김경종
19 KiB
text_image
critical state line K = 1.0 β = 0.5 β = 1.0 p_t a p_c p
Figure 23.3.4–1 Clay yield surfaces in the p { - } \tilde { t } plane.
radar
| Curve | K |
|---|---|
| a | 1.0 |
| b | 0.8 |
Figure 23.3.4–2 Isotropic clay yield surface sections in the -plane ( and \tilde { q } = q for the isotropic yield function).
The hardening law can have an exponential form (Abaqus/Standard only) or a piecewise linear form.
Exponential form in Abaqus/Standard
The exponential form of the hardening law can be used only in conjunction with the Abaqus/Standard porous elastic material model and the isotropic form of the yield surface with p _ { t } = 0 . The size of the yield surface at any time is determined by the initial value of the hardening parameter, a _ { 0 } , and the amount of inelastic volume change that occurs according to the equation
a = a _ {0} \exp \left[ (1 + e _ {0}) \frac {1 - J ^ {p l}}{\lambda - \kappa J ^ {p l}} \right],
where
Jpl J ^ { p l } is the inelastic volume change (that part of J, the ratio of current volume to initial volume, attributable to inelastic deformation);
\kappa ( \theta , f _ { i } ) is the logarithmic bulk modulus of the material defined for the porous elastic material behavior;
\lambda ( \theta , f _ { i } ) is the logarithmic hardening constant defined for the clay plasticity material behavior; and
e _ { 0 } is the user-defined initial void ratio (“Defining initial void ratios in a porous medium” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
Specifying the initial size of the yield surface directly
The initial size of the yield surface is defined for clay plasticity by specifying the hardening parameter, a _ { 0 } , as a tabular function or by defining it analytically.
a _ { 0 } can be defined along with , M, , and K, as a tabular function of temperature and other predefined field variables. However, a _ { 0 } is a function only of the initial conditions; it will not change if temperatures and field variables change during the analysis.
Input File Usage: Use all of the following options:
*INITIAL CONDITIONS, TYPE=RATIO
*POROUS ELASTIC
*CLAY PLASTICITY, HARDENING=EXPONENTIAL
Abaqus/CAE Usage: Use all of the following options:
Property module: material editor:
Mechanical→Elasticity→Porous Elastic
Mechanical→Plasticity→Clay Plasticity: Hardening: Exponential
Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step
Specifying the initial size of the yield surface indirectly
The hardening parameter a _ { 0 } can be defined indirectly by specifying e _ { 1 } , which is the intercept of the virgin consolidation line with the void ratio axis in the plot of void ratio, e, versus the logarithm of the effective pressure stress, (Figure 23.3.4–3).
line
| ln p | e, voids ratio |
|---|---|
| 0 | 0 |
| 1 | -1 |
| 2 | -2 |
| 3 | -3 |
| 4 | -4 |
| 5 | -5 |
| 6 | -6 |
| 7 | -7 |
| 8 | -8 |
| 9 | -9 |
| 10 | -10 |
| 11 | -11 |
| 12 | -12 |
| 13 | -13 |
| 14 | -14 |
| 15 | -15 |
| 16 | -16 |
| 17 | -17 |
| 18 | -18 |
| 19 | -19 |
| 20 | -20 |
Figure 23.3.4–3 Pure compression behavior for clay model.
If this method is used, a _ { 0 } is defined by
a _ {0} = \frac {1}{2} \exp \left(\frac {e _ {1} - e _ {0} - \kappa \ln p _ {0}}{\lambda - \kappa}\right),
where p _ { 0 } is the user-defined initial value of the equivalent hydrostatic pressure stress (see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). You define e _ { 1 } , \lambda , M , \beta , , and \kappa ; all the parameters except e _ { 1 } can be dependent on temperature and other predefined field variables. However, a _ { 0 } is a function only of the initial conditions; it will not change if temperatures and field variables change during the analysis.
