Contact Pairs
A contact pair describes contact between two deformable surfaces or between a deformable surface and a rigid surface. You can also use a contact pair to describe self-contact interactions between different areas on a single surface. You can create a contact pair in a Nonlinear Structural case, an Explicit Dynamics case, or a Thermal case. See Defining contact pairs in Abaqus/Standard in the Abaqus Interactions Guide, and Defining contact pairs in Abaqus/Explicit in the Abaqus Interactions Guide for more information. Alternatively, you can create general contact in an Explicit Dynamics case, as described in General Contact. The general contact algorithm allows very simple definitions of contact with very few restrictions on the types of surfaces involved. See Defining Contact Interactions in the Abaqus Interactions Guide for more information.
A contact pair is the link between two part bodies that are prevented from interpenetrating at their common boundary. When they come into contact, the bodies can still separate or slide relative to each other in the tangential plane. Since part bodies can be meshed independently, contact pairs are designed to handle incompatible meshes. Contact pairs take into account the elastic deformability of the interfaces.
You can use a general analysis connection or a Contact or Coincidence assembly constraint to define the surfaces that are interacting. For more information, see Specifying Contact Surfaces. Table 6–1 summarizes the constraints and connections that can be used to define a contact pair in Abaqus for CATIA V5.
| Assembly Design Workbench | Abaqus for CATIA V5 | |
|---|---|---|
| Coincidence Constraint | Contact Constraint | General Analysis Connection |
 | | |
You cannot select a GPS contact connection properties to define the surfaces for use with contact pairs. However, existing contact connection properties will be accounted for in the nonlinear case.
You must use a general analysis connection defined in Abaqus for CATIA V5 to define contact involving shells and beams; you cannot use an assembly constraint. You can specify which side of a shell surface should be involved in contact. By default, the positive side is used; the positive side is defined as the side in the direction of the positive element normal, which is indicated by arrows.
You must create a contact pair to include self-contact in your model. To include self-contact, you select a general analysis connection that refers to the same face for both the first and second components. You can use a Contact or Coincidence assembly constraint for defining only solid-to-solid contact.
For each node on the “slave” surface, Abaqus attempts to find the closest point on the “master” surface of the contact pair where the master surface's normal passes through the node on the slave surface. The contact connection is then discretized between the point on the master surface and the slave node. You can reverse the order of the two surfaces.
The default behavior for a contact pair in mechanical simulations 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 thermal simulations the default behavior for a contact pair consists of a perfectly conducting interface when surfaces have no clearance and a perfectly insulated, or adiabatic, interface when the pair is separated by the maximum allowed clearance distance (1e+6).
Note: The default conductance behavior leads to high conductance values for the relatively small clearances allowed for a contact pair. It is strongly recommended that you create a thermal connection behavior to modify these values.
You can modify either of these behaviors by assigning a new mechanical or thermal connection behavior, respectively, to the contact pair. See Creating a Connection Behavior for more information.
If you need to create multiple contact pairs in a model, you should consider using the interaction wizard. The interaction wizard automates many of the steps involved in defining contact pairs and can create multiple contact pairs simultaneously. See Using the Interaction Wizard for more information.
You can request history output of contact variables, such as contact displacement (CDISP), from a contact pair. However, if you defined surface-to-surface contact using the finite-sliding contact formulation, you cannot use Abaqus for CATIA V5 to generate images of contact variables and you cannot export history output of contact variables.
The default quadratic tetrahedral element in Abaqus for CATIA V5 is C3D10M, and that element is suitable for many contact-related analyses. However, if you are specifying Surface-to-surface as the contact formulation for a contact pair, C3D10 elements can yield improved results.
The Contact Pair dialog box includes a Defaults button that you can click to restore all contact pair options in the dialog box to their default values.
This task shows you how to create a contact pair.
Click the Contact Pair icon
.The Contact Pair dialog box appears, and a Contact Pair object appears in the specification tree under the Connections objects set for the current step in the active analysis case.
You can change the identifier of the contact pair by editing the Name field.
In the specification tree, select a general analysis connection or a Contact or Coincidence assembly positioning constraint to apply to the contact pair.
The Support field is updated to reflect your selection, and arrows indicate the surfaces involved in contact and the direction of the surface normal (red arrows indicate the master surface and green arrows indicate the slave surface).
