Surface Properties for General Contact in Abaqus/Standard
Surface property assignments:
can be used to specify geometric corrections for regions of a surface;
can be used to change the contact thickness used for regions of a
surface based on structural elements or to add a contact thickness for regions
of a surface based on solid elements;
can be used to specify surface offsets for regions of a surface based
on shell, membrane, rigid, and surface elements; and
can be applied selectively to particular regions within a general
contact domain.
You can assign nondefault surface properties to surfaces involved in general
contact interactions. These properties are considered only when the surfaces
are involved in general contact interactions; they are not considered when the
surfaces are involved in other interactions such as contact pairs. The general
contact algorithm does not consider surface properties specified as part of the
surface definition. The regions with nondefault surface properties are
identified with surface names or material names. For example, surface property
SurfProp_A can assign a nondefault surface thickness
to surface
Surf_1 or to the surface whose underlying elements
have a section assignment with material
Rubber. Material names cannot be used to control beam
smoothing or to assign geometric corrections.
Surface properties for general contact in
Abaqus/Standard
are assigned at the beginning of an analysis and cannot be modified across
steps.
The surface names used to specify the regions with nondefault surface
properties do not have to correspond to the surface names used to specify the
general contact domain. In many cases the contact interaction will be defined
for a large domain, while nondefault surface properties will be assigned to a
subset of this domain. Any surface property assignments for regions that fall
outside the general contact domain will be ignored. The last assignment will
take precedence if the specified regions overlap.
This option must be used in conjunction with the
CONTACT option and should appear at most once for each value of
the PROPERTY parameter discussed below; the data line can be repeated as
often as necessary to assign surface properties to different
regions.
Geometry-Based Corrections for Curved Surfaces
Contact calculations are based on unsmoothed, faceted representations of the
finite element surfaces in a general contact domain. For curved surfaces, the
finite element representation of a surface can deviate significantly from the
original geometry that was used to generate the finite element mesh. A contact
smoothing technique based on the original geometric representation can be
employed for a more realistic simulation of contact interactions between curved
surfaces, resulting in improved accuracy of stresses and distances between the
contacting surfaces. This contact smoothing technique is discussed in more
detail in
Smoothing Contact Surfaces in Abaqus/Standard.
Surface Thickness
The default surface thickness is equal to the original parent element
thickness. Alternatively, you can specify a value for the surface thickness or
a thickness scaling factor. A nonzero thickness can be assigned to solid
element surfaces; for example, to model the effect of a finite thickness
surface coating.
Using the Original Parent Element Thickness
The default surface thickness is equal to the original parent element
thickness.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESSsurface or material, ORIGINAL (default), , SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
fourth entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Specifying a Value for the Surface Thickness
You can specify the surface thickness value directly.
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
fourth entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Applying a Scale Factor to the Surface Thickness
You can apply a scale factor to any value of the surface thickness. For
example, if you specify that the original parent element thickness should be
used for surf1 and apply a scale factor of 0.5,
a value of one half the original parent element thickness will be used for
surf1 when it is involved in a general contact
interaction (all other surfaces included in the general contact domain will use
the default original parent element thickness). Scaling the surface thickness
in this way can be used to avoid initial overclosures in some situations.
Abaqus/Standard
will automatically adjust surface positions to resolve initial overclosures
(see
Contact Initialization for General Contact in Abaqus/Standard)
associated with general contact. However, if nodal position adjustments are
undesirable (for example, if they would introduce an imperfection in an
otherwise flat part, resulting in an unrealistic buckling mode), you may prefer
to reduce the surface thickness and avoid the overclosures entirely.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESSsurface or material, value or label, scale_factor, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
fourth entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Surface Offset
A surface offset is the distance between the midplane of a thin body and its
reference plane (defined by the nodal coordinates and element connectivities).
It is computed by multiplying the offset fraction (specified as a fraction of
the surface thickness) by the surface thickness and the element facet normal.
This defines the position of the midsurface and, thus, the position of the body
with respect to the reference surface; the coordinates of the nodes on the
reference surface are not modified. Surface offsets can be specified only for
surfaces defined on shell and similar elements (i.e., membrane, rigid, and
surface elements). Surface offsets specified for other elements (e.g., solid or
beam elements) will be ignored. By default, surface offsets specified in
element section definitions will be used in the general contact algorithm.
You specify the surface offset as a fraction of the surface thickness. The
surface offset fraction can be set equal to the offset fraction used for the
surface's parent elements or to a specified value. Surface offsets specified
for general contact do not change the element integration.