Input File Usage: Use all of the following options:
\ast \mathrm { I N I T I A L ~ C O N D I T I O N S , ~ T Y P E = R A T I O }
*INITIAL CONDITIONS, TYPE=STRESS
*POROUS ELASTIC
*CLAY PLASTICITY, HARDENING=EXPONENTIAL, INTERCEPT=
Abaqus/CAE Usage: Use all of the following options:
Property module: material editor:
Mechanical→Elasticity→Porous Elastic
Mechanical→Plasticity→Clay Plasticity: Hardening:
Exponential, Intercept: e _ { 1 }
Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step
Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Stress for the Types for Selected Step
Piecewise linear form
If the piecewise linear form of the hardening rule is used, the user-defined relationship relates the yield stress in hydrostatic compression, p _ { c } , and, optionally, the yield stress in hydrostatic tension, p _ { t } , , to the corresponding volumetric plastic strain, \varepsilon _ { \mathrm { v o l } } ^ { p l } (Figure 23.3.4–4):
p _ {c} = p _ {c} (\varepsilon_ {\mathrm{vol}} ^ {p l}),
p _ {t} = p _ {t} (\varepsilon_ {\mathrm{vol}} ^ {p l}).
line
| ε_vol^pl | p_c | | -------- | --- | | -ε_vol^pl | 0 | | -ε_vol^pl + ε_vol^pl | p_c / 0 |
Figure 23.3.4–4 Typical piecewise linear clay hardening/softening curve.
The evolution parameter, a, is then given by
a = \frac {p _ {c} - p _ {t}}{(1 + \beta)}.
The volumetric plastic strain axis has an arbitrary origin: \varepsilon _ { \mathrm { v o l } } ^ { p l } | _ { 0 } is the position on this axis corresponding to the initial state of the material, thus defining the initial hydrostatic pressure in compression, p _ { c } | _ { 0 } . , and, optionally, in tension, p _ { t } | _ { 0 } and, hence, the initial yield surface size, a _ { 0 } . This relationship is defined in tabular form as clay hardening data. The range of values for which p _ { c } and p _ { t } is defined should be sufficient to include all values of equivalent pressure stress to which the material will be subjected during the analysis. Data for p _ { c } must be specified; data for p _ { t } is optional.
This form of the hardening law can be used in conjunction with either the linear elastic or, in Abaqus/Standard, the porous elastic material models. This is the only form of the hardening law supported in Abaqus/Explicit.
Input File Usage:
Use both of the following options to define the hardening behavior by providing the hydrostatic compression yield stress as a function of volumetric plastic strain:
*CLAY PLASTICITY, HARDENING=TABULAR
*CLAY HARDENING, TYPE=COMPRESSION (default)
Optionally, add the following option to define the tensile hardening behavior by providing the hydrostatic tension yield stress as a function of volumetric plastic strain:
*CLAY HARDENING, TYPE=TENSION
Abaqus/CAE Usage:
Property module: material editor: Mechanical→Plasticity→Clay Plasticity: Hardening: Tabular, Suboptions→Compressive Clay Hardening and/or Tensile Clay Hardening
Softening regularization
Granular materials often exhibit strain localization with increasing plastic deformation. Post-failure solutions from conventional finite element methods can be strongly mesh dependent. To mitigate the mesh dependency of the solutions, a regularization method is often used to introduce a micro-structural length scale ia crack band, he constitutive formulation. Let the characteristic length of the l _ { c } ^ { ( m ) } denote ent, and aracteristic width of a shear band orthe inelastic strain for the element. l _ { c } ^ { ( e ) } \varepsilon _ { \mathrm { v o l , e } } ^ { p l } Then the inelastic strain in the localization band, \varepsilon _ { \mathrm { v o l , m } } ^ { p l } , is defined to be
\varepsilon_ {\mathrm{vol,m}} ^ {p l} = \varepsilon_ {\mathrm{vol,e}} ^ {p l} \mathrm{min} \left(\left(\frac {l _ {c} ^ {(e)}}{l _ {c} ^ {(m)}}\right) ^ {n _ {r}}, f _ {m a x}\right),
where n _ { r } is a material parameter and f _ { m a x } is a positive number used for bounding the magnitude of regularization. This strain regularization method is valid only when the characteristic length of the element is greater than the width of the localization band; i.e., \bar { l } _ { c } ^ { ( e ) } \ge l _ { c } ^ { ( m ) } .
