Contact Modeling in Ansys Mechanical for Beginners

Contacts Overview

Contact modeling in Ansys Mechanical is a critical aspect of simulating how different parts of a structure interact under various conditions. It involves defining how surfaces come into contact, whether they touch, slide, or separate. Ansys Mechanical offers a wide range of contact options to accurately model these interactions, including bonded, frictional, and no-separation contacts. Each option provides unique control over the behavior of the interacting surfaces, allowing engineers to tailor the simulation to reflect real-world scenarios. The choice of contact type, along with fine-tuning parameters like stiffness, damping, and contact detection methods, plays a pivotal role in ensuring accurate and reliable simulation results. Properly implementing these options requires a deep understanding of the physical behavior of materials and the specific demands of the simulation, making contact modeling a sophisticated yet powerful tool in the design and analysis process.

There are several different types of contact types available in Mechanical:

• Bonded: In bonded contacts, faces or edges within the pinball region experience no penetration, separation, or sliding. This means that the connected surfaces behave as if they are permanently fused, ensuring a fixed relationship between them throughout the analysis, regardless of applied loads or deformations. The pinball region helps define the area where this rigid bonding behavior is enforced.
  
  
• No Separation: In no separation contact, similar to bonded contact, there is no penetration or separation between the contacting faces. However, unlike bonded contact, frictionless sliding is allowed in the direction tangent to the surfaces. This means the faces remain in constant contact but can freely slide along one another without resistance, making it ideal for scenarios where parts are in continuous contact but not rigidly fixed.
  
  
• Frictionless: In frictionless contact, penetration is not allowed, but the contacting surfaces are free to slide against each other and separate without any resistance. This type of contact is ideal for scenarios where surfaces interact without any frictional forces, allowing unrestricted relative motion while ensuring they do not pass through each other. It’s useful for simulating smooth interactions between parts that are not expected to remain in constant contact.
  
  
• Rough: In rough contact, penetration is prevented, and instead of allowing sliding, the surfaces exhibit sticking behavior. This means that once the surfaces touch, they become locked together and cannot move or slide relative to each other in any direction. However, they can still separate when needed. This sticking behavior contrasts with sliding, where surfaces can move freely along one another without restriction. Rough contact is useful in situations where parts must remain fixed in position upon contact but are allowed to detach when necessary.
  
  
• Frictional: In frictional contact, sliding is permitted with resistance proportional to a user-defined coefficient of friction, while the surfaces can separate freely without any resistance. This option usually provides the most general and physically representative behavior.
  

The surfaces on one side of a contact region are referred to as the Contact side (Red), and the surfaces on the other side are referred to as the Target side (Blue). These Contact and Target surfaces each get their own Contact and Target Elements associated with them.

The Contact and Target elements are what allow us to enforce the contact through the idea of Contact Detection Points. The Contact Detection Points cannot pass through the target face. These Contact Detection Points can either be the integration points or the nodes (can be controlled by the user). Therefore, a higher mesh density will yield more Contact Detection Points. Additionally, to further refine the accuracy of contact interactions, the concept of the pinball radius is introduced. 

The pinball radius is used to define a spherical region around each contact detection point where contact forces and interactions are calculated. This radius helps to smooth and approximate the contact force distribution, ensuring more accurate and stable contact interactions. The pinball radius is automatically calculated based on the size of the geometry. However, it can also be manually adjusted in the details of each contact definition. By adjusting the pinball radius, you can improve the precision of the contact modeling, especially in complex geometries or where detailed force distribution is important.

• In cases where one body has a more complex geometry and the other is relatively flat or simple, the complex surface should be assigned as the contact side, while the simpler, flatter surface should be set as the target. This setup helps the solver better detect and manage the points of interaction, as the complex surface will likely make contact at multiple points, while the simpler surface provides a stable reference for contact detection.
• When simulating contact between two bodies with different materials, the softer material should be assigned to the "Contact" side, while the stiffer material should be designated as the target side. This approach ensures that the contact is more accurately represented, as the softer material will deform more, allowing for better interaction with the stiffer, less deformable surface.
• Set the target side to the surface expected to experience less deformation, as the contact side should typically be assigned to the more flexible or deformable body to enhance contact resolution.

