Contact Properties

You can use Nonlinear Structural Analysis and Thermal Analysis to model contact between two bodies. For example, you can model the assembly of a cylinder head gasket, metal forming simulations, and analyses of rubber seals being compressed between two components. You can also model finite-sliding self-contact of a single deformable body; for example, a complex rubber seal that folds over on itself. Nonlinear Structural Analysis and Thermal Analysis use contact pairs to model contact interactions.

The following section discusses contact modeling in Nonlinear Structural Analysis and Thermal Analysis:

Contact Pairs: Prevents two bodies from penetrating each other at a common interface.

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 or a Thermal case.

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 Nonlinear Structural Analysis and Thermal Analysis.

Table 6–1 Contact pairs.

Assembly Design Workbench Nonlinear Structural Analysis and Thermal Analysis
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 Nonlinear Structural Analysis or Thermal Analysis 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, the solver 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 Nonlinear Structural Analysis and Thermal Analysis to generate images of contact variables and you cannot export history output of contact variables.

This task shows you how to create a contact pair.

  1. 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.

  2. You can change the identifier of the contact pair by editing the Name field.

  3. 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).

  4. By default, Nonlinear Structural Analysis and Thermal Analysis choose 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.

  5. Toggle on Stabilize rigid body modes to allow calculation of the default damping coefficient that will be used to stabilize rigid body motions in contact problems using viscous damping.

  6. 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.

  1. From the Contact Pair dialog box, select the General tab.

  2. 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. Nonlinear Structural Analysis and Thermal Analysis indicate 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.

  3. 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. Nonlinear Structural Analysis and Thermal Analysis update the colored arrows under Flip Master and Flip Slave accordingly as well.

  4. 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.

  5. 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.

  6. Select the Formulation Options.

    • If you are creating a Nonlinear Structural case, do the following:

      1. By default, the Formulation Option is Node to Surface, and the solver formulates contact at the point where the slave node projects onto the master surface. If you select Surface to Surface, the solver formulates contact such that the stress accuracy is optimized for the selected master and slave surfaces. 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.

      2. 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.

Configuring the Separation Options in a Contact Pair

This task shows you how to configure the separation options in a contact pair.

  1. From the Contact Pair dialog box, select the Separation tab.

  2. 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. The solver treats the two surfaces as not being in contact, regardless of their nodal coordinates.

    Specifying a clearance is useful when the solver would not compute it accurately enough from the nodal coordinates; for example, if the initial clearance is very small compared to the coordinate values. The solver 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. The solver treats the two surfaces as an interference fit and attempts to resolve the overclosure in the first increment. See Creating a Mechanical Connection Behavior for more information.

  3. 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, the solver ignores the adjustment value.

    Adjusting the position of the surfaces at the start of the analysis can eliminate small gaps or penetrations caused by numerical roundoff and, thus, prevent possible convergence problems in the analysis. Adjusting surface nodes does not create strains in the model. You cannot adjust the slave nodes if you are defining self-contact.

    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 Nonlinear Structural Analysis and Thermal Analysis.

    • Choose Move nodes to view the mesh of the model after the adjustment options are applied. Nonlinear Structural Analysis and Thermal Analysis use 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).

    Both surfaces involved in the contact pair must be meshed to preview the adjustment options. The node adjustment previews are approximations only; the nodes affected by the preview display may not be the same nodes that are adjusted by the solver. However, the preview should identify general regions of interest in the model when configuring adjustment options. The model display returns to the original geometry when you exit the Contact Pair dialog box.

  4. 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.

  5. 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:

  1. Create a new empty .CATAnalysis document with an empty Analysis case.

  2. 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.

  1. From the Contact Pair dialog box, select the Advanced tab.

  2. If desired, in the Scale default damping by field, enter a value for the scaling factor. The damping coefficient will be multiplied by this value.

  3. 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, the default clearance value is computed 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.

Configuring the Interference Fit Settings in a Contact Pair

If there are large overclosures in the initial configuration of the model, the solver may not be able to resolve the interference fit in a single increment. You can specify interference fit options that help the solver to resolve excessive overclosure between contacting surfaces gradually over multiple increments.

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.

  1. From the Separation tabbed page of the Contact Pair dialog box, click the Interference fit settings tool.

  2. By default, an interference fit is not allowed. To prescribe allowable interferences, toggle on Gradually remove overclosure of slave nodes during step.

  3. 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.

  4. If you chose Uniform allowable interference, do the following:

    1. By default, the solver 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.

    2. In the Magnitude at start of step field, enter the magnitude of the allowable interference at the start of the step.

    3. If desired, toggle on Along direction to specify a shift direction vector. The relative shift is applied to the slave nodes before the solver 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.

  5. Click OK to save your interference fit settings.