are used to define layers of uniaxial reinforcement in membrane,
shell, and surface elements (such layers are treated as a smeared layer with a
constant thickness equal to the area of each reinforcing bar divided by the
reinforcing bar spacing);
can be used to add layers of reinforcement in a solid by embedding
reinforced surface or membrane elements in the “host” solid elements as
described in
Embedded Elements;
can be used to add additional stiffness, volume, and mass to the
model;
can be used to add discrete axial reinforcement in beam elements in
Abaqus/Standard;
can be used in coupled temperature-displacement analysis but do not
contribute to the thermal conductivity and specific heat;
can be used in coupled thermal-electrical-structural analysis but do
not contribute to the electrical conductivity, thermal conductivity and
specific heat;
cannot be used in heat transfer or mass diffusion analysis; and
have material properties that are distinct from those of the
underlying or host element.
do not include the mass or volume of the underlying elements.
You can specify one or multiple layers of reinforcement in membrane, shell,
or surface elements. For each layer you specify the rebar properties including
the rebar layer name; the cross-sectional area of each rebar; the rebar spacing
in the plane of the membrane, shell, or surface element; the position of the
rebars in the thickness direction (for shell elements only), measured from the
midsurface of the shell (positive in the direction of the positive normal to
the shell); the rebar material name; the initial angular orientation, in
degrees, measured relative to the local 1-direction; and the isoparametric
direction from which the rebar angle output will be measured.
You can model rebar layers in solid (continuum) elements by embedding a set
of surface or membrane elements with rebar layers defined as discussed above in
a set of host continuum elements.
Assigning a Name to the Rebar Layer
You must assign each layer of rebar in a particular element or element set a
separate name. This name can be used in defining rebar prestress and output
requests.
Specifying Rebar Geometry
The rebar geometry is always defined with respect to a local coordinate
system. Defining an appropriate local system is described in the next section.
The rebar geometry can be constant, vary as a function of radial position in a
cylindrical coordinate system, or vary according to the tire “lift” equation.
In each case you must specify the spacing, s, and the
area, A, which are used to determine the thickness of the
equivalent rebar layer, ,
as well as the angular orientation, ,
of the rebar with respect to this local system.
In addition, for shell elements you must specify the position of the rebars
in the shell thickness direction measured from the midsurface of the shell
(positive in the direction of the positive normal to the shell). If the shell's
thickness is defined by nodal thicknesses (Nodal Thicknesses),
this distance will be scaled by the ratio of the thickness defined by the nodal
thickness to the thickness defined by the section definition. If the shell's
thickness is defined with a distribution (Distribution Definition), this
distance is scaled by the ratio of the element thickness defined by the
distribution to the default thickness.
Defining Rebar with Constant Spacing
You can specify the geometry to be constant in the local rebar coordinate
system. In this case the spacing, s, is specified as a
length measure.
Defining Rebar Spacing as a Function of Radial Position
You can specify the spacing, s, in terms of angular
spacing in degrees as shown in
Figure 1.
Angular spacing values can also be used for non-radial rebars as well as
for rebars having nonzero orientation angles from the meridional plane. In
these cases the orientation angles of the rebars do not change. The angular
spacing option is used only to compute the spacing between rebars in units of
length by multiplying the angular spacing by the radial distance of the
concerned point on the rebar from the axis of axisymmetry. A local cylindrical
coordinate system must be defined for the rebar if the rebar is associated with
three-dimensional elements.
Defining Rebar Using the Tire “Lift” Equation
Structural tire analysis is often performed using the cured tire geometry
as the reference configuration for the finite element model. However, the cord
geometry is more conveniently specified with respect to the “green,” or
uncured, tire configuration. The tire lift equation provides mapping from the
uncured geometry to the cured geometry (see
Figure 2).
You can specify the spacing and orientation of the rebar cords with
respect to the uncured configuration and let
Abaqus
map these properties to the reference configuration of the cured tire. Using a
cylindrical coordinate system, the spacing, s, and angular
orientation, ,
in the cured tire are obtained from
where r is the position of the rebar along the radial
direction in the cured geometry,
is the position of the rebar in the uncured geometry,
is the spacing in the uncured geometry,
is the angle measured with respect to the projected local 1-direction in the
uncured geometry, and e is the cord extension ratio. In a
tire e represents the pre-strain that occurs during the
curing process; e =1 means a 100% extension. When
is equal to 90°, the rebar is assumed to have a constant spacing of
.
A local cylindrical coordinate system must be defined for the rebar if the
rebar is associated with three-dimensional elements.
Local Rebar Orientation System
The rebar geometry, such as rebar orientation and spacing, is defined with
respect to a local orientation system. This local rebar orientation system is
entirely independent from the local orientation system used for the underlying
assignment.
The rebar angle is always defined with respect to the local 1-direction as
shown in
Figure 3.
Rebar defined with either angular spacing or spacing defined by the tire
lift equation is specified with respect to a cylindrical orientation system.
