About General Contact in Abaqus/Explicit

Abaqus/Explicit provides two algorithms for modeling contact and interaction problems: the general contact algorithm and the contact pair algorithm. See About Contact Interactions for a comparison of the two algorithms. This section describes how to include general contact in an Abaqus/Explicit analysis, how to specify the regions of the model that might be involved in general contact interactions, and how to obtain output from a general contact analysis.

The general contact algorithm in Abaqus/Explicit:

  • is specified as part of the model or history definition of the model;

  • allows very simple definitions of contact with very few restrictions on the types of surfaces involved;

  • uses sophisticated tracking algorithms to ensure that proper contact conditions are enforced efficiently;

  • can be used simultaneously with the contact pair algorithm (that is, some interactions can be modeled with the general contact algorithm, while others are modeled with the contact pair algorithm);

  • can be used with two-dimensional, axisymmetric, and three-dimensional surfaces;

  • can be used only in mechanical finite-sliding contact analyses; and

  • does not support kinematic constraint enforcement (contact constraints are enforced with the penalty method).

This page discusses:

See Also
About Contact Interactions
In Other Guides
*CONTACT
*CONTACT INCLUSIONS
*CONTACT EXCLUSIONS

ProductsAbaqus/Explicit

Defining a General Contact Interaction

The definition of a general contact interaction consists of specifying:

Surfaces Used for General Contact

The general contact algorithm allows for very general characteristics in the surfaces that it uses, as discussed in About Contact Interactions. For detailed information on defining surfaces in Abaqus/Explicit for use with the general contact algorithm, see Element-Based Surface Definition, Node-Based Surface Definition, Analytical Rigid Surface Definition, Eulerian Surface Definition, and Operating on Surfaces.

A convenient method of specifying the contact domain is using cropped surfaces. Such surfaces can be used to perform “contact in a box” by using a contact domain that is enclosed in a specified rectangular box in the original configuration. For more information, see Operating on Surfaces.

In addition, Abaqus/Explicit automatically defines an all-inclusive surface that is convenient for prescribing the contact domain, as discussed later in this section. The all-inclusive automatically defined surface includes all element-based surface facets as well as all analytical rigid surfaces and surfaces on all Eulerian materials.

The general contact algorithm generates contact forces to resist node-into-face, node-into-analytical rigid surface, and edge-into-edge contact penetrations. The primary mechanism for enforcing contact is node-to-face contact (the only mechanism used in the contact pair algorithm). If analytical rigid surfaces are present in the contact domain, the general contact algorithm also enforces node-to-analytical rigid surface contact.

General contact can be used for a two-dimensional (plane strain, plane stress, or axisymmetric) model, in which case node-into-face and node-into-analytical rigid surface contact is considered.

Considerations for Edge-to-Edge Contact

The general contact algorithm also considers edge-to-edge contact, which is very effective in enforcing contact that cannot be detected as penetrations of nodes into faces. For example, contact between beam segments and shell perimeter edges (see Figure 1) usually is detected only as edge-to-edge contact.

Figure 1. General contact domain, including edge-to-edge contact.

The terminology “contact edges” refers to feature edges of surface facets (on both shells and solids) as well as to segments representing beam and truss elements. The contact edges representing beam and truss elements have a circular cross-section, regardless of the actual cross-section of the beam or truss element. The radius of a contact edge representing a truss element is derived from the cross-sectional area specified on the truss section definition (it is equal to the radius of a solid circular section with an equivalent cross-sectional area). For beams with circular cross-sections, the radius of the contact edge is equivalent to the section radius. For beams with noncircular cross-sections, the radius of the contact edge is equal to the radius of a circumscribed circle around the section. If connected edges have different radii, a nodal radius is first computed as the minimum radius of the adjacent contact edges, and the radius of the edge cross-section is interpolated linearly over the length of the contact edge from the nodal values. Shell element edges reflect the shell thickness in the normal direction and do not extend past the perimeter (similar to shell nodes and facets). Some numerical rounding of features occurs for both node-to-facet and edge-to-edge contact.

