is limited to a proportion of the total solid . The third term, , is used to describe the rapid transition to detonation observed in some energetic materials.

Input File Usage:	Use both of the following options to define the reaction rate:
	*EOS, TYPE=IGNITION AND GROWTH *REACTION RATE

Abaqus/CAE Usage:

Property module: material editor: MechanicalEos: Type: Ignition and growth: Reaction Rate tabbed page

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY

An ideal gas equation of state can be written in the form of

One of the important features of an ideal gas is that its specific energy depends only upon its temperature; therefore, the specific energy can be integrated numerically as

Modeling with an ideal gas equation of state is typically performed adiabatically; the temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increase caused by the work , where v is the specific volume (the volume per unit mass, ). Therefore, unless a fully coupled temperature-displacement analysis is performed, an adiabatic condition is always assumed in Abaqus/Explicit.

When performing a fully coupled temperature-displacement analysis, the pressure stress and specific energy are updated based on the evolving temperature field. The energy increase due to the change in state will be accounted for in the heat equation and will be subject to heat conduction.

For the ideal gas model in Abaqus/Explicit you define the gas constant, R, and the ambient pressure, . For an ideal gas R can be determined from the universal gas constant, , and the molecular weight, , as follows:

*EOS, TYPE=IDEAL GAS
*SPECIFIC HEAT, DEPENDENCIES=n

Initial state

There are different methods to define the initial state of the gas. You can specify the initial density, , and either the initial pressure stress, , or the initial temperature, . The initial value of the unspecified field (temperature or pressure) is determined from the equation of state. Alternatively, you can specify both the initial pressure stress and the initial temperature. In this case the user-specified initial density is replaced by that derived from the equation of state in terms of initial pressure and temperature.

By default, Abaqus/Explicit automatically computes the initial specific energy, , from the initial temperature by numerically integrating the equation

Optionally, you can override this default behavior by defining the initial specific energy for the ideal gas directly.

Input File Usage:	Use some or all of the following options, as required:
	*DENSITY, DEPENDENCIES=n *INITIAL CONDITIONS, TYPE=STRESS *INITIAL CONDITIONS, TYPE=TEMPERATURE Use the following option to specify the initial specific energy directly: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY

Abaqus/CAE Usage:	Property module: material editor: GeneralDensity
	Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE.

*PHYSICAL CONSTANTS, ABSOLUTE ZERO=

A special case

In the case of an adiabatic analysis with constant specific heat (both and are constant), the specific energy is linear in temperature

The pressure stress can, therefore, be recast in the common form of

where is the ratio of specific heats and can be defined as

where

for a monatomic;

for a diatomic; and

for a polyatomic gas.

The equation of state defines only the material's hydrostatic behavior. It can be used by itself, in which case the material has only volumetric strength (the material is assumed to have no shear strength). Alternatively, Abaqus/Explicit allows you to define deviatoric behavior, assuming that the deviatoric and volumetric responses are uncoupled. Two models are available for the deviatoric response: a linear isotropic elastic model and a viscous model. The material's volumetric response is governed then by the equation of state model, while its deviatoric response is governed by either the linear isotropic elastic model or the viscous fluid model.

Elastic shear behavior

For the elastic shear behavior the deviatoric stress is related to the deviatoric strain as

where is the deviatoric stress and is the deviatoric elastic strain. See “Defining isotropic shear elasticity for equations of state in Abaqus/Explicit” in “Linear elastic behavior,” Section 22.2.1, for more details.

Input File Usage:	Use both of the following options to define elastic shear behavior:
	*EOS *ELASTIC, TYPE=SHEAR

Abaqus/CAE Usage:

Property module: material editor: MechanicalElasticityElastic; Type: Shear; Shear Modulus

Viscous shear behavior

For the viscous shear behavior the deviatoric stress is related to the deviatoric strain rate as

where is the deviatoric stress, is the deviatoric part of the strain rate, is the viscosity, and is the engineering shear strain rate.

Abaqus/Explicit provides a wide range of viscosity models to describe both Newtonian and non-Newtonian fluids. These are described in “Viscosity,” Section 26.1.4.