By default, Abaqus for CATIA V5 chooses the Finite-sliding formulation. This formulation allows for arbitrary separation, sliding, and rotation of the surfaces. Alternatively, you can choose the Small sliding formulation. Small-sliding contact assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other and a slave node will interact with the same local area of the master surface throughout the analysis. Therefore, small-sliding contact is less expensive computationally than finite-sliding contact.
Self-contact is typically the result of large deformation in a model. Therefore, self-contact cannot use the small-sliding contact formulation. See Contact formulations in Abaqus/Standard in the Abaqus Interactions Guide, and Contact constraint enforcement methods in Abaqus/Explicit in the Abaqus Interactions Guide for more information on the finite- and small-sliding formulations.
If you are creating a Nonlinear Structural case, you can toggle on Stabilize rigid body modes.
This option allows Abaqus/Standard to calculate the default damping coefficient that it will use to stabilize rigid body motions in contact problems using viscous damping (see Adjusting contact controls in Abaqus/Standard in the Abaqus Interactions Guide for more information)
The following sections describe the options that allow you to define a contact pair. The most commonly used settings are grouped with the general options.
Configuring the General Options in a Contact Pair
This task shows you how to configure the general options in a contact pair.
From the Contact Pair dialog box, select the General tab.
Optionally, if either or both of the surfaces involved in contact are shells, click Flip Master and/or Flip Slave to reverse the direction of the contact normals. Abaqus for CATIA V5 indicates which face is colored in red and which face is colored in green with colored arrow icons under the Flip Master and Flip Slave buttons.
To reverse the order of the master and slave surfaces in the contact connection definition, toggle on Swap master and slave surfaces.
The red arrows indicating the master surface replace the green arrows indicating the slave surface and vice versa. Abaqus for CATIA V5 updates the colored arrows under Flip Master and Flip Slave accordingly as well.
Optionally, in the specification tree, select a Mechanical or Thermal Connection Behavior to apply to the contact connection. See Creating a Connection Behavior for information on defining connection behaviors.
The Connection Behavior field is updated to reflect your selection.
To help you view the configuration of the master and slave surfaces in a complex model, you can use the Visibility Options to view only the part containing the master surface or only the part containing the slave surface.
Select the Formulation Options.
If you are creating a Nonlinear Structural case, do the following:
By default, the Formulation Option is Surface to Surface, and Abaqus formulates contact such that the stress accuracy is optimized for the selected master and slave surfaces. If you select Node to Surface, Abaqus formulates contact at the point where the slave node projects onto the master surface. While the surface-to-surface method provides improved stress accuracy, the computational cost can be significant, for example, if a large fraction of your model is involved in contact. See Defining contact pairs in Abaqus/Standard in the Abaqus Interactions Guide for more information.
Accounting for initial shell element thicknesses in contact calculations is generally desirable. If you choose to account for shell thickness in your model, you must separate the contact surfaces by the appropriate distance and toggle on Include shell element thickness if the option is available. Shell thickness cannot be accounted for if you are using the finite-sliding, node-to-surface contact formulation.
For surface-to-surface formulations in a Nonlinear Structural case, toggle on Automatically smooth geometry surfaces to apply geometric corrections in the contact formulation for the contact surfaces. The contact smoothing definition recognizes cylindrically or spherically shaped surfaces and automatically smooths the surfaces. Using the smoothed surface geometry can greatly improve the results in some cases.
If you are creating an Explicit Dynamics case, select the contact Formulation Option. By default, Abaqus/Explicit uses a Kinematic contact algorithm to strictly enforce contact constraints (for example, no penetrations are allowed). Alternatively you can choose a Penalty contact algorithm, which has a weaker enforcement of contact constraints but allows for treatment of more general types of contact. See Contact constraint enforcement methods in Abaqus/Explicit in the Abaqus Interactions Guide for more information.
Configuring the Separation Options in a Contact Pair
This task shows you how to configure the separation options in a contact pair. Only the Clearance option is available in an Explicit Dynamics case.
From the Contact Pair dialog box, select the Separation tab.
If desired, toggle on Clearance, and specify a precise initial clearance. In a Nonlinear Structural case, you can also enter a negative clearance to specify an overclosure value. A positive or zero clearance value (used to specify a known gap between the surfaces) means that the surfaces can approach each other through the specified distance until they come in contact. Abaqus treats the two surfaces as not being in contact, regardless of their nodal coordinates.