To model contact between edges that are not cylindrical in shape, surface elements can be attached to the edge nodes using surface-based tie constraints and node-to-face contact can be defined between the surface elements (see Surface Elements). This technique is useful for modeling geometric details important to the contact definition that are not modeled with the underlying element geometry. Surface elements can also be defined around shell elements in which Abaqus has reduced the contact thickness (that is, if the thickness exceeds the surface facet edge lengths or diagonal lengths) so that the true surface thickness can be modeled. However, using surface elements with general contact requires a physically reasonable mass to be associated with the surface element nodes, and care must be taken not to alter the bulk mass properties when transferring mass to the surface elements from the underlying elements.

By default, when a surface is used in a general contact interaction, all applicable facets, analytical rigid surfaces, nodes, perimeter edges, currently active feature edges, and beam and truss segments are included in the contact definition. You can control which feature edges are considered for edge-to-edge contact, as discussed in Assigning Surface Properties for General Contact in Abaqus/Explicit.

Contact Surface Representation for Beams

Figure 2 shows examples of beam element profile rendering for portions of beams with circular and rectangular cross-sections. These beams are modeled with several beam elements on either side of a kink. By default, Abaqus/Explicit uses a circular cross-section contact surface representation for beams, regardless of the actual cross-section shape. For noncircular beam element cross-sections, the default circumferential representation for contact encompasses the actual cross-section. Default contact surface representations for both beams of Figure 2 are identical and approximately correspond to the image on the left in Figure 2, except for the addition of a smooth transition at the kink. The default contact representation for beams involves contact nodes co-located with beam nodes and contact edges associated with beam reference edges that pass through nodes of individual beam elements; it does not involve contact faces on beams.

Figure 2. Beam element profile rendering for circular versus rectangular cross-section beams.

An alternative contact surface representation method for beams leads to a more accurate contact representation of noncircular beams. This method uses an automatically generated internal mesh of contact faces, nodes, and edges (such as shown in Figure 3). Beams with circular cross-sections have the same contact surface representation (involving contact nodes and contact edges only) for the default and alternative contact surface representation methods. For the alternative contact surface representation method, internal nodes are positioned at vertices of the cross-section at axial locations of each original beam node. The motion of each of these internal nodes is driven by the corresponding beam node (via a rigid connection). The internal contact faces, nodes, and edges generated by Abaqus/Explicit are not available for postprocessing, but the shape they form closely resembles the beam mesh with beam profile rendering activated.

Figure 3. Internal mesh representations of beam contact surface.

Simulating contact among the beams shown in Figure 4 calls for the alternative contact surface representation. Both node-to-surface and edge-to-edge contact can occur among contact nodes, faces, and edges of such a simulation.

Figure 4. Beams with various cross-sections.

Assigning a nonzero surface thickness for contact (see Surface Thickness) to an alternative beam surface representation has the effect of expanding the contact cross-section and rounding the corners (without influencing the beam stiffness), as shown in Figure 5.

Figure 5. Effect of surface thickness for a rectangular beam cross-section.

Input File Usage

Use the following option to activate contact calculations based on a circumferential approximation of the beam element (default):

CONTACT CONTROLS ASSIGNMENT, BEAM CROSS SECTION=CIRCUMSCRIBED CIRCLE

Use the following option to activate contact calculations based on the actual cross-section of the beam element:

CONTACT CONTROLS ASSIGNMENT, BEAM CROSS SECTION=EXACT

Eulerian-Lagrangian Contact

The general contact algorithm also enforces contact between Eulerian materials and Lagrangian surfaces. This algorithm automatically compensates for mesh size discrepancies to prevent penetration of Eulerian material through the Lagrangian surface. The all-inclusive surface that is defined by Abaqus/Explicit can be used to enforce contact between all Eulerian materials and all Lagrangian bodies in a model; you can also specify individual Eulerian surfaces in the contact domain (see Eulerian Surface Definition). Eulerian-Lagrangian contact is enforced only for Lagrangian surfaces defined on solid and shell elements. Other surface types, such as beam edges and analytical rigid surfaces, are ignored. Contact interactions between Eulerian materials and interactions due to Eulerian material self-contact are handled naturally by the Eulerian formulation; these interactions do not require a general contact definition. See Interactions for more information.

