김경종
136 lines
12 KiB
Markdown
136 lines
12 KiB
Markdown
<!-- source-page: 61 -->
|
||
|
||
# 21.2.1 DENSITY
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Material library: overview,” Section 21.1.1
|
||
• \*DENSITY
|
||
• “Specifying material mass density,” Section 12.8.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
A material’s mass density:
|
||
|
||
• must be defined in Abaqus/Standard for eigenfrequency and transient dynamic analysis, transient heat transfer analysis, adiabatic stress analysis, and acoustic analysis;
|
||
• must be defined in Abaqus/Standard for gravity, centrifugal, and rotary acceleration loading;
|
||
• must be defined in Abaqus/Explicit for all materials except hydrostatic fluids;
|
||
• must be defined in Abaqus/CFD for all fluids;
|
||
• can be specified as a function of temperature and predefined variables;
|
||
• can be distributed from nonstructural features (such as paint on sheet metal panels in a car) to the underlying elements using a nonstructural mass definition; and
|
||
• can be defined with a distribution for solid continuum elements in Abaqus/Standard.
|
||
|
||
# Defining density
|
||
|
||
Density can be defined as a function of temperature and field variables. Based on user-defined data Abaqus internally estimates the material density as follows:
|
||
|
||
• For acoustic, heat transfer, and coupled thermal-electrical elements in Abaqus/Standard and acoustic elements in Abaqus/Explicit, the density is continually updated to the value corresponding to the current temperature and field variables.
|
||
• For coupled temperature-displacement elements in Abaqus/Standard, the density is continually updated to the value corresponding to the current temperature and field variables for heat transfer computations only. Structural body force computations ensure mass conservation during the analysis by assuming the density to be a function of the initial temperature and field variables and changes in volume only.
|
||
• For all other elements in Abaqus/Standard and Abaqus/Explicit, the density is taken to be a function of the initial temperature and field variables and changes in volume only. It is not updated if temperatures and field variables change during the analysis.
|
||
• For Abaqus/CFD the density is considered constant for incompressible flows.
|
||
|
||
<!-- source-page: 62 -->
|
||
|
||
In an Abaqus/Standard analysis a spatially varying mass density can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include a default value for the density. If a distribution is used, no dependencies on temperature and/or field variables for the density can be defined.
|
||
|
||
Input File Usage: Use either of the following options:
|
||
|
||
\*DENSITY
|
||
|
||
\*DENSITY, DEPENDENCIES=n
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: General→Density
|
||
|
||
You can toggle on Use temperature-dependent data to define the density as a function of temperature and/or select the Number of field variables to define the density as a function of field variables.
|
||
|
||
# Units
|
||
|
||
Since Abaqus has no built-in dimensions, you must ensure that the density is given in consistent units. The use of consistent units, and density in particular, is discussed in “Conventions,” Section 1.2.2. If American or English units are used, you must be particularly careful that the density used is in units of ML , where mass is defined in units of $\mathrm { F T ^ { 2 } L ^ { - 1 } }$ .
|
||
|
||
# Elements
|
||
|
||
The density behavior described in this section is used to specify mass density for all elements, except rigid elements. Mass density for rigid elements is specified as part of the rigid body definition (see “Rigid elements,” Section 30.3.1).
|
||
|
||
In Abaqus/Explicit a nonzero mass density must be defined for all elements that are not part of a rigid body.
|
||
|
||
In Abaqus/Standard density must be defined for heat transfer elements and acoustic elements; mass density can be defined for stress/displacement elements, coupled temperature-displacement elements, and elements including pore pressure. For elements that include pore pressure as a degree of freedom, the density of the dry material should be given for the porous medium in a coupled pore fluid flow/stress analysis.
|
||
|
||
If you have a complex density for an acoustic medium, you should enter its real part here and convert the imaginary part into a volumetric drag, as discussed in “Acoustic medium,” Section 26.3.1.
