The initial geometry of a cohesive element is defined:
by the nodal connectivity of the element and the position of these
nodes;
by the stack direction, which can be used to specify the top and the
bottom faces of the cohesive element independent of the nodal connectivity; and
by the magnitude of the initial constitutive thickness, which can
either correspond to the geometric thickness implied by the nodal positions and
stack direction or be specified directly.
The connectivity of a cohesive element is like that of a continuum element;
however, it is useful to think of a cohesive element as being composed of two
faces (a bottom and a top face) separated by the cohesive zone thickness. The
element has nodes on its bottom face and corresponding nodes on its top face.
Pore pressure cohesive elements include a third, middle face, which is used to
model fluid flow within the element.
Three methods are available to define the element connectivity.
By Directly Defining the Element's Complete Connectivity
By Defining the Bottom-Face Element Connectivity and an Integer Offset
Alternatively, you can specify the connectivity of the bottom face plus a
positive integer offset (see
Defining Cohesive Elements)
that will be used to determine the remaining cohesive element nodes.
The integer offset will be used to define node numbers of the top face of
the cohesive element.
Abaqus
will automatically position the nodes of the top face to be coincident with
those of the bottom face unless the nodes of the top face have already been
assigned coordinates directly with a node definition (Node Definition).
Use with Pore Pressure-Displacement Cohesive Elements
When you define only the bottom face nodes, the integer offset will first
be used to define the node numbers of the top face of the cohesive element,
with the numbering of the top-face nodes offset from the bottom face node
numbers. The integer offset will again be used to define the middle surface
node numbers offset, with the numbering of the middle-face nodes offset from
the top face node numbers.
Abaqus
will automatically position the nodes of the top and middle faces to be
coincident with those of the bottom face unless the nodes of the top face have
already been assigned coordinates directly with a node definition (Node Definition).
By Defining the Bottom- and Top-Face Element Connectivities and an Integer Offset
For pore pressure cohesive elements, you also can specify the connectivity
of the bottom and top faces plus a positive integer offset (see
Defining Cohesive Elements)
that will be used to determine the middle face cohesive element nodes.
When you define the bottom and top face nodes, the integer offset will be
used to define the node numbers of the middle face, with the numbering of the
middle-face nodes offset from the bottom face node numbers.
Abaqus
will automatically position the nodes of the middle face to be halfway between
those of the bottom and top faces unless the nodes of the middle face have
already been assigned coordinates directly with a node definition (Node Definition).
Specifying the out-of-Plane Thickness for Two-Dimensional Elements
For two-dimensional cohesive elements the out-of-plane thickness is
required. You specify this additional information in the cohesive section
definition; the default value is 1.0.
Property module:
cohesive section editor: toggle on Out-of-plane thickness:
and specify the out-of-plane
thickness
Specifying the Constitutive Thickness
You can specify the constitutive thickness of the cohesive element directly
or allow
Abaqus
to compute it based on nodal coordinates such that the constitutive thickness
is equal to the geometric thickness. The default behavior depends on the nature
of the application.
If the geometric thickness of the cohesive element is very small compared to
its surface dimensions, the thickness computed from the nodal coordinates may
be inaccurate. In such cases you can specify a constant thickness directly when
defining the section properties of these elements.
The characteristic element length of a cohesive element is equal to its
constitutive thickness. The characteristic element length is often useful in
defining the evolution of damage in materials (see
Mesh Dependency).
When the Cohesive Element Response Is Based on a Continuum Approach
When the response of the cohesive elements is based on a continuum approach,
by default the constitutive thickness of the element is computed by
Abaqus
based on the nodal coordinates. You can override this default by specifying the
constitutive thickness directly.
