Creating a Mechanical Connection Behavior

The default behavior for a mechanical contact connection consists of a frictionless relationship in the tangential direction and a “hard” contact relationship in the normal direction, in which no penetration of the slave nodes into the master surface is allowed and no tensile stress is transferred across the interface. In addition, the classical Lagrangian method is used to enforce the contact constraints in the normal direction; for this method you can use the hard contact relationship, or you can define a “softened” contact relationship in the normal direction in which the contact pressure is either an exponential or piecewise linear (tabular) function of the clearance between the surfaces. Alternatively, you can enforce constraints using the augmented Lagrange multiplier method or the penalty contact method; both of these methods require hard contact. You can specify a contact stiffness for either the augmented Lagrange method or the penalty contact method, and both of these methods are available only for Abaqus/Standard analyses.

You can choose from several forms of friction for the contact behavior in the tangential direction. The following friction types are available:

Penalty friction limits motion between the surfaces to an elastic slip within a defined distance. Rough friction prevents any motion between the contact surfaces. User-defined friction allows you to prescribe the time variation of the friction coefficient in a user subroutine, which is sometimes preferable when the time history of the magnitude is complex. Static-kinetic exponential decay provides for an exponential decay of the friction coefficient from a static value to a kinetic value. See Frictional behavior in the Abaqus Interactions Guide for more information on each of the available friction types.

You must define a mechanical connection behavior to describe nondefault behavior for a contact pair. See Contact Pairs for information on assigning a connection behavior to a contact connection. In addition, you can use a mechanical connection behavior to describe nondefault behavior for general contact, as described in General Contact. You describe and assign mechanical connection behaviors in the Nonlinear Structural Analysis workbench.

This task shows you how to define a mechanical connection behavior.

  1. Click the Mechanical Connection Behavior icon .

    The Mechanical Connection Behavior dialog box appears, and a Mechanical Connection Behavior object appears in the specification tree under a Nonlinear and Thermal Properties feature.

  2. You can change the connection behavior identifier by editing the Name field. This name will be used in the specification tree.

  3. Enter a description for the connection behavior in the Description field.

  4. Specify the tangential behavior for the interaction by choosing the default Frictionless behavior or by selecting one of the following friction methods:

    Penalty

    Choose this method and click to open the Penalty Friction dialog box. In the Friction tab, enter the friction coefficient. You can also include data based on the slip rate, contact pressure, or temperature. In the Shear Stress tab, you can specify a shear stress limit or keep the default unlimited shear stress. In the Elastic Slip tab, you can specify the maximum elastic slip for Abaqus/Standard as a fraction of the characteristic surface dimension or as an absolute distance—this option has no meaning in Abaqus/Explicit. See Shear stress versus elastic slip while sticking in Frictional behavior in the Abaqus Interactions Guide for more information.

    Rough

    Choose this method to prevent any motion between the contact surfaces by specifying an infinite coefficient of friction. See Preventing slipping regardless of contact pressure in Frictional behavior in the Abaqus Interactions Guide for more information.

    User-Defined

    Choose this method if you want to define a nonuniform variation of the friction coefficient in user subroutine FRIC (in a Structural case) or VFRIC (in an Explicit Dynamics case). For more information, see Using User Subroutines; FRIC in the Abaqus User Subroutines Guide; and VFRIC in the Abaqus User Subroutines Guide.

    Static-Kinetic Exponential Decay

    Choose this method and click to open the Static-Kinetic Exponential Decay dialog box. Enter the static, kinetic, and decay coefficients that Abaqus will use to calculate the exponentially decaying friction coefficient.

    Experimental data show that the friction coefficient that opposes the initiation of slipping from a sticking condition is different from the friction coefficient that opposes established slipping. The former is typically referred to as the “static” friction coefficient, and the latter is referred to as the “kinetic” friction coefficient. Abaqus assumes that the friction coefficient decays exponentially from the static value to the kinetic value, where the rate of decay is a function of the decay coefficient. See Specifying static and kinetic friction coefficients in Frictional behavior in the Abaqus Interactions Guide for more information.

  5. If you choose the default classical Lagrange multiplier method, you can specify the contact pressure-overclosure relationship used to define the contact model. See Contact pressure-overclosure relationships in the Abaqus Interactions Guide for more information.

    Hard Contact

    Choose Hard Contact to use the default “hard” contact pressure-overclosure relationship.

    By default, the “hard” contact relationship allows separation of the two surfaces after contact has been established. Toggle off Allow separation after contact to prevent the two surfaces from separating once they have come into contact.

    Exponential

    Choose Exponential to define a “softened” contact pressure-overclosure relationship with an exponential law for the classical Lagrange multiplier constraint enforcement method. Specify the clearance at zero contact pressure and the contact pressure at zero clearance.

    In this relationship the surfaces begin to transmit contact pressure once the clearance between them, measured in the contact (normal) direction, reduces to the clearance at zero pressure. The contact pressure transmitted between the surfaces then increases exponentially as the clearance continues to diminish.

    Tabular

    Choose Tabular to define a “softened” contact pressure-overclosure relationship in tabular form for the classical Lagrange multiplier constraint enforcement method. Specify data pairs of pressure versus overclosure (where overclosure corresponds to negative clearance). You must specify the data as an increasing function of pressure and overclosure.

    In this relationship the surfaces transmit contact pressure when the overclosure between them, measured in the contact (normal) direction, is greater than the overclosure at zero pressure. For overclosures greater than the last one you specify, the pressure-overclosure relationship is extrapolated based on the last slope computed from the user-specified data.

  6. From the Constraint enforcement method field, select the method that will be used to enforce contact constraints. For more information, see Contact constraint enforcement methods in Abaqus/Standard in the Abaqus Interactions Guide.

    Default

    Choose Default to enforce constraints using a contact pressure-overclosure relationship. This option is available only for the default “hard” contact pressure-overclosure relationship.

    Augmented Lagrange (Standard)

    Choose Augmented Lagrange (Standard) to enforce constraints using the augmented Lagrange contact constraint enforcement method instead of the default classical Lagrange multiplier method. The augmented Lagrange method cannot be used for an Explicit Dynamics case. See Contact constraint enforcement methods in Abaqus/Standard in the Abaqus Interactions Guide for more information.

    Penalty (Standard)

    Choose Penalty (Standard) to enforce contact constraints using the penalty method. The penalty method cannot be used for an Explicit Dynamics case. See Contact constraint enforcement methods in Abaqus/Standard in the Abaqus Interactions Guide for more information.

  7. If you selected the Augmented Lagrange (Standard) or the Penalty (Standard) constraint enforcement method, enter data to define the contact behavior:

    1. Toggle off Allow separation after contact if you want to prevent surfaces from separating once they have come into contact.

    2. Specify the contact stiffness in the Contact stiffness options.

      • Choose Use default to have Abaqus calculate the penalty contact stiffness automatically.

      • Choose Specify to enter a custom value for the penalty contact stiffness, and enter a positive value for the contact penalty stiffness.

    3. Specify a factor by which to multiply the chosen penalty stiffness in the Stiffness scale factor field.

    4. Specify the Clearance at which contact pressure is zero. The default value is 0.

  8. Click OK in the Mechanical Connection Behavior dialog box.