Input File Usage
Use the following
option to use the surface offset fraction from the surface's parent elements
(default):
SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTIONsurface or material, ORIGINAL, SURFACE (default) or MATERIAL
Use the following option to specify a value for the surface
offset fraction:
SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTIONsurface or material, offset, SURFACE (default) or MATERIAL
The offset can be specified as a value or a label
(SPOS or
SNEG). Specifying
SPOS is equivalent to specifying a value of
0.5; specifying SNEG is equivalent to
specifying a value of −0.5.
The third entry indicates whether the
first entry refers to a surface or material name. If omitted,
Abaqus
assumes that a surface name is used.
Feature Edges
Feature edges of a model are defined on beam and truss elements and on edges
of faces (perimeter and otherwise) of solid and structural elements. General
contact in
Abaqus/Standard
includes an edge-to-surface contact formulation and an edge-to-edge contact
formulation (as supplements to the surface-to-surface formulation), as
discussed in
About General Contact in Abaqus/Standard.
By default, the edge-to-surface contact formulation considers “edges” of beam
and truss elements, perimeter edges, and edges corresponding to initial
geometric feature angles of 45° and higher. You can control the feature edge
criterion globally or locally for both edge-to-surface and edge-to-edge
contact. Feature edge criteria have no effect on “edges” of beam and truss
elements—they are activated by their inclusion in the contact domain.
Some aspects of the contact property assignment options apply only to the
surface-to-surface formulation (see
Contact Properties for General Contact in Abaqus/Standard
for further discussion of contact properties for general contact). The
edge-to-surface and edge-to-edge formulations always use the penalty
enforcement method and only involve displacement degrees of freedom. For
example, the edge-to-surface formulation or the cross edge-to-edge formulation
does not contribute to thermal gap conductance across a contact interface.
Specifying a Cutoff Feature Angle
The feature angle is the angle formed between normals of two facets
connected to an edge. The angles between facets are based on the initial
configuration. A negative angle results at concave meetings of facets;
therefore, these edges are never included in the contact domain.
Figure 1
shows some examples of how the feature angle is calculated for different edges.
Figure 1. Calculating the feature angle.
The feature angle for edge A is 90° (the angle between
and );
the feature angle for edge B is −25° (the angle between
and ).
Edge C forms a T-intersection with three facets (shown in two dimensions in
Figure 2);
its feature angles are 0°, −90°, and −90°.
Figure 2. Feature angles for a T-intersection.
Perimeter edges (for example, edge D in
Figure 1)
can be thought of as a special type of feature edge where the feature angle is
180°.
If a feature angle criterion is in effect (by default or because you
specified it), geometric edges of solid and shell bodies with feature angles
greater than or equal to the specified angle are included in the general
contact domain. The contact inclusion and exclusion options (discussed in
About General Contact in Abaqus/Standard)
apply to the surface-to-surface contact formulation, the edge-to-surface
contact formulation, and the edge-to-edge contact formulation (and further
control which portions of surfaces may interact with either formulation). The
sign of the feature angle is considered when determining whether or not a
geometric feature edge should be included in the general contact domain. For
example, if a cutoff feature angle of 20° were specified, edge A would be
activated as a feature edge in the contact model (because the feature angle of
90° is greater than the cutoff of 20°) but edges B and C would not be activated
(because the feature angle at edge B is −25° and the maximum feature angle at
edge C is 0°, which are both less than the cutoff of 20°). The cutoff feature
angle cannot be set to less than 0° or more than 180°. Specifying a small
cutoff feature angle (for example, less than 20°) may considerably increase run
time without a major impact on the results compared to a larger cutoff angle
(> 20°). The default feature angle cutoff for edge-to-surface contact is
45°, while the default is not to include feature edges in edge-to-edge contact.
The criterion for including edges for edge-to-surface contact can be different
from the criterion for including edges for edge-to-edge contact; the two are
completely independent.
Figure 3
illustrates further how the feature angle is used to determine which geometric
feature edges are activated in the general contact domain.
Figure 3. Feature edges activated in the general contact domain for a cutoff
feature angle of 45°.
The table to the right of the figure lists the feature angle values for
various edges in the model. Edges connected to shell facets, but not on the
shell perimeter, have more than one corresponding feature angle. The largest
feature angle at an edge is compared to the default or specified cutoff feature
angle. For example, if the default cutoff feature angle of 45° is in effect,
edges A, D, and E would be considered for edge-to-surface contact, while edges
B, C, and F would be ignored for edge-to-surface contact.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIAsurface or material, feature_angle_value_edge_to_surface, , feature_angle_value_edge_to_edge, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
fifth entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Specifying That Only Perimeter Edges Should Be Activated
You can specify that only perimeter edges should be considered by the
edge-to-surface and/or edge-to-edge formulation globally or in a local region.