If softening regularization is included, it is applied to all hardening data (tension and compression) by default. You can optionally turn off softening regularization for a specific type of hardening.
Input File Usage: Use the following options to include softening regularization:
*CLAY PLASTICITY
*CLAY HARDENING, SR=ON (default)
*SOFTENING REGULARIZATION
Use the following option to turn off softening regularization:
*CLAY HARDENING, SR=OFF
Abaqus/CAE Usage: Use the following options to include softening regularization:
Property module: material editor: Mechanical→Plasticity→Clay Plasticity: Suboptions→Softening Regularization
Calibration
At least two experiments are required to calibrate the simplest version of the Cam-clay model: a hydrostatic compression test (an oedometer test is also acceptable) and a triaxial compression test (more than one triaxial test is useful for a more accurate calibration).
Hydrostatic compression tests
The hydrostatic compression test is performed by pressurizing the sample equally in all directions. The applied pressure and the volume change are recorded.
The onset of yielding in the hydrostatic compression test immediately provides the initial position of the yield surface, a _ { 0 } . The logarithmic bulk moduli, and \lambda , are determined from the hydrostatic compression experimental data by plotting the logarithm of pressure versus void ratio. The void ratio, e , is related to the measured volume change as
J = \exp (\varepsilon_ {v o l}) = \frac {1 + e}{1 + e _ {0}}.
The slope of the line obtained for the elastic regime is , and the slope in the inelastic range is . For a valid model \lambda > \kappa .
Triaxial tests
Triaxial compression experiments are performed using a standard triaxial machine where a fixed confining pressure is maintained while the differential stress is applied. Several tests covering the range of confining pressures of interest are usually performed. Again, the stress and strain in the direction of loading are recorded, together with the lateral strain so that the correct volume changes can be calibrated.
The triaxial compression tests allow the calibration of the yield parameters M and \beta . M is the ratio of the shear stress, { \pmb q } , to the pressure stress, { \pmb p } , at critical state and can be obtained from the stress values
when the material has become perfectly plastic (critical state). \beta represents the curvature of the cap part of the yield surface and can be calibrated from a number of triaxial tests at high confining pressures (on the “wet” side of critical state). \beta must be between 0.0 and 1.0.
To calibrate the parameter K, which controls the yield dependence on the third stress invariant, experimental results obtained from a true triaxial (cubical) test are necessary. These results are generally not available, and you may have to guess (the value of K is generally between 0.8 and 1.0) or ignore this effect.
To calculate the yield stress in hydrostatic tension, you can plot the data obtained from the triaxial compression tests on the p { - } q plane and extend the curve obtained from fitting these experimental data to the pressure axis in the tensile region.
Unloading measurements
Unloading measurements in hydrostatic and triaxial compression tests are useful to calibrate the elasticity, particularly in cases where the initial elastic region is not well defined. From these we can identify whether a constant shear modulus or a constant Poisson’s ratio should be used and what their values are.
Initial conditions
If an initial stress at a point is given (see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) such that the stress point lies outside the initially defined yield surface, Abaqus will try to adjust the initial position of the surface to make the stress point lie on it and issue a warning. However, if the yield stress in hydrostatic tension, p _ { t } , is zero and does not evolve with volumetric plastic strain and the stress point is such that the equivalent pressure stress, { \pmb p } , is negative, an error message will be issued and execution will be terminated.
The initial condition on volumetric plastic strain, \varepsilon _ { \mathrm { v o l } } ^ { p l } | _ { 0 } , can be defined in the definition of the clay plasticity model. Abaqus also allows a general method of specifying the initial plastic strain field on elements (see “Defining initial values of plastic strain” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). The volumetric plastic strain is then calculated as
\varepsilon_ {\mathrm{vol}} ^ {p l} = \varepsilon_ {\mathrm{vol}} ^ {p l} | _ {0} - t r \left(\varepsilon^ {p l}\right).
