Contact In FEA - What Is It And How Should It Be Implemented?
Contacts are an essential part of model definitions in a multibody analysis. These problems are commonly encountered in engineering scenarios such as assemblies with moving parts like seals, gears, pins, punches, rollers, bearings etc. Once contact occurs between two bodies, they can interact in different ways. Bonded, friction, frictionless, no separation, rough contact are a few examples of how contact interactions can progress. Because of the relative motion and change in contact conditions between the moving parts, the stiffness of the whole assembly changes, introducing nonlinearity into the analysis.
The surfaces between the two bodies involved in the contact interactions are distinguished as primary and secondary surfaces in the Abaqus FEA software. Each contact pair is composed of a primary and secondary surface.
Primary surface: Contact behavior is defined and controlled typically by the primary surface. It is the surface that initiates contact with another body and is responsible for generating contact forces and reactions. It is defined in the section of the input file where contact properties and behavior are specified.
Secondary surface: This interacts with the primary surface and experiences contact forces and reactions. The secondary surface is not responsible for initiating contact, but it merely responds to the contact behavior defined on the respective primary surface.
The contact between multiple components in a mechanical assembly can transpire in multiple ways as demonstrated in the figure below:
Surface to surface
Surface to edge
Edge to edge
Vertex to surface
When setting up contact problems in Abaqus, you'll typically need to define contact pairs (unless using the general contact algorithm), specify contact behavior (friction, separation, etc.), assign appropriate contact properties, and apply appropriate boundary conditions to simulate the desired contact behavior accurately. In Abaqus/Standard, we have three ways for defining contact:
General Contact Algorithm
General contact is specified as a part of model definition, which allows simple contact definitions with very few restrictions on the surfaces involved. This uses robust tracking algorithms to ensure proper contact conditions are enforced efficiently. It has a simple interface and allows for highly automated contact definition. However, it is computationally very expensive because of this. Self-contact and multibody contacts can be specified using a single definition.
The simplest way to define contact is to specify self-contact for a default unnamed, all-inclusive surface which is automatically defined by Abaqus. This way, all the regions that can potentially come into contact in an assembly are enveloped into the general contact domain. This default domain encompasses all exterior element faces and all analytical rigid surfaces and it is defined only once at the beginning of the analysis. The computational performance and robustness of this algorithm can be improved by just adding specific contact inclusions and exclusions at assembly level in the general contact domain.
Specified using pairwise contact interactions for certain contact surfaces. The contact pair is defined by indicating the surfaces that may come into contact during an analysis. Be aware that extending these contact surfaces to include surface faces and nodes that may never come into contact results in significant memory usage, which increases the computational cost. Every contact pair must be specified with an appropriate interaction property. This may result in efficient analysis if there are only a few contacting pairs in the model.
This is rarely used, and the contact is specified though elements or slide lines. Abaqus has a library of contact elements such as GAPCYL, GAPSPHER, CAXAn and DGAP, which can be used based on the model requirements. Heat flow in a discontinuous piping system is an example where contact elements should be utilized.
Common Difficulties While Modeling Contact
It is important to note that contact problems can be computationally intensive, especially for large-scale simulations with many contact interactions. Proper meshing, convergence criteria, and solution techniques should be considered to ensure accurate and efficient simulations. Some of the things to think about while modelling contact are briefly explained here.
This occurs when the two contacting surfaces overlap in the model at the beginning of analysis. This can be caused by poor CAD modelling, mesh discretization or intended overlap for interference fits as shown in figure below.
Initial overclosure can be resolved in two ways: with strain-free adjustment or with interference fits. In strain free adjustment, the nodes on the secondary surface are moved until the overclosure is removed without any stresses and strains generated in the elements. This is appropriate for unintended overlaps occurring due to CAD modeling and mesh discretization.
The initial overlap can also be treated as interference fit for contacting surfaces. The interference between the surface pair is gradually removed in the first step of the analysis resulting in realistic stresses and strains in the deformed geometries. This can be specified only in the first step of a Standard analysis in Abaqus.
This occurs when there is gap between the contacting surfaces as the beginning of the analysis. an initial gap can lead to rigid body motion of components during the analysis, which will, in turn, lead to convergence issues. Numerical singularity warning messages and very large displacements indicate the unconstrained motion in a static analysis. Large initial gaps should be avoided whenever possible in the model and small initial gaps can be removed using strain free adjustments of the elements. If large initial gaps are inevitable in the model, the contact stabilization option, which introduces artificial damping in the analysis, can be used.
Poor mesh quality can lead to roughly defined surfaces causing undesirable behaviors such as excessive penetration, unexpected opening, and inaccurate force application between the contacting surfaces. This can cause nonconvergence and termination of the analysis.
When the meshes on the primary and secondary surfaces do not match, the primary nodes can grossly penetrate the secondary surface without any resistance as shown in the above figure. This problem can be alleviated by refining the mesh on secondary surfaces. Also, using surface-to-surface contact can resist the penetration of primary nodes into the secondary surface. Coarser meshes on two contact surfaces with dissimilar curvatures can also lead to contact interactions occurring entirely within the bounds of a single element as shown in the figure below. This will lead to unreliable and unrealistic results as the primary node penetrates the secondary surface until it encounters a secondary node. Refining the mesh to spread the contact interaction over multiple element faces can help while modelling contact surfaces with dissimilar curvatures. However, unless perfectly matching meshes are used, local oscillations may be observed in the contact stresses and pressures, even in the refined models.
Contacts are an essential part of model definition in FEA, which can lead to nonlinearity and convergence issues. These problems can be computationally expensive for large-scale simulations with multiple contact interactions. Hence, Proper meshing, convergence criteria, and solution techniques should be considered to ensure accurate and efficient simulations. Hopefully this article has given a good overview of different ways of defining contact and overcoming commonly observed issues in a multibody analysis.
We’re always here to help, so if you have questions about contact in your models, or just FEA in general, don’t hesitate to reach out!