Abaqus/Standard 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/Standard analysis, how to specify the regions of the model that may be involved in general contact
interactions, and how to obtain output from a general contact analysis.
The general contact
algorithm in Abaqus/Standard:
is specified as part of the model definition;
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- or three-dimensional surfaces; and
by default, uses the finite-sliding, surface-to-surface contact formulation as the
primary contact formulation, supplemented by the edge-to-surface, edge-to-edge, and
vertex-to-surface contact formulations. You can also specify a small-sliding tracking
approach over portions or the entire general contact domain.
An example of an analysis that uses general contact to define contact
between the various components of an assembly is described in
Impact analysis of a pawl-ratchet device.
Surfaces Used for General Contact
The general contact algorithm in
Abaqus/Standard
allows for quite general characteristics in the surfaces that it uses, as
discussed in
About Contact Interactions.
For detailed information on defining surfaces in
Abaqus/Standard
for use with the general contact algorithm, see
Element-Based Surface Definition.
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/Standard
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, crack surfaces for enriched elements, and analytical rigid surfaces.
The general contact algorithm does not consider contact involving node-based
surfaces, although these surfaces can be included in contact pairs in analyses
that also use general contact.
Types of Contact Formulations within General Contact Targeting Various Scenarios
The general contact algorithm in
Abaqus/Standard
offers capabilities to model surface-to-surface contact, edge-to-surface
contact, edge-to-edge contact, and vertex-to-surface contact with the default
finite-sliding tracking approach. The surface-to-surface contact formulation is
the primary formulation in that case with three-dimensional models and is the
only formulation for general contact with two-dimensional and axisymmetric
models.
As a nondefault option, the small-sliding tracking approach can be specified
to model surface-to-surface contact. Small sliding is not supported with edges
and vertices. Specifying small sliding within general contact alleviates many
of the limitations with small-sliding contact pairs for modeling
surface-to-surface contact related to surface topology (for example, disjoint
regions, complex intersections, and wraparound surfaces) and contact tracking.
As a result, potential small-sliding constraints based on the initial
configuration are automatically established in a robust manner. The
finite-sliding tracking approach is still the preferred approach due to its
generality in handling arbitrary relative surface motions. However, small
sliding in general contact provides a highly automated and convenient contact
modeling approach in situations where relative surface motions are known to be
small.
Pure heat transfer and coupled thermal-electrical contact interactions support edge-to-surface
contact with the edge as the main in addition to surface-to-surface contact.
For three-dimensional models, the surface-to-surface contact formulation primarily treats cases
with contact over an area of dimensions significant compared to the surface facet
dimensions, such as the case on the left in Figure 1. General
contact with finite sliding for three-dimensional models uses the other contact formulations
as supplementary formulations. For example, the second, third, and fourth cases in Figure 1 would be
treated with the edge-to-surface, edge-to-edge, and vertex-to-surface formulations,
respectively. The supplementary formulations are also used by general contact to treat
contact involving three-dimensional beam and truss elements. The surface-to-surface,
edge-to-surface, and vertex-to-surface formulations can treat contact interactions in which
one surface (which does not represent an edge or a vertex) is an analytical rigid surface.
General contact does not consider contact between two analytical rigid surfaces.
Contact scenario types for two blocks.
Transitions between the predominant type of contact formulation active in a
local region are common. For example, the edge-to-surface contact formulation
would be predominant at the stage of the snap-fit simulation shown in
Figure 2
because the active contact zone corresponds to a feature edge.
Snap-fit example involving feature edge-to-surface contact with an
oblique angle between surface normals in the contact region.
Upon further insertion, the surface-to-surface contact formulation would
become predominant once the top surface of the darker colored part is in
contact with the other part over a significant area. General contact
automatically handles transitions between predominant contact formulations as
contact conditions evolve. Multiple types of contact constraints will be
locally active during transitions. The supplementary contact formulations are
always enforced with a penalty method, which helps avoid numerical issues with
“over-constraints” while multiple constraint types are active.
