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).
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 elements with a circular cross-section and truss elements have a
circular cross-section. 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, a method that automatically
generates an internal mesh of contact faces, nodes, and edges to represent the geometry
properly is used by default (see Contact Surface Representation for Beams). 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
By default, Abaqus/Explicit treats the beam cross-section geometry realistically for all cross-sections, including
those shown in Figure 2. To achieve this realistic treatment for beams with circular cross-sections, Abaqus/Explicit uses contact edges and contact nodes with the same radius as the beam
cross-section.Figure 2. Beams with various cross-sections.
For other cross-sections, Abaqus/Explicit uses an automatically generated internal mesh of triangular contact faces, nodes, and
edges. For example, Figure 3 shows such a mesh for a beam with a rectangular cross-section.
Internal nodes of the triangular facet mesh are offset to vertices of the cross-section at
axial locations of beam nodes. The motion of each internal node is driven by the
corresponding beam node via a rigid connection. Contact forces acting on these internal
nodes are redistributed to the original beam nodes as forces and moments. The internal
contact surface mesh for noncircular beam cross-sections is not available for
postprocessing, but it closely resembles the beam profile rendering.Figure 3. Internal contact surface for a beam with rectangular cross-section.
Beams can participate in contact formulations in the following ways:
Circular beams:
Nodes of circular beams can participate in node-to-surface contact.
Edges of circular beams can participate in edge-to-edge contact.
Noncircular beams:
Nodes and faces of the internal surface representation can participate in
node-to-surface contact.
Edges of the internal surface representation can participate in edge-to-edge
contact.
Assigning a nonzero surface thickness for contact (see Surface Thickness) to a noncircular beam cross section has the same effect on the internally generated
faceted as for a solid surface. Nonzero surface thickness effectively expands the contact
cross-section for the beam and rounds the corners (without influencing the beam
stiffness), as shown in Figure 4.Figure 4. Effect of surface thickness for a rectangular beam cross-section.
Alternatively, the contact surface geometry of a noncircular beam cross-section can be
approximated with a circular cross-section encompassing the actual cross-section. Figure 5 shows a rectangular
cross-section beam on the left side and the optional, nondefault circular representation
for contact on the right side of Figure 5. The default representation with an internal mesh was shown in
Figure 3. Figure 5. Beam element profile rendering for circular versus rectangular cross-section
beams.
Input File Usage
Use the following option to activate contact calculations based on the actual
cross-section of the beam element (default):
Interaction module: Create Interaction: General
contact (Explicit):Contact Controls Assignment: toggle
on Beam Cross Section assignment, select Circumscribed
Circle or 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
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:
This option can be used multiple times per steps, and the options will be
concatenated.
Abaqus/CAE Usage
Interaction module: Create Interaction: General contact (Explicit)
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. This method is the only way to reintroduce
interactions that were part of prior contact exclusions.
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.
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):
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:
The CONTACT INCLUSIONS option should
have no data lines when the
ALL EXTERIOR parameter is
used.
Abaqus/CAE Usage
Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: All* with self
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:
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.
Abaqus/CAE Usage
Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the
surfaces in the columns on the left, and click the arrows in the middle to
transfer them to the list of included pairs
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:
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:
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:
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.
Abaqus/CAE Usage
Interaction module: Create Interaction: General contact (Explicit):
Excluded surface pairs: Edit, select the surfaces in the columns on the left,
and click the arrows in the middle to transfer them to the list of excluded pairs
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:
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:
Define an element set named ELERODE that contains all
of the solid elements in the model that refer to a material failure model.
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.
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 and Table 2.
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,
Table 2. Contact inclusions definitions in Abaqus/CAE.
Contact inclusions
Abaqus/CAE syntax
Self-contact for the default all-inclusive surface specifies contact
between every exterior face in the model
First Surface: (All*); Second Surface: (Self)
Contact between the default all-inclusive surface and
SURFERODE specifies contact between every
exterior face and SURFERODE
First Surface: (All*); Second Surface: SURFERODE
Self-contact for SURFERODE specifies
self-contact between the eroding bodies
First Surface: SURFERODE; Second Surface: (Self)
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.
Internal surfaces can be viewed using display groups in the Visualization module of Abaqus/CAE (see the Introduction). 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 and can be
contoured in Abaqus/CAE. 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 and can be plotted as vectors in
a symbol plot in Abaqus/CAE.
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, (CTANDIR1) or (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.
Requesting Element Output When Modeling Surface Erosion
When modeling the erosion of surfaces, it is useful to request additional element field
output of the element status (output variable
STATUS). Failed elements (with an
element status of zero) can then be excluded from the display group in the Visualization module of Abaqus/CAE so that the active contact surface can be identified and contact results on the active
contact surface can be viewed.
Extending the Range for Which Contact Opening Output Is Provided for Gaps
To reduce computational costs, detailed computations to monitor potential points of
interaction are avoided by default where surfaces are separated by a distance greater than
the minimum gap distance at which contact forces (or thermal fluxes, for example) might be
transmitted. Therefore, contact opening
(COPEN) output is typically not provided
where surfaces are opened by more than a small amount compared to surface facet
dimensions. You can extend the range for which Abaqus/Explicit provides contact opening output;
COPEN will be provided up to gap
distances equal to a specified “tracking thickness.” Using this control might increase
computational cost due to extra contact tracking computations, especially if you specify a
large tracking thickness value.