Contact Involving DEM or SPH Particles

The general contact algorithm enforces the following types of contact involving DEM or SPH particles:

  • contact between DEM or SPH particles and other Lagrangian surfaces; and

  • contact among DEM particles.

See Discrete Element Method and Smoothed Particle Hydrodynamics for more information regarding contact involving DEM and SPH particles, respectively.

Including General Contact in an Analysis

If a general contact definition does not appear in a step, any general contact definition active in the previous step will be propagated to the current step.

For convenience, general contact can be defined as model data. A general contact definition specified as model data is considered to be defined in the initial step, or “Step 0,” of the analysis; it can be modified or removed in Step 1 or later steps.

Input File Usage

Use the following option to indicate the beginning of a general contact definition:

CONTACT

This option can be used multiple times per steps, and the options will be concatenated.

Removing General Contact Definitions

You can remove the previously specified general contact definition and specify a new one. Contact state information (such as the proper contact normal orientation for double-sided surfaces) is transferred across step boundaries for interactions that are part of both the old and the new contact definitions. Only *CONTACT, OP=NEW can be used to re-introduce interactions that were part of prior contact exclusions.

Input File Usage

CONTACT, OP=NEW

Modifying General Contact Definitions

Alternatively, you can make changes to an existing general contact definition. In this case the existing general contact definition remains active and any additional information specified is appended to the general contact definition. Prior contact exclusions cannot be converted into contact inclusions with this method.

Contact state information (such as the proper contact normal orientation for double-sided surfaces) is transferred across step boundaries even if the contact domain is modified.

Input File Usage

CONTACT, OP=MOD

Example

Each part of a general contact definition is considered independently when it is modified. For example, the following contact definition is specified in Step 1 (the individual options are discussed later in this section): 

CONTACT
CONTACT INCLUSIONS
surf_1, 
CONTACT EXCLUSIONS
surf_a, surf_b

This contact definition is then modified in Step 2 with the following input: 

CONTACT, OP=MOD
CONTACT INCLUSIONS
surf_2, surf_3 
CONTACT EXCLUSIONS
surf_a, surf_c

An equivalent contact definition for Step 2 could be specified as follows: 

CONTACT, OP=NEW
CONTACT INCLUSIONS
surf_1,
surf_2, surf_3 
CONTACT EXCLUSIONS
surf_a, surf_b 
surf_a, surf_c

Defining the General Contact Domain

You specify the regions of the model that can potentially come into contact with each other by defining general contact inclusions and exclusions. Only one contact inclusions definition and one contact exclusions definition are allowed per step.

All contact inclusions in an analysis are applied first, then all contact exclusions are applied, regardless of the order in which they are specified. The contact exclusions take precedence over the contact inclusions. The general contact algorithm will consider only those interactions specified by the contact inclusions definition and not specified by the contact exclusions definition.

General contact interactions typically are defined by specifying self-contact for the default automatically generated surface provided by Abaqus/Explicit. All surfaces used in the general contact algorithm can span multiple unattached bodies, so self-contact in this algorithm is not limited to contact of a single body with itself. For example, self-contact of a surface that spans two bodies implies contact between the bodies as well as contact of each body with itself.

Specifying Contact Inclusions

Define contact inclusions to specify the regions of the model that should be considered for contact purposes.