For two-dimensional and axisymmetric models, surfaces based on solid, shell,
beam, and truss elements are comprised of linear or quadratic segments
(sometimes referred to as two-dimensional faces). For three-dimensional models,
beam and truss surfaces are comprised of segments (sometimes referred to as
"edges"), whereas surfaces based on three-dimensional solid, shell, and
membrane elements are comprised of triangular or quadrilateral faces (and edges
of face boundaries). Due to the similarity of two-dimensional surfaces among
element types, the two-dimensional surface-to-surface contact formulation can
treat surfaces based on solid, shell, beam, and truss elements. The
three-dimensional surface-to-surface contact formulation treats surfaces based
on solid and shell elements but does not treat beam or truss surfaces.
General contact in
Abaqus/Standard
is defined at the beginning of an analysis. Only one general contact definition
can be specified, and this definition is in effect for every step of the
analysis.
Defining the General Contact Domain
The general contact domain is the envelope of the regions in the model that can potentially
come into contact. It is determined once for use throughout the analysis based on general
contact inclusions you specify at the model level. Surfaces that participate in contact
inclusions are automatically part of the general contact domain. You can specify contact
exclusions in addition to contact inclusions at the model level. While contact exclusions do
not influence the contact domain, they take precedence over contact inclusions to exclude
specific contact interactions at the beginning of the analysis. You can have only one
contact inclusions definition and one contact exclusions definition at the model level.
Because exclusions take precedence over inclusions, the order in which you specify these
definitions does not matter.
Interactions that you specify at the model level can be activated/reactivated or
deactivated in later steps by specifying contact inclusions and exclusions at the step
level.
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/Standard.
This default surface contains, with the exceptions noted below, all exterior
element faces and all analytical rigid surfaces. This is the simplest way to
define the contact domain.
The default surface does not include faces that belong only to cohesive
elements. In fact, the 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.
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. In some cases computational
performance and robustness can be improved by including only portions of
surfaces in the general contact domain that will experience contact during an
analysis.
Multiple surface pairings can be included in the contact domain. All of
the surfaces specified must be element-based surfaces. Edge-based surfaces
cannot be included using this method.
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:
You can refine the contact domain definition by specifying the regions of
the model to exclude from contact. Possible motivations for specifying contact
exclusions include:
improving computational performance by excluding parts of the model that
are not likely to interact.
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. All of
the surfaces specified must be element-based surfaces. 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.
Automatically Generated Contact Exclusions
Abaqus/Standard
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/Standard
generates a contact exclusion for general contact between
surface_1 and
surface_2 so that interactions between these
surfaces are modeled only with the contact pair algorithm. These automatically
generated contact exclusions are in effect throughout the analysis.
Abaqus/Standard
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 Numerical Controls for General Contact in Abaqus/Standard for more information on this type of
contact exclusion).
Abaqus/Standard assigns default pure main-secondary roles for contact involving disconnected
bodies within the general contact domain, and contact exclusions are generated by
default for the opposite main-secondary orientations. Options to override the
default pure main-secondary assignments with alternative pure main-secondary
assignments or balanced main-secondary assignments are discussed in Numerical Controls for General Contact in Abaqus/Standard.
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:
Activating and Deactivating Contact Interactions across Steps
You can activate contact interactions and initialize them or deactivate them in a step
using contact inclusions and exclusions. Within a step, all new inclusions are processed
first and new exclusions are processed subsequently, in turn, to modify the active and
inactive specification from the previous step. During deactivation, contact forces (and
heat or electrical fluxes in the case of additional thermal and electrical interactions)
are ramped down for contact constraints that were closed and active in the previous
general step. The details are very similar to contact pairs (see Removal of Contact Forces Associated with Closed Contact Pairs).
Step-dependent activation and deactivation are not supported for heat transfer, coupled
thermal-electrical, and coupled thermal-electrochemical procedures. Similarly,
step-dependent activation and deactivation are not allowed for general contact with XFEM
surfaces anywhere in the model. For the small-sliding tracking approach in general
contact, portions of the model where small-sliding is specified also cannot participate
in step-dependent activation and deactivation.
Example: Activating and Deactivating Contact Interactions across Steps
In this example, the all-inclusive, automatically generated surface is active at the
beginning for contact based on the contact inclusions specified at the model level. An
interaction involving surfaces surf_a and
surf_d is excluded at the start. Both surfaces
surf_a and surf_d are still
part of the contact domain because they can potentially come into contact with other
surfaces.
