22.2.1 Equation of state

Products: Abaqus/Explicit Abaqus/CAE

References

Overview

Equations of state:

provide a hydrodynamic material model in which the material's volumetric strength is determined by an equation of state;
determine the pressure (positive in compression) as a function of the density, , and the specific energy (the internal energy per unit mass), : ;
are available as Mie-Grüneisen equations of state (thus providing the linear Hugoniot form);
are available as tabulated equations of state linear in energy;
are available as equations of state for the compaction of ductile porous materials and must be used in conjunction with either the Mie-Grüneisen or the tabulated equation of state for the solid phase;
are available as JWL high explosive equations of state;
are available in the form of an ideal gas;
assume an adiabatic condition unless a dynamic fully coupled temperature-displacement analysis is used;
can be used to model a material that has only volumetric strength (the material is assumed to have no shear strength) or a material that also has isotropic elastic or viscous deviatoric behavior;
can be used with the Mises (“Classical metal plasticity,” Section 20.2.1) or the Johnson-Cook (“Johnson-Cook plasticity,” Section 20.2.7) plasticity models; and
can be used with the tensile failure model (“Dynamic failure models,” Section 20.2.8) to model dynamic spall or a pressure cutoff.

Energy equation and Hugoniot curve

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

where p is the pressure stress defined as positive in compression,

is the pressure stress due to the bulk viscosity,

is the deviatoric stress tensor,

is the deviatoric part of strain rate, and

is the heat rate per unit mass.

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

which defines all the equilibrium states that can exist in a material. The internal energy can be eliminated from the above equation to obtain a p versus V relationship (where V is the current volume) or, equivalently, a p versus

relationship that is unique to the material described by the equation of state model. This unique relationship is called the Hugoniot curve and is the locus of p–V states achievable behind a shock (see Figure 22.2.1–1).

Figure 22.2.1–1 A schematic representation of a Hugoniot curve.

The Hugoniot pressure,

, is a function of density only and can be defined, in general, from fitting experimental data.

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

where

and

are functions of density only and depend on the particular equation of state model.

Mie-Grüneisen equations of state

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

where

and

are the Hugoniot pressure and specific energy (per unit mass) and are functions of density only, and

is the Grüneisen ratio defined as

where

is a material constant and

is the reference density.

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

where

is the nominal volumetric compressive strain. Elimination of

and

from the above equations yields

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 linear 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

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 )
OtherEos: 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,” Section 30.2.1). 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:

Initial specific energy and initial stress are not supported in Abaqus/CAE.

Tabulated equation of state

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

where

and

are functions of the logarithmic volumetric strain

only, with

, and

is the reference density.

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.

Input File Usage:	Use both of the following options:
	DENSITY (to specify the reference density )* EOS, TYPE=TABULAR (to specify and as functions of )*

Abaqus/CAE Usage:

The tabulated equation of state is not supported in Abaqus/CAE.

Initial state

The initial state of the material is determined by the initial values of specific energy, , and pressure stress, p. Abaqus/Explicit automatically computes the initial density, , that satisfies the equation of state. You can define the initial specific energy and initial stress state (see “Initial conditions,” Section 30.2.1). The initial pressure used by the equation of state is inferred from the specified stress states. If no initial conditions are specified, Abaqus/Explicit assumes 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:

Initial specific energy and initial stress are not supported in Abaqus/CAE.

P–α equation of state

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:

For a fully compacted material

; otherwise,

is greater than 1. Assuming that the density of the pores is negligible compared to that of the solid phase,

can be expressed in terms of the porosity n as

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

Assuming that the pores carry no pressure, it follows from equilibrium considerations that when a pressure p is applied to the porous material, it gives rise to a volume-average pressure in the solid phase equal to

. Assuming that the specific internal energies of the porous material and the solid matrix are the same (i.e., neglecting the surface energy of the pores), the equation of state of the porous material can be expressed as

where

is the equation of state of the solid material. For the fully compacted material (that is, when

), the

equation of state reduces to that of the solid phase, therefore predicting the correct thermodynamic behavior at high pressures.