Specifying “Automatic” Contact for the Entire Model

You can specify self-contact for a default unnamed, all-inclusive surface defined automatically by Abaqus/Explicit. This default surface contains, with the exceptions noted below, all exterior element faces, all analytical rigid surfaces and all edges based on beam and truss elements in the model, as well as the nodes attached to these faces and edges; in addition, feature edges are included according to the user-specified criteria (see Assigning Surface Properties for General Contact in Abaqus/Explicit). This is the simplest way to define the contact domain. With this approach contact is modeled for all node-to-facet, node-to-analytical rigid surface, and edge-to-edge interactions of the nodes, facets, analytical rigid surfaces, and contact edges of the default surface. This default surface does not include the following:

  • Nodes that cannot be part of an element-based surface; for example, nodes attached only to point masses or connectors.

  • Faces, edges, and nodes that belong only to cohesive elements. In fact, this default surface is generated as if cohesive elements were not present. See Modeling with Cohesive Elements for further discussion of contact modeling issues related to cohesive elements.

Input File Usage

Use both of the following options to specify “automatic” contact for the entire model:

CONTACT
CONTACT INCLUSIONS, ALL EXTERIOR

The CONTACT INCLUSIONS option should have no data lines when the ALL EXTERIOR parameter is used.

Specifying Individual Contact Interactions

Alternatively, you can define the general contact domain directly by specifying the individual contact surface pairings. Self-contact will be modeled only if the two surfaces specified in a pair overlap (or are identical) and will be modeled only in the overlapping region.

Multiple surface pairings can be included in the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface.

Input File Usage

Use both of the following options to specify individual contact interactions:

CONTACT
CONTACT INCLUSIONS
surface_1, surface_2

At least one data line must be specified when the ALL EXTERIOR parameter is omitted. Either or both of the data line entries can be left blank, but each data line must contain at least a comma; an error message will be issued for empty data lines. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Leaving both data line entries blank is equivalent to using the ALL EXTERIOR parameter.

Examples

The following input specifies that contact should be enforced between the default all-inclusive, automatically generated surface and surface_2, including self-contact in any overlap regions: 

CONTACT
CONTACT INCLUSIONS
 , surface_2

Either of the following methods can be used to define self-contact for surface_1: 

CONTACT
CONTACT INCLUSIONS
surface_1,

or 

CONTACT
CONTACT INCLUSIONS
surface_1, surface_1

The following input can be used to introduce a node-based surface containing point masses to the contact domain as well as specify self-contact for the default all-inclusive, automatically generated surface: 

CONTACT
CONTACT INCLUSIONS
 ,
 , node_based_surf

Specifying Contact Exclusions

You can refine the contact domain definition by specifying the regions of the model to exclude from contact.

The primary motivation for specifying contact exclusions is to avoid physically unreasonable contact interactions. For example, a finite element model might contain multiple forming tools, but not all of the tools participate in the forming process simultaneously; you can specify contact exclusions to prevent certain tools from participating in the contact model in certain steps.

You do not need to be concerned with specifying contact exclusions for parts of the model that are not likely to interact, since these exclusions typically will have minimal effect on computational performance.

Contact will be ignored for all the surface pairings specified, even if these interactions are specified directly or indirectly in the contact inclusions definition.

Multiple surface pairings can be excluded from the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact exclusions are not limited to exclusions of single-body contact.

You cannot exclude only one side of shell-like surfaces. If a side label (SPOS or SNEG) is used in defining an element-based shell-like surface and that surface is excluded from contact, Abaqus/Explicit will exclude all faces associated with these elements.

Input File Usage

Use both of the following options to specify contact exclusions:

CONTACT
CONTACT EXCLUSIONS
surface_1, surface_2

Either or both of the data line entries can be left blank. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is excluded from the contact domain.

Automatically Generated Contact Exclusions

Abaqus/Explicit automatically generates contact exclusions for general contact in some situations.

  • Contact exclusions are generated automatically for interactions that are defined with the contact pair algorithm or surface-based tie constraints to avoid redundant (and possibly inconsistent) enforcement of these interaction constraints. For example, if a contact pair is defined for surface_1 and surface_2 and “automatic” general contact is defined for the entire model, Abaqus/Explicit would generate a contact exclusion for general contact between surface_1 and surface_2, so that interactions between these surfaces would be modeled only with the contact pair algorithm. These automatically generated contact exclusions are in effect only during the steps in which the contact pair algorithm or surface-based tie constraint interactions are active.

