Skip to content

Material Data

In FrontISTR, a "material" is a named unit used to manage, as a group, the material-property data assigned to elements. Specifically, it groups property values such as elastic constants, density, and thermal conductivity, as well as constitutive-law parameters for elastoplasticity, viscoelasticity, creep, and similar models, under a single name. Assignment to element groups is performed with !SECTION, which associates an element type (solid, shell, interface, etc.) with a material name. The material contents themselves are defined either by !MATERIAL in the mesh data or by a !MATERIAL block in the analysis control data.

Constraints on material data are determined by three factors: the analysis type, the element type, and how the material is specified in the input files. The following sections first summarize the correspondence among available material models, element types, and analysis types (Feature Overview), then explain how to choose among material models (Choosing a Material Model), and finally describe the specifications of each model (Linear Elasticity and subsequent sections). See the keyword reference for the syntax and default values of individual keywords.

Feature Overview

Material data can be broadly divided into mechanical material models used in structural analysis and thermal properties used in heat-conduction and thermal-stress analyses. In structural analysis, select linear elasticity, hyperelasticity, elastoplasticity, viscoelasticity, creep, or a user-defined material according to the application. Each is an independent constitutive law; elastoplastic, viscoelastic, and creep models use linear elasticity in the same material for the elastic part (hyperelasticity uses its own strain-energy function and therefore does not refer to linear-elastic stiffness). In heat-conduction analysis, density, specific heat, and thermal conductivity are assigned to elements.

Category Main applications Main input keywords Main references
Linear elasticity Small-deformation linear analysis, modal analysis, linear dynamic analysis, elastic part of nonlinear materials !ELASTIC, !MATERIAL ITEM=1 !ELASTIC, !MATERIAL (mesh data)
Hyperelasticity Large-deformation elastic response of rubber-like materials, etc. !HYPERELASTIC !HYPERELASTIC
Elastoplasticity Permanent strain after yielding, metal plasticity, geomaterials !PLASTIC !PLASTIC
Viscoelasticity Time-dependent response with relaxation or retardation !VISCOELASTIC, !TRS !VISCOELASTIC, !TRS
Creep Deformation that progresses with time under stress !CREEP !CREEP
Thermal properties Heat-conduction analysis, thermal-stress analysis !MATERIAL ITEM=1–3, !EXPANSION_COEFF !EXPANSION_COEFF
User-defined material User-implemented constitutive law !USER_MATERIAL, !ELASTIC TYPE=USER, !HYPERELASTIC TYPE=USER, !PLASTIC YIELD=USER !USER_MATERIAL

In structural analysis, if a material with the same name is defined in both the mesh data and the analysis control data, the analysis-control-data definition takes precedence. However, a material definition in the mesh data itself is still required; when a material of the same name is defined in the analysis control data, the values on the mesh-data side are not referenced and may therefore be dummy values. In heat-conduction analysis, by contrast, material specification in the analysis control data is not supported, and the values specified in the mesh data are used as-is.

Support by analysis type can be summarized as follows. Linear static analysis, modal analysis, and linear dynamic analysis use linear elasticity. Nonlinear static and nonlinear dynamic analyses using three-dimensional continuum solid elements can use hyperelasticity, elastoplasticity, viscoelasticity, creep, and user-defined materials on a linear-elastic basis. Heat-conduction analysis uses density, specific heat, and thermal conductivity rather than structural material models. See Analysis Types for an overview of analysis types.

There are also restrictions by element type. Three-dimensional continuum solid elements can use nonlinear material models for structural analysis. Plane-stress, plane-strain, and axisymmetric elements primarily use linear elasticity; these two-dimensional element families do not support elastoplasticity, hyperelasticity, viscoelasticity, or creep. Shell elements support linear elasticity and can be specified as single-layer or laminated, isotropic or anisotropic. Shell elements do not support elastoplasticity, hyperelasticity, viscoelasticity, or creep. Interface elements are used to model gap heat transfer and radiation in heat-conduction analysis; gap parameters are specified on the data line of !SECTION, not as material data. See also the Element Library for examples of association with element groups and laminate input.

The following table summarizes availability of material models by element type.

Element type Linear elasticity (isotropic) Linear elasticity (orthotropic/laminated) Hyperelasticity Elastoplasticity Viscoelasticity Creep Thermal properties
3D solid ○ ○ ○ ○ ○ ○ ○
Plane stress / plane strain / axisymmetric ○ — — — — — ○
Shell (single-layer/laminated) ○ ○ — — — — —
Beam / truss ○ — — — — — —
Interface — — — — — — ○

(Symbols: ○ available / — not supported). For interface elements, thermal properties for gap heat transfer and radiation are specified with !SECTION.

