A few applications for contact analysis
But simulating contact is not always simple, even with cutting-edge software. Many parameters must be specified to properly simulate contact including the type of contact, stiffness, tolerance, interaction distance, time-step size, and more. And although the latest FEA software selects most of these parameters, some models benefit from user adjustments.
How you set up a contact analysis can help quickly and easily get a converged and accurate solution. But beware: Less-than-optimal setups can make the software run longer than necessary, compromise results, and even fail.
WHAT CAN GO WRONG
A few common difficulties encountered in contact analysis include:
Nonsmooth surfaces. When surfaces in contact have irregular edges, their roughness can cause convergence problems. For instance, the software will repeatedly try to solve the contact problem by adjusting parameters until satisfactory values are found, thus lengthening the analysis run-time. Nonsmooth surfaces can also lead to inaccurate results. For example, fitting a small cylinder inside a larger one should produce a uniform stress contour along the contact surface. But insufficiently smooth surfaces can produce stress variations.
A soft material contacting a harder one can cause a default contact-stiffness calculation that leads to poor convergence, an effect called "chattering." Or, the software may generate an unrealistic penetration in which one surface passes through another.
Fast-moving impacts produce high-frequency loads that force the solver to take smaller time steps that lengthen run times. A high-energy loss may also lead to an overdamped behavior. Finally, parts might penetrate each other incorrectly because one moved too fast for the solver to "see" contact.
Large displacements or deformations, more than 50% strain, mean the basic assumptions used in calculating contact parameters may no longer be valid due to changes in geometry.
BASIC STEPS OF CONTACT ANALYSIS
Avoiding these difficulties means understanding at least seven basic steps for contact analysis. For instance:
Create the geometry and mesh. Reasonably smooth surfaces with a uniform mesh work best in contact analyses. Thus, it's important to know how to use software tools to generate and refine the mesh.
Identify possible contact areas. Before starting a contact analysis, specify where contact might occur. A part could touch itself in large-deformation problems such as rubber-elasticity analyses. In such cases, make certain that multiple contact areas are defined (either automatically or by you) to cover all potential contact situations.
Determine the contact parameters. FEA software often calculates contact-parameter values based on geometry, mesh, and material constants. But you may need to adjust values for anticipated contact problems, such as large deformation. For example, you might try increasing the contact interaction distance so the software can better detect the nodes that are in contact. Determine the solution method. FEA software typically provides several options for the numerical-solution technique used in contact problems. The full Newton-Raphson method is often recommended for nonlinear contact analyses.
Apply necessary loads and constraints. Although it may seem realistic to "leave parts free to fly around" and come into contact, contact analyses are often greatly simplified by partially restraining parts. Take a pin that passes through a yoke and clevis, for example. Applying constraints prevents the pin from rotating and thereby reduces chattering.
Run the analysis. Most processors generate messages on the status of contact analysis during a solution. Problems, such as slow convergence, can be spotted, letting the user stop the analysis, adjust parameters, and restart.
Review results. When two smooth surfaces contact, they create a relatively smooth stress contour. However, nonsmooth surfaces with a coarse mesh produce less uniform stress contours. In such cases, users must refine or modify the mesh and analyze the model again. No single set of contact-parameter values provides an accurate solution for all models. Many problems solve without difficulty using automatic and default settings, while some models benefit from changes to controlling parameters. Hence, you must understand the purpose of each parameter to determine a proper set of values for the given problem.
When encountering convergence problems or poor results from a contact analysis, carefully check the geometry, mesh, material properties and all contact parameters. As with all CAE analyses, simplify where possible.
What to adjust when looking for contact
Here are a few adjustable contact parameters users have access to in Algor's FEA software:
Contact stiffness is calculated from the geometry and material properties of the parts in the contact pair. A custom value can be specified. It will be adjusted based on contact status, such as penetration or none, to provide improved accuracy and convergence.
Contact tolerance is the distance between any two nodes on surfaces that may contact. The software applies a contact stiffness when the two nodes are within the tolerance.
Contact interaction distance tells the software to consider contact calculations when two surfaces are closer than this value.
Maximum penetration distance tells the software not to calculate surface contact when a point on a secondary surface is farther away than this value.
Maximum initial distance is an initial distance between elements. When greater than this value, contact is not created. It limits the amount of checking the software must do for contact and thus speeds the analysis.
Extend contact element sides can specify the length for extending contact-element boundaries. It's used to resolve incorrect penetration.
Algor Inc., (412) 967-2700, algor.com