The computational model follows from the material properties described in the name.i2 file, optionally the name.DAT file, and from the input parameters in the name.iP file:
IP KREST NLC NCYC KMOD KCRP KLARG KCNT KTPR KURHS 0 $L_1$ $L_2$ $\dots$ $L_\mathtt{NLC}$ RP 10*0 $t_1$ $t_2$ $\dots$ $t_\mathtt{NLC}$
The plasticity model is selected using the KMOD key:
$=0$ … elasticity (default)
$=1$ … von Mises model
$=2$ … generalized associated model
$=3$ … generalized non-associated model
$=4$ … Feigenbaum-Dafalias model
The material properties specified in the name.i2 file must correspond to the selected model.
The time sequence $t_i$ is not specified.
The creep model is selected using the KCRP key:
$=0$ … no creep (default)
$=1$ … PMD model
$=2xx$ … Bina model
$=2$ … Norton model
$=3$ … Norton-Bailey model
$=4$ … Time Hardening model
$=5$ … MPC Project Omega model
$=6$ … Kloc model
while the key $\mathtt{KMOD}=0$.
For $\mathtt{KCRP}=1$, the relation $\dot\varepsilon_c=\dot\varepsilon_c(\sigma_e,\varepsilon_c,T)$ is specified in the name.i2 file.
For $\mathtt{KCRP}>1$, the description of the material’s creep properties is read from the name.DAT file.
On the RP line, times $t_i$ (in hours) are assigned to all load cases $L_i$, see Load case sequence.
The procedure follows the previous paragraphs. The key $\mathtt{KMOD}>0$ selecting the plastic model and the key $\mathtt{KCRP}>0$ selecting the creep model are specified, and the time sequence $t_i$ is specified simultaneously.
If $t_{i+1}=t_i$, the transition from $L_i$ to $L_{i+1}$ occurs abruptly, with creep excluded. It is advisable to run the combined computation only after the separate problems have been debugged.
It is activated with the KLARG key:
$=0$ … geometrically linear (default)
$=1$ … total Lagrangian formulation (large displacements, small strains)
$=2$ … updated Lagrangian formulation (large displacements, small strains)
$=3$ … logarithmic formulation (large displacements, large strains)
$=4$ … co-rotational formulation
$=5$ … Mooney-Rivlin hyperelastic model
$=6$ … Ogden hyperelastic model
Key KURHS
It is activated by the KCNT key when $\mathtt{KCNT}=1$.
In the name.i2 file, pairs of contact surfaces must be specified as SV batches with $\mathtt{KQT}=10$ and $11$, $12$ and $13$, etc.
In the name.iL file, the penalty value $\mathtt{PENAL}$ must be set. For contact between steel materials, $\mathtt{PENAL}\approx10^{13}$ is chosen. If the problem does not converge, it is recommended to decrease the value of $\mathtt{PENAL}$ or to split the load step into several substeps using the parameter $\mathtt{NSUBI}$. If the contact results are not optimal, it is recommended to increase the value of $\mathtt{PENAL}$. It is also possible to start with a lower value of $\mathtt{PENAL}$ and increase it gradually.
Bodies in contact must be regularly supported. The support stiffness chosen for the “free” body in the contact direction must be such that it does not affect the solution.