There are two routes for defining materials. In mesh data, !SECTION associates an element group with a material name, while !MATERIAL and !ITEM define material properties. In analysis control data, material models are defined by placing !MATERIAL, !ELASTIC, !HYPERELASTIC, and similar keywords inside a !PLASTIC block. If !MATERIAL is defined in the analysis control data, that definition is used instead of the same-named material definition in the mesh data. See !SECTION (mesh data) and !MATERIAL (mesh data) for details of !SECTION and !MATERIAL on the mesh-data side. See !MATERIAL (analysis control data) for the material block on the analysis-control-data side.

Choosing a Material Model

When selecting a material model, first determine whether linear elasticity is sufficient. Use linear elasticity when deformation is small, stress does not exceed the yield point, and time-dependent relaxation or creep need not be considered. Select hyperelasticity for large-deformation elastic response, elastoplasticity for plastic strain after yielding, viscoelasticity for materials with relaxation times, and creep for deformation that progresses during long-term load holding.

Problem characteristics Candidate material model Guideline
Small deformation with a linear stress-strain relation Linear elasticity When Young's modulus and Poisson's ratio are sufficient
Returns to the original shape after unloading even under large deformation Hyperelasticity Rubber-like materials or cases requiring a nonlinear elastic potential
Permanent strain remains after exceeding the yield point Elastoplasticity When a yield function and hardening law must be selected
Stress relaxation or delayed response occurs while a load is held Viscoelasticity When behavior can be represented by relaxation coefficients and relaxation times
Strain accumulates under long-term loading Creep When the Norton law provides an adequate approximation
Cannot be represented by built-in models User-defined material When implementing the constitutive law in an external subroutine

When temperature dependence is required, check support for each material model. Linear elasticity, creep, and the thermal expansion coefficient support temperature-dependent tables. Viscoelasticity uses temperature shifting through !TRS rather than temperature interpolation of the Prony coefficients themselves. For elastoplasticity, temperature-dependent tables are available when multilinear hardening is used with Mises yielding. Mohr-Coulomb and Drucker-Prager do not support temperature dependence.

When anisotropy or laminates are required, also consider the element type. Solid elements support orthotropic linear elasticity. Within the range of linear elasticity, shell elements support isotropic single-layer, anisotropic single-layer, isotropic laminated, and anisotropic laminated materials. Nonlinear material models cannot be used with shell elements.

For nearly incompressible materials, do not set Poisson's ratio to 0.5. FrontISTR does not support specification of a perfectly incompressible material. In large-deformation problems where incompressibility has a strong effect, the choice of element formulation is also important; check the formulation options in the Element Library as well.

Linear Elasticity

Linear elasticity is the most fundamental material model in FrontISTR structural analysis. Linear static analysis, modal analysis, and linear dynamic analysis use linear elasticity. When elastoplasticity, viscoelasticity, or creep is used, linear elasticity is also defined in the same material for the elastic part. → See !ELASTIC for details.

For isotropic linear elasticity, specify Young's modulus and Poisson's ratio. When temperature dependence is required, Young's modulus and Poisson's ratio can be tabulated as functions of temperature. For orthotropy, specify nine independent constants in total: Young's moduli in three directions, three Poisson ratios, and three shear moduli. Because orthotropy requires a material coordinate system, specify a local coordinate system in the corresponding !SECTION.

To specify linear elasticity in mesh data, combine !SECTION and !MATERIAL. In the following example, material ALL is assigned to solid element group M1; ITEM=1 defines Young's modulus and Poisson's ratio, ITEM=2 defines mass density, and ITEM=3 defines the coefficient of linear thermal expansion.

!SECTION, TYPE=SOLID, EGRP=ALL, MATERIAL=M1

!MATERIAL, NAME=M1, ITEM=3
!ITEM=1, SUBITEM=2
  4000., 0.3
!ITEM=2
  8.0102E-10
!ITEM=3
  1.0E-5

For shell elements, both single-layer and laminated definitions are available within linear elasticity. Use SUBITEM=4 for a single-layer isotropic material and SUBITEM=9 for a single-layer anisotropic material. For a laminate, place material constants and layer weights for all layers in the same !ITEM. Layer weights are normalized by their total and used as integration weights through the thickness. The physical thickness of the entire shell is specified by the thickness in !SECTION, TYPE=SHELL.

The following is an example of a single-layer shell with an isotropic material.