Elements
The clay plasticity model can be used with plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements in Abaqus. This model cannot be used with elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements).
Output
In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variable has special meaning for material points in the clay plasticity model:
PEEQ
Center of the yield surface, a.
23.3.5 CRUSHABLE FOAM PLASTICITY MODELS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Material library: overview,” Section 21.1.1
• “Inelastic behavior,” Section 23.1.1
• “Rate-dependent yield,” Section 23.2.3
• *CRUSHABLE FOAM
• *CRUSHABLE FOAM HARDENING
• *RATE DEPENDENT
• “Defining crushable foam plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
The crushable foam plasticity models:
• are intended for the analysis of crushable foams that are typically used as energy absorption structures;
• can be used to model crushable materials other than foams (such as balsa wood);
• are used to model the enhanced ability of a foam material to deform in compression due to cell wall buckling processes (it is assumed that the resulting deformation is not recoverable instantaneously and can, thus, be idealized as being plastic for short duration events);
• can be used to model the difference between a foam material’s compressive strength and its much smaller tensile bearing capacity resulting from cell wall breakage in tension;
• must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1);
• can be used when rate-dependent effects are important; and
• are intended to simulate material response under essentially monotonic loading.
Elastic and plastic behavior
The elastic part of the response is specified as described in “Linear elastic behavior,” Section 22.2.1. Only linear isotropic elasticity can be used.
For the plastic part of the behavior, the yield surface is a Mises circle in the deviatoric stress plane and an ellipse in the meridional (p–q) stress plane. Two hardening models are available: the volumetric hardening model, where the point on the yield ellipse in the meridional plane that represents hydrostatic tension loading is fixed and the evolution of the yield surface is driven by the volumetric compacting plastic strain, and the isotropic hardening model, where the yield ellipse is centered at the origin in the
p–q stress plane and evolves in a geometrically self-similar manner. This phenomenological isotropic model was originally developed for metallic foams by Deshpande and Fleck (2000).
The hardening curve must describe the uniaxial compression yield stress as a function of the corresponding plastic strain. In defining this dependence at finite strains, “true” (Cauchy) stress and logarithmic strain values should be given. Both models predict similar behavior for compression-dominated loading. However, for hydrostatic tension loading the volumetric hardening model assumes a perfectly plastic behavior, while the isotropic hardening model predicts the same behavior in both hydrostatic tension and hydrostatic compression.
Crushable foam model with volumetric hardening
The crushable foam model with volumetric hardening uses a yield surface with an elliptical dependence of deviatoric stress on pressure stress. It assumes that the evolution of the yield surface is controlled by the volumetric compacting plastic strain experienced by the material.
Yield surface
The yield surface for the volumetric hardening model is defined as
F = \sqrt {q ^ {2} + \alpha^ {2} (p - p _ {0}) ^ {2}} - B = 0,
where
| $p = -\frac{1}{3} \text{trace } \sigma$ | is the pressure stress, |
| $q = \sqrt{\frac{3}{2} \mathbf{S} : \mathbf{S}}$ | is the Mises stress, |
| $\mathbf{S} = \sigma + p \mathbf{I}$ | is the deviatoric stress, |
| $A$ | is the size of the (horizontal) $p$ -axis of the yield ellipse, |
| $B = \alpha \ A = \alpha \ \frac{p_c + p_t}{2}$ | is the size of the (vertical) $q$ -axis of the yield ellipse, |
| $\alpha = B/A$ | is the shape factor of the yield ellipse that defines the relative magnitude of the axes, |
| $p_0 = \frac{p_c - p_t}{2}$ | is the center of the yield ellipse on the $p$ -axis, |
| $p_t$ | is the strength of the material in hydrostatic tension, and |
| $p_c$ | is the yield stress in hydrostatic compression ( $p_c$ is always positive). |
The yield surface represents the Mises circle in the deviatoric stress plane and is an ellipse on the meridional stress plane, as depicted in Figure 23.3.5–1.