In reality, when two bodies are in physical contact, they do not penetrate or intersect each other. To accurately simulate this physical interaction, the program must establish a clear relationship between the surfaces to prevent them from passing through one another throughout the analysis. This process, known as enforcing contact compatibility, ensures that the interaction between the bodies reflects real-world behavior. To achieve this, Mechanical offers a variety of contact formulations that manage how surfaces interact and maintain compatibility at the contact interface, allowing for accurate and reliable simulation of complex contact scenarios.

Contact Algorithms in Ansys Mechanical

Penalty Based Methods

In nonlinear solid body contact analysis, penalty-based methods such as Pure Penalty and Augmented Lagrange formulations are widely utilized. These methods compute the contact force, F_Normal, as the product of contact stiffness, k_Normal, and penetration, X_Penetration. Essentially, a higher contact stiffness results in less penetration, indicating a stiffer and more resistant contact interaction.

While theoretically, an infinite contact stiffness k_Normal would eliminate all penetration, achieving this is numerically impractical. Instead, penalty-based methods allow for a small amount of penetration, assuming it is negligible. This means that while some minor penetration may be present, it is minimized to a degree where it does not significantly impact the accuracy of the simulation. By adjusting the stiffness to a high enough value, these methods ensure that the contact forces are calculated with sufficient precision, closely approximating real-world interactions despite the allowable minimal penetration.

Normal stiffness, represented by the factor FKN, adjusts the code-calculated stiffness previously explained. For Bonded and No Separation behaviors, FKN is set to 10.0 by default, while for all other behaviors, it is 1.0. In bending-dominated situations where convergence issues arise, a smaller value, such as FKN = 0.01 or 0.1, can be beneficial. This factor applies exclusively to penalty-based formulations like Pure Penalty or Augmented Lagrange. 

Normal stiffness is automatically updated at each iteration, based on the current mean stress of the underlying elements and the allowable penetration. If bisections occur early in the analysis, the normal contact stiffness is reduced by a program-determined factor with each bisection. Additionally, the tangential contact stiffness is adjusted at each iteration according to the current contact pressure, coefficient of friction (μ), and allowable slip (SLTO).

The formulations for the Augmented Lagrange and Pure Penalty contact algorithms are shown below

Pure Penalty:

F_Normal=k_Normal∗X_Penetration

Augmented Lagrange

F_Normal=k_Normal∗X_Penetration+λ

Note, because of the extra λ term, the Augmented Lagrange method is less sensitive to the magnitude of the contact stiffness. This added robustness makes Augmented Lagrange the default contact algorithm in Ansys Mechanical, as it provides reliable convergence and accuracy across various contact scenarios.

Lagrangian Contact Formulation

Another available option is the Normal Lagrange formulation, which differs from penalty-based methods by introducing an additional degree of freedom (DOF) in the form of contact pressure to enforce contact compatibility. Instead of calculating contact force as a function of contact stiffness and penetration, this method explicitly solves for contact force (contact pressure) as an extra DOF. This formulation ensures zero or nearly zero penetration without requiring a normal contact stiffness, resulting in no elastic slip. However, it necessitates the use of the Direct Solver, which can increase computational demands. A common issue with the Normal Lagrange method is "chattering," where the contact status oscillates between open and closed states because no penetration is allowed. This step-function behavior can make convergence more challenging. Allowing slight penetration can mitigate this issue by smoothing the transition between contact states, thereby improving convergence.

As a review, Pure Penalty and Augmented Lagrange are both penalty-based formulations used in Ansys Mechanical for contact modeling. Pure Penalty calculates contact force based on contact stiffness and penetration, while Augmented Lagrange enhances this approach by adding a Lagrange multiplier to improve convergence. However, both methods may allow small penetrations, which are acceptable as long as they do not affect the accuracy of the results. On the other hand, the Normal Lagrange formulation is not penalty-based; instead, it introduces an extra degree of freedom in the form of contact pressure to enforce zero or nearly zero penetration, eliminating the need for contact stiffness. While this method can lead to more accurate results in terms of penetration, it requires the Direct Solver and may face convergence challenges due to the potential for "chattering." The table below outlines the advantages and disadvantages of each method in Ansys Mechanical.