!MATERIAL, NAME=M1, ITEM=1
!ITEM=1, SUBITEM=4
0, 200000, 0.3, 2.0

The following is an example of a two-layer laminated shell with isotropic materials.

!MATERIAL, NAME=M1, ITEM=1
!ITEM=1, SUBITEM=7
0, 200000, 0.3, 2.0, 200000, 0.3, 2.0

The following is an example of a single-layer shell with an anisotropic material. The anisotropy angle is specified in degrees.

!MATERIAL, NAME=M1, ITEM=1
!ITEM=1, SUBITEM=9
1, 28600., 0.15, 32.3, 28600., 12434., 12434., 12434., 0.0

The following is an example of a two-layer laminated shell with anisotropic materials.

!MATERIAL, NAME=M1, ITEM=1
!ITEM=1, SUBITEM=17
1, 28600., 0.15, 32.3, 28600., 12434., 12434., 12434., 0.0,
   28600., 0.15, 32.3, 28600., 12434., 12434., 12434., 0.0

Hyperelasticity

Hyperelasticity is a nonlinear elastic material model in which stress is defined from a strain-energy function. It is used for rubber-like materials that return to their original shape after unloading even after large deformation. In the input, specify !MATERIAL inside a !HYPERELASTIC block. → See !HYPERELASTIC for details.

FrontISTR supports the following hyperelastic models. The OGDEN model is not supported.

Model Input type Main coefficients Characteristics
Neo-Hookean NEOHOOKE \(C_{10}\), \(D\) Simple isotropic hyperelastic model corresponding to \(C_{01}=0\) in Mooney-Rivlin
Mooney-Rivlin MOONEY-RIVLIN \(C_{10}\), \(C_{01}\), \(D\) Isotropic hyperelastic model using two reduced invariants
Arruda-Boyce ARRUDA-BOYCE \(\mu\), \(\lambda_m\), \(D\) Rubber-like material model based on a molecular-chain network
Anisotropic Mooney-Rivlin MOONEY-RIVLIN-ANISO Ten coefficients are read from the input, but the current constitutive law uses the first five Model representing anisotropic hyperelastic response such as a fiber direction
User-defined hyperelasticity USER User constants Model in which the hyperelastic constitutive law is implemented in an external subroutine

Hyperelasticity uses the coefficient \(D\) associated with volume change to represent compressibility. Perfectly incompressible materials are not supported, so do not use a specification corresponding to Poisson's ratio \(\nu=0.5\). For nearly incompressible materials, it is necessary to select not only the hyperelastic-model coefficients but also the element formulation to be used.

Hyperelasticity is handled by default within the Total Lagrange framework. See Hyperelasticity (Theory) for definitions of the strain-energy function, stress, and tangent stiffness.

Elastoplasticity

Elastoplasticity separates the elastic and plastic regions using a yield function and represents the post-yield response with a hardening law. In the input, combine !MATERIAL and !ELASTIC in the same !PLASTIC block. → See !PLASTIC for details.

In FrontISTR, an elastoplastic model is specified by combining a yield function and a hardening law. The supported range is as follows.

Yield function Input type Supported hardening laws Main applications
Mises MISES BILINEAR, MULTILINEAR, SWIFT, RAMBERG-OSGOOD, KINEMATIC, COMBINED Isotropic yielding such as in metals
Mohr-Coulomb MOHR-COULOMB BILINEAR, MULTILINEAR Soil and rock materials represented by friction angle and cohesion
Drucker-Prager DRUCKER-PRAGER BILINEAR, MULTILINEAR Pressure-dependent yielding that smoothly approximates Mohr-Coulomb
User-defined yield USER User-defined When implementing the tangent stiffness and return mapping in an external subroutine

Multilinear hardening with Mises yielding supports temperature-dependent tables. Bilinear hardening, Swift hardening, Ramberg-Osgood hardening, kinematic hardening, and combined hardening with Mises yielding are evaluated as constant expressions. Mohr-Coulomb and Drucker-Prager do not support temperature dependence. When multilinear hardening is used, the input must be such that plastic strain is nonnegative and the first plastic strain is 0.

Shell, plane-stress, plane-strain, and axisymmetric elements do not support elastoplasticity. Use three-dimensional continuum solid elements for elastoplastic materials.

Elastoplasticity is handled by default within the Updated Lagrange framework. If !PLASTIC is specified for INFINITESIMAL, it is treated as a small-deformation constitutive law. Stress updating uses integration based on return mapping; see Elastoplasticity (Theory) for algorithmic details.