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

where

is a state variable corresponding to the minimum value attained by

during plastic (irreversible) compaction of the material. The state variable is initialized to the elastic limit

for a material that is at its virgin state. The specific form of the function

used by Abaqus/Explicit is illustrated in Figure 22.2.1–2 and is discussed next.

Figure 22.2.1–2 elastic and plastic curves for the description of compaction of ductile porous materials.

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:

These expressions can be inverted to solve for p:

The equation for the plastic curve takes the form

or, alternatively,

The elastic curve originally proposed by Hermann (1968) is given by the differential equation

where

is the elastic bulk modulus of the solid material at small nominal strains;

is the reference density of the solid; and

and

are the reference sound speeds in the solid and virgin (porous) materials, respectively.

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

and

Input File Usage:

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

*DENSITY

Use one of the following two 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

Abaqus/CAE Usage:

Only the Mie-Grüneisen equation of state is supported for the solid phase in Abaqus/CAE.

Property module: material editor: GeneralDensity (to specify the reference density )
OtherEos: Type: Us - Up (to specify the variables , s, and )
OtherEos: Suboptions Eos Compaction (to specify the reference sound speed, ; the porosity of the unloaded material, ; the pressure required to initialize plastic behavior, ; and the pressure at which all pores are crushed, )

Initial state

The initial state of the porous material is determined from the initial values of porosity, ; specific energy, ; and pressure stress, p. Abaqus/Explicit automatically computes the initial density, , that satisfies the equation of state, . You can define the initial porosity, initial specific energy, and initial stress state (see “Initial conditions,” Section 30.2.1). If no initial conditions are given, Abaqus/Explicit assumes that the material is at its virgin state:

Abaqus/Explicit will issue an error message if the initial state lies outside the region of allowed states (see Figure 22.2.1–2). When initial conditions are specified only for p (or for ), Abaqus/Explicit will compute (or p) assuming that the state lies on the primary (monotonic loading) curve.

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

Abaqus/CAE Usage:

Initial specific energy, initial stress, and initial porosity are not supported in Abaqus/CAE.

JWL high explosive equation of state

The Jones-Wilkens-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

where

and

are user-defined material constants;

is the user-defined density of the explosive; and

is the density of the detonation products.

Input File Usage:	Use both of the following options:
	DENSITY (to specify the density of the explosive )* EOS, TYPE=JWL (to specify the material constants and )*

Abaqus/CAE Usage:

Property module: material editor: GeneralDensity (to specify the density of the explosive )
OtherEos: 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.

Defining detonation points

You can define any number of detonation points for the explosive material. Coordinates of the points must be defined along with a detonation delay time. Each material point responds to the first detonation point that it sees. The detonation arrival time at a material point is based upon the time that it takes a detonation wave (traveling at the detonation wave speed ) to reach the material point plus the detonation delay time for the detonation point. If there are multiple detonation points, the arrival time is based on the minimum arrival time for all the detonation points. In a body with curved surfaces care should be taken that the detonation arrival times are meaningful. The detonation arrival times are based on the straight line of sight from the material point to the detonation point. In a curved body the line of sight may pass outside of the body.

Input File Usage:	Use both of the following options to define the detonation points:
	EOS, TYPE=JWL DETONATION POINT

Abaqus/CAE Usage:

Property module: material editor: OtherEos: Type: JWL: SuboptionsDetonation Point

Initial state

Explosive materials generally have some nominal volumetric stiffness before detonation. It may be useful to incorporate this stiffness when elements modeled with a JWL equation of state are subjected to stress before initiation of detonation by the arriving detonation wave. You can define the pre-detonation bulk modulus, . The pressure will be computed from the volumetric strain and until detonation, at which time the pressure will be determined by the procedure outlined above. The initial relative density () used in the JWL equation is assumed to be unity. The initial specific energy is assumed to be equal to the user-defined detonation energy .

If you specify a nonzero value of , you can also define an initial stress state for the explosive materials.