Input File Usage
Use the following option to have
Abaqus
compute the thickness based on the nodal coordinates:
Use the following option to specify the thickness
directly:
COHESIVE SECTION, RESPONSE=CONTINUUM,
THICKNESS=SPECIFIEDthickness (1.0 by default)
Abaqus/CAE Usage
Property module:
cohesive section editor: Response:
Continuum: Initial thickness:
Use nodal coordinates, Specify:
thickness, or Use analysis
default
When the Cohesive Element Response Is Based on a Traction-Separation Approach
When the response of the cohesive elements is based on a traction-separation
approach,
Abaqus
assumes by default that the constitutive thickness is equal to one. This
default value is motivated by the fact that the geometric thickness of cohesive
elements is often equal to (or very close to) zero for the kinds of
applications in which a traction-separation-based constitutive response is
appropriate. This default choice ensures that nominal strains are equal to the
relative separation displacements (see
Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description
for further details). You can override this default by specifying another value
or specifying that the constitutive thickness should be equal to the geometric
thickness.
Input File Usage
Use the following option to specify the thickness
directly:
COHESIVE SECTION, RESPONSE=TRACTION SEPARATION,
THICKNESS=SPECIFIED (default)
thickness (1.0 by default)
Use the following option to have
Abaqus
compute the thickness based on the nodal coordinates:
Property module:
cohesive section editor: Response: Traction
Separation: Initial thickness:
Specify: thickness,
Use analysis default, or Use nodal
coordinates
When the Cohesive Element Response Is Based on a Uniaxial Stress State
When the response of the cohesive elements is based on a uniaxial stress
state, there is no default method for computing the constitutive thickness. You
must indicate your choice of the method of determining the constitutive
thickness.
Input File Usage
Use the following option to specify the thickness:
COHESIVE SECTION, RESPONSE=GASKET,
THICKNESS=SPECIFIEDthickness (1.0 by default)
Use the following option to have
Abaqus
compute the thickness based on the nodal coordinates:
Property module:
cohesive section editor: Response:
Gasket: Initial thickness:
Specify: thickness or
Use nodal
coordinates
Element Thickness Direction Definition
It is important to define the orientation of cohesive elements correctly,
since the behavior of the elements is different in the thickness and in-plane
directions. By default, the top and bottom faces of cohesive elements are as
shown in
Figure 1
for three-dimensional cohesive elements and
Figure 2
for two-dimensional and axisymmetric cohesive elements. Options for overriding
the default orientation of cohesive elements are discussed below along with an
explanation of how the local thickness direction and in-plane direction vectors
are established.
Figure 1. Default thickness direction for three-dimensional cohesive
elements. Figure 2. Default thickness direction for two-dimensional and axisymmetric
cohesive elements.
Setting the Stack Direction Equal to an Isoparametric Direction
The “stack direction” refers to the isoparametric direction along which the
top and bottom faces of a cohesive element are stacked. By default, the top and
bottom faces are stacked along the third isoparametric direction in
three-dimensional cohesive elements and along the second isoparametric
direction in two-dimensional and axisymmetric cohesive elements. You can choose
to stack the top and bottom faces along an alternate isoparametric direction
for most element types (the COH3D6 element can have only the third isoparametric direction as the
stack direction). The choice of the isoparametric direction depends on the
element connectivity. For a mesh-independent specification, use an
orientation-based method as described below. The isoparametric direction
choices for three-dimensional cohesive elements are shown in
Figure 3.
Figure 3. Stack directions for COH3D8 (left) and COH3D6 (right) elements.
Input File Usage
Use the following option to define the element top and
bottom faces based on the element's isoparametric directions:
You cannot define the stack direction based on isoparametric directions
in
Abaqus/CAE.
The stack direction will correspond to the default discussed
above.
Setting the Stack Direction Based on a User-Defined Orientation
You can also control the orientation of the stack direction through a
user-defined local orientation (Orientations).
When you define an orientation for cohesive elements, you also specify an axis
about which the local 1 and
2 material directions may be rotated. This
axis also defines an approximate normal direction. The stack direction will be
the element isoparametric direction that is closest to this approximate normal
(see
Figure 4).
