can model the finite-sliding interaction between two deforming bodies
when the sliding occurs along a line (“slide line”) that lies in a specific
plane;
assume that tangential motions orthogonal to a slide line are zero or
small (Abaqus/Standard
treats such motions as being infinitesimal);
can be used with axisymmetric stress/displacement elements;
are recommended for specific applications, such as when a contact
surface is the surface of a substructure or when CAXA or SAXA elements are involved in contact;
are available for first- and second-order elements; and
use the same “master-slave” concepts for enforcing contact constraints
seen in surface-based contact.
Modeling contact between deformable bodies with slide lines
Determining the location of the areas of contact and the surface tractions
between contacting structures are common goals of
Abaqus
simulations (see
Figure 1).
Slide lines and slide line contact elements can provide this information for
simulations where both structures are deformable and the finite sliding of the
structures occurs along well-defined lines.
Figure 1. Interaction between deformable structures.
Local basis system for contact stresses and relative motions of the
bodies
Abaqus/Standard
reports the contact stresses between the bodies and the relative motions of the
bodies in a local basis system that is attached to the slide line surface. The
local basis system is defined by the normal to the slide line,
n, and two orthogonal
local tangent directions, t1
and t2
(see
Figure 2).
Figure 2. Local system for interface contact normal and shear traction.
Defining the local basis system
The sequence of the nodes forming the slide line defines the tangent,
t. The plane formed by
the slide line normal, n, and
t is called the contact
plane.
Abaqus/Standard
defines the slide line normal as n=s×t
(see
Figure 3),
where s=(0,0,1)
is the vector that is orthogonal to the contact plane.
As shown in
Figure 3,
a slide line is created using nodes i,
j, k, …, p,
which are specified in that order, thereby identifying the slide line tangent.
Nodes I, J, K,
…, N are the nodes of the slide line elements that are
associated with this slide line. The slide line normal
n is defined by
specifying s, the normal to the
contact plane.
Figure 3. Defining the local basis for a slide line.
The tangent to the slide line coincides with the first local tangent
direction, t1,
of the local basis system. The second local tangent direction,
t2,
is in the opposite direction of s.
The master-slave concept for slide lines and slide line elements
When creating a model that contains slide line elements, it is useful to
remember that
Abaqus/Standard
uses a strict “master-slave” concept to enforce the contact constraints. The
slide line contact elements form the “slave” surface. The nodes that you
specify to define the slide line define the “master” surface. The nodes of the
slide line contact elements are constrained not to penetrate the master
surface.
The considerations for choosing the master and slave surfaces are the same
regardless of whether surfaces or elements are used to define contact. The
master surface should be chosen as the surface of the stiffer body if the
materials are different or as the surface with the coarser mesh. If the
materials and mesh density are the same on both surfaces, the choice is
arbitrary.
Defining the slide line (master surface)
You can specify the nodes that make up the slide line, or they can be
generated as described below. If you choose to specify the nodes directly, you
must specify them in a sequence that defines a continuous slide line. The nodal
sequence defines a tangent vector, t, for the slide line.
The slide line can be made up of linear or parabolic segments, depending on
whether the model is made up of first-order or second-order elements. In either
case convergence may be improved by smoothing the slide line.
Defining a linear slide line
When the surfaces of the bodies are meshed with first-order elements, define
a slide line made up of linear element segments. As shown in
Figure 4),
nodes i, j, k,
…, p are specified in that order, thereby identifying a
slide line progressing from i through
p. Nodes I, J,
K, …, N are the nodes of the
ISL-type elements that are associated with
this slide line.
Input File Usage
SLIDE LINE, ELSET=element_set_name, TYPE=LINEARfirst node number, second node number, etc.
Figure 4. First-order (linear) slide line example.
Defining a parabolic slide line
When the surfaces of the bodies are meshed with second-order elements,
define a slide line made up of second-order element segments. In this case the
slide line should consist of an odd number of nodes. As shown in
Figure 5,
nodes i, j, k,
…, u are specified in that order, thereby identifying a
slide line progressing from i through
u. Nodes I, J,
K, …, O are the nodes of the
ISL-type elements that are associated with
this slide line.
Figure 5. Second-order (parabolic) slide line example.
Input File Usage
SLIDE LINE, ELSET=element_set_name, TYPE=PARABOLICfirst node number, second node number, etc.
Generating the slide line nodes
Alternatively, you can indicate that the slide line nodes should be
generated and specify only a first node number, a last node number, and an
increment between node numbers.
Input File Usage
SLIDE LINE, ELSET=element_set_name, GENERATEfirst node number, last node number, increment between node numbers
Smoothing the slide line
Convergence is often improved by smoothing the discontinuities in surface
tangents between slide line segments, thereby providing a smoothly varying
tangent along the slide line. For details about smoothing slide lines, see
Contact formulations in Abaqus/Standard.
Defining slide line elements (slave surface)
Many finite-sliding contact simulations can use the surface-based contact
approach, described in
Defining Contact Interactions,
to define the model. Axisymmetric stress/displacement and coupled
temperature-displacement slide line elements are recommended only for specific
applications, such as when a contact surface is the surface of a substructure
or when CAXA or SAXA elements are involved in contact (see
Contact modeling if asymmetric-axisymmetric elements are present).
The slide line contact elements define the slave surface. The contact area
associated with each node on the slave surface is calculated using the current
length of the slide line contact element and the constant “width” assigned to
the element, which depends on the underlying finite elements.
Associating the slide line elements with a slide line
You must associate the slide line with a set of slide line contact elements.
Details on defining slide lines are discussed below.
Defining nondefault mechanical surface interactions with slide line
elements
By default,
Abaqus/Standard
uses “hard,” frictionless contact with slide line elements. You can assign
optional mechanical surface interaction models. The following mechanical
surface interaction models are available:
Obtaining the “maximum torque” that can be transmitted across
axisymmetric slide lines
When modeling contact with slide lines with axisymmetric elements (type CAX and CGAX elements),
Abaqus/Standard
can calculate the maximum torque that can be transmitted across the
axisymmetric slide lines. This capability is often of interest when modeling
threaded connectors. The maximum torque, T, is defined as
T=∫∫r2pdsdθ,
where p is the pressure transmitted across the
interface, r is the radius to a point on the interface,
and s is the current distance along the interface in the
r–z plane. This definition of
“torque” effectively assumes a friction coefficient of unity.
You can request that this torque output be written to the data
(.dat) file. The data are provided for every slide line in
the model. You can specify the output frequency to limit how often
Abaqus/Standard
writes this output to the data file. The default output frequency is 1.
For surface-based contact with axisymmetric elements, output variable
CTRQ provides functionality similar to this torque
output request (see
About contact pairs in Abaqus/Standard).