The contact interaction involving surfaces surf_a and
surf_b and all interactions involving surf_c
are deactivated in a later step. In the same step, the interaction
involving surf_a and surf_d is
reactivated.
In a subsequent step, a contact interaction involving surf_a
and surf_e (of which surf_b is a
subset) is activated. Internally, only the contact interaction involving surfaces
surf_a and surf_b is reactivated
as the interaction of surf_a with the portion of
surf_e not containing surf_b is
already active.
The general contact algorithm can consider three-dimensional edge-to-surface
contact. In addition to modeling contact between segments of beam or truss
elements and faceted surfaces, it is more effective at resolving some
interactions than the surface-to-surface contact formulation.
Figure 2
and
Figure 3
show examples in which the edge-to-surface contact formulation is most
effective for resolving contact.
Edge-to-surface contact examples.
The bottom-right example in
Figure 3
shows a feature edge of an element-based surface in contact with an analytical
rigid surface. The feature edges of an analytical rigid surface do not act as
edges in the edge-to-surface formulation. You can enhance convergence behavior
by avoiding feature edges and corners in analytical rigid surfaces used for
contact: Instead, use smooth analytical rigid surfaces with continuously
varying surface normal directions for contact.
Contact edges representing three-dimensional 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 three-dimensional
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 three-dimensional beams with circular
cross-sections, the radius of the contact edge is equivalent to the section
radius. For three-dimensional beams with non-circular cross-sections, the
radius of the contact edge is equal to the radius of a circumscribed circle
around the section. Edge-to-surface contact for three-dimensional beam or truss
elements is activated by including the associated surfaces into the general
contact domain. By default, the all-inclusive surface contains surfaces based
on beam or truss elements.
The surface thickness for two-dimensional beam segments corresponds to the
in-plane thickness of the beam section. The surface thickness for
two-dimensional truss segments corresponds to the radius of a solid circular
section with an equivalent cross-sectional area as specified for the truss
section. Beams and trusses are treated only with the surface-to-surface contact
formulation in general contact, as discussed in
Types of Contact Formulations within General Contact Targeting Various Scenarios.
The edge-to-surface contact formulation is commonly used to resist penetrations of feature edges
of one surface into a relatively smooth portion of another surface (which may be an
analytical rigid surface), with the contact normal direction based on the relatively smooth
surface. The main and secondary roles of surfaces in the edge-to-surface contact formulation
are reversed for some situations involving large-diameter beams. By default, if half of the
beam radius exceeds the facet dimensions of the other surface, the beam acts as the main
surface such that the edge-to-surface contact formulation resists penetrations of a smooth
portion of a neighboring solid or shell surface into a beam, with the contact normal
direction based on the radial direction of the beam. The bottom-left example in Figure 3 corresponds to such a case with a relatively large diameter beam (see Main and Secondary Surface Roles of a Contact Formulation for details about how to control main and secondary
assignment).
In pure heat transfer and coupled thermal-electrical analyses, only the edge-to-surface
formulation with the one-dimensional line ("beam") element–based surfaces acting as the main
is supported. Consequently, these line element–based surfaces act as the main by default.
The line elements are intended to model higher dimensional physics with a one-dimensional
idealization. They are expected to have a cross-sectional (beam) radius that is comparable
to the facet dimensions of the surrounding surfaces to obtain accurate results for
thermal/electrical interactions.
The edge-to-surface contact formulation considers twisting of beams only for
cases in which the contact normal is based on the radial direction of the beam.
When considered, beam twisting influences the calculation of incremental slip.
By default, when a surface is used in a general contact interaction, all
applicable facets are included in the contact definition along with edges of
solid and shell elements with feature angles of at least 45°. See
Feature Edges
for a discussion of controls related to which feature edges are considered for
edge-to-surface contact. Edge-to-surface contact constraints never participate
in thermal, electrical, or pore pressure contact properties. For example, in a
coupled temperature-displacement analysis, surface-to-surface constraints can
influence mechanical and thermal interactions; but, if edge-to-surface
constraints are included, they will only help resist penetrations.
The contact area associated with a feature edge depends on the mesh size;
therefore, contact pressures (in units of force per area) associated with
edge-to-surface contact are mesh dependent.
