# 36.5.5 CONTACT CONTROLS FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE # References • “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1 • \*CONTACT CONTROLS • “Specifying contact controls in an Abaqus/Explicit analysis,” Section 15.13.10 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview Contact controls for Abaqus/Explicit contact pairs can be used • to scale the stiffness used by penalty contact constraints, and • to adjust the search algorithms that track the motions between two surfaces. # Scaling default penalty stiffnesses If you use the penalty method to enforce contact constraints in a contact pair (see “Contact constraint enforcement methods in Abaqus/Explicit,” Section 38.2.3), Abaqus/Explicit resists penetrations between surfaces by applying a “spring” stiffness to penetrating nodes. The “spring” stiffness that relates the contact force to the penetration distance is chosen automatically by Abaqus/Explicit, such that the effect on the time increment is minimal yet the allowed penetration is not significant in most analyses. Significant penetrations may develop in an analysis if any of the following factors are present: • Displacement-controlled loading • Materials at the contact interface that are purely elastic or stiffen with deformation • Deformable elements (especially membrane and surface elements) that have relatively little mass of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact • Rigid bodies that have relatively little mass or rotary inertia of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact See “The Hertz contact problem,” Section 1.1.11 of the Abaqus Benchmarks Guide, for an example in which the first two of these factors combine such that the contact penetrations with the default penalty stiffness are significant. You can specify a scale factor by which to modify penalty stiffnesses for specified contact pairs. This scaling may affect the automatic time incrementation. Use of a large scale factor is likely to increase the computational time required for an analysis because of the reduction in the time increment that is necessary to maintain numerical stability (see “Contact constraint enforcement methods in Abaqus/Explicit,” Section 38.2.3, for further discussion).

Input File Usage:	Use both of the following options to scale the default penalty stiffnesses:*CONTACT PAIR, MECHANICAL CONSTRAINT=PENALTY,CPSET=contact_pair_set_namesurface_1, surface_2*CONTACT CONTROLS, CPSET=contact_pair_set_name,SCALE PENALTY=factor
Abaqus/CAE Usage:	Interaction module:Create Contact Controls: Name: contact_controls_name,Abaqus/Explicit contact controls: Penalty stiffness scaling factor: factorInteraction editor: Mechanical constraint formulation: Penalty contact method, Contact controls: contact_controls_name

# Adjusting the finite-sliding contact tracking algorithm In a finite-sliding contact pair, searches are conducted continually throughout an analysis to track the relative motion between the two contacting surfaces. The contact tracking algorithm consists of an expensive, periodic global search and a less expensive, regular local search; the search algorithms are discussed in detail in “Contact tracking algorithms” in “Contact formulations for contact pairs in Abaqus/Explicit,” Section 38.2.2. You can use contact controls to adjust the frequency and cost of these searches. # Specifying more frequent global contact searches By default for two-surface contact pairs, Abaqus/Explicit performs a more thorough search of the master faces near each slave node every one hundred increments, which is sufficient for most analyses. However, there are some valid contact situations where a global search needs to be used more or less often during the step. Figure 36.5.5–1 illustrates a situation that might require more frequent global tracking. The master surface is a valid surface, but it contains a hole. The slave node shown identifies the shaded element facet as the closest master surface facet during an increment. The local contact search looks at this master surface facet and its neighbors. If the slave node displaces across the hole in relatively few increments, the potential contact between the slave node and the master surface facets across the hole will not be detected because the local contact search will still be checking the shaded facet. This same situation can occur when a slave node moves rapidly across a deep valley in the master surface. The solution to this problem is to conduct global contact searches more frequently. You can specify the number of increments between global searches, n, for a given contact pair, if a value other than the default of 100 is desired. Input File Usage: Use both of the following options: \*CONTACT PAIR, CPSET=contact\_pair\_set\_name \*CONTACT CONTROLS, CPSET=contact\_pair\_set\_name, GLOBTRKINC=n 

text_image

master surface • slave node ■ previous nearest master face trajectory of slave node