|
||
|
||
The mass contribution from features that have negligible structural stiffness can be added to the model by smearing the mass over an element set that is typically adjacent to the nonstructural feature. The nonstructural mass can be specified in the form of a total mass value, a mass per unit volume, a mass per unit area, or a mass per unit length (see “Nonstructural mass definition,” Section 2.7.1). A nonstructural mass definition contributes additional mass to the specified element set and does not alter the underlying material density.
|
||
|
||
<!-- source-page: 63 -->
|
||
|
||
# 22. Elastic Mechanical Properties
|
||
|
||
Overview 22.1
|
||
|
||
Linear elasticity 22.2
|
||
|
||
Porous elasticity 22.3
|
||
|
||
Hypoelasticity 22.4
|
||
|
||
Hyperelasticity 22.5
|
||
|
||
Stress softening in elastomers 22.6
|
||
|
||
Linear viscoelasticity 22.7
|
||
|
||
Nonlinear Viscoelasticity 22.8
|
||
|
||
Rate sensitive elastomeric foams 22.9
|
||
|
||
<!-- source-page: 64 -->
|
||
|
||
<!-- source-page: 65 -->
|
||
|
||
# 22.1 Overview
|
||
|
||
• “Elastic behavior: overview,” Section 22.1.1
|
||
|
||
<!-- source-page: 66 -->
|
||
|
||
<!-- source-page: 67 -->
|
||
|
||
# 22.1.1 ELASTIC BEHAVIOR: OVERVIEW
|
||
|
||
The material library in Abaqus includes several models of elastic behavior:
|
||
|
||
• Linear elasticity: Linear elasticity (“Linear elastic behavior,” Section 22.2.1) is the simplest form of elasticity available in Abaqus. The linear elastic model can define isotropic, orthotropic, or anisotropic material behavior and is valid for small elastic strains.
|
||
• Plane stress orthotropic failure: Failure theories are provided (“Plane stress orthotropic failure measures,” Section 22.2.3) for use with linear elasticity. They can be used to obtain postprocessed output requests.
|
||
• Porous elasticity: The porous elastic model in Abaqus/Standard (“Elastic behavior of porous materials,” Section 22.3.1) is used for porous materials in which the volumetric part of the elastic strain varies with the logarithm of the equivalent pressure stress. This form of nonlinear elasticity is valid for small elastic strains.
|
||
• Hypoelasticity: The hypoelastic model in Abaqus/Standard (“Hypoelastic behavior,” Section 22.4.1) is used for materials in which the rate of change of stress is defined by an elasticity matrix multiplying the rate of change of elastic strain, where the elasticity matrix is a function of the total elastic strain. This general, nonlinear elasticity is valid for small elastic strains.
|
||
• Rubberlike hyperelasticity: For rubberlike material at finite strain the hyperelastic model (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) provides a general strain energy potential to describe the material behavior for nearly incompressible elastomers. This nonlinear elasticity model is valid for large elastic strains.
|
||
• Foam hyperelasticity: The hyperfoam model (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) provides a general capability for elastomeric compressible foams at finite strains. This nonlinear elasticity model is valid for large strains (especially large volumetric changes). The low-density foam model in Abaqus/Explicit (“Low-density foams,” Section 22.9.1) is a nonlinear viscoelastic model suitable for specifying strain-rate sensitive behavior of low-density elastomeric foams such as used in crash and impact applications. The foam plasticity model (“Crushable foam plasticity models,” Section 23.3.5) should be used for foam materials that undergo permanent deformation.
|
||
• Anisotropic hyperelasticity: The anisotropic hyperelastic model (“Anisotropic hyperelastic behavior,” Section 22.5.3) provides a general capability for modeling materials that exhibit highly anisotropic and nonlinear elastic behavior (such as biomedical soft tissues, fiber-reinforced elastomers, etc.). The model is valid for large elastic strains and captures the changes in the preferred material directions (or fiber directions) with deformation.