  • Abaqus/Explicit automatically generates contact exclusions for self-contact of each rigid body in the model, because it is not possible for a rigid body to contact itself.

  • When you specify pure main-secondary contact surface weighting for a particular general contact surface pair, contact exclusions are generated automatically for the main-secondary orientation opposite to that specified (see Contact Formulation for General Contact in Abaqus/Explicit for more information on this type of contact exclusion).

  • The general contact algorithm, unlike the contact pair algorithm, activates and deactivates contact faces and contact edges in the contact domain based on the failure status of the underlying elements. See Modeling Surface Erosion below for details.

Examples

The following input specifies that the contact domain is based on self-contact of an all-inclusive, automatically generated surface but that contact (including self-contact in any overlap regions) should be ignored between the all-inclusive, automatically generated surface and surface_2: 

CONTACT
CONTACT INCLUSIONS, ALL EXTERIOR
CONTACT EXCLUSIONS
 , surface_2

Either of the following methods can be used to exclude self-contact for surface_1 from the contact domain: 

CONTACT EXCLUSIONS
surface_1,

or 

CONTACT EXCLUSIONS
surface_1, surface_1

Modeling Surface Erosion

General contact allows the use of element-based surfaces to model surface erosion for analyses that include material failure. If an appropriate “interior” or “eroding” surface is defined (as discussed in Generating an Interior Surface Automatically), the surface topology evolves to match the exterior of the elements that have not failed. Because of reduced memory usage, eroding surfaces are preferred over interior surfaces. Alternatively, if only one of the bodies can erode, a node-based surface can be used to model surface erosion; this approach can be used with either the general contact or contact pair algorithms. However, even if only one body can erode, it is recommended to define an element-based surface for the eroding body to avoid the usual limitations of node-based surfaces (see Node-Based Surface Definition).

The general contact algorithm modifies the list of contact faces and contact edges that are active in the contact domain based on the failure status of the underlying elements (element failure is discussed in Dynamic Failure Models). General contact considers a face only if its underlying element has not failed and it is not coincident with a face from an adjacent element that has not failed; thus, exterior faces are initially active, and interior faces are initially inactive. Once an element fails, its faces are removed from the contact domain, and any interior faces that have been exposed are activated. A contact edge is removed when all the elements that contain the edge have failed. New contact edges are not created as elements erode. Based on this algorithm, the active contact domain evolves during the analysis as elements fail (see Figure 6 for an example of an eroding solid).

Figure 6. Topology of an eroding contact surface.

You can control whether contact nodes remain in the contact domain after all the surrounding elements have failed. By default, these nodes remain in the contact domain and act as free-floating point masses that can experience contact with faces that are still part of the contact domain. You can specify that nodes of element-based surfaces should erode (that is, be removed from the contact domain) once all contact faces and contact edges to which they are attached have eroded. Further discussion of this technique, including reasons for and against nodal erosion, can be found in Contact Controls for General Contact in Abaqus/Explicit.

Erosion of Surfaces Specified on Solid Elements

For a solid element mesh consisting of elements that might fail, every currently exposed face can potentially be involved in contact. Defining eroding contact surfaces and including them in the general contact domain includes the following steps:

  1. Define an element set named ELERODE that contains all of the solid elements in the model that refer to a material failure model.
  2. Create an eroding surface named SURFERODE for this element set, as described in Creating Surfaces on Solid, Continuum Shell, and Cohesive Elements. The general contact algorithm activates and deactivates faces as necessary as elements fail and the free surface evolves.
  3. Explicitly include this surface in the contact domain. Defining “automatic” general contact for the entire model is not sufficient because the contact domain created when this method is used does not include any interior faces. Therefore, you must define the pairwise interactions with the erodable surface explicitly in the contact inclusions definition, as outlined in Table 1.
Table 1. Contact inclusions definitions.
Contact inclusions Input file syntax
Self-contact for the default all-inclusive surface specifies contact between every exterior face in the model ,  
Contact between the default all-inclusive surface and SURFERODE specifies contact between every exterior face and SURFERODE , SURFERODE 
Self-contact for SURFERODE specifies self-contact between the eroding bodies SURFERODE,

