This section gives a general overview of how to work with contact regions. Many of the adjustments described here can be made at different stages of the analysis - such as modifying individual contact settings after an initial solution - to improve accuracy or convergence through iterative solving. As a general guideline, Ansys recommends starting with Program-Controlled and default settings, especially for users who are new to contact modeling. When fine-tuning a solution, it's best to adjust one setup variable at a time to better understand its impact. Detailed descriptions of all steps mentioned here can be found at the links provided.
Tip: To learn more about the workflow for modeling contact, check out the following resources.
Ansys Innovation Space Courses
Fundamental Topics in Contact – Discusses contact concepts and how to model contact in the Mechanical application.
Tutorials
Prepare to define contact regions
Understand how parts are intended to interact to guide your contact type selection. Do they touch? How might they move: stick, slide, separate, come together, or stay bonded? Is friction expected between sliding parts?
Ensure your geometry is clean with no unnecessary small features or gaps that could cause meshing issues or unintended contact regions. Merge coincident faces, repair gaps and overlaps, and simplify complex curves wherever possible. A cleaner and simpler geometry results in more reliable contact definitions and calculations.
Import Geometry – the Mechanical application Automatically detects contact pairs based on a defined tolerance. Always review automatically generated contact pairs and manually modify them as needed. You can also define contact pairs manually.
Use named selections for faces or edges to facilitate scoping contact regions and later re-selection if needed.
Generate the mesh. Use Contact Sizing to automatically apply an element size to both the contact and the target side, aiming for a consistent mesh density across the interface. If needed, refine the mesh on contact surfaces to have at least 3-5 elements across the width of a contact region. Examine mesh quality in contact regions using mesh matrics (see the Mesh Metric section of the Meshing User's Guide). For more details, see Troubleshooting Contact Settings.
Set or adjust contact region options
Designate the contact and target surfaces for each contact pair. Generally, the contact side should be the body with softer material properties, a finer mesh, or a more convex or complex geometry. The target side should be the stiffer material, coarser mesh, and flatter or simpler geometry.
Choose the contact type. If your model is a complex assembly, begin with simpler contact types like bonded or no separation to establish stability. Then, transition to more complex types like frictional as needed to more accurately capture the physics.
Use the Contact Tool to diagnose contact issues. Check for problems and initial status first to quickly spot errors before solving.
Fine-tune contact settings
Set the Pinball Radius just large enough to encompass all likely contact surfaces without causing unwanted detections. Only target surface elements within the pinball radius are included in contact calculations. If the initial gap between surfaces is larger than the default pinball radius, you may need to increase it. If there are multiple parts close together, you may have to reduce it to avoid unwanted contact detection.
Use Interface Treatment options like “Adjust to Touch” to close small initial gaps and minimize penetrations, improving convergence behavior.
Choose the Formulation used for contact calculations. Augmented Lagrange is the default formulation for non-bonded interaction because it provides a good balance between accuracy and convergence stability. If the contact type is bonded, the default is MPC. However, you may want to change to a different formulation, depending on the requirements of your simulation. Generally, there is a tradeoff between accuracy and computational expense.
Set Update Stiffness to iteratively adjust contact stiffness and improve convergence for nonlinear analyses with convergence issues.
Solve, refine mesh or fine-tune contact settings, and verify results
Use contact result trackers to monitor contact results during solution.
Use the Contact Tool after generating a solution to analyze contact behavior. If your analysis failed to converge or showed unexpected behavior, the contact tool can help identify if contact interactions were the cause. Use it to generate contour plots of contact status, penetration, gap, or contact pressure and forces across contact surfaces at different time or load steps.
Check for erratic pressure distributions and refine the mesh to improve resolution and obtain a smoother result.
Analyze the impact of mesh refinement on contact results by progressively refining the mesh at critical contact interfaces and high-stress regions. Plot key results against mesh density and identify when results stabilize, indicating that further mesh refinement is unnecessary.
Verify that results match expectations. Adjust the model and contact settings and re-solve as needed until contact results converge to the expected values.