Figure 36.5.5–1 Example where local search may fail. Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact\_controls\_name, Abaqus/Explicit contact controls: Specify max number of increments: n Interaction editor: Contact controls: contact\_controls\_name # Using a more conservative local contact search The default local contact search used by Abaqus/Explicit uses techniques that allow it to use a minimum amount of computational time. If the local contact search has difficulty enforcing the appropriate contact conditions, a more conservative local contact search may resolve the problem. The contact search specified has no effect on contact pairs using self-contact. Input File Usage: Use both of the following options: \*CONTACT PAIR, CPSET=contact\_pair\_set\_name \*CONTACT CONTROLS, CPSET=contact\_pair\_set\_name,FASTLOCALTRK=NO Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact\_controls\_name, Abaqus/Explicit contact controls: toggle off Fast local tracking Interaction editor: Contact controls: contact\_controls\_name # Tracking contact with highly warped surfaces Calculating the correct contact conditions along a surface that is highly warped is very difficult, especially when the relative velocity of the contacting surfaces is very large. By default, Abaqus/Explicit monitors the orientation of every deformable master surface formed by element faces every 20 increments to check that the surface is not highly warped; rigid faceted surfaces are checked for large warping only at the beginning of a step. If a surface becomes highly warped, a warning message is issued in the status (.sta) file (see “Contact diagnostics in an Abaqus/Explicit analysis,” Section 39.2.1), and a more accurate algorithm is used to calculate each slave node’s nearest point on the warped master surface. The alternate algorithm provides a more accurate solution but uses slightly more computational time. # Redefining the criteria for a highly warped surface By default, Abaqus/Explicit considers a surface to be highly warped when the angle between surface normals at the nodes of a facet varies by more than 20°. The maximum variation of the surface normal over a facet is called the out-of-plane warping angle. You can change the default value of the out-of-plane warping angle cutoff from step to step for any contact pair in the model. Input File Usage: \*CONTACT CONTROLS, CPSET=contact\_pair\_set\_name, WARP CUT OFF=angle Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact\_controls\_name, Abaqus/Explicit contact controls: Angle criteria for highly warped facet (degrees): angle Interaction editor: Contact controls: contact\_controls\_name # Modifying how frequently Abaqus/Explicit checks for warped surfaces You can specify the frequency, in increments, at which Abaqus/Explicit checks for warped surfaces for any contact pair in the model. The frequency can be changed from step to step. Checking for warped surfaces more frequently (the default is every 20 increments) will cause a slight increase in computational time for the analysis. Input File Usage: \*CONTACT CONTROLS, CPSET=contact\_pair\_set\_name, WARP CHECK PERIOD=n Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact\_controls\_name, Abaqus/Explicit contact controls: Warp check increment: n Interaction editor: Contact controls: contact\_controls\_name # 37. Contact Property Models Mechanical contact properties 37.1 Thermal contact properties 37.2 Electrical contact properties 37.3 Pore fluid contact properties 37.4 # 37.1 Mechanical contact properties • “Mechanical contact properties: overview,” Section 37.1.1 • “Contact pressure-overclosure relationships,” Section 37.1.2 • “Contact damping,” Section 37.1.3 • “Contact blockage,” Section 37.1.4 • “Frictional behavior,” Section 37.1.5 • “User-defined interfacial constitutive behavior,” Section 37.1.6 • “Pressure penetration loading,” Section 37.1.7 • “Interaction of debonded surfaces,” Section 37.1.8 • “Breakable bonds,” Section 37.1.9 • “Surface-based cohesive behavior,” Section 37.1.10 # 37.1.1 MECHANICAL CONTACT PROPERTIES: OVERVIEW # References • “Contact interaction analysis: overview,” Section 36.1.1 • “Defining contact pairs in Abaqus/Standard,” Section 36.3.1 • “Assigning contact properties for general contact in Abaqus/Explicit,” Section 36.4.3 • “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 36.5.3 • “Contact pressure-overclosure relationships,” Section 37.1.2 • “Contact damping,” Section 37.1.3 • “Contact blockage,” Section 37.1.4 • “Frictional behavior,” Section 37.1.5 • “User-defined interfacial constitutive behavior,” Section 37.1.6 • “Pressure penetration loading,” Section 37.1.7 • “Interaction of debonded surfaces,” Section 37.1.8 • “Breakable bonds,” Section 37.1.9 • “Surface-based cohesive behavior,” Section 37.1.10 • \*SURFACE INTERACTION • “Understanding interaction properties,” Section 15.4 of the Abaqus/CAE User’s Guide # Overview In a mechanical contact simulation the interaction between contacting bodies is defined by assigning a contact property model to a contact interaction (see “Defining contact pairs in Abaqus/Standard,” Section 36.3.1; “Assigning contact properties for general contact in Abaqus/Explicit,” Section 36.4.3; and “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 36.5.3, for details). Mechanical contact property models: • may include a constitutive model for the contact pressure-overclosure relationship that governs the motion of the surfaces; • may include a damping model that defines forces resisting the relative motions of the contacting surfaces; • may include a friction model that defines the force resisting the relative tangential motion of the surfaces; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine UINTER in Abaqus/Standard; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine VUINTER in Abaqus/Explicit when using the contact pair algorithm; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine VUINTERACTION in Abaqus/Explicit when using the general contact algorithm; • in Abaqus/Standard may include a constitutive model for the penetration of fluid between two contacting surfaces; • in Abaqus/Standard may include a constitutive model for the interaction of debonded surfaces; • in Abaqus/Explicit may include a constitutive model that simulates the failure of bonds connecting the interacting bodies; and • may include surface-based cohesive behavior that allows modeling of delamination of bonds or “sticky” contact using progressive damage evolution models. This section provides a general outline of how to define the components of a mechanical contact property model. Specific details about the different components of the contact property models and the algorithms used for the contact calculations are found in other sections of this chapter. # Defining the contact property model There are different methods for defining the components of a mechanical contact property model. # Defining the contact pressure-overclosure relationship The default contact pressure-overclosure relationship used by Abaqus is referred to as the “hard” contact model. Hard contact implies that: • the surfaces transmit no contact pressure unless the nodes of the slave surface contact the master surface; • no penetration is allowed at each constraint location (depending on the constraint enforcement method used, this condition will either be strictly satisfied or approximated); • there is no limit to the magnitude of contact pressure that can be transmitted when the surfaces are in contact. You can define a nondefault pressure-overclosure relationship for a surface interaction. The various pressure-overclosure relationships available in Abaqus are discussed in “Contact pressure-overclosure relationships,” Section 37.1.2, and the constraint methods available to enforce these relationships are discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2. # Defining a surface interaction model with damping between the surfaces You can define damping forces to oppose the relative motion between the interacting surfaces. In Abaqus/Standard the specified contact damping affects the motion in the normal direction only, whereas in Abaqus/Explicit contact damping can affect both the relative tangential motion and the motion normal to the surfaces. The details of the contact damping model are discussed in “Contact damping,” Section 37.1.3.