Alternatively, you could create a more concise definition of the same contact domain by first defining a surface named SURFALL that includes all exterior faces in the entire model and all interior faces of element set ELERODE. In this case, since all faces (exterior and interior) in the contact domain are defined in one surface, there is no need to define contact explicitly between the exterior and interior faces. It would be adequate to specify only self-contact for SURFALL.

Abaqus/Explicit automatically computes a nonzero contact thickness associated with interior faces based on element dimensions, and this default value cannot be changed via a surface property assignment.

Erosion of Surfaces Specified on Structural Elements

For structural elements, the general contact algorithm checks the underlying elements of the faces (or “contact edges” on beam and truss elements) for failure. Once the underlying element fails, the face is removed. As with solids, feature edges on structural elements are removed once all of the surrounding faces have failed. A perimeter edge (e.g., on the perimeter of a shell element mesh) is removed once the face it is connected to fails. New perimeter edges are not created to conform to the new perimeter created by the removal of a face.

Output

The surfaces that compose the general contact domain are available as output in addition to the contact analysis output variables.

General Contact Domain and Component Surfaces in Abaqus/Explicit

Abaqus/Explicit generates the following internal surfaces when a general contact domain is defined:

  • General_Contact_Faces_Stepk,

  • General_Contact_Edges_Stepk, and

  • General_Contact_Nodes_Stepk,

where k is the step number. General_Contact_Nodes_Stepk contains only nodes in the general contact domain that are not included in the other two surfaces. For example, General_Contact_Faces_Step2 would contain all surface faces (interior and exterior) that were initially included in the general contact domain for Step 2. These surfaces contain the contact faces, edges, and nodes that were included in the contact domain at the beginning of the step and are not modified to reflect surface erosion.

Abaqus/Explicit generates the following internal surfaces associated with “component surfaces”:

  • General_Contact_Faces_Stepk_Compm and

  • General_Contact_Edges_Stepk_Compm,

where m is the automatically assigned “component number.” Each feature edge component surface, General_Contact_Edges_Stepk_Compm, has a subset of face edges (satisfying the feature edge criteria) of the corresponding face component surface, General_Contact_Faces_k_Compk. The face component surfaces have no nodes in common with each other.

Abaqus/Explicit also generates internal surfaces associated with general contact when material names are used to identify regions where nondefault contact properties or surface properties are assigned, as discussed in Assigning Contact Properties and Assigning Surface Properties. These internal surfaces are named _MATSURF_Material Name_, where Material Name corresponds to the name of the material specified for the property assignment.

The internal surface names used by Abaqus/Explicit should not appear in the input file.

General Contact Output Variables

You can write the contact surface variables associated with general contact interactions to the Abaqus output database (.odb) file (see Writing Surface Output to the Output Database for more information). The available variables are contact pressure, normal contact force, frictional force, and whole surface resultant quantities (that is, force, moment, center of pressure, and total area in contact).

Field Output

The generic variables CSTRESS and CFORCE are valid field output requests for general contact in Abaqus/Explicit. If CSTRESS is requested for the general contact domain, the variables CPRESS (contact pressure) and CSHEARMAG (magnitude of the frictional shear stress) are available in the output database. If CFORCE is requested for the general contact domain, the variables CNORMF (normal contact force) and CSHEARF (shear contact force) are available in the output database.

For general contact CPRESS is calculated as the magnitude of the net contact normal force (the CNORMF vector) per unit area (it is an unsigned value). This convention for reporting contact pressure is different from the convention used for contact pairs. The direction of action of the net contact pressure for general contact can be determined by examining a plot of CNORMF.

