add documents

.raw/AbaqusAnalysisUserGuide3/AbaqusAnalysisUserGuide3_060.md

@@ -0,0 +1,172 @@
+<!-- source-page: 591 -->
+
+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 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.
+
+Input File Usage: Use the following options:
+
+\*EOS
+
+\*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
+
+$$
+\rho c _ {v} (\theta) \frac {\partial \theta}{\partial t} = (p - p _ {b v}) \frac {1}{\rho} \frac {\partial \rho}{\partial t} + \mathbf {S}: \dot {\mathbf {e}},
+$$
+
+where $c _ { v }$ 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
+
+$$
+\rho \frac {\partial E _ {m}}{\partial t} = \rho c _ {v} (\theta) \frac {\partial \theta}{\partial t}.
+$$
+
+<!-- source-page: 592 -->
+
+# Modeling fluids
+
+A linear $U _ { s } \mathrm { ~ - ~ } U _ { p }$ 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 27.1.4).
+
+# 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 $P - \alpha$ porous material. The current porosity is equal to one minus the inverse of : $n = 1 - \alpha ^ { - 1 }$
+
+<!-- source-page: 593 -->
+
+PALPHMIN Minimum value, $\alpha _ { m i n }$ , of the distension attained during plastic compaction of the $P - \alpha$ porous material.
+
+PEEQ Equivalent plastic strain, $\bar { \varepsilon } ^ { p l } = \bar { \varepsilon } ^ { p l } | _ { 0 } + \int _ { 0 } ^ { t } \sqrt { \frac 2 3 \dot { \varepsilon } ^ { p l } : \dot { \varepsilon } ^ { p l } } a$ where $\bar { \varepsilon } ^ { p l } | _ { 0 }$ 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, Johnson-Cook, or extended Drucker-Prage plasticity models.
+
+# Additional references
+
+• Carroll, M., and A. C. Holt, “Suggested Modification of the $P - \alpha$ 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 $P \mathrm { ~ - ~ } \alpha$ Equation of State in the DYSMAS Code,” Naval Surface Warfare Center, Dahlgren Division, Report Number: NSWCDD/TR-95/107, May 1996.
+
+<!-- source-page: 594 -->
+
+<!-- source-page: 595 -->
+
+# 26. Other Material Properties
+
+Mechanical properties 26.1
+
+Heat transfer properties 26.2
+
+Acoustic properties 26.3
+
+Mass diffusion properties 26.4
+
+Electromagnetic properties 26.5
+
+Pore fluid flow properties 26.6
+
+User materials 26.7
+
+<!-- source-page: 596 -->
+
+<!-- source-page: 597 -->
+
+# 26.1 Mechanical properties
+
+• “Material damping,” Section 26.1.1   
+• “Thermal expansion,” Section 26.1.2   
+• “Field expansion,” Section 26.1.3   
+• “Viscosity,” Section 26.1.4
+
+<!-- source-page: 598 -->
+
+<!-- source-page: 599 -->
+
+# 26.1.1 MATERIAL DAMPING
+
+Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
+
+# References
+
+• “Dynamic analysis procedures: overview,” Section 6.3.1   
+• “Material library: overview,” Section 21.1.1   
+• \*DAMPING   
+• “Defining damping” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
+
+# Overview
+
+Material damping can be defined:
+
+• for direct-integration (nonlinear, implicit or explicit), subspace-based direct-integration, direct-solution steady-state, and subspace-based steady-state dynamic analysis; or   
+• for mode-based (linear) dynamic analysis in Abaqus/Standard.
+
+# Rayleigh damping
+
+In direct-integration dynamic analysis you very often define energy dissipation mechanisms—dashpots, inelastic material behavior, etc.—as part of the basic model. In such cases there is usually no need to introduce additional damping: it is often unimportant compared to these other dissipative effects. However, some models do not have such dissipation sources (an example is a linear system with chattering contact, such as a pipeline in a seismic event). In such cases it is often desirable to introduce some general damping. Abaqus provides “Rayleigh” damping for this purpose. It provides a convenient abstraction to damp lower (mass-dependent) and higher (stiffness-dependent) frequency range behavior.