Input File Usage:

Use the following option to define the initial stress:

*INITIAL CONDITIONS, TYPE=STRESS

Optionally, you can also define the initial specific energy directly:

*INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY

Abaqus/CAE Usage:

Initial stress and initial specific energy are not supported in Abaqus/CAE.

Ideal gas equation of state

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

where

is the ambient pressure, R is the gas constant,

is the current temperature, and

is the absolute zero on the temperature scale being used. It is an idealization to real gas behavior and can be used to model any gases approximately under appropriate conditions (e.g., low pressure and high temperature).

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

where

is the initial specific energy at the initial temperature

and

is the specific heat at constant volume (or the constant volume heat capacity), which depends only upon temperature for an ideal gas.

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:

In general, the value R for any gas can be estimated by plotting

as a function of state (e.g., pressure or temperature). The ideal gas approximation is adequate in any region where this value is constant. You must specify the specific heat at constant volume,

. For an ideal gas

is related to the specific heat at constant pressure,

, by

Input File Usage:	Use both of the following options:
	EOS, TYPE=IDEAL GAS SPECIFIC HEAT, DEPENDENCIES=n

Abaqus/CAE Usage:

Property module: material editor: OtherEos: Type: Ideal Gas
ThermalSpecific Heat

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

Initial specific energy and initial stress are not supported in Abaqus/CAE.

The value of absolute zero

When a non-absolute temperature scale is used, you must specify the value of absolute zero temperature.

Input File Usage:

*PHYSICAL CONSTANTS, ABSOLUTE ZERO=

Abaqus/CAE Usage:

Any module: ModelEdit Attributesmodel_name: Absolute zero temperature

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.

Comparison with the hydrostatic fluid model

The ideal gas equation of state can be used to model wave propagation effects and the dynamics of a spatially varying state of a gaseous region. For cases in which the inertial effects of the gas are not important and the state of the gas can be assumed to be uniform throughout a region, the hydrostatic fluid model (“Hydrostatic fluid models,” Section 23.4.1) is a simpler, more computationally efficient alternative.

Deviatoric behavior

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, a linear isotropic deviatoric model or a viscous deviatoric model, are available. 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 increment in the deviatoric stress is defined from the deviatoric elastic strain increment as

where

is the deviatoric stress and

is the deviatoric elastic strain. You must provide the elastic shear modulus,

, when you define the elastic deviatoric behavior.

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

Abaqus/CAE Usage:

Property module: material editor: OtherEos: SuboptionsEos Shear: Type: Elastic

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.

Newtonian fluids are characterized by a viscosity that only depends on temperature, . In the more general case of non-Newtonian fluids the viscosity is a function of the temperature and shear strain rate:

where

is the equivalent shear strain rate. In terms of the equivalent shear stress,

, we have:

Non-Newtonian fluids can be classified as shear-thinning (or pseudoplastic), when the apparent viscosity decreases with increasing shear rate, and shear-thickening (or dilatant), when the viscosity increases with strain rate.

In addition to the Newtonian viscous fluid model, Abaqus/Explicit supports several models of nonlinear viscosity to describe non-Newtonian fluids: power law, Carreau-Yasuda, Cross, Herschel-Bulkey, Powell-Eyring, and Ellis-Meter. Other functional forms of the viscosity can also be specified in tabular format or in user subroutine VUVISCOSITY.

Input File Usage:	Use both of the following options to define viscous shear behavior:
	EOS EOS SHEAR, TYPE=VISCOUS

Abaqus/CAE Usage:

Property module: material editor: OtherEos: SuboptionsEos Shear: Type: Viscous

Newtonian

The Newtonian model is useful to model viscous laminar flow governed by the Navier-Poisson law of a Newtonian fluid, . Newtonian fluids are characterized by a viscosity that depends only on temperature, . You need to specify the viscosity as a tabular function of temperature when you define the Newtonian viscous deviatoric behavior.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=NEWTONIAN (default)

Abaqus/CAE Usage:

Property module: material editor: OtherEos: SuboptionsEos Shear: Type: Viscous

Power law

The power law model is commonly used to describe the viscosity of non-Newtonian fluids. The viscosity is expressed as

where

is the flow consistency index and

is the flow behavior index. When

, the fluid is shear-thinning (or pseudoplastic): the apparent viscosity decreases with increasing shear rate. When

, the fluid is shear-thickening (or dilatant); and when

, the fluid is Newtonian. Optionally, you can place a lower limit,

, and/or an upper limit,

, on the value of the viscosity computed from the power law.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=POWER LAW

Abaqus/CAE Usage:

The power law model is not supported in Abaqus/CAE.

Carreau-Yasuda

The Carreau-Yasuda model describes the shear thinning behavior of polymers. It is more realistic than the power law model as it provides a better fit for both high and low shear strain rates. The viscosity is expressed as

where

is the low shear rate Newtonian viscosity,

is the infinite shear viscosity (at high shear strain rates),

is the natural time constant of the fluid (

is the critical shear rate at which the fluid changes from Newtonian to power law behavior), and

represents the flow behavior index in the power law regime. The coefficient

is a material parameter. The original Carreau model is recovered when

=2.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=CARREAU-YASUDA

Abaqus/CAE Usage:

The Carreau-Yasuda model is not supported in Abaqus/CAE.

Cross

The Cross model is commonly used when it is necessary to describe the low-shear-rate behavior of the viscosity. The viscosity is expressed as

where

is the Newtonian viscosity,

is the infinite shear viscosity (usually assumed to be zero for the Cross model),

is the natural time constant of the fluid (

is the critical shear rate at which the fluid changes from Newtonian to power-law behavior), and

is the flow behavior index in the power law regime.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=CROSS

Abaqus/CAE Usage:

The Cross model is not supported in Abaqus/CAE.

Herschel-Bulkey

The Herschel-Bulkey model can be used to describe the behavior of viscoplastic fluids, such as Bingham plastics, that exhibit a yield response. The viscosity is expressed as

Here

is the “yield” stress and

is a penalty viscosity to model the “rigid-like” behavior in the very low strain rate regime (

), when the stress is below the yield stress,

. With increasing strain rates, the viscosity transitions into a power law model once the yield threshold is reached,

. The parameters

and

are the flow consistency and the flow behavior indexes in the power law regime, respectively. Bingham plastics correspond to the case

=1.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=HERSCHEL-BULKEY

Abaqus/CAE Usage:

The Herschel-Bulkey model is not supported in Abaqus/CAE.

Powell-Eyring

This model, which is derived from the theory of rate processes, is relevant primarily to molecular fluids but can be used in some cases to describe the viscous behavior of polymer solutions and viscoelastic suspensions over a wide range of shear rates. The viscosity is expressed as

where

is the Newtonian viscosity,

is the infinite shear viscosity, and

represents a characteristic time of the measured system.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=POWELL-EYRING

Abaqus/CAE Usage:

The Powell-Eyring model is not supported in Abaqus/CAE.

Ellis-Meter

The Ellis-Meter model expresses the viscosity in terms of the effective shear stress, , as:

where

is the effective shear stress at which the viscosity is 50% between the Newtonian limit,

, and the infinite shear viscosity,

, and

represents the flow index in the power law regime.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=ELLIS-METER

Abaqus/CAE Usage:

The Ellis-Meter model is not supported in Abaqus/CAE.

Tabular

The viscosity can be specified directly as a tabular function of shear strain rate and temperature.

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=TABULAR

Abaqus/CAE Usage:

Specifying the viscosity directly as a tabular function is not supported in Abaqus/CAE.

User-defined

You can specify a user-defined viscosity in user subroutine VUVISCOSITY (see “VUVISCOSITY,” Section 1.2.18 of the Abaqus User Subroutines Reference Manual).

Input File Usage:

*EOS SHEAR, TYPE=VISCOUS, DEFINITION=USER

Abaqus/CAE Usage:

User-defined viscosity is not supported in Abaqus/CAE.

Temperature dependence of viscosity

The temperature-dependence of the viscosity of many polymer materials of industrial interest obeys a time-temperature shift relationship in the form:

where

is the shift function and

is the reference temperature at which the viscosity versus shear strain rate relationship is known. This concept for temperature dependence is usually referred to as thermo-rheologically simple (TRS) temperature dependence. In the Newtonian limit for low shear rates, when

, we have

Thus, the shift function is defined as the ratio of the Newtonian viscosity at the temperature of interest to that of the chosen reference state:

See “Thermo-rheologically simple temperature effects” in “Time domain viscoelasticity,” Section 19.7.1, for a description of the different forms of the shift function available in Abaqus.

Input File Usage:	Use the following options to define a thermo-rheologically simple (TRS) temperature-dependent viscosity:
	EOS SHEAR, TYPE=VISCOUS TRS

Abaqus/CAE Usage:	Use the following options for the same material:
	Property module: material editor: OtherEos: SuboptionsEos Shear: Type: Viscous MechanicalElasticityViscoelastic Domain: Time, Time: *any method, and SuboptionsTrs*

Use with the Mises or the Johnson-Cook plasticity models

An equation of state model can be used with the Mises (“Classical metal plasticity,” Section 20.2.1) or the Johnson-Cook (“Johnson-Cook plasticity,” Section 20.2.7) 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.

Input File Usage:	Use the following options:
	EOS EOS SHEAR, TYPE=ELASTIC *PLASTIC

Abaqus/CAE Usage:

Property module: material editor:
OtherEos: SuboptionsEos Shear: Type: Elastic
MechanicalPlasticityPlastic

Initial conditions

You can specify initial conditions for the equivalent plastic strain, (“Initial conditions,” Section 30.2.1).

Input File Usage:

*INITIAL CONDITIONS, TYPE=HARDENING

Abaqus/CAE Usage:

Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step

Use with the tensile failure model

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 20.2.8) 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.

Input File Usage:	Use the following options:
	EOS EOS SHEAR *TENSILE FAILURE

Abaqus/CAE Usage:

The tensile failure model is not supported in Abaqus/CAE.

Adiabatic assumption

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

where

is the specific heat at constant volume. Specifying temperature as a predefined field has no effect on the behavior of this model.

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

Modeling fluids

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.

Elements

Equations of state can be used with any solid (continuum) elements in Abaqus/Explicit except plane stress elements. For three-dimensional applications exhibiting high confinement, the default kinematic formulation is recommended with reduced-integration solid elements (see “Section controls,” Section 24.1.4).

Output

In addition to the standard output identifiers available in Abaqus (“Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the equation of state models:

PALPH

Distension, , of the porous material. The current porosity is equal to one minus the inverse of :

PALPHMIN

Minimum value, , of the distension attained during plastic compaction of the porous material.

PEEQ	Equivalent plastic strain, where is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”). This is relevant only if the equation of state model is used in combination with the Mises or Johnson-Cook plasticity models.

Additional references

Carroll, M., and A. C. Holt, “Suggested Modification of the Model for Porous Materials,” Journal of Applied Physics, vol. 43, no.2, pp. 759–761, 1972.
Dobratz, B. M., “LLNL Explosives Handbook, Properties of Chemical Explosives and Explosive Simulants,” UCRL-52997, Lawrence Livermore National Laboratory, Livermore, California, January 1981.
Herrmann, W., “Constitutive Equation for the Dynamic Compaction of Ductile Porous Materials,” Journal of Applied Physics, vol. 40, no.6, pp. 2490–2499, 1968.
Lee, E., M. Finger, and W. Collins, “JWL Equation of State Coefficients for High Explosives,” UCID-16189, Lawrence Livermore National Laboratory, Livermore, California, January 1973.
Wardlaw, A. B., R. McKeown, and H. Chen, “Implementation and Application of the Equation of State in the DYSMAS Code,” Naval Surface Warfare Center, Dahlgren Division, Report Number: NSWCDD/TR-95/107, May 1996.