Figure 4. Example illustrating the use of a cylindrical system to define the
stack direction.
Input File Usage
Use the following option to define the element thickness
direction based on a user-defined orientation:
You cannot define the stack direction based on an orientation definition
in
Abaqus/CAE.
The stack direction will correspond to the default discussed
above.
Verifying the Stack Direction
The stack direction can be verified visually in
Abaqus/CAE
by using the stack direction query tool (see
Understanding the role of the Query toolset).
For three-dimensional elements
Abaqus/CAE
colors the top face brown and the bottom face purple. For two-dimensional and
axisymmetric elements, arrows indicate the orientation of the element. In
addition,
Abaqus/CAE
highlights any element faces and edges that have inconsistent orientations.
Alternatively, the material axes can be plotted in the
Visualization module of
Abaqus/CAE
to verify that the 3-axis points in the desired normal direction for
three-dimensional elements; and if the element is oriented improperly, one of
the in-plane axes (either the 1- or 2-axis) will point in the normal direction.
For two-dimensional and axisymmetric elements, the stack direction is
consistent with the 2-axis material direction.
Thickness Direction Computation for Two-Dimensional and Axisymmetric Elements
To compute the thickness direction for two-dimensional and axisymmetric
elements,
Abaqus
forms a midsurface by averaging the coordinates of the node pairs forming the
bottom and top surfaces of the element. This midsurface passes through the
integration points of the element, as shown in
Figure 5
for the default choice of the bottom and top surfaces. For each integration
point
Abaqus
computes a tangent whose direction is defined by the sequence of nodes given on
the bottom and top surfaces. The thickness direction is then obtained as the
cross product of the out-of-plane and tangent directions.
Figure 5. Thickness direction for a two-dimensional or axisymmetric
element.
Thickness Direction Computation for Three-Dimensional Elements
To compute the thickness direction for three-dimensional elements,
Abaqus
forms a midsurface by averaging the coordinates of the node pairs forming the
bottom and top surfaces of the element. This midsurface passes through the
integration points of the element, as shown in
Figure 6
for the default choice of the bottom and top surfaces.
Abaqus
computes the thickness direction as the normal to the midsurface at each
integration point; the positive direction is obtained with the right-hand rule
going around the nodes of the element on the bottom or top surface.
Figure 6. Thickness direction for a three-dimensional element.
Local Directions at Integration Points
Abaqus
computes default local directions at each integration point. The local
directions are used for output of all quantities that describe the current
deformation state of a cohesive element. Details of local directions are
discussed separately below for cohesive elements with two versus three local
directions.
Local Directions for Two-Dimensional and Axisymmetric Cohesive Elements
The local 2-direction for two-dimensional and axisymmetric cohesive elements
corresponds to the thickness direction, which is computed as discussed above in
Element Thickness Direction Definition.
The local 1-direction is defined such that the cross product between the local
1- and 2-directions gives the out-of-plane direction (see
Figure 7).
You cannot modify either local direction for these elements for a given stack
orientation. Transverse shear behavior is defined in the 1–2 plane for these
elements.
Figure 7. Local directions for two-dimensional and axisymmetric cohesive
elements.
Local Directions for Three-Dimensional Cohesive Elements
The local 3-direction for three-dimensional cohesive elements corresponds to
the thickness direction, which is computed as discussed above in
Element Thickness Direction Definition
and cannot be modified for a given stack orientation. The local 1- and
2-directions are normal to the thickness direction and, by default, are defined
by the standard
Abaqus
convention for local directions on surfaces (Conventions).
The default local directions for a three-dimensional cohesive element are shown
in
Figure 8.
Figure 8. Local directions for three-dimensional cohesive elements.
Transverse shear behavior is defined in the local 1–3 and 2–3 planes for
these elements. You can modify the local 1- and 2-directions for
three-dimensional cohesive elements in the plane normal to the thickness
direction by using a local orientation definition (Orientations).