For axisymmetric analysis the global coordinate system is used as the
cylindrical system. For three-dimensional analysis you must provide a
user-defined cylindrical orientation definition.
Local Orientation System for Three-Dimensional Elements
You can define the local system by referring to a user-defined local
coordinate system. See
Orientations
for a description of how the local coordinate system is calculated from the
user-defined directions for definition of rebar in shell, membrane, and surface
elements.
If you do not specify a user-defined orientation, the local 1-direction is
based on the default projected local coordinate system. See
Conventions
for a definition of the default projected local directions on a surface in
space.
A positive angle
defines a rotation from local direction 1 to local direction 2 around the
element's normal direction or the user-defined normal direction. If the shell,
membrane, or surface element is curved in space, the local 1-direction will
vary across the element and the initial rebar angular orientation will also
vary accordingly. The orientation definition that can optionally be associated
with a shell or membrane section definition has no influence on the rebar
angular orientation definitions. For example, in a membrane section, shell
section, or surface section, the following data would result in the rebar layer
definition shown in
Figure 4:
A=0.01; s=0.1; distance of rebar from
the shell midsurface=0.0; =30.;
and the rebar definition refers to a local rectangular orientation defined to
have its X-axis go through the point (−0.7071, 0.7071,
0.0), its
plane include the point (−0.7071, −0.7071, 0.0), and an additional rotation of
0.0 degrees about the 3-direction.
The following data would result in the rebar layer definition shown in
Figure 5:
A=0.01, s=0.1, distance of rebar from
the shell midsurface=0.0, and =45.
Local Orientation System for Axisymmetric Elements
Rebars in an axisymmetric membrane element or an axisymmetric surface
element must lie in the element reference surface, whereas rebars in an
axisymmetric shell can lie in the shell reference surface or can be offset from
the midsurface. Rebars in axisymmetric membrane, shell, and surface elements
can be defined to have any angular orientation with respect to the
r–z plane. See
Figure 6
for an example of circumferential rebars and
Figure 1
for an example of radial rebars in axisymmetric shells.
You cannot specify a user-defined orientation for rebar layers in
axisymmetric membrane, shell, and surface elements. Instead, in the rebar layer
definition you specify the angular orientation of the rebar layer, in degrees,
with respect to the r–z plane; this
orientation is measured positive about the positive normal to the membrane,
shell, or surface element.
If you specify an orientation angle other than 0° or 90° for rebar in an
axisymmetric membrane without twist, axisymmetric shell, or axisymmetric
surface without twist,
Abaqus
assumes that the rebars are balanced (i.e., half the rebar lie at the specified
angle
and the other half at an angle of )
and internal calculations are handled accordingly. Such a rebar definition
should not be used with the symmetric model generation capability (Symmetric Model Generation).
The recommended modeling technique is to define unbalanced rebar in
axisymmetric elements with twist. Balanced rebar, on the other hand, can be
defined in regular axisymmetric elements or in axisymmetric elements with twist
and should be defined by specifying half the rebar at the specified angle
and the other half at an angle of .
Large-Displacement Considerations
In geometrically nonlinear analyses as the rebar-reinforced element deforms,
the initially defined geometric properties and orientation of the rebar layer
can change as a result of finite-strain effects. The deformation of the rebar
layer is determined from the deformation gradient of the underlying shell,
membrane, or surface element. Rebars rotate with the actual deformation and not
with the average rigid body rotation of the material point in the underlying
element. See
Rebar modeling in shell, membrane, and surface elements
for details.
For example, consider a plate modeled with a first-order element under large
pure shear deformation as shown in
Figure 7,
where rebars are initially aligned with the element isoparametric directions.
As a result of finite-strain effects, rebars rotate but remain aligned with
the element isoparametric directions. If the same problem is modeled using
anisotropic material properties rather than rebars and the material directions
(1 and 2) are initially aligned with the element isoparametric directions,
under such large shear deformation the material directions rotate and are no
longer aligned with the element isoparametric directions. The material
directions in this case are determined based on the average rigid body rotation
of the material point. Hence, if the material is not truly a continuum, the
anisotropic behavior is better modeled with rebars.
Defining Rebar in Abaqus/Standard Beam Elements
You must use element-based rebar, described in
Defining Rebar as an Element Property,
to model discrete rebar in beam elements in
Abaqus/Standard.
You specify the elements that contain the rebar, the cross-sectional area of
each rebar, and the location of each rebar with respect to the local beam
section axis (see
Figure 8).
Each individual rebar must be assigned a separate name in a particular
element or element set. This name can be used in defining rebar prestress and
output requests.
Defining the Rebar Material
The material properties of the rebars are distinct from those of the
underlying element and are defined by a separate material definition (Material Data Definition).
You must associate each rebar layer (or, for beam elements in
Abaqus/Standard,
each rebar definition) with a set of material properties.
