The Hertz contact problem

Because of symmetry, the contact problem can be modeled as a deformable cylinder being pressed against a flat, rigid surface. Therefore, two contact surfaces are required: one (the slave surface in Abaqus/Standard) on the deformable cylinder and the other (the master surface in Abaqus/Standard) on the rigid body.

For illustrative purposes several different techniques are used to define the contacting surface pairs. The slave surface is defined by (1) grouping the free faces of elements in an element set that includes all elements in the region that potentially will come into contact (Abaqus defines the faces automatically), (2) specifying the faces of the elements (or the element sets) in the contact region, or (3) identifying the nodes on the deformable body in the contact region that may come into contact. The master surface is defined by (1) specifying the faces of the rigid elements (or element sets) used to define the rigid body or (2) defining the rigid surface with a surface definition and rigid body constraint. Any combination of these techniques can be used together.

By default, Abaqus uses a finite-sliding contact formulation for modeling the interaction between contact pairs. The contacting surfaces undergo negligible sliding relative to each other, which makes this problem a candidate for the small-sliding contact formulation. For a discussion of small- versus finite-sliding contact, see Contact formulations in Abaqus/Standard or Contact formulations for contact pairs in Abaqus/Explicit.

The surface contact formulation in Abaqus/Standard gives an accurate solution for the contact area and pressure distribution between the surfaces because of the choice of integration scheme used. Irons and Ahmad (1980) suggest a Gaussian integration rule for calculating self-consistent areas for surface boundary condition problems, which for second-order elements can lead to oscillating results for the pressure distribution on the surface. Oden and Kikuchi explain why this behavior occurs (1980) and present the remedy of using Simpson's integration rule instead. This technique is used in Abaqus/Standard, and no oscillations in the pressure distribution are found.

The default contact pair formulation in the normal direction in Abaqus/Standard is hard contact, which gives strict enforcement of contact constraints. Some standard analyses of this problem are conducted with both hard and augmented Lagrangian contact to demonstrate that the default penalty stiffness chosen by the code does not affect stress results significantly. The hard and augmented Lagrangian contact algorithms are described in Contact constraint enforcement methods in Abaqus/Standard.

The default contact pair formulation in Abaqus/Explicit is kinematic contact, which gives strict enforcement of contact constraints. (Note: the small-sliding contact option mentioned previously is available only with kinematic contact.) The explicit dynamic analyses of this problem are conducted with both kinematic and penalty contact to demonstrate that the penetration characteristic of the penalty method can affect stress results significantly in problems with displacement-controlled loading and purely elastic response. The kinematic and penalty contact algorithms are described in Contact constraint enforcement methods in Abaqus/Explicit.

This type of contact problem is very suitable for analysis using the substructuring technique in Abaqus/Standard, since the only nonlinearity in the problem is the contact condition, which is quite local. The cylinder can be defined as a substructure and, thus, reduced to a small number of retained degrees of freedom on the surface where contact may occur or where boundary conditions may be changed. During the iterative solution for contact only these external degrees of freedom on the substructure appear in the equations, thus substantially reducing the cost per iteration. Once the local nonlinearity has been resolved, the solution in the cylinder is recovered as a purely linear response to the known displacements at these retained degrees of freedom. This technique is particularly effective in this case because the rigid surface is flat and there is no friction on the surface; therefore, only the displacement component normal to the surface needs to be retained in the nonlinear iterations.

All information that is relevant to the substructure generation must be given within the substructure generation step, including the degrees of freedom that will be retained. The substructure creation and usage cannot be included in the same input file. Only one substructure can be generated per input file. Any number of unit load cases can be defined for the substructure by using a substructure load case. Although this feature is not necessary in this example, it is used in one of the input files for verification purposes.

Substructures are introduced into an analysis model using elements, where the element number and nodes are defined for each usage of each substructure. Node and element numbers within a substructure and at the usage level are independent—the same node and element numbers can be reused in different substructures and on the usage level. It is also possible to refer to a substructure several times if the structure has identical sections. Thus, once a substructure has been created, it is used just as a standard element type.

A simple dynamic example is created in Abaqus/Standard by giving the cylinder a uniform initial velocity with the contact conditions all open. This represents the experiment of dropping the cylinder onto a rigid, flat floor under a gravity field.

The impact algorithm used in Abaqus/Standard for dynamic contact is based on the assumption that, when any contact occurs, the total momentum of the bodies remains unchanged while the points that are contacting will acquire the same velocity instantaneously. In this example the cylinder contacts a rigid surface, which implies that each contacting point will suddenly have zero vertical velocity. This means that a compressive stress wave will emanate from the contacting point and will travel back into the cylinder. After some time this will cause the cylinder to rebound.

It is important to understand that the Abaqus/Standard dynamic contact algorithm is a “locally perfectly plastic impact” algorithm, as described above, which gives excellent results when it is used correctly. However, it is readily seen that, if the cylinder were modeled as a concentrated mass, with one vertical degree of freedom, the algorithm would imply that the cylinder stops instantaneously when it hits the rigid surface. In reality neither the cylinder nor the surface it hits are rigid: stress waves are started in each. Enough of this detail must be modeled for the results to be meaningful. In this example the cylinder itself is modeled in reasonable detail to capture at least the overall dynamic behavior. If the physical problem from which the example has been developed is that of two cylinders with equal and opposite velocities, this solution is probably useful. If the physical problem is that of a single cylinder hitting a flat surface, it may be necessary to include some elements to model the material below the surface (and the propagation of energy into that domain), unless that material is very dense so that this propagation can be neglected.