Input File Usage:	Use both of the following options to define viscous shear behavior:
	*EOS *VISCOSITY

Abaqus/CAE Usage:

Property module: material editor: MechanicalViscosity

An equation of state model can be used with the Mises (“Classical metal plasticity,” Section 23.2.1) or the Johnson-Cook (“Johnson-Cook plasticity,” Section 23.2.7) plasticity models to model elastic-plastic behavior. In this case you must define the elastic part of the shear behavior. The material's volumetric response is governed by the equation of state model, while the deviatoric response is governed by the linear elastic shear and the plasticity model.

*EOS
*ELASTIC, TYPE=SHEAR
*PLASTIC

*INITIAL CONDITIONS, TYPE=HARDENING

An equation of state model can be used in conjunction with the extended Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) plasticity models to model pressure-dependent plasticity behavior. This approach can be appropriate for modeling the response of ceramics and other brittle materials under high velocity impact conditions. In this case you must define the elastic part of the shear behavior. The material's deviatoric response is governed by the linear elastic shear and the pressure-dependent plasticity model, while the volumetric response is governed by the equation of state model. In particular, no plastic dilation effects are taken into account (if you specify a dilation angle other than zero, the value is ignored and Abaqus/Explicit issues a warning message).

“High-velocity impact of a ceramic target,” Section 2.1.18 of the Abaqus Example Problems Guide illustrates the use of an equation of state model with the extended Drucker-Prager plasticity models.

*EOS
*ELASTIC, TYPE=SHEAR
*DRUCKER PRAGER
*DRUCKER PRAGER HARDENING

*INITIAL CONDITIONS, TYPE=HARDENING

An equation of state model (except the ideal gas equation of state) can also be used with the tensile failure model (“Dynamic failure models,” Section 23.2.8) to model dynamic spall or a pressure cutoff. The tensile failure model uses the hydrostatic pressure stress as a failure measure and offers a number of failure choices. You must provide the hydrostatic cutoff stress.

You can specify that the deviatoric stresses should fail when the tensile failure criterion is met. In the case where the material's deviatoric behavior is not defined, this specification is meaningless and is, therefore, ignored.

The tensile failure model in Abaqus/Explicit is designed for high-strain-rate dynamic problems in which inertia effects are important. Therefore, it should be used only for such situations. Improper use of the tensile failure model may result in an incorrect simulation.

*EOS
*TENSILE FAILURE

An adiabatic condition is always assumed for materials modeled with an equation of state unless a dynamic coupled temperature-displacement procedure is used. The adiabatic condition is assumed irrespective of whether an adiabatic dynamic stress analysis step has been specified. The temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increase caused by the mechanical work

When performing a fully coupled temperature-displacement analysis, the specific energy is updated based on the evolving temperature field using

A linear equation of state model can be used to model incompressible viscous and inviscid laminar flow governed by the Navier-Stokes equation of motion. The volumetric response is governed by the equations of state, where the bulk modulus acts as a penalty parameter for the incompressible constraint.

To model a viscous laminar flow that follows the Navier-Poisson law of a Newtonian fluid, use the Newtonian viscous deviatoric model and define the viscosity as the real linear viscosity of the fluid. To model non-Newtonian viscous flow, use one of the nonlinear viscosity models available in Abaqus/Explicit. Appropriate initial conditions for velocity and stress are essential to get an accurate solution for this class of problems.

To model an incompressible inviscid fluid such as water in Abaqus/Explicit, it is useful to define a small amount of shear resistance to suppress shear modes that can otherwise tangle the mesh. Here the shear stiffness or shear viscosity acts as a penalty parameter. The shear modulus or viscosity should be small because flow is inviscid; a high shear modulus or viscosity will result in an overly stiff response. To avoid an overly stiff response, the internal forces arising due to the deviatoric response of the material should be kept several orders of magnitude below the forces arising due to the volumetric response. This can be done by choosing an elastic shear modulus that is several orders of magnitude lower than the bulk modulus. If the viscous model is used, the shear viscosity specified should be on the order of the shear modulus, calculated as above, scaled by the stable time increment. The expected stable time increment can be obtained from a data check analysis of the model. This method is a convenient way to approximate a shear resistance that will not introduce excessive viscosity in the material.

If a shear model is defined, the hourglass control forces are calculated based on the shear resistance of the material. Thus, in materials with extremely low or zero shear strengths such as inviscid fluids, the hourglass forces calculated based on the default parameters are insufficient to prevent spurious hourglass modes. Therefore, a sufficiently high hourglass scaling factor is recommended to increase the resistance to such modes.