The following material behavior cannot be used in
Abaqus/Standard
to define rebar materials:
If a nonzero density is specified for the material in a rebar layer, the
mass of the rebar is taken into account for dynamic analysis as well as for
gravity, centrifugal, and rotary acceleration distributed loads.
The mass is not taken into account for rebar in beam elements (available
only in
Abaqus/Standard);
you should adapt the density of the beam material to account for the rebar
mass.
Initial Conditions
Initial conditions (Initial Conditions)
can be used to define prestress or solution-dependent values for rebars.
Defining Prestress in Rebar
For structures in which reinforcing is defined (such as reinforced concrete
structures), you can use initial conditions to define the prestress in the
rebars.
In such cases in
Abaqus/Standard the
structure must be brought to a state of equilibrium before it is actively
loaded by means of an initial static analysis step (Static Stress Analysis)
with no external loads applied (or, perhaps, with the “dead” loads only)—see
Initial Conditions.
Holding Prestress in Rebar in Abaqus/Standard
If prestress is defined in the rebars and unless the prestress is held
fixed, it will be allowed to change during an equilibrating static analysis
step; this is a result of the straining of the structure as the
self-equilibrating stress state establishes itself. An example is the
pretension type of concrete prestressing in which reinforcing tendons are
initially stretched to a desired tension before being covered by concrete.
After the concrete cures and bonds to the rebar, release of the initial rebar
tension transfers load to the concrete, introducing compressive stresses in the
concrete. The resulting deformation in the concrete reduces the stress in the
rebar.
Alternatively, you can keep the initial stress defined in some or all of the
rebars constant during this initial equilibrium solution. An example is the
post-tension type of concrete prestressing; the rebars are allowed to slide
through the concrete (normally they are in conduits), and the prestress loading
is maintained by some external source (prestressing jacks). The magnitude of
the prestress in the rebar is normally part of the design requirements and must
not be reduced as the concrete compresses under the loading of the
prestressing. Normally, the prestress is held constant only in the first step
of an analysis. This is generally the more common assumption for prestressing.
If the prestress is not held constant in analysis steps following the step
in which it is held constant, the stress in the rebar will change due to
additional deformation in the concrete. If there is no additional deformation,
the stress in the rebar will remain at the level set by the initial conditions.
If the loading history is such that no plastic deformation is induced in the
concrete or rebar in steps subsequent to the steps in which the prestress is
held constant, the stress in the rebar will return to the level set by the
initial conditions upon removal of the loading applied in those steps.
Defining the Initial Values of Solution-Dependent State Variables for Rebars
You can define the initial values of solution-dependent state variables for
rebars within elements. See
Initial Conditions
for details.
Output
Rebar force output is available at the rebar integration locations with
output variable RBFOR. The rebar force is equal to the rebar stress times the current
rebar cross-sectional area. The current cross-sectional area of the rebar is
calculated by assuming the rebar is made of an incompressible material,
regardless of the actual material definition. For rebars in membrane, shell, or
surface elements output variables RBANG and RBROT identify the current orientation of rebar within the element
and the relative rotation of the rebar as a result of finite deformation,
respectively. These quantities are measured with respect to the user-specified
isoparametric direction in the element, not the default local element system or
the orientation-defined system. See
Rebar modeling in shell, membrane, and surface elements.
See
Abaqus/Standard Output Variable Identifiers
and
Abaqus/Explicit Output Variable Identifiers
for information on additional output quantities such as stress and strain. For
rebars in membrane, shell, or surface elements with multiple integration
points, output quantities are available at the integration points and at the
centroid of the element.
Specifying the Direction for Rebar Angle Output
The output quantities RBANG and RBROT can be measured from either of the isoparametric directions in
the plane of the membrane, shell, or surface elements. You can specify the
desired isoparametric direction from which the rebar angle will be measured (1
or 2). The rebar angle is measured from the isoparametric direction to the
rebar with a positive angle defined as a counterclockwise rotation around the
element's normal direction. The default direction is the first isoparametric
direction.
In axisymmetric shell, surface, and membrane elements the first
isoparametric direction coincides with the meridional direction, and the second
isoparametric direction coincides with the hoop direction. In triangular
elements
Abaqus
defines the isoparametric directions as follows: for a 3-node triangle the
first isoparametric direction is a straight line going from node 1 to the
midpoint of the second element edge, and the second isoparametric direction is
a straight line going from the midpoint of the first element edge to the
midpoint of the third element edge; for a 6-node triangle the first
isoparametric direction is a straight line going from node 1 to node 5, and the
second isoparametric direction is a straight line going from node 4 to node 6
(see
About the Element Library
for the element node ordering).
Example
As an example, a user-defined local coordinate system is used to define
rebar in a shell element (
= ),
and the output value of RBANG is 75°, as illustrated in
Figure 9:
The rebars are located at the midsurface of the shell. Output variable RBANG is measured from the second isoparametric direction to the
rebar. If the first isoparametric direction were chosen instead, output
variable RBANG would report an angle of 165°.