CNORMF and CSHEARF are resultant force quantities. If a double-sided surface is contacted on both sides, the resultant force is a vector sum of the force from each side of the surface (for example, the contact normal force will be zero for a double-sided surface that is pinched with equal and opposite forces on each side of the surface).

Some small noise in contact stress and contact force output is likely near the perimeters of thin shells. This behavior is expected and does not negatively impact the overall solution.

Displacement field output (U) for the entire model is written to the output database automatically when any of the contact field output variables are requested.

Several output variables associated with quantities computed at secondary nodes or edge nodes are also available, with generic output variable names CDISP, CSLIPR, and CTANDIR. These output variables are not available for Eulerian-Lagrangian contact or contact involving particles. If these generic output variables names are requested, the specific output variables written as field output are as follows:

  • Contact “displacements” (opening distance and accumulated slips) CDISP: COPEN, CSLIPEQ, CSLIP1, and CSLIP2;

  • Contact slip rates CSLIPR: CSLIPRMAG, CSLIPR1, and CSLIPR2;

  • Contact tangent directions CTANDIR: CTANDIR1, and CTANDIR2.

COPEN is reported only for secondary or edge nodes in contact or very close to being in contact. The accumulated slip variables remain constant when a node is out of contact. The slip rate and tangent direction output variables are reported only for secondary or edge nodes in contact. CSLIPEQ represents the total slip length at a secondary or edge node while in contact. Incremental contributions to CSLIP1 and CSLIP2 are computed as the scalar product of the incremental relative nodal displacement vector and the respective local tangent direction, t 1 (CTANDIR1) or t 2 (CTANDIR2).

The algorithm used to establish and evolve local tangent directions for general contact is described in Local Tangent Directions for Contact. As local tangent directions for contact evolve across increments, previously accumulated slip components are resolved into the new local system before incremental contributions are added to them.

For two-dimensional or axisymmetric analyses, the components in the local tangent 2-direction for the contact output variables such as CSLIP2, CSLIPR2, and CTANDIR2 have no physical meaning and, therefore, are not provided.

History Output

Several whole surface contact force-derived variables are available as history output. You can specify the surface from which the contact force resultants will be calculated.

Force distributions on the surface due to general contact are used to calculate the surface force resultants; forces due to contact pair interactions are not included and must be output separately. The contact state of a surface is output as a set of force (CFN, CFS, and CFT) and moment (CMN, CMS, and CMT) resultants with respect to the origin. Additional variables give the center of force (XN, XS, and XT) on the surface (defined as the point closest to the centroid of the surface that lies on the line of action of the resultant force for which the resultant moment is minimal). The last letter of each variable name denotes which contact force distribution on the surface is used to calculate the resultant: the letter N denotes that the normal contact forces are used to derive the resultant quantity; the letter S denotes that the shear contact forces are used to derive the resultant quantity; and the letter T denotes that the sum of the normal and shear contact forces are used to derive the resultant quantity.

Each total moment output variable will not necessarily equal the cross product of the respective center of force vector and resultant force vector. Forces acting on two different nodes of a surface might have components acting in opposite directions, such that these nodal force components generate a net moment but not a net force; therefore, the total moment might not arise entirely from the resultant force. The center of force output variables tend to be most meaningful when the surface nodal forces act in approximately the same direction.

The total area in contact at a given time can be requested using output variable CAREA, defined as the sum of all the facets where there is contact force. The contact area reported by CAREA is generally slightly larger than the true contact area for reasonably meshed contact surfaces; therefore, interpretation of CAREA should be done with care. The discrepancy between the CAREA output and the true contact area decreases as the mesh density increases. Using contact inclusions or exclusions to limit CAREA output to smaller contact surfaces might also reduce the discrepancy in some cases. Since the CAREA output is an approximation of the true contact area, deriving force or stress values using this output might not yield accurate values; requesting contact force and stress directly is the most appropriate way to obtain accurate results.