Perimeter edges occur on “physical” perimeters of shell elements and on
“artificial” edges that occur when a subset of exposed facets on a body are
included in the general contact domain. The classification of an edge as being
on the perimeter of the contact domain (or as a geometric edge with a
particular feature angle) is based on the contact inclusion and contact
exclusion definitions and the mesh characteristics. When structural elements
share nodes with continuum elements, the perimeter edges will not be activated
on the structural elements because the criterion to designate them as such is
no longer satisfied.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIAsurface or material, PERIMETER EDGES, , PERIMETER EDGES, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The fifth
entry indicates whether the first entry refers to a surface or material name.
If omitted,
Abaqus
assumes that a surface name is used.
Specifying That Feature Edges Should Not Be Included
You can specify that no edges should be considered by the edge-to-surface
formulation globally or in a local region. However, doing so does not
deactivate “contact edges” associated with beam and truss elements. By default,
feature edges are not included for edge-to-edge contact.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIAsurface or material, NO FEATURE EDGES, , , SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
fifth entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Vertex Nodes
Vertex nodes of a model are defined on convex corners of shell and
structural surfaces and end points and kinks in beam and truss surfaces. Vertex
nodes are eligible to participate as vertices in the vertex-to-surface contact
formulation for general contact in
Abaqus/Standard.
The vertex-to-surface contact formulation is discussed in
About General Contact in Abaqus/Standard.
Some aspects of the contact property assignment options apply only to the
surface-to-surface formulation (see
Contact Properties for General Contact in Abaqus/Standard
for further discussion of contact properties for general contact). The
edge-to-surface and vertex-to-surface formulations always use the penalty
enforcement method and involve only displacement degrees of freedom. For
example, the vertex-to-surface formulation does not contribute to thermal gap
conductance across a contact interface.
Usually, only a small subset of surface nodes satisfy one of the criteria
for being a vertex node. The following algorithm is used to determine if a node
satisfies the vertex criterion for a convex corner of a solid or shell-like
surface, based on the original configuration:
Abaqus/Standard
computes an average surface normal direction for the node and an associated
plane that passes through the node and is perpendicular to this direction. Two
examples of such normal directions and planes are shown in
Figure 4.
The node is considered a vertex node if each surface edge emanating from
this node is “inside” of this plane (that is, on the opposite side of this
plane as the average surface normal direction vector) and forms an angle
greater than or equal to the vertex angle threshold with this plane, by
default. For example, the example node on the right of
Figure 4
has all adjacent surface edges on the “inside” of the plane perpendicular to
the average surface normal direction. For the other example node in
Figure 4
for which an average normal direction and corresponding plane is shown, two
adjacent surface edges lie outside of this plane (on the same side as the
outward normal direction vector), so this node would not satisfy this vertex
node criterion.
Figure 4. Examples of average surface normal directions and corresponding
planes associated with vertex node criterion.
The following additional vertex criterion is applied at nodes of perimeter
feature edges, based on the original configuration:
Abaqus/Standard
computes an average outward perimeter direction for the node and an associated
plane that passes through the node and is perpendicular to this direction.
The node is considered a vertex node if each feature edge connected to
the node is inside of this plane and forms an angle greater than or equal to
the vertex angle threshold with this plane, by default.
The following vertex criterion is applied at nodes of feature edges
associated with beams and trusses, based on the original configuration:
Abaqus/Standard
computes an average edge direction for the node and an associated plane that
passes through the node and is perpendicular to this direction.
If the average edge direction is zero, the node is not a vertex node;
otherwise, the node is considered a vertex node if each feature edge connected
to the node forms an angle greater than or equal to the vertex angle threshold
with this plane, by default.
The default vertex angle threshold is 20°. The circular dots in
Figure 5
represent examples of nodal locations that would satisfy one of the vertex node
criteria, with the default vertex angle threshold in effect.
Figure 5. Examples of vertex locations represented by circular dots.
Specifying That All Vertex Nodes Should Be Included
You can specify that all vertex nodes should be considered by the
vertex-to-surface formulation globally or in a local region.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=VERTEX CRITERIAsurface or material, ALL VERTICES, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
third entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Specifying a Vertex Angle Threshold
You can control the vertex criteria globally or locally.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=VERTEX CRITERIAsurface or material, vertex_angle_threshold, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
third entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
Specifying That Vertex Nodes Should Not Be Included
You can specify that no vertex nodes should be considered by the
vertex-to-surface formulation globally or in a local region. However, doing so
does not deactivate “contact edges” associated with beam and truss elements.
Input File Usage
SURFACE PROPERTY ASSIGNMENT, PROPERTY=VERTEX CRITERIAsurface or material, NO VERTICES, SURFACE (default) or MATERIAL
If the first entry is omitted, a default surface that
encompasses the entire general contact domain is assumed.
The
third entry indicates whether the first entry refers to a surface or material
name. If omitted,
Abaqus
assumes that a surface name is used.