Edge-to-Edge Contact Scenarios
The general contact algorithm can optionally consider three-dimensional
edge-to-edge contact except on crack surfaces for enriched elements. Feature
edges on solid and shell-like surfaces, shell perimeter edges, and edges
representing beams (and trusses) can be included.
Figure 4
shows examples in which the edge-to-edge contact formulation is most effective
for resolving contact.
Edge-to-edge contact examples.
Two edge-to-edge contact formulations are available. One formulation bases
the contact normal direction on the cross product between the two respective
edges considered for contact, and the other formulation uses a radial direction
of one of the beams as the contact direction (similar to what is done for
tube-to-tube contact elements, which are discussed in
Tube-to-Tube Contact Elements).
Four of the examples in
Figure 4
rely on the formulation with the cross product normal to resist penetrations,
and the example on the bottom right of
Figure 4
relies on the formulation with the radial normal. The edge-to-edge contact
formulation with the radial normal is applicable only to cases with some
thickness contributing to the contact calculations.
The example shown in
Figure 5
involves compression of a spring modeled with beam elements. This example
relies on the edge-to-edge contact formulation with a radial normal direction
to resolve contact between adjacent spring coils, and it relies on the
edge-to-surface contact formulation to resolve contact between the spring and
other surfaces.
Compressing a spring modeled with beam elements.
The edge-to-edge contact formulation with a radial normal can involve the
“exterior” of beam, shell, and solid feature edges and the “interior” of hollow
beams, as shown in the example in
Figure 6.
This example involves a wire modeled with beam elements being wound onto a
cylinder modeled with solid elements. The wire passes through a hollow
cylindrical guide before coming onto the cylinder. The “radial” edge-to-edge
formulation resolves contact between adjacent coils of the wire and also
resolves contact between the wire and the interior of the hollow beam
representing the guide. The edge-to-surface contact formulation resolves
contact between the wire and the cylinder.
Winding a wire onto a cylinder.
The edge-to-edge contact formulation with a contact normal direction based
on the cross product of the edge directions is applicable only while edges are
not nearly parallel. The edge-to-edge contact formulation with a radial contact
normal direction is typically most applicable while contact edges are nearly
parallel, but
Figure 7
shows an exception. The hollow beam is simultaneously in contact with the two
other beams. The cross product version of the edge-to-edge contact formulation
resolves contact between the exterior of the hollow beam and the beam that is
near the top of
Figure 7.
The radial version of the edge-to-edge contact formulation resolves contact
between the interior of the hollow beam and the spiral-shaped beam, with the
contact direction corresponding to the interior radial direction of the hollow
beam. The radial version of the edge-to-edge contact formulation is effective
in this case because individual segments of the spiral-shaped beam span
relatively small arcs of the hollow tube.
Edge-to-edge contact example with an internal beam spiral.
In addition to choosing to activate one or both types of edge-to-edge
contact formulations, you must specify a feature angle criterion to activate
feature and perimeter edges to participate in edge-to-edge contact. See
Feature Edges
for a discussion of controls related to which feature edges are considered for
edge-to-edge contact. If only beam edges are present, specifying the contact
formulation alone is sufficient.
Edge-to-edge contact formulations do not consider twisting of the beams.
Beam-to-beam contact cannot be used to model contact between beam-like elements
that share nodes with underlying solid or shell elements (for example, beam
elements that are used to model stringers).
Vertex-to-Surface Contact Scenarios
The general contact algorithm can consider three-dimensional
vertex-to-surface contact except on crack surfaces for enriched elements.
Figure 8
shows examples in which the vertex-to-surface contact formulation is most
effective for resolving contact. The vertex-to-surface contact formulation is
intended to avoid localized penetration of a node at a convex corner of a solid
or shell/membrane surface or at an end point or kink of a beam/truss into a
relatively smooth portion of another surface (which may be an analytical rigid
surface). Most vertex nodes are along feature edges, although, for example, a
node at the tip of a cone may satisfy the vertex node criteria. See
Vertex Nodes
for a discussion of the vertex node criteria. Vertex nodes are effectively
treated as spherical in the vertex-to-surface formulation. The spherical radius
of the contact vertex corresponds to the surface thickness at the node.
