<!-- source-page: 171 -->

You must use element-based rebar, described in “Defining rebar as an element property,” Section 2.2.4, 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 2.2.3–8).

![](images/page-171_0822eab9340a20825c73523bc8c9ea055135f51d39c1b03cd603ddedbcc0ab8c.jpg)

<details>
<summary>text_image</summary>

Local beam
section axes
2
Rebar
X₂
X₁
1
</details>

Figure 2.2.3–8 Rebar location in a beam section.

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.

Input File Usage: \*REBAR, ELEMENT=BEAM, MATERIAL=mat, NAME=name

Abaqus/CAE Usage: Rebar in Abaqus/Standard beam elements are not supported in Abaqus/CAE.

# 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,” Section 21.1.2). 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:

• “Porous metal plasticity,” Section 23.2.9.

The following material behaviors cannot be used in Abaqus/Explicit to define rebar materials:

• “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1;   
• “Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1;   
• “Equation of state,” Section 25.2.1;   
• “Anisotropic yield/creep,” Section 23.2.6;   
• “Porous metal plasticity,” Section 23.2.9;   
• “Extended Drucker-Prager models,” Section 23.3.1;

<!-- source-page: 172 -->

• “Modified Drucker-Prager/Cap model,” Section 23.3.2;   
• “Crushable foam plasticity models,” Section 23.3.5; or   
• “Cracking model for concrete,” Section 23.6.2.

Although Abaqus/Standard will allow for a rebar material to be defined with orthotropic elasticity (“Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1) or anisotropic elasticity (“Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1), $D _ { 1 1 1 1 }$ is the only meaningful material constant in these definitions. $D _ { 1 1 1 1 }$ is used to compute the strain in the rebar direction, , using the corresponding stress component, $\sigma _ { 1 1 }$ , as discussed in “Linear elastic behavior,” Section 22.2.1; no other strain or stress components exist in rebars.

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.

<table><tr><td>Input File Usage:</td><td>*REBAR LAYERrebar layer name, A, s, distance of rebar from shell midsurface,rebar material name</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Property module: membrane, shell, or surface section editor: Rebar Layers: Material rebar material name</td></tr></table>

# Initial conditions

Initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) 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,” Section 6.2.2) with no external loads applied (or, perhaps, with the “dead” loads only)—see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.

<table><tr><td>Input File Usage:</td><td>*INITIAL CONDITIONS, TYPE=STRESS, REBAR element number or element set name, rebar name, prestress value</td></tr></table>

Abaqus/CAE Usage: Rebar prestress is not supported in Abaqus/CAE.

# 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 selfequilibrating 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.

<!-- source-page: 173 -->

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.

Input File Usage: \*PRESTRESS HOLD

Abaqus/CAE Usage: Rebar prestress is not supported in Abaqus/CAE.

# 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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, for details.

Input File Usage: \*INITIAL CONDITIONS, TYPE=SOLUTION, REBAR

Abaqus/CAE Usage: Initial solution-dependent state variables are not supported in Abaqus/CAE.

# 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,” Section 3.7.3 of the Abaqus Theory Guide.

See “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2, 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.

<!-- source-page: 174 -->

# 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 “Element library: overview,” Section 27.1.1, for the element node ordering).

Input File Usage: \*REBAR LAYER

rebar layer name, A, s, distance of rebar from shell midsurface,

rebar material name, angular orientation of rebar, isoparametric direction

Abaqus/CAE Usage: You cannot specify the direction for rebar angle output in Abaqus/CAE; the first isoparametric direction is always used.

# 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 2.2.3–9:

```csv
*REBAR LAYER, ORIENTATION=ORIENT
Rbname, 0.01, 0.1, 0.0, Rbmat, 30., 2
*ORIENTATION, SYSTEM=RECTANGULAR, NAME=ORIENT
-0.7071, 0.7071, 0.0, -0.7071, -0.7071, 0.0
3, 0.0 
```

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°.

