Interactions

Wear calculations in a steady-state transport procedure require non-local calculations involving averaging local wear rates at all nodes belonging to individual streamlines due to the mixed Eulerian/Lagrangian framework the steady-state transport procedure is built on.

In earlier releases, the only option available was to use an adaptive meshing user subroutine. The user subroutine approach can be rather cumbersome because you have to carefully define node sets for the individual streamlines and code the wear rate calculations all within the user subroutine to drive mesh motion for adaptive meshing. For complex geometries like the tire model shown here, such an approach might be impractical.

The animation below shows a passenger car tire rolling at 70 km/h and accumulating wear over a distance of 58,880 km. The 3D tire model is generated from periodic symmetric-model generation of a wedge with repeating tread configurations. Surface wear properties are specified on the tread surface. The wear distance contours show that a maximum wear distance of 3.96 mm is accumulated, which is approximately 63% of the tread depth. The animation also shows that the contact footprint expands as wear accumulates and the wear rate slows down as the contact foot print expands due to redistribution of contact stresses. In the wear calculations shown here, wear distances are treated as offsets for contact penetration calculations and the nodal locations of the underlying elements due to wear are not modified.

In earlier releases, Abaqus/Standard approximately represented beams in contact calculations with nodes and edges of the beam mesh having a radius encompassing the actual beam cross-section.

The new default beam representation for contact uses an automatically generated mesh of contact faces, nodes, and edges close to the exterior of noncircular beam cross-sections. Some surface thickness is assigned automatically, which provides an accurate contact representation of the beam geometry with some rounding of edges.

The animation below shows a hexagonal cross-section beam inserted into the end of a part resembling tweezers and then rotated. Both parts are modeled with beam elements. In this example, the beam elements of the tweezers have a rectangular cross-section. The response of the tweezers to the insertion and rotation of the other part is intuitive. Realistic representation of the beam contact surfaces is crucial to the accuracy of this simulation.

You can revert to the previous default behavior, as discussed in *CONTACT CONTROLS ASSIGNMENT.

The animation below shows two views of an Abaqus/Explicit beating heart simulation. As the heart contracts in this simulation, it remains in contact with, and slides relative to, the pericardium (membrane sac). Despite tensile contact stress developing, it represents the effects of fluid within the pericardial cavity (although this fluid is not modeled directly in this simulation). The ability for contact to resist separation as sliding occurs is crucial to obtaining realistic behavior in this simulation. In earlier releases, you could only specify no-separation behavior in combination with “rough” friction for general contact in Abaqus/Explicit.

However, “no separation” contact behavior in the normal direction does not prevent loss of contact for general contact in Abaqus/Explicit when one surface slides off another surface, as shown in the animation below.

The default contact surface representation for a part modeled with shell elements is a double-sided shell reference surface that considers the shell thickness and shell offset. The example below shows two bodies meshed with shell elements in contact. The perimeter of one part is in contact with the shell element faces of the other part. The left image shows no thickness rendering, while the right image includes thickness rendering.

Now, you can specify that Abaqus/Standard internally generate surface elements near shell perimeters, as shown in the example below. Surface elements are created right at the shell perimeter, with an additional row of elements extending inward toward the shell interior, ensuring a continuous reference surface representation of the shell. These surface elements can be removed from display in the postprocessor to return to a view such as in the left image above.

In many contact wear workflows, surface wear accumulates over thousands of physical wear cycles. It is often prohibitively expensive to simulate each physical wear cycle, so each simulated cycle typically represents a "batch" of multiple similar physical cycles. The animation below shows a wear simulation over five simulated cycles that represent 110,000 physical wear cycles in total. Step cycling allows the "batch size" to evolve during the simulation based on the maximum incremental wear distance in the simulated cycle. The number of simulated cycles is often not known before running such a simulation. For each simulated cycle, the user-specified wear coefficients are scaled by the current batch size.

The animation shows the wear distance accumulation on the slider and the bottom block as the slider repeatedly moves back and forth. In this example, the simulated wear cycle is modeled in two steps:

• In “Step-2” the slider moves to the right and returns to the center.
• In “Step-3” the slider moves to the left and returns to the center.

These two steps are repeated using step cycling until a threshold wear distance exceeds 0.012 or reaches a cap of 10 repetitions of the simulated wear cycle. The batch size for scaling the wear coefficients has an initial value of 10,000 and a cap of 25,000. The target incremental wear distance is 0.006 accumulated per simulated cycle. The batch size for the next simulated wear cycle is internally calculated so that the estimated maximum wear accumulation is less than the target value of 0.006 while respecting the batch size cap. The example simulation reaches the threshold wear distance in 5 simulated cycles. The batch size for the initial cycle is 10,000 based on user input. For the subsequent cycles, the batch sizes are calculated to be 25,000 (the cap value) while maintaining the maximum wear accumulated in each simulated cycle to be less than 0.006.

