Deformation Plasticity

In one dimension the model is

where

$\sigma$

is the stress;

$\epsilon$

is the strain;

E

is Young's modulus (defined as the slope of the stress-strain curve at zero stress);

$\alpha$

is the “yield” offset;

${\sigma }^0$

is the yield stress, in the sense that, when $\sigma ={\sigma }^0$, $\epsilon =\left(1+\alpha \right){\sigma }^0/E$; and

n

is the hardening exponent for the “plastic” (nonlinear) term: $n>1$.

The material behavior described by this model is nonlinear at all stress levels, but for commonly used values of the hardening exponent ($n\sim 5$ or more) the nonlinearity becomes significant only at stress magnitudes approaching or exceeding ${\sigma }^0$.

The one-dimensional model is generalized to multiaxial stress states using Hooke's law for the linear term and the Mises stress potential and associated flow law for the nonlinear term:

where

$\mathit{\epsilon }$

is the strain tensor,

$\mathit{\sigma }$

is the stress tensor,

$p=-\frac{1}{3}\mathit{\sigma }:\mathbf{I}$

is the equivalent hydrostatic stress,

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

is the Mises equivalent stress,

$\mathbf{S}=\mathit{\sigma }+p\mathbf{I}$

is the stress deviator, and

$\nu$

is the Poisson's ratio.

The linear part of the behavior can be compressible or incompressible, depending on the value of the Poisson's ratio, but the nonlinear part of the behavior is incompressible (because the flow is normal to the Mises stress potential). The model is described in detail in Deformation plasticity.

You specify the parameters E, $\nu$, ${\sigma }^0$, n, and $\alpha$ directly. They can be defined as a tabular function of temperature.

DEFORMATION PLASTICITY

Property module: material editor: MechanicalDeformation Plasticity

The deformation plasticity model is most commonly applied in static loading with small-displacement analysis, where the fully plastic solution must be developed in a part of the model. Generally, the load is ramped on until all points in the region being monitored satisfy the condition that the “plastic strain” dominates and, hence, exhibit fully plastic behavior, which is defined as

or

You can specify the name of a particular element set to be monitored in a static analysis step for fully plastic behavior. The step will end when the solutions at all constitutive calculation points in the element set are fully plastic, when the maximum number of increments specified for the step is reached, or when the time period specified for the static step is exceeded, whichever comes first.

STATIC, FULLY PLASTIC=ElsetName

Step module: Create Step: General: Static, General: Other: Stop when region region is fully plastic.