Vertex-to-surface contact examples.
The bottom-right example in
Figure 8
shows a vertex node of an element-based surface in contact with an analytical
rigid surface. The corners of an analytical rigid surface do not act as
vertices in the vertex-to-surface formulation. Convergence behavior can be
enhanced by avoiding feature edges and corners in analytical rigid surfaces
used for contact and instead using smooth analytical rigid surfaces with
continuously varying surface normal directions for contact.
Output
Output variables associated with contact fall into two categories: nodal
variables (sometimes called constraint variables) and whole surface variables.
In addition,
Abaqus
outputs an array of diagnostic information associated with contact
interactions, as discussed in
Contact Diagnostics in an Abaqus/Standard Analysis,
and internal surfaces generated for general contact.
General Contact Domain and Component Surfaces in Abaqus/Standard
Abaqus/Standard
generates the following internal surfaces associated with general contact:
General_Contact_Faces,
General_Contact_Edges,
General_Contact_Vertices,
General_Contact_Faces_k,
General_Contact_Edges_k,
and
General_Contact_Vertices_k,
where k
corresponds to an automatically assigned “component number.” The three internal
surfaces for general contact without a component number contain all surface
faces, all feature edges, and all vertices, respectively, included in the
general contact domain.
Each feature edge component surface,
General_Contact_Edges_k,
has a subset of face edges (satisfying the feature edge criteria) of the corresponding
face component surface,
General_Contact_Faces_k.
Each vertex component surface,
General_Contact_Vertices_k,
has a subset of vertices (satisfying the vertex criteria) of the corresponding face
component surface,
General_Contact_Faces_k. The
face component surfaces have no nodes in common with each other, except if beams and
trusses are part of the contact domain that may share nodes with other faceted component
surfaces. By default, a lowered-numbered component surface will act as a main surface to a
higher-numbered component surface for the surface-to-surface and the radial version of the
edge-to-edge formulations. Component numbers do not influence what is considered by the
edge-to-surface, vertex-to-surface, and cross version of the edge-to-edge formulations. A
component surface consisting of beam and truss elements will act as a main surface in the
edge-to-surface formulation if half of the average element radius is larger than the
average smallest facet length of the faceted component surface. Component surfaces are
referred to in diagnostic messages for all formulation types.
Abaqus/Standard
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 surface names generated by
Abaqus/Standard
should not be used in model definitions.
Nodal Contact Variables
Nodal contact variables include contact pressure and force, frictional shear
stress and force, relative tangential motion (slip) of the surfaces during contact,
clearance between surfaces, heat or fluid flux per unit area, and fluid pressure. Many of
the nodal contact variables written to the output database (.odb)
file are often available for all contact nodes, regardless of whether they act as
secondary or main nodes. Other nodal contact variables are available only at nodes acting
as secondary nodes. Most contact output to the data (.dat) file,
results (.fil) file, and the utility subroutine
GETVRMAVGATNODE is associated with
individual constraints. For contact output to the output database
(.odb) file, some filtering is applied to reduce contact output
noise.
Contact Pressure
The contact pressure distribution is of key interest in many
Abaqus
analyses. You can view the contact pressure on all contact surfaces except for
analytical rigid surfaces and discrete rigid surfaces based on rigid-type
elements (the latter restriction does not apply to general contact). You can
view a contour plot of the contact pressure error indicator next to a contour
plot of the contact pressure to gain perspective on local accuracy of the
contact pressure solution in regions where the contact pressure solution is of
interest.
In some cases you may observe the contact pressure extending beyond the
actual contact zone due to the following factors:
The contour plots are constructed by interpolating nodal values, which
can cause nonzero values to appear within portions of facets outside of the
contact region. For example, this effect is often noticeable at corners, such
as when two same-sized, aligned blocks are in contact—if the contact surfaces
wrap around the corners, the contact pressure contours will extend slightly
around the corners.
Abaqus/Standard outputs postprocessed contact stresses to the output database. During
postprocessing, nodal contact stresses are calculated as weighted averages of values
associated with active contact constraints in which the node participates. For
example, a main node can participate in multiple constraints whose connectivities
contain the node. Similarly, a secondary node can participate in multiple
constraints from different formulations (such as surface-to-surface,
edge-to-surface, and vertex-to-surface) at secondary node locations that are corners
and edge features.
