A stiffness relationship between two bodies must be established for contact to
occur. Without a contact stiffness, bodies will pass through one another. The
relationship is generated through an 'elastic spring' that is put between the two
bodies, where the contact force is equal to the product of the contact stiffness (k)
and the penetration (δ). The amount of penetration (δ), or incompatibility,
between the two bodies is therefore dependent on the stiffness k. Ideally, there
should be no penetration, but this implies that k =
, which will lead to numerical instabilities. The value of k that
is used depends on the relative stiffness of the bodies in contact. In the ANSYS LS-DYNA
program, the contact stiffness is determined by the following relationships:
| Area = area of contact segment |
| K = bulk modulus of contacted element |
| fs = penalty factor (0.1 by default) |
In almost all cases, the contact stiffness parameter automatically determined by
the ANSYS LS-DYNA program will provide excellent results. The contact stiffness, however,
can be changed for all contact surfaces by entering a new value for the penalty
factor, fs, with the SFSI field of the
EDCONTACT command. In practice, increasing the value of
SFSI above 0.1 will typically cause instabilities to
occur.
If the contact stresses of contact and target surfaces are badly mismatched due to
large differences in material properties or element size, then instabilities or
unrealistic behavior may arise. This can be avoided by adjusting the penalty
stiffness option, PENO of the
EDCONTACT command. For example, by setting
PENO to 1, both the contact and target stiffnesses
are taken into account and the least stresses of the surfaces are used.
If there are very large differences in the contact stiffnesses, the program scales them to closer values, overwriting user input for the scale factor.
Together with the related mass, a closed contact element is a spring-mass system for which the current stability criterion yields a critical time step in the explicit analysis. The program reports the least one of the time steps with a message. If the actual time step size used is larger than the one listed in this message, then you should scale the penalty value of the offending surface with the EDCONTACT command or reduce the actual time step size with the EDCTS command. If the difference between the two time steps is small, this approach may not be necessary.
In addition to using the SFI and
PENO options of the EDCONTACT
command to control penalty stiffness between contact surfaces, individual contact
(slave) and target (master) stiffness values can be adjusted using the
EDCMORE command. Unlike the EDCONTACT
command, which is applied to all contact definitions within a model, the
EDCMORE command allows the specification of additional
contact parameters for a single contact surface specification. The
Val1 and Val2 fields of
the EDCMORE command can be used to adjust the slave and master
penalty stiffnesses in cases where the default contact stiffness determined by the
ANSYS LS-DYNA program is found to be inadequate.