Read time: 15 minutes

Target audience: CAE Analysts and Team Leads, FEA Engineers, Researchers

Contact non-linearity is critical in many engineering applications, where two or more bodies come into contact, leading to changes in the load path and stress distribution. For example, in a gear assembly, the contact between the teeth of the gears involves complex interactions that can include sticking, sliding, and separation. Such interactions are inherently non-linear because the contact conditions change dynamically as the gears rotate, leading to varying contact areas and pressure distributions.

Convergence issues arise because the contact status (whether two surfaces are touching, separating, or sliding relative to each other) can change abruptly, leading to discontinuities in the stiffness matrix. This can make it challenging for the solver to find a stable solution within the specified tolerance.

To improve convergence when dealing with contact non-linearity, Abaqus offers various strategies such as adjusting the contact algorithm (e.g., switching between surface-to-surface and node-to-surface discretization), fine-tuning the convergence criteria, and using stabilization techniques. Properly setting up contact interactions and using appropriate solver settings are crucial for ensuring that the simulation converges to an accurate solution.

In this article, we will discuss on the contact interactions in Abaqus, the formulations and controls, thumb rules to follow for convergence, other tips and tricks, etc.

Contact Domain

Abaqus provides two algorithms for modelling contact interactions, the contact pair algorithm and the general contact algorithm. The general contact algorithm in Abaqus utilizes an automatic, global contact detection method that dynamically identifies and enforces contact interactions across all surfaces in the model. The contact pair algorithm in Abaqus employs a master-slave formulation to handle contact interactions between explicitly defined surface pairs. The choice between general contact and contact pairs is a trade-off between ease of defining contact and analysis performance. Both contact can be used together in the same analysis (general contact will ignore contact pair interactions).Contact pairs are defined as surface – to – surface contact in Abaqus/CAE. In Abaqus/Standard, general contact can be defined only in the initial step. This don’t apply for Abaqus/Explicit.

Contact Formulation and Controls

In Abaqus, contact formulation refers to the methods used to define and simulate interactions between surfaces in a finite element model. Contact problems are a type of nonlinearity often encountered in structural mechanics simulations where two or more bodies may come into contact, separate, or slide relative to each other. Contact formulations specify how these interactions are managed and resolved during the simulation.

Each contact formulation in Abaqus is determined by the choice of contact discretization, tracking approach, and surface role assignments. For general contact, these options are automatically selected, whereas for contact pairs, they must be chosen individually. Here are the general guidelines:

Surface Role Assignment

Main Surface vs. Secondary Surface:

1. The more refined surface should be the secondary surface.
2. The stiffer body should be the main surface.
3. The main surface should experience rapidly changing active contact regions to minimize changes in contact status.

Tracking Approach

Represents the possible path along which a secondary node can slide on the main surface:

1. Finite Sliding: Captures arbitrarily large sliding and rotations, providing a true representation of the main surface.
2. Small Sliding: Captures small relative sliding between surfaces, using a planar representation of the main surface to reduce computational cost.

Contact Discretization

Node-to-Surface:

• Contact is enforced between a node and surface facets local to the node.
• The secondary surface is treated as a collection of points.
• Slave nodes are constrained not to penetrate the master surface, though master nodes can penetrate the slave surface.
• The contact direction is based on the normal of the master surface.

Surface-to-Surface:

1. Contact is enforced in a weighted sense, between the slave node and a larger number of master surface facets surrounding it.
2. Both secondary and main surfaces are treated as continuous surfaces.
3. Offers many advantages over node-to-surface and should be used when possible.
4. Not applicable if a node-based surface is used in the contact pair definition.

Constraint Enforcement Method

Constraint Enforcement Method refers to the technique used to enforce contact constraints between interacting surfaces during a simulation. These methods are critical in ensuring that the physical conditions of contact, such as no penetration, friction, and relative motion, are accurately represented and adhered to throughout the simulation.

There are three contact constraint enforcement methods in Abaqus/Standard:

1. Direct Method: Strictly enforces the pressure-overclosure behaviour per constraint without approximation or augmentation iterations.
2. Penalty Method: Uses a stiff approximation of hard contact.
3. Augmented Lagrange Method: Similar to the penalty method but includes augmentation iterations to improve approximation accuracy.

