Interference fits, both intentional and unintentional, are common in engineering design and finite element analysis (FEA). These occur when two components overlap or come into contact, creating stress and deformation that must be carefully analyzed to ensure proper functionality. Intentional interference, such as a press fit between a shaft and a bearing or a shrink fit for securing metal rings, is often used to create high-strength, reliable assemblies. However, unintended interferences can arise due to manufacturing tolerances, misaligned components, or geometric adjustments introduced during the meshing process, leading to unexpected challenges in simulation.
In FEA, resolving interference fits requires careful consideration of contact definitions, mesh quality, and solver settings to handle the nonlinearities introduced by these overlaps. CAD models represent mathematically perfect geometries, but when meshed, the discretization process can slightly alter the model, introducing small overlaps or gaps that were not present in the original design. As the simulation progresses, mesh deformation and contact interactions can further complicate convergence, impacting the stability and accuracy of results.
Ansys Mechanical provides powerful tools to address these challenges, including advanced contact algorithms, contact control methods, and multistep analysis capabilities. These features enable engineers to accurately simulate interference fits, capturing critical stress distributions, deformation patterns, and contact pressures that influence the behavior of an assembly.
Understanding Interference Fits in FEA
Interference fits in simulations can occur for several reasons:
Intentional Interferences
Designed overlaps in CAD models—such as press fits, shrink fits, or interference-based mechanical assemblies—ensure a secure connection between components. These fits rely on material deformation to generate high contact pressures, providing frictional resistance or sealing.
Unintentional Interferences
Differences between CAD representation and FEA mesh can create unintended overlaps or gaps. While CAD models depict idealized geometry, the meshing process discretizes the model, sometimes altering the dimensions slightly. Additionally, manufacturing tolerances introduce real-world deviations that may not be accounted for in an idealized CAD model, leading to unexpected contact conditions in simulations.
This blog explores effective strategies for resolving interference fits in Ansys Mechanical. We will cover available contact algorithms, the role of mesh quality, the impact of normal stiffness in the contact methods, and techniques for managing contact interactions. Additionally, we’ll discuss how to use multistep analysis and manage mesh deformation to overcome convergence challenges and achieve accurate, reliable results. Whether you're designing a critical assembly or troubleshooting unexpected overlaps, these insights will help you navigate interference fits with confidence.
The Contact Tool
In Ansys Mechanical, the Contact Tool helps manage contact interactions that arise due to mesh discretization. This tool provides a comprehensive overview of all contact pairs, helping users identify and address potential issues before solving. When interference fits occur, whether intentional or unintentional, the contact tool can be used to garner more information about each contact in your model. It can be inserted into the Connections branch of your workflow tree and the initial information can be processed once the mesh has been generated. It is a very useful tool for reviewing any potentially problematic contacts before running your model.
Contact Algorithms in Ansys Mechanical
Ansys Mechanical provides several contact algorithms to handle interference fits effectively. Choosing the right algorithm significantly impacts the stability and accuracy of the solution. Below is a short summary of the available methods. For a more in depth review on both contact and the contact tool, please refer to our blog Contact Modeling in Ansys Mechanical for Beginners.
The Pure Penalty Method calculates contact forces based on penetration depth and a stiffness factor (kn). It is computationally efficient but requires careful tuning of kn to prevent excessive penetration or solver instability. Lowering kn improves convergence but may reduce accuracy, while increasing kn limits penetration but can cause convergence difficulties.
The Augmented Lagrange Method builds on the pure penalty method by introducing an additional Lagrangian multiplier term that iteratively adjusts the contact stiffness factor (kn) to minimize penetration. This hybrid approach enhances accuracy in contact force calculations while maintaining a balance between stability and computational efficiency. The Augmented Lagrange method is less sensitive to adjustments in kn compared to the pure penalty method. Since the additional Lagrangian term actively corrects for penetration, the solver does not rely solely on kn to enforce contact constraints. This makes it a more robust choice in many applications, as small variations in kn will not drastically affect convergence or accuracy. However, this method does involve additional iterations, which can slightly increase solution times.
The Multi-Point Constraint (MPC) Method strictly enforces contact constraints by linking nodes between contacting surfaces. This method is well-suited for rigid-body motions or small deformations but is less flexible when handling significant nonlinearities like large deformations or sliding.
The Frictionless Contact Algorithm models contact interactions based purely on normal forces, ignoring tangential resistance. It is computationally efficient and useful when friction is negligible, such as in preliminary analyses or simplified studies.
The Frictional Contact Algorithm accounts for both normal and tangential interactions, simulating realistic sliding resistance. This method captures real-world contact behavior but increases computational complexity and requires careful solver settings.
By default, Ansys Mechanical uses the Augmented Lagrange Method because it provides a balance between accuracy and convergence. It adapts well to most contact scenarios, including interference fits, and minimizes penetration without compromising solution stability, making it a robust choice for general-purpose analyses.
Tips for Resolving Interference Fits - Multistep Analysis and Contact Controls
For interference fits, a good starting point is switching the contact algorithm to the pure penalty method and reducing the normal stiffness (kn). This is especially useful when significant initial interference exists or when the force convergence criteria are high. Lowering kn allows the solver to tolerate greater penetration in early iterations, helping to stabilize the model.
For complex interference scenarios or highly nonlinear problems, leveraging a multistep analysis with contact controls can significantly improve stability and accuracy. The Contact Step Control tool in Ansys Mechanical allows you to dynamically modify contact behavior at specific time steps throughout the analysis. Once inserted into the Mechanical interface (as shown below), you can select any defined contact, specify the desired time step, and determine whether the contact should be active (alive) or inactive (dead) at that stage. This flexibility enables you to switch between different contact algorithms as needed, ensuring the most appropriate method is applied to effectively resolve interference fits and other evolving contact conditions in your model.
Once the interference is resolved and the solution progresses, the stiffness can be gradually increased, or the algorithm can be switched back to Augmented Lagrange for improved accuracy. This stepwise approach enhances convergence and prevents solver instability caused by abrupt changes in contact forces.
These controls can be used to switch the contact algorithm between analysis steps or to make incremental adjustments to parameters like contact stiffness (kn). For example, gradually increasing kn throughout the simulation improves accuracy as the interference is resolved and the contact pressure stabilizes.
Other effective techniques include:
Mesh Deformation and Convergence Instabilities
During the analysis, mesh deformation can impact solver performance and create convergence challenges. Mesh quality and element size play a crucial role in resolving interference fits successfully.
If elements in the interference region are too large, they may not accurately capture localized deformations and stress concentrations, leading to unrealistic results or convergence issues. Conversely, poor-quality elements—such as highly distorted tetrahedral elements—can introduce numerical instability, making it difficult for the solver to track the evolution of contact forces and deformations.
To improve convergence, consider the following:
Conclusion
Successfully resolving interference fits in Ansys Mechanical requires a combination of careful preprocessing, appropriate contact settings, and solver adjustments. Ensuring high-quality mesh generation, selecting the right contact algorithm, and fine-tuning solution controls can significantly improve convergence and accuracy. By following these best practices, engineers can minimize solver instability, reduce computational effort, and achieve reliable results. The following guidelines, summarized from the information above, will help optimize your workflow and improve the resolution of interference fits in FEA simulations.