In earlier releases of Abaqus/Explicit, similar internally generated meshes could be used for simulations but they were not available for postprocessing. The following images compare plots of contact forces and contact opening distances on beam elements to plots on internally generated surface-element representations of the beams. Plots on surface elements show variations over the surfaces, similar to plots that would occur on the outer surface of a solid body, whereas plots based on beam elements are limited in that they represent a single value at each axial location.

Furthermore, some rounding of edges in the contact representation to improve numerics is achieved by offsetting nodes of internally generated surface elements inward and adding a small corresponding contact thickness. This contact thickness is not represented in plots, so the parts appear a bit smaller than the actual size.

Figure 1. Tweezers beam model contact force vector plot across versions (beam rendering not available for vector plots).

Figure 2. Tweezers beam model contact opening distance output in previous versions (beam rendering shown for Abaqus 2024).

The capability to simulate wear in general contact in Abaqus/Explicit was introduced in 2024 FD02. In that release Abaqus/Explicit treated the evolution of wear exclusively by considering nodal wear distances in contact penetration calculations. Now you can use arbitrary Lagrangian-Eulerian (ALE) adaptive meshing together with wear in Abaqus/Explicit to account for surface wear (erosion) in part geometries while preserving mesh quality, even for wear distances on the order of element dimensions.

The simulation on the left below shows the preexisting behavior (wear distances accounted for with offsets in contact penetration calculations). The simulation on the right demonstrates the use of ALE in the context of wear modeling. Similar wear accumulation occurs for both models, but it is much easier to interpret the wear configurations with ALE. Most wear occurs on the smaller block in this model, with the maximum wear distance being approximately half of the original element depth. In this example, ALE mesh smoothing effectively provides a realistic representation of the evolving part geometry while maintaining good mesh quality.

Enhancements to cohesive contact in Abaqus/Explicit make cohesive contact a preferred alternative to surface-based tie constraints for modeling permanent, stiff bonds in more cases (for example, models where ties result in large implicit constraint systems or when you require interfacial traction results across connected surfaces).

Performance improvements for cohesive contact are most noticeable for models with a large fraction of nodes participating in cohesive contact. For example, simulations for the models shown in Figure 3 and Figure 4 with permanent, stiff cohesive contact bonds have sped up by 13% and 12%, respectively, compared to simulations in 2024 FD01.

Figure 3. Two plates modeled with solid elements bonded together with permanent, stiff cohesive contact.

Figure 4. Two plates modeled with shell elements (shown with shell thickness rendering) bonded together with permanent, stiff cohesive contact.

A second enhancement allows the default cohesive stiffness to be scaled by existing options to scale the contact penalty stiffness in Abaqus/Explicit. Cohesive contact, like other contact constraints, has a finite bond stiffness. You can assign the bond stiffness or allow it to take on the same contact penalty stiffness that would be in effect to resist penetrations for regular contact behavior, as discussed in Contact Cohesive Behavior. You can use a scale factor to increase the cohesive stiffness relative to the default value.

Figure 5 shows two blocks bonded together with uniform tensile (negative pressure) loading of 1 × 10⁶ N/m² applied to the top face of the top block while the bottom of the bottom block is constrained. Loading is smoothly ramped on and damping is included to obtain a quasi-static solution.

Figure 5. Model characteristics.

Figure 6 shows that the axial stress results correspond to the expected uniaxial stress solution regardless of details of how the bond is modeled.

Figure 6. Vertical stress (S11) for three model variants.

Figure 7 shows that some additional displacement occurs when a penalty stiffness is used to enforce the bond. Increasing the penalty stiffness via a scale factor is a convenient mechanism to control the resistance to relative motion across the bond.

Figure 7. Vertical displacement (U1) for four model variants.

The mesh is quite coarse in this example. The default penalty stiffness would be greater with a more refined mesh. Increasing the penalty stiffness tends to decrease the time increment size in Abaqus/Explicit unless contact mass scaling is used (see Mass Scaling to Account for Contact Stiffness).

Alternatively, you can directly specify cohesive stiffness components, as discussed in Cohesive Stiffness. When you specify the cohesive stiffness, the penalty stiffness scale factor has no effect.