37.1.1 Mechanical contact properties: overview

References

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.

Defining contact blockage in Abaqus/Explicit

In Abaqus/Explicit you can control the combination of surfaces that can cause blockage of flow out of a surface-based fluid cavity. The details of contact blockage are discussed in “Contact blockage,” Section 37.1.4.

Defining a friction model

By default, Abaqus assumes that contact between surfaces is frictionless. You can include a friction model as part of a surface interaction definition.

Details of the various friction models available in Abaqus are discussed in “Frictional behavior,” Section 37.1.5.

User-defined interfacial constitutive behavior

Instead of choosing one or some combination of the various interfacial behavior models that are available in Abaqus, you can define any special or proprietary interfacial constitutive behavior through a user subroutine. In Abaqus/Standard you can use the subroutine UINTER; whereas in Abaqus/Explicit you can use VUINTER if you are using the contact pair algorithm and VUINTERACTION if you are using the general contact algorithm.

In Abaqus/Explicit a penalty enforcement of the contact constraint must be used for interacting surfaces whose interfacial behavior is governed by VUINTER or VUINTERACTION.

Details of the definition of a user-defined interfacial constitutive behavior are discussed in “User-defined interfacial constitutive behavior,” Section 37.1.6.

Defining a pressure penetration load in Abaqus/Standard

You can define pressure penetration loads to simulate the penetration of fluid between two contacting surfaces in Abaqus/Standard. The details of the pressure penetration model are discussed in “Pressure penetration loading,” Section 37.1.7.

Defining the interaction of debonded surfaces in Abaqus/Standard

You can allow two initially bonded surfaces to debond in Abaqus/Standard, as discussed in “Crack propagation analysis,” Section 11.4.3. The details of the contact interaction model after debonding are discussed in “Interaction of debonded surfaces,” Section 37.1.8.

Defining breakable bonds in Abaqus/Explicit

In Abaqus/Explicit you can define breakable bonds that connect the interacting surfaces. The kinematic contact pair algorithm must be used when defining breakable bonds.

The breakable bonds affect both the relative tangential motion and the motion normal to the surfaces. Breakable bonds cannot be used with analytical rigid surfaces. The details of the breakable bond model, known as the spot weld model, are discussed in “Breakable bonds,” Section 37.1.9.

Defining surface-based cohesive behavior

You can define surface-based cohesive behavior to model delamination of initially bonded surfaces or to model “sticky” contact between parts that are initially separated but bond on coming into contact, with the possibility that the bond may undergo progressive damage and fail.

Surface-based cohesive behavior is modeled within the general contact framework in Abaqus/Explicit and within the contact pair framework in Abaqus/Standard. The details of the surface-based cohesive behavior model are discussed in “Surface-based cohesive behavior,” Section 37.1.10.