# Visualizing rebar orientation and results in rebar

Abaqus/CAE supports visualization of rebar direction and results in rebar layers. Plots of rebar orientation are available only if you request element output for rebars (see “Element output” in “Output to the output database,” Section 4.1.3). Element variables for rebar can be contoured as field output or plotted as history output in the Visualization module. Each rebar layer will have a unique name and represents one additional section point in a membrane, shell, or surface element. You can select a

<!-- source-page: 175 -->

![](images/page-175_965e79e2005b3572380a9f5c0584dc9bd5c2d08dfd4fa7e973115683be4475f3.jpg)

<details>
<summary>text_image</summary>

RBANG = 75°
2, ISO₂
OR₁
4
α = 30°
3
1, ISO₁
1
2
y
z
x
</details>

ISO = isoparametric directions   
OR = user-defined local directions   
1, 2 = default local directions

Figure 2.2.3–9 RBANG measurement for rebar defined relative to user-defined local coordinate directions.

named rebar layer in a membrane, shell, or surface element to display its results in the Visualization module. Abaqus/CAE does not yet support rebar in beams.

<!-- source-page: 176 -->

<!-- source-page: 177 -->

# 2.2.4 DEFINING REBAR AS AN ELEMENT PROPERTY

Products: Abaqus/Standard Abaqus/Explicit

# References

• \*PRESTRESS HOLD   
• \*REBAR

# Overview

The preferred method for defining rebar in shell and membrane elements is defining layers of reinforcement as part of the element section definition (documented in “Defining reinforcement,” Section 2.2.3). The preferred method for defining rebar in solids is embedding reinforced surface or membrane elements in “host” solid elements as described in “Embedded elements,” Section 35.4.1. This section describes an alternative method of defining rebar in shell, membrane, and continuum elements as an element property. This method is more cumbersome than the method described in “Defining reinforcement,” Section 2.2.3, and does not allow visualization of the rebar and rebar results in Abaqus/CAE.

Element-based rebars:

• are used to define uniaxial reinforcement in solid, membrane, and shell elements;   
• can be defined as individual reinforcing bars in solid elements;   
• can be defined as layers of uniformly spaced reinforcing bars in shell, membrane, and solid 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 with coupled temperature-displacement elements but do not contribute to the thermal conductivity and specific heat;   
• can be used with coupled thermal-electrical-structural elements but do not contribute to the electrical conductivity, thermal conductivity and specific heat;   
• do not contribute to the mass of the model in Abaqus/Standard;   
• cannot be used in elements intended for heat transfer or mass diffusion analysis;   
• cannot be used with triangular shell and membrane elements or with triangular, triangular prism, and tetrahedral solid elements; and   
• have material properties that are distinct from those of the underlying element.

# Assigning a name to the rebar set

You must assign a name to the rebar set. This name can be used in defining rebar prestress and output requests. Each layer of rebar must be assigned a separate name in a particular element or element set.

Input File Usage: $* { \mathrm { R E B A R } } , { \mathrm { E L E M E N T } } { = } e l e m , { \mathrm { M A T E R I A L } } { = } m a t , { \mathrm { N A M E } } { = } n a m e$

<!-- source-page: 178 -->

# Defining rebars in three-dimensional shell and membrane elements

Both isoparametric and skew rebars can be defined in three-dimensional shell and membrane elements. Rebars cannot be used with triangular shells or membranes.

If triangular-shaped shells or membranes are needed, collapsed quadrilateral shells or membranes can be used. The resulting rebar directions will depend on the type of rebar (isoparametric or skew) used. The rebar must be defined carefully since the element is distorted. This technique should be used only in regions of the mesh where results are not critical and stress gradients are not high.

The stiffness calculations for the rebars use the same integration points as the calculations for the underlying shell or membrane elements. See “Shell elements: overview,” Section 29.6.1, and “Membrane elements,” Section 29.1.1, for more information about shell and membrane elements.

# Defining isoparametric rebars in three-dimensional shell and membrane elements

Isoparametric rebars are aligned along the mapping of constant isoparametric lines in the element (see Figure 2.2.4–1).

![](images/page-178_2c757dffcaeb0900a8579f5be19f730165e855c535fb7a120123684d1d1917a5.jpg)  
Figure 2.2.4–1 “Isoparametric” rebar in an undistorted three-dimensional shell or membrane element.

If opposite edges of the element containing the rebar are not parallel, the rebar directions will be different at each of the integration points within an element (see Figure 2.2.4–2).

The spacing of the rebar will be fixed in physical space. The spacing, s, and the area of the rebar, A, are used to determine the thickness of the equivalent smeared layer, $t = A / s$ . If the edges of the element containing the rebar are not parallel, the number of actual rebar with this spacing passing through one edge will be different than the number passing through the opposite edge (opposite in isoparametric space).

You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing in the plane of the shell, s; and the edge number to which the rebars are parallel when plotted in isoparametric space (see Figure 2.2.4–1). In addition, for shell elements