An important parameter in the settings for the Contact node is the penalty factor. When running into convergence problems, check the penalty factor settings and consider changing the current value. It is used by all contact methods, but its interpretation differs:
The default value for the penalty factor is based on a characteristic stiffness. The default is an “equivalent” Young’s modulus (
Eequ) of the material on the destination side. For linear elastic isotropic materials,
Eequ is the actual Young’s modulus. For other types of materials,
Eequ is defined by an estimate of a similar stiffness at zero strain. For materials that are user defined or in other ways nonstandard (for example, anisotropic with large differences in stiffness in different directions),
Eequ might need to be replaced with another estimate.
If, during the iterations, a contact problem comes into a state where it is far from the converged solution, it is unlikely that the solution will ever converge. In such a case, much computing time can be spent before the maximum number of iterations is reached, and the solver makes an attempt with a smaller time or parameter step. To speed up this process, you can select the Trigger cutback check box when using the augmented Lagrangian method. You can then enter a logical expression that will force the solver to immediately abandon the iterations and try a smaller step when fulfilled. Such an expression can, for example, be a maximum displacement (like
solid.disp > 5[mm]), based on what is physically realizable for the structure. The expression is evaluated in all points on the boundary, but you can also use a global value, like an average or a maximum.
When the source and destination boundaries are curved, the discretization introduced by the meshing may lead to small variations in the computed distance between the source and destination boundaries, even though the geometrical shapes of the two objects are ideal. When modeling for example a shrinkage fit, this effect can cause significant fluctuations in the contact pressure. If you select Force zero initial gap, the computed distance from destination to source will be adjusted by the initial gap distance detected by the contact search. Positive gap distances smaller than the tolerance
Δgap are adjusted to be zero. By default,
Δgap is set to
Inf, which means that all gaps and overclosures detected are adjusted to be zero. This adjustment can be combined with an offset. The offset is applied to the adjusted gap value.
For a discretization other than Linear, the lumped solver is no longer optimal for the contact pressure update when using a segregated solution method. In such cases, a standard segregated step should be used. The default solver generation takes this into account, but if you later modify the discretization, you should update the solver sequence.
The weak equations set up by the Contact node and its subnodes typically involve discontinuous functions. These originate from the contact mapping, where the source and destination meshes, in most cases, are nonconforming. The default quadrature used in the numerical integration of these integrals is equal to the order used by the displacement field. For a quadratic displacement field, this means integration order equal to four.
In the Advanced section of the Contact node, there is an option to specify the type of
Jacobian contribution from the contact equations. The default
Automatic option will choose a suitable setting depending on the mapping method used by the contact pair. However, if controlled manually the
Nonsymmetric option is the preferable choice especially when the source boundaries undergoes large deformations, since it is more robust. The
Symmetric option can be attractive for large models since it preserves the symmetry of the global stiffness matrix, as long as no other features cause it to be nonsymmetric. This can decrease the solution time and memory requirements when solving the model.
When adding a Friction node, you can specify a constitutive model (friction model) for the behavior of the tangential contact. This model includes conditions for switching between sticking and sliding, as well as computation of the current friction forces.
This section provides similar settings as described in Penalty Factor of the
Contact node, but the penalty factor is here used to regularize the stick constraint. However, the same considerations for how to set an appropriate value apply. For convenience, it is also possible to utilize the penalty factor set in the parent contact node.
The Slip Velocity node facilitates a simplified form of slip friction modeling, which can be used in the case that the direction and speed of the sliding is known. The same friction models as for the
Friction node are available. However, it is here assumed that the tangential contact is in a sliding state, and that the slip velocity is known beforehand. The latter is supplied to the feature as a user input in the local coordinate system.
When adhesion is active, it is possible to break the bond between the source and destination boundaries by adding a Decohesion subnode to
Contact. To model decohesion, it is required that an
Adhesion node is present and active in the same parent
Contact node.
Two alternative CZM are available. The Displacement-based damage models defines damage growth as a function of a mixed mode displacement quantity. It comes with several traction separation laws that associate the onset of damage with the peak strength of the interface. For some of them, it is possible to choose between different mixed mode failure criteria. The
Energy-based damage models define damage growth as a function of the stored undamaged elastic energy density of the interface. It also comes with several different traction separation laws. However, these are more general and define the onset of damage at an arbitrary elastic energy density. In principle, you can define the model so that damage initiates immediately during loading of the adhesive layer, that is for zero energy density. The strength of the interface is then determined by the critical energy release rate and the shape of the damage evolution function. In this way, the energy-based damage models can be viewed as a regularization of linear elastic fracture mechanics.
For time-dependent studies, it is possible regularize the CZM with a viscous delay by selecting Delayed damage in the
Regularization list. This option adds a delay to the release of energy, which is controlled by the
Characteristic time τ. Using this option can help to suppress the instability of the solution when the step size or mesh size is too large. If the viscous damage is used to stabilize a rate-independent decohesion problem, the value of
τ must be chosen with care. As a rule of thumb,
τ should at least be one or two orders of magnitude smaller than the expected time step.
By adding a Wear subnode to a
Contact node, it is possible to model adhesive or abrasive wear of the material when the contacting boundaries are sliding along each other. Since wear involves solving evolution equations, the
Wear node only adds a contribution for time-dependent studies. Moreover, wear is typically a slow process where dynamic effects are of small significance. You should, therefore, usually set
Structural transient behavior to
Quasistatic in the
Structural Transient Behavior section of the physics interface settings.
The most general technique to model the removal of material during the wear process relies on the deformed geometry concept. When selecting the Deformed geometry formulation, the wear feature adds a (hidden)
Deforming Domain feature that controls the material frame through an adaptive mesh smoothing. The wear, as computed in the
Wear node is fed as a (hidden)
Prescribed Normal Mesh Displacement boundary condition to the deforming domain, and thus describes the actual removal of material from the geometry. When using this formulation, you must be aware that the adaptive mesh means that state variables stored in Gauss points, for example plastic strains or creep strains, will not represent the same material points all the time. Whether or not this effect is acceptable must be judged on a case-by-case basis. Unless the amount of material that is removed is large, or gradients are strong, this is mainly an issue close to the boundary where material is removed by the wear process.
The slip velocity used for the wear computation can be obtained from either a Friction node or a
Slip Velocity node, so one of these two nodes should be present and active under the same
Contact parent node. For the
Generalized Archard wear model, this is a requirement. In most cases, the orientation of the slip velocity is known a priori in a wear analysis, in which case
Slip Velocity provides the more efficient solution.
In general, modeling wear on the destination side is slightly more accurate, since it is there that the contact pressure and slip velocity are originally computed. When modeling wear on the source side, these quantities are mapped from the destination boundary. Multiple Wear nodes under the same
Contact node contributes with each other, which means that it is possible to model wear on both source and destination simultaneously. However, adding multiple wear contributions to either source or destination may give unphysical results. On the source side it is possible to also use the
Rigid Material material model; this is not permitted on the destination due to general restrictions of the
Contact node.