Soft Rock Plasticity Model

The model is based on the yield surface (Figure 1)

where

$p=-\frac{1}{3}\mathrm{trace}\sigma$

is the equivalent pressure stress;

$q=\sqrt{\frac{3}{2}S:S}$

is the Mises equivalent stress;

$p_c$

is the yield stress in hydrostatic compression;

$p_c^0$

is the initial value of $p_c$;

$p_t$

is the yield stress in hydrostatic tension;

$\beta$

is the friction angle;

$n_y$

is the material parameter that controls the shape of the yield surface in the $p$-$q$ plane (Figure 1); and

$e_0$

is the eccentricity parameter.

Yield surface of the soft rock plasticity model in the $p$-$q$ plane.

$g\left(\sigma \right)$ captures the transition of the yield surface in the $\mathrm{\Pi }$-plane from a rounded-triangular shape to a circular shape with an increase in pressure and is defined as follows (Figure 2):

where $r={(\frac{9}{2}S:S\cdot S)}^{\frac{1}{3}}$ is the third stress invariant; and $\alpha$, $f_0$, and $f_1$ are material parameters.

Abaqus requires that the function $f\left(p\right)$ should satisfy the following conditions to ensure that the yield surface remains convex (Bigoni and Piccolroaz, 2004).

Yield surface of the soft rock plasticity model in the $\mathrm{\Pi }$ plane (Crook, et al., 2006).

Plastic flow is based on a nonassociated rule with iso-surfaces of the flow potential being used for the calculation of plastic strain rate. The flow potential surface is defined by the following function:

where $\psi$ is the dilation angle and all other constants are same as in the expression for the yield surface.

The hardening law has a piecewise linear form. 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, ${\epsilon }_{\mathrm{vol}}^{pl}$ (Figure 4):

Typical piecewise linear soft rock hardening/softening curve.

The volumetric plastic strain axis has an arbitrary origin: ${{\epsilon }_{\mathrm{vol}}^{pl}|}_0$ 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, ${p_t|}_0$. This relationship is defined in tabular form as soft rock hardening data. The range of values for which $p_c$ and $p_t$ are 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.

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 into the constitutive formulation. Let $l_c^{\left(m\right)}$ denote the characteristic width of a shear band or a crack band, $l_c^{\left(e\right)}$ denote the characteristic length of the element, and ${\epsilon }_{\mathrm{vol},e}^{pl}$ denote the inelastic strain for the element. Then the inelastic strain in the localization band, ${\epsilon }_{\mathrm{vol},m}^{pl}$, is defined to be

where $n_r$ is a material parameter and $f_{max}$ 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., $l_c^{\left(e\right)}\ge l_c^{\left(m\right)}$.

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.

If an initial stress at a point is given (see Defining Initial Stresses) 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, p, is negative, Abaqus issues an error message and execution is terminated.

The initial condition on volumetric plastic strain, ${{\epsilon }_{\mathrm{vol}}^{pl}|}_0$ , can be defined in the definition of the soft rock plasticity model. Abaqus also allows a general method of specifying the initial plastic strain field on elements (see Defining Initial Values of Plastic Strain). The volumetric plastic strain is then calculated as