|
||
• Fabric materials: The fabric model in Abaqus/Explicit (“Fabric material behavior,” Section 23.4.1) for woven fabrics captures the directional nature of the stiffness along the fill and the warp yarn directions. It also captures the shear response as the yarn directions rotate relative to each other. The model takes into account finite strains including large shear rotations. It captures the highly nonlinear elastic response of fabrics through the use of test data or a user subroutine, VFABRIC (see “VFABRIC,” Section 1.2.5 of the Abaqus User Subroutines Reference Guide) for the material characterization. The test data based
|
||
|
||
<!-- source-page: 68 -->
|
||
|
||
fabric behavior can include nonlinear elasticity, permanent deformation, rate-dependent response, and damage accumulation.
|
||
|
||
• Viscoelasticity: The viscoelastic model is used to specify time-dependent material behavior (“Time domain viscoelasticity,” Section 22.7.1). In Abaqus/Standard it is also used to specify frequency-dependent material behavior (“Frequency domain viscoelasticity,” Section 22.7.2). It must be combined with linear elasticity, rubberlike hyperelasticity, or foam hyperelasticity.
|
||
• Parallel rheological framework: The parallel rheological framework (“Parallel rheological framework,” Section 22.8.2) is intended for modeling nonlinear behavior for materials subjected to large strains, such as elastomers and polymers. The models defined within this framework consist of multiple parallel viscoelastic networks and, optionally, an elastoplastic network to allow modeling permanent set and material softening using the Mullins effect. The elastic response is defined using the hyperelastic material model; the plastic response is based on the theory of incompressible isotropic hardening plasticity; and the viscous response is specified using the flow rule derived from a creep potential.
|
||
• Hysteresis: The hysteresis model in Abaqus/Standard (“Hysteresis in elastomers,” Section 22.8.1) is used to specify rate-dependent behavior of elastomers. It is used in conjunction with hyperelasticity.
|
||
• Mullins effect: The Mullins effect model (“Mullins effect,” Section 22.6.1) is used to specify stress softening of filled rubber elastomers due to damage, a phenomenon referred to as Mullins effect. The model can also be used to include permanent energy dissipation and stress softening effects in elastomeric foams (“Energy dissipation in elastomeric foams,” Section 22.6.2). It is used in conjunction with rubberlike hyperelasticity or foam hyperelasticity.
|
||
• No compression or no tension elasticity: The no compression or no tension models in Abaqus/Standard (“No compression or no tension,” Section 22.2.2) can be used when compressive or tensile principal stresses should not be generated. These options can be used only with linear elasticity.
|
||
|
||
# Thermal strain
|
||
|
||
Thermal expansion can be introduced for any of the elasticity or fabric models (“Thermal expansion,” Section 26.1.2).
|
||
|
||
# Elastic strain magnitude
|
||
|
||
Except in the hyperelasticity and fabric material models, the stresses are always assumed to be small compared to the tangent modulus of the elasticity relationship; that is, the elastic strain must be small (less than 5%). The total strain can be arbitrarily large if inelastic response such as metal plasticity is included in the material definition.
|
||
|
||
For finite-strain calculations where the large strains are purely elastic, the fabric model (for woven fabrics), the hyperelastic model (for rubberlike behavior), or the foam hyperelasticity model (for elastomeric foams) should be used. The hyperelasticity and fabric models are the only models that give realistic predictions of actual material behavior at large elastic strains. The linear or, in Abaqus/Standard, porous elasticity models are appropriate in other cases where the large strains are inelastic.
|
||
|
||
<!-- source-page: 69 -->
|
||
|
||
In Abaqus/Standard the linear elastic, porous elastic, and hypoelastic models will exhibit poor convergence characteristics if the stresses reach levels of 50% or more of the elastic moduli; this limitation is not serious in practical cases because these material models are not valid for the resulting large strains.
|
||
|
||
<!-- source-page: 70 -->
|