Default Constraint Enforcement Methods

1. Penalty Method: Default for finite-sliding, surface-to-surface contact with a hard pressure-overclosure relationship. Used by default for general contact with both small- and finite-sliding tracking approaches.
2. Augmented Lagrange Method: Default for three-dimensional self-contact with node-to-surface discretization and a hard pressure-overclosure relationship.
3. Direct Method: Default in all other cases.

We can tabulate the features as:

Convergence Criteria

In Abaqus, contact convergence refers to the process of ensuring that the contact conditions (such as no penetration or frictional sliding) are satisfied accurately throughout the simulation. Achieving convergence in contact problems can be challenging due to the highly nonlinear nature of contact interactions, where surfaces may repeatedly open (separate) and close (come into contact) during the analysis. Closures and openings of contact surfaces induce ‘Severe Discontinuity Iteration’ which cut back the iteration increment.

In Abaqus, for finite-sliding surface-to-surface contact, a tolerance of 5.0% is applied, while for other types of contact, a stricter tolerance of 0.1% is used to ensure convergence without global stabilization control.

Depending on the problem, Abaqus performs multiple checks viz. convergence checks for severe discontinuity iteration, convergence check for force and moment etc. for any analysis to start solving error-free. An analysis approaches solution if and only if these criteria are fulfilled. Given below are examples of two such convergence criteria which Abaqus uses:

1. Force Residual Criterion

The force residual criterion checks whether the residual contact forces are sufficiently small for the simulation to be considered converged. By default, Abaqus/Standard requires that the maximum residual (out-of-balance force) is less than or equal to 0.5% of the time averaged force 𝑞 ̃ in the model to accept an iteration as converged:

2. Displacement Criterion

The displacement criterion ensures that the change in displacement during iterations is within an acceptable range. Convergence is accepted if the largest correction to the solution, 𝒄, is also small compared to the largest incremental change in the corresponding solution variable, ∆𝒖_𝑚𝑎𝑥. By default, this is limited to less than or equal to 1% of the maximum solution increment. It can be expressed as:

Common mistakes, measures and best practices

Basic modelling errors are the most frequent causes of convergence issues. Listed below are some common modelling mistakes:

1. Incorrect inputs such as boundary conditions, contact definitions, and kinematic constraints.
2. Inconsistent unit systems used within the model.
3. Mesh issues like distorted element shapes and improperly connected nodes.
4. Insufficient contact surfaces:
   1. Abaqus contact is efficient, so there’s usually no need to restrict surface extents.
5. Unresolved initial penetrations:
   1. Either eliminate them or manage them correctly in the load history.
   2. Or adjust initial clearances using the INTERFERENCE FIT feature to resolve overlaps or gaps
6. Using small-sliding in a finite-sliding application.
7. Opting for direct enforcement when penalty enforcement is sufficient.

We need to know how to minimize the number of mistakes. Following are a few measures for minimizing errors:

1. Utilize a checklist of best modelling practices tailored to your application. This checklist serves as a systematic guide to verify various aspects when constructing or debugging a model, helping you prevent more complex convergence issues.
2. Remember to perform a data check.
3. Every partial solution has value. Use your intuition and understanding of the expected behavior to compare it against what is actually occurring in the partial solution.
4. If friction is included, ensure that the friction coefficients are realistic and not excessively high, as this can hinder convergence.
5. Define master surface such that it extends beyond the slave surface.
6. Double check normals on contact surfaces. Contact normal direction is based on the master surface. So, if normal direction is critical choose the master surface accordingly.
7. Double check edges on contact surfaces. Eliminate cracks on master surface.
8. Increase the maximum number of allowed severe discontinuity iterations (DEFAULT=50) if the severe discontinuities are decreasing.
9. Create an initial step that is very small for the purpose of initiating contact
10. For severely discontinuous behavior such as frictional sliding, apply the discontinuous control. This could increase run time, especially for problems that are not severely discontinuous.

CONTROLS, ANALYSIS=DISCONTINUOUS

The convergence of contact problems depends on various problem specific factors like the mesh density, contact formulation, constraint enforcement method, frictional conditions, and the complexity of the contact interaction itself. Discussed above are only a few among the best practices.

Abaqus has a unique feature named ‘Job Diagnostics’ ,which provides real-time insights into the analysis process, helping users monitor solution progress, identify issues like convergence problems, and optimize performance during simulations. We will be discussing this exclusively in our upcoming blog.

Please reach out to us if you need more assistance in the understanding or execution of the discussed topics.