Specifying a clearance is useful when Abaqus would not compute it accurately enough from the nodal coordinates, for example, if the initial clearance is very small compared to the coordinate values. Abaqus uses the value that you supply to overwrite the initial clearance value calculated at every slave node based on the coordinates of the slave node and the master surface. This procedure does not alter the coordinates of the slave nodes. You can define an initial clearance value only for small-sliding contact.
In a Nonlinear Structural case a negative clearance (overclosure) models a pressure fitting. The mechanical connection behavior specifies the friction coefficient between the parts in the pressure fitting. Abaqus/Standard treats the two surfaces as an interference fit and attempts to resolve the overclosure in the first increment. See Creating a Mechanical Connection Behavior,and Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs in the Abaqus Interactions Guide for more information.
In an Explicit Dynamics case you can define an initial clearance value only for the first step of an analysis, and you cannot specify a negative clearance. Abaqus/Explicit automatically adjusts the positions of surfaces to remove any initial overclosures, except when the slave surface is defined on a rigid body. The adjustments are made with strain-free initial displacements to the slave nodes on the surfaces. Therefore, when a balanced master-slave contact pair is defined, Abaqus/Explicit may adjust nodes on both surfaces. This automatic adjustment of surface position is intended to correct only minor mismatches associated with mesh generation. See Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit in the Abaqus Interactions Guide for more information.
To adjust the slave nodes in a Nonlinear Structural case, do one of the following:
Choose Do not adjust slave nodes to maintain the original position of the slave nodes. Slave nodes that are overclosed in the initial configuration will remain overclosed at the start of the simulation, which may cause convergence problems.
Choose Adjust only overclosed nodes to move any slave nodes that are penetrating the master surface so they are precisely on the master surface.
Choose Adjust nodes within, and enter a value for the distance of the nodes from the master surface; any slave nodes that are within this “adjustment zone” in the initial mesh of the model are moved precisely onto the master surface. If you define a Clearance value for the contact pair, Abaqus ignores the adjustment value.
If you selected the Adjust nodes within option, you can preview which nodes are affected by choosing one of the following options and clicking Preview:
Choose Highlight nodes to highlight those nodes in the model that will be moved by the adjustment options.
Note: Nodes of 1D beams cannot be highlighted in Abaqus for CATIA V5.
Choose Move nodes to view the mesh of the model after the adjustment options are applied. Abaqus for CATIA V5 uses color coding to identify the quality of elements in the adjusted model display: green elements are considered good quality, yellow elements are considered poor quality, and red elements are considered bad quality. These colors are based on the quality criteria currently defined in the CATIA V5 Quality Analysis tool (see Using Abaqus Element Quality Checks for more information).
If you chose to adjust slave nodes, you can toggle on Tie adjusted surfaces to indicate that the surfaces of the contact pair are to be “tied” together for the duration of the simulation. You must adjust the slave nodes because it is very important that the tied surfaces be precisely in contact at the start of the simulation. See Defining tied contact in Abaqus/Standard in the Abaqus Interactions Guide for more information.
In a Nonlinear Structural Case, click the Interference Fit Settings. See “Configuring the Interference Fit Settings in a Contact Pair for more information.
Note: Displacement results for a contact analysis do not show adjusted node positions when attached to the original model; the undeformed model shows the original positions, and the deformed model shows the final positions. To display results including the nodal adjustments, do the following:
Create a new empty .CATAnalysis document with an empty Abaqus Analysis case.
Import the output database file created by the analysis.
Viewing the Status of a Contact Pair
To view the status of a contact pair, click the Status tab. The Status tabbed page indicates the following:
Whether the contact pair was Created in this step or Propagated into this step.
Whether the contact pair is Active or Inactive.
Configuring the Advanced Options in a Contact Pair
The standard solution controls are usually sufficient, but additional controls are helpful to obtain cost-effective solutions for models involving complicated geometries and numerous contact interfaces, as well as for models in which rigid body motions are initially not constrained.
This task shows you how to configure the advanced options in a contact pair.
From the Contact Pair dialog box, select the Advanced tab.
If you are creating a Nonlinear Structural case, do the following (see Adjusting contact controls in Abaqus/Standard in the Abaqus Interactions Guide for more information):
If desired, in the Scale default damping by field, enter a value for the scaling factor. The damping coefficient calculated by Abaqus/Standard will be multiplied by this value.