+
+Rayleigh damping can also be used in direct-solution steady-state dynamic analyses and subspace-based steady-state dynamic analyses to get quantitatively accurate results, especially near natural frequencies.
+
+To define material Rayleigh damping, you specify two Rayleigh damping factors: $\alpha _ { R }$ for mass proportional damping and $\beta _ { R }$ for stiffness proportional damping. In general, damping is a material property specified as part of the material definition. For the cases of rotary inertia, point mass elements, and substructures, where there is no reference to a material definition, the damping can be defined in conjunction with the property references. Any mass proportional damping also applies to nonstructural features (see “Nonstructural mass definition,” Section 2.7.1).
+
+For a given mode i the fraction of critical damping, , can be expressed in terms of the damping factors $\alpha _ { R }$ and $\beta _ { R }$ as:
+
+$$
+\xi_ {i} = \frac {\alpha_ {R}}{2 \omega_ {i}} + \frac {\beta_ {R} \omega_ {i}}{2},
+$$
+
+<!-- source-page: 600 -->
+
+where $\omega _ { i }$ is the natural frequency at this mode. This equation implies that, generally speaking, the mass proportional Rayleigh damping, $\alpha _ { R } ,$ damps the lower frequencies and the stiffness proportional Rayleigh damping, $\beta _ { R }$ , damps the higher frequencies.
+
+# Mass proportional damping
+
+The $\alpha _ { R }$ factor introduces damping forces caused by the absolute velocities of the model and so simulates the idea of the model moving through a viscous “ether” (a permeating, still fluid, so that any motion of any point in the model causes damping). This damping factor defines mass proportional damping, in the sense that it gives a damping contribution proportional to the mass matrix for an element. If the element contains more than one material in Abaqus/Standard, the volume average value of $\alpha _ { R }$ is used to multiply the element’s mass matrix to define the damping contribution from this term. If the element contains more than one material in Abaqus/Explicit, the mass average value of $\alpha _ { R }$ is used to multiply the element’s lumped mass matrix to define the damping contribution from this term. $\alpha _ { R }$ has units of (1/time).
+
+Input File Usage: \*DAMPING, ALPHA=
+
+Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: Alpha: $\alpha _ { R }$
+
+Defining variable mass proportional damping in Abaqus/Explicit
+
+In Abaqus/Explicit you can define $\alpha _ { R }$ as a tabular function of temperature and/or field variables. Therefore, mass proportional damping can vary during an Abaqus/Explicit analysis.
+
+Input File Usage: \*DAMPING, ALPHA=TABULAR
+
+# Stiffness proportional damping
+
+The $\beta _ { R }$ factor introduces damping proportional to the strain rate, which can be thought of as damping associated with the material itself. $\beta _ { R }$ defines damping proportional to the elastic material stiffness. Since the model may have quite general nonlinear response, the concept of “stiffness proportional damping” must be generalized, since it is possible for the tangent stiffness matrix to have negative eigenvalues (which would imply negative damping). To overcome this problem, $\beta _ { R }$ is interpreted as defining viscous material damping in Abaqus, which creates an additional “damping stress,” $\sigma _ { d } .$ , proportional to the total strain rate:
+
+$$
+\pmb {\sigma} _ {d} = \beta_ {R} \mathbf {D} ^ {e l} \dot {\pmb {\varepsilon}},
+$$
+
+where $\dot { \varepsilon }$ is the strain rate. For hyperelastic (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) and hyperfoam (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) materials $\mathbf { D } ^ { e l }$ is defined as the elastic stiffness in the strain-free state. For all other linear elastic materials in Abaqus/Standard and all other materials in Abaqus/Explicit, $\mathbf { D } ^ { e l }$ is the material’s current elastic stiffness. $\mathbf { D } ^ { e l }$ will be calculated based on the current temperature during the analysis.
+
+This damping stress is added to the stress caused by the constitutive response at the integration point when the dynamic equilibrium equations are formed, but it is not included in the stress output. As a result, damping can be introduced for any nonlinear case and provides standard Rayleigh damping for linear