#### Command list

• Input handling
• Solution control and techniques
• Output
• Mesh commands
• Nodes and connectivity
• Material properties
• Initial conditions
• Boundary conditions
• Contact and tied interfaces
• Rigid bodies
• Connectors
• Parameters and functions
• Geometries
• Sets
• Coordinate system
• Particle
• SPH

### PROP_DAMAGE_CL_REGULARIZE

###### Material properties
Attention: This command is in the beta stage and the format may change over time.
*PROP_DAMAGE_CL_REGULARIZE
"Optional title"
did, erode, noic
$W_c$, $R_0$, $D_0$, $c$

#### Parameter definition

VariableDescription
did Unique damage identification number
erode Element erosion flag
options:
0 $\rightarrow$ failed element is not eroded
1 $\rightarrow$ failed element is eroded
2 $\rightarrow$ node splitting at failure (crack plane orthogonal to max principal strain)
3 $\rightarrow$ node splitting at failure (crack plane orthogonal max principal stress)
noic Flag to turn off cracking along interface between different materials
options:
0 $\rightarrow$ material interface cracks are allowed
1 $\rightarrow$ material interface cracks are not allowed
$W_c$ Damage parameter
$R_0$ Threshold element size to wall thickness ratio
$D_0$ Threshold damage for activation of regularization
$c$ Regularization exponent

#### Description

This is a Cockcroft-Latham based failure criterion. The damage evolution is scaled (accelerated) if the mesh is considered too coarse for an accurate description of the local post necking behaviour.

The material will fail once the damage parameter, $D$, has evolved from 0 to 1.

$\displaystyle{ D = \frac{1}{W_c} \int_0^{\epsilon_{eff}^p} sf \cdot \mathrm{max}(0,\sigma_1) \mathrm{d}\epsilon_{eff}^p}$

$\sigma_1$ is the maximum principal stress and $\epsilon_{eff}^p$ is the effective plastic strain. $sf$ is the scale factor for the damage evolution. $sf>1$ if damage has exceeded a threshold value $D_0$ and if the element size divided by the local component wall thickness is larger than $R_0$.

$\displaystyle{ sf = \left\{ \begin{array}{ccc} 1 & : & D \leq D_0 \\ \mathrm{max}\left( 1, \frac{R}{R_0} \right)^c & : & D > D_0 \end{array} \right. }$

The element size is defined differently, depending on element type. Hexahedra elements have three size values, one for each parametric direction. Sizes and directions are stored in a tensor $\mathbf Q$. The element size to wall thickness ratio $R$ is defined by projecting $\mathbf Q$ in the direction of the maximum principal stress $\mathbf{\lambda}_1$.

$\displaystyle{ R = \frac{\vert\vert \mathbf{Q} \cdot \mathbf{\lambda}_1 \vert\vert}{t_c} }$

Here $t_c$ is the local component wall thickness. It is computed automatically by the solver. Tetrahedra elements are assigned a scalar value for the element size. This scalar value is the average element height in the four different parametric directions.

Model parameters can be defined from a simple tensile specimen test. $W_c$ is a ductility parameter for an element grid that is so fine that the results have converged. $R_0$ is the ratio below which the results have converged. $D_0$ is typically the damage at onset of diffuse necking. That is, the damage level in uni-axial tension where $\sigma(\epsilon_{eff}^p) = \mathrm{d}\sigma / \mathrm{d}\epsilon_{eff}^p$. $c$ is a dimensionless tuning parameter. Typical values for both $R_0$ and $c$ are $\approx 0.5$.