If desired, click the Damping parameters icon
and do the following:Enter a value for the Tangent friction. This is the fraction of the normal stabilization by which to modify the tangential stabilization. By default, the tangential and normal stabilization are the same.
Enter a value for the Fraction of damping at end of step. Enter a value of 1 to keep the damping constant over the step. If you specify a nonzero value, convergence problems may occur in a subsequent step if stabilization is not used in that step. The default value is zero.
By default, Abaqus/Standard computes the default clearance value based on the facet size associated with the contact pair. Alternatively, you can toggle on Specify and enter a value for the clearance at which the damping becomes zero. Enter a large value to obtain damping independent of the opening distance.
Toggle on Automatic overclosure tolerances to allow small overclosures or separations to occur during the analysis without changing the contact status between the surfaces involved. These tolerances, which are based on the solution convergence criteria currently active in the analysis, may improve the convergence of the analysis by ignoring the effects of insignificant contact between surfaces.
Enter a value for the Critical penetration. This value is the distance by which a point on the slave surface must penetrate the master surface before Abaqus/Standard abandons the current increment and tries again with a smaller increment. The default value is half of the length of a characteristic element face on the slave surface. This parameter does not apply to contact pairs that use the finite-sliding, surface-to-surface contact formulation.
Enter a value for the Extension zone. Abaqus/Standard equates this value to a fraction of the end segment or facet edge length by which the master surface is extended to avoid numerical roundoff errors associated with contact modeling. The value must be between 0.0 and 0.2. The default is 0.1. Abaqus/Standard uses the extension zone only during node-to-surface contact.
If you are creating an Explicit Dynamics case, do the following:
Enter a value for the Penalty stiffness scaling factor. This is the factor by which Abaqus/Explicit scales the default penalty stiffnesses to obtain the stiffnesses used for the penalty contact pairs. By default, the value is 1.0. See Penalty contact algorithm in Contact constraint enforcement methods in Abaqus/Explicit in the Abaqus Interactions Guide for more information.
Choose the contact surface weighting (Balanced master/slave or Pure master/slave). Choose Analysis default to let Abaqus for CATIA V5 automatically select a surface weighting based on the contact formulation and the types of surfaces involved. See Contact surface weighting in Contact formulations for contact pairs in Abaqus/Explicit in the Abaqus Interactions Guide for more information.
Configuring the Interference Fit Settings in a Contact Pair
If there are large overclosures in the initial configuration of the model, Abaqus/Standard may not be able to resolve the interference fit in a single increment. You can specify interference fit options that help Abaqus/Standard to resolve excessive overclosure between contacting surfaces gradually over multiple increments. See Modeling contact interference fits in Abaqus/Standard in the Abaqus Interactions Guide for more information.
This task shows you how to configure the interference fit options in a contact pair. Interference fit options are not available in the Initialization step.
From the Separation tabbed page of the Contact Pair dialog box, click the Interference fit settings tool.
By default, Abaqus/Standard does not allow for an interference fit. To prescribe allowable interferences, toggle on Gradually remove overclosure of slave nodes during step.
Choose the Overclosure Adjustment method.
Choose Automatic shrink fit (first general analysis step only) if you want to assign a different allowable interference to each slave node that is equal to that node's initial penetration. You can select this option only in the first general static step of an analysis.
Choose Uniform allowable interference to specify a single allowable interference that will be applied to every slave node.
If you chose Uniform allowable interference, do the following:
By default, Abaqus/Standard applies the prescribed interference immediately at the beginning of the step and ramps it down to zero linearly over the step. Alternatively, you can toggle on Select amplitude and select an existing amplitude from the specification tree. Abaqus/Standard uses the selected amplitude curve to define the magnitude of the prescribed interference during the step. For more information, see Amplitudes.
In the Magnitude at start of step field, enter the magnitude of the allowable interference at the start of the step.
If desired, toggle on Along direction to specify a shift direction vector. The relative shift is applied to the slave nodes before Abaqus/Standard determines the contact conditions. In certain applications, such as contact simulations of threaded connectors, shifting the surfaces in a specified direction is more effective than simply allowing an interference. If you select this option, enter the following:
Enter the X-direction cosine of the shift direction vector.
Enter the Y-direction cosine of the shift direction vector.
Enter the Z-direction cosine of the shift direction vector.
Click OK to save your interference fit settings.