Viscoelasticity

Viscoelasticity is a material model that adds time-dependent relaxation to elastic response. FrontISTR takes a generalized Maxwell model as a Prony series. Define !MATERIAL and !ELASTIC in the same !VISCOELASTIC block. → See !VISCOELASTIC for details.

For a Prony series, specify pairs of relaxation coefficients and relaxation times on multiple lines. A relaxation time of 0 cannot be specified. To account for temperature dependence, place !TRS after !VISCOELASTIC and specify a temperature shift factor. → See !TRS for details.

Temperature shifting supports WLF and Arrhenius forms, both of which define the shift factor \(A\) as a function of the analysis temperature \(\theta\) and reference temperature \(\theta_0\). In either case, the input supplies two material constants (C1, C2) and a reference temperature, but their meaning depends on the selected shift model (the two coefficients of the Williams-Landel-Ferry equation for the WLF form, and two activation-energy-related coefficients for the Arrhenius form). See the theory manual Viscoelasticity for the specific functional forms and derivation of the shift factor.

Creep

Creep is a material model for deformation that progresses with time under a constant load or constant stress. FrontISTR !CREEP supports the Norton law. Define !MATERIAL and !ELASTIC in the same !CREEP block. → See !CREEP for details.

In the Norton law, the creep strain rate is represented by a power-law expression of equivalent stress, time, and material constants \(A\), \(n\), and \(m\) (see the theory manual Creep for the specific functional form). The material constants support temperature-dependent tables, so values can be specified for each temperature.

!CREEP for TYPE=USER is not supported. Use a user-defined material when implementing a custom constitutive law that includes creep.

Material Properties for Heat-Conduction Analysis

Heat-conduction analysis defines density, specific heat, and thermal conductivity rather than the elastic and plastic materials used in structural analysis. For link, plane, solid, and shell elements, use !MATERIAL–ITEM=1 in mesh-data 3. Thermal properties can be supplied as temperature-dependent tables.

In the following example, density, specific heat, and thermal conductivity are defined for material M1 as temperature-dependent data. After SECTION assigns material ALL to solid element group M1, !MATERIAL of ITEM=1 gives density, ITEM=2 gives specific heat, and ITEM=3 gives thermal conductivity, each paired with temperature.

!SECTION, TYPE=SOLID, EGRP=ALL, MATERIAL=M1

!MATERIAL, NAME=M1, ITEM=3
!ITEM=1, SUBITEM=1
7850., 300.
7790., 500.
7700., 800.
!ITEM=2
0.465, 300.
0.528, 500.
0.622, 800.
!ITEM=3
43., 300.
38.6, 500.
27.7, 800.

For interface elements, material data are not used; the data line of !SECTION, TYPE=INTERFACE specifies the gap width, gap heat-transfer coefficient, and radiation coefficients.

!SECTION, TYPE=INTERFACE, EGRP=GAP
1.0, 20.15, 8.99835E-9, 8.99835E-9

For shell-element heat-conduction analysis, thermal properties are specified with material !MATERIAL, as for solid elements. Shell thickness and the number of through-thickness integration points are specified on the !SECTION side.

Thermal-stress analysis defines the coefficient of linear thermal expansion in order to calculate thermal strain from the temperature field. Isotropic and orthotropic thermal-expansion coefficients are supported, including temperature dependence. → See !EXPANSION_COEFF for details. To specify the mass density used in structural or dynamic analysis on the analysis-control-data side, see !DENSITY. Density for heat-conduction analysis is specified with mesh-data !MATERIAL ITEM=1 as shown here.

User-Defined Materials

User-defined materials provide an entry point for implementing, in an external subroutine, constitutive laws that cannot be represented by FrontISTR built-in material models. In the input, !USER_MATERIAL specifies the number of state variables and user constants. → See !USER_MATERIAL for details.

!USER_MATERIAL is treated by default as an Updated-Lagrange-type constitutive law and is treated as Total-Lagrange type when KIRCHHOFF is specified. The number of state variables is specified by NSTATUS. Up to 100 user constants can be passed on data lines. These constants and state variables are used as internal variables of the constitutive law in the user subroutine.

With !USER_MATERIAL, implement the constitutive law itself in uMatlMatrix and uUpdate. uMatlMatrix returns the material tangent stiffness, and uUpdate updates stress and state variables. For user elasticity under small deformation, use !ELASTIC, TYPE=USER; for a user hyperelastic model, use !HYPERELASTIC, TYPE=USER, implementing the elastic response in uElasticMatrix and uElasticUpdate. For a user-defined yield function, use !PLASTIC, YIELD=USER and implement the elastoplastic tangent stiffness and return mapping.