MPC Formulation

Another method for handling Bonded and No Separation contact types is the Multi-Point Constraint (MPC) approach, which differs from penalty-based or Lagrangian multiplier methods. MPC offers a straightforward and efficient way to model contact interactions by using internal constraint equations to "tie" the displacements of the contacting surfaces together. This approach circumvents the need for penalty or Lagrange multiplier methods, effectively managing large deformations and providing linear contact behavior in small-deflection cases. It is particularly advantageous when facing convergence issues, serving as an alternative to adjusting contact stiffness. Moreover, MPC does not introduce artificial stiffness in cases with gaps between curved surfaces, although Joints might be considered as an alternative. It is well-suited for contact between shell-to-solid, shell-to-shell, and beam-to-shell interfaces. However, caution is necessary, as MPC is very sensitive to over-constraint and should be avoided when other contact regions or boundary conditions share the same topology.

The Contact Tool

In finite element analysis, contacts between parts are enforced based on the model's mesh, which often introduces complexities during preprocessing. While CAD geometry is perfectly defined, the mesh discretization process can result in small gaps or initial penetrations between contacting surfaces due to the approximation of continuous surfaces by elements. These mesh-induced inaccuracies are crucial to address, as they affect how contact interactions are modeled and can impact the accuracy and stability of simulations. The Contact Tool in Ansys Mechanical provides essential preprocessing capabilities to manage these challenges, ensuring that contact regions are properly aligned and contact conditions are well-defined before running the simulation.

The Contact Tool’s preprocessing capabilities allow users to evaluate and adjust contact settings before solving the model. It provides an overview of all contact pairs, indicating whether they are open, and helping to identify mesh-related issues such as gaps or initial penetrations. Based on this information, users can adjust key contact properties like stiffness, friction coefficients, and allowable penetration tolerances to ensure accurate contact enforcement and improve solution convergence. In addition, the tool offers contact stabilization options to handle small gaps and reduce instability in the model. These preprocessing features are vital for fine-tuning the contact behavior, especially in complex assemblies where misalignment from the mesh could otherwise cause convergence difficulties or inaccurate results.

Additionally, the Contact Tool is also very helpful for post-processing. In the post-processing stage, the Contact Tool offers robust visualization and analysis features to help users interpret contact behavior. By providing a range of detailed metrics, it enables users to gain deeper insights into how contact pairs interact under load and how their conditions evolve throughout the simulation.

One of the primary metrics is Gap, which measures the distance between the nearest nodes in a contact pair. This is crucial for understanding whether contact regions are properly engaged or if there are unintended separations.

Penetration is another important metric that quantifies the overlap between nodes in a contact pair, giving users insight into areas where surfaces may be unintentionally intruding on one another, often due to mesh inaccuracies or physical deformation. It's crucial to keep contact penetration minimal compared to local displacements, as penetration is physically unrealistic. If penetration is too high, potential solutions include increasing the contact stiffness, lowering the penetration tolerance, or switching the contact formulation to Normal Lagrange. These adjustments help improve the accuracy and reliability of the simulation by reducing unrealistic penetrations.

Pressure is a metric that represents the ratio of the normal load to the actual contact area, providing a clear indication of how the load is distributed across the contact surfaces. This is essential for ensuring that the contact forces are within acceptable limits and that the model is performing as expected.

Frictional Stress sums the in-plane stress components within the contact pair, offering a detailed view of the shear forces acting at the interface, which is especially relevant in models involving frictional contact.

One of the more complex metrics is Sliding Distance, which tracks the cumulative sliding displacement between contact surfaces. This value accounts for both elastic slip and frictional slip. Elastic slip occurs when two surfaces pressed together experience slight reversible motion before full sliding begins, as the surfaces initially resist sliding due to friction. This behavior is influenced by the tangential stiffness of the contact pair—the stiffer the material, the smaller the elastic slip before sliding occurs. Elastic slip is important for understanding how much energy is temporarily stored in the system before sliding takes place, and it can be monitored using the Contact Result Tracker for precise analysis.

The Fluid Pressure metric measures the penetration pressure between surfaces in contact, which is particularly useful in surface-to-surface contact models involving fluids or lubricants.

Finally, the Status of the contact pair can be monitored to understand the overall interaction between surfaces. The tool classifies the contact status as "Far" when the nodes are farther apart than the pinball radius, indicating no contact; "Near" when the nodes are within the pinball radius, suggesting potential contact engagement; "Sliding" when the sum of tangential forces exceeds the frictional forces, indicating relative motion between the surfaces; and "Sticking" when the tangential forces are less than the frictional forces, implying no relative motion and that the surfaces are adhering to each other.

These metrics allow for a comprehensive understanding of contact behavior in simulations, aiding in the refinement of models to ensure accuracy and reliability in real-world applications.