The weighting depends on the contact constraint area and a scaling factor based on the
strength of the participation of the node in a constraint. The weighted averaging is
intended to reduce contact stress noise. Modifications are made for calculating
weightings, for example, at the corner nodes of quadratic faces (with zero
consistent nodal areas) and main nodes that are outside the active contact region
but participate in contact weakly through an active contact constraint. These
modifications also have a filtering effect in terms of reducing contact stress
values reported for nodes on the fringe of the active contact region. For such
locations, contact nodal areas that are simply cumulative scaled constraint areas
across constraints in which a node participates do not have much bearing on contact
stress values.
In addition to averaging and filtering, contact stresses are also
smoothed during the postprocessing operations. However, this filtering and
subsequent smoothing are not "perfect" and can result in the contact zone size
appearing somewhat exaggerated. Similarly, contact status output is also
affected at nodes that lie on the fringe of the active contact region. In such
cases, the contact status may be reported as closed at nodes in the exaggerated
region even though it is open.
Due to these factors, trying to infer the contact force distribution from
the contact stress distribution can be somewhat misleading. Instead, you can
request nodal contact force output, which accurately represents the contact
force distribution present in the analysis.
Contact Stresses due to Edge-to-Surface, Edge-to-Edge, and Vertex-to-Surface Interactions
For edge-to-surface contact and for edge-to-edge contact with the radial
formulation where the active contact is along a line, the output variable CLINELOAD can be requested to the output database
(.odb) in
Abaqus/Standard.
This contact load has units of force per length and is mesh independent.
Contact stresses (in units of force per area) solely due to edge-to-surface
contact (CSTRESSETOS) can be output for visualizing regions where the
edge-to-surface constraints are active. The edge-to-surface formulation
computes contact stresses in units of force per area by dividing contact force
per edge length by a representative surface facet length. Since the contact
area depends on the mesh size, edge-to-surface contact stresses are mesh
dependent. For edge-to-edge contact using the cross product formulation where
the active contact region is idealized as a point, the mesh-independent output
variable CPOINTLOAD (with units of force) can be requested.
For vertex-to-surface contact, the mesh-independent output variable CPOINTLOAD (with units of force) can be requested to the output database
(.odb) in
Abaqus/Standard.
Contact stresses (CSTRESS) contain contributions from surface-to-surface,
edge-to-surface, edge-to-edge, and vertex-to-surface constraints, if active.
While accumulating contributions from edge-to-surface, edge-to-edge, and
vertex-to-surface contact constraints, the constraint values are divided by
either a representative surface facet length or its squared value to
appropriately scale them to have units of force per area.
Edges and vertices represent a discontinuity in the surface smoothness,
and the true contact stress solution near an edge or a vertex is commonly
characterized by a strong gradient. Subsequently, error indicator output for
contact stresses (CSTRESSERI) are typically quite high and acceptable for regions in which
constraints involving edges and vertices are significant.
Whole Surface Variables
Whole surface variables are only marginally supported for general contact in Abaqus/Standard because these variable are associated with the overall general contact domain by
default rather than individual surfaces associated with general contact. The only way to
limit whole surface variables to be affected by a portion of the general contact domain is
to specify a node set in the output request. Whole surface variables are computed as sums
over all nodes (or optionally limited to a particular node set) of general contact while
acting as secondary nodes. For example,
CFN is the total force acting on
secondary nodes due to contact pressure.
CFN and other whole surface variables
for general contact are typically of little utility, because contributions to the variable
from different interactions within general contact will often cancel one another and the
net result will typically depend on internal assignments of main and secondary roles.
Requesting Output
Certain contact variables must be requested as a group. For example, to
output the clearance between surfaces (COPEN), you must request the variable CDISP (contact displacements). CDISP outputs both COPEN and CSLIP (tangential motion of the surfaces during contact). A complete
listing of available contact variables and identifiers is given in
Abaqus/Standard Output Variable Identifiers.
Output requests can be limited by specifying a node set containing a subset of the nodes acting
as secondary nodes for some general contact interactions. Instructions on forming these
output requests are available in the following sections:
Abaqus
reports the values of tangential variables (frictional shear stress, viscous
shear stress, and relative tangential motion) with respect to the local tangent
directions defined on the surfaces. The local tangent directions CTANDIR1 and CTANDIR2 can be output by requesting the generic output variable CTANDIR. The definition of local tangent directions is explained in
Local Tangent Directions on a Surface.
These directions do not always correspond to the global coordinate system, and
they rotate with the contact pair in a geometrically nonlinear analysis.
Abaqus/Standard
calculates tangential results at each constraint point by taking the scalar
product of the variable's vector and a local tangent direction,
or ,
associated with the constraint point. The number at the end of a variable's
name indicates whether the variable corresponds to the first or second local
tangent direction. For example, CSHEAR1 is the frictional shear stress component in the first local
tangent direction, while CSHEAR2 is the frictional shear stress component in the second local
tangent direction.
Definition of Accumulated Incremental Relative Motion (Slip)
Abaqus/Standard defines the incremental relative motion (also known as slip) as the scalar product of
the incremental relative nodal displacement vector and a local tangent direction. The
incremental relative nodal displacement vector measures the motion of a secondary node
relative to the motion of the main surface. The incremental slip is accumulated only
when the secondary node is contacting the main surface. The sums of all such incremental
slips during the analysis are reported as
CSLIP1 and
CSLIP2. Details about the calculation
of this quantity can be found in Small-sliding interaction between bodies, Finite-sliding interaction between deformable bodies, and Finite-sliding interaction between a deformable and a rigid body.
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, etc.) may 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/Standard
provides contact opening output; COPEN will be provided up to gap distances equal to a specified
“tracking thickness.” Using this control may increase computational cost due to
extra contact tracking computations, especially if you specify a large tracking
thickness value.
Energy stored among all penalty springs and
“softened” contact constraints associated with normal contact constraints
ALLCCEN
Energy stored among all penalty springs
associated with tangential contact constraints
ALLCCET
Energy stored among all penalty springs and
“softened” contact constraints associated with normal and tangential contact
constraints (equal to the sum of ALLCCEN and ALLCCET)
ALLCCE
Energy dissipation associated
with contact stabilization and contact damping
Normal contact direction for the whole model
ALLCCSDN
Tangential contact direction for the whole
model
ALLCCSDT
Whole model (equal to the sum of ALLCCSDN and ALLCCSDT)
ALLCCSD
Energy associated with contact constraint
“discontinuity work”
Accounts for the portion of the work done by
contact forces when contact conditions change that is not accounted for by
other contact energy variables
ALLCCDW
The output variables ALLSD and ALLVD also account for dissipative energies associated with contact
stabilization and contact damping.
The elastic contact energies and dissipative energies associated with
contact stabilization and contact damping are associated with numerical effects
that would be zero in idealized situations, such as infinite penalty stiffness
or zero stabilization stiffness. Significant values of these output variables
compared to other physically based energies in a model, such as internal energy
(ALLIE), are sometimes indicative of solution inaccuracy. The contact
constraint discontinuity work will tend to zero as the time increment size
becomes very small. However, as discussed in
Energy computations in a contact analysis,
it is quite common for ALLCCDW to have a significant value without causing solution
inaccuracy.
The modified external work (ALLWK + ALLCCDW) is often representative of the physical external work in
contact problems in terms of being equal to the sum of the stored and
dissipated energies (see
Energy computations in a contact analysis).
Consider a particular contact constraint having a gap distance,
,
in one increment and becoming closed with contact force,
,
in the next increment (see
Figure 9).
A trapezoidal rule for integrating the work done by the contact force
multiplies the average force by the relative incremental motion. In this case
the resulting contribution to ALLCCDW is negative .
This energy contribution is nonphysical and would disappear in the numerics as
the time increment tends to zero. When contact opens up, similar behavior
happens with sign reversals. Numerical integration for ALLWK is also limited with respect to accounting accurately for
sudden changes in external forces. Summing ALLWK and ALLCCDW often cancels the respective nonphysical energy contributions,
and the net effect on the total energy balance ETOTAL is zero.
One contact point example to illustrate contributions to ALLCCDW.
