General Contact Settings

A General Contact Settings heading appears within the browser for all analysis types. Double-click this heading, or right-click it and choose Edit Settings, to access the General Contact Settings dialog. The contents of this dialog are dependent upon the current analysis type. The tabs the dialog can contain, and the settings within each tab, are described in the sections that follow.

Surface Tab (Linear Analyses)

Iteration method: If you are performing an analysis with contact, there are three methods that can be used during the iterative process that the program uses to determine which nodes are in contact. Choose one of the following three methods from the drop-down menu:

• The Individual points option is the most conservative approach. It activates/deactivates each point individually, and only considers multiple points simultaneously if all have identical states. This method is suggested for hand-built models employing gap elements.
• The Mixed option simultaneously activates all inactive contact points in compression but deactivates those not in compression one at a time.
• The Multiple option is the most aggressive. It simultaneously activates or deactivates all gaps requiring a change in state. This last option can lead to unstable solutions, but, when stable, can result in the most expedient solution. All three methods are applicable to surface and edge contact, with the latter two being recommended.

Maximum number of iterations: The essentially nonlinear behavior associated with surface contact is linearized into many piecewise linear calculation steps in which individual contact elements are activated or deactivated. This process is continued until equilibrium is reached or until the number of iterations exceeds the value specified in the Maximum number of iterations field. The default value is 200 iterations.

The Threshold tolerance field is used to prevent unwanted oscillatory behavior during contact. Contact elements with an absolute strain below this small value do not change state from one iteration to the next. Thus, elements which would otherwise have their state changed from enabled to disabled, or vice versa, remain in their current state during this particular iteration. A typical value for this entry is usually less than 0.01. The default value is zero.

Stabilization method: Many contact problems result in unstable solutions for the first iteration. Furthermore, if rigid-body motion is possible, then unstable solutions occur for all iterations. This is purely an artifact that the underlying mathematics results in singular or in very ill-conditioned systems when structures are not affixed. This type of problem occurs when a part is constrained in one or more directions only by virtue of contact with an adjacent part. To prevent such solution problems, a stabilization method is usually employed. Three different options are available in the Stabilization method drop-down menu. All of these stabilization options pre-activate all contact points for the first iteration.

• None: No stabilization method is used. This option is suitable for situations where the model is statically stable even when the contact elements are inactive. It is also suitable for models that you have manually stabilized (for example, by applying low-stiffness spring constraints where needed to prevent rigid-body motion).
• The Global/Initial option utilizes a constant small value of constraining stiffness throughout the model to prevent rigid body motion. This is the default stabilization method. The stabilizing stiffness is only applied prior to the first iteration and is removed from the second and subsequent iterations. Thus, it is particularly well suited for models not exhibiting rigid-body motion.
• Local/Automatic: Unlike the Global/Initial option, simulated constraints are added for all iterations to prevent rigid-body motion. The program automatically determines the stiffness of the applied simulated constraints.
• The Local option, like the Local/Automatic option, adds simulated constraints for all iterations. However, you must specify a factor to be used in establishing the stiffness. (See Stabilization factor (next item). The input number is the ratio of this stiffness relative to the largest stiffness present in the structural model. This number should lie between 0 and 1.

Stabilization factor: This input field is only applicable to the Local stabilization method. Specify a value used to establish the stiffness of the simulated constraints. The input number is the ratio of the constraining stiffness relative to the largest stiffness present in the structural model. The factor should be between 0 and 1. Too large a factor skews the analysis results due to the supporting effects of the artificial constraints. Whereas, too small a factor may not sufficiently stabilize the structure, causing the maximum number of iterations to be reached without achieving a converged solution.

Stiffness reduction attempts: If a solution has not converged when the maximum number of iterations is reached, the contact stiffness can be automatically reduced by a factor of 10 and the contact solution attempt is repeated. This stiffness reduction happens as many times as specified in the Stiffness reduction attempts field. The default is 2.

Smart Bonding Tab (Linear and Thermal Analyses)

Please see the Smart Bonding page for information regarding the settings in this tab.

Contact Element Updating Tab

This tab only appears for nonlinear analyses. Please refer to the General Contact Settings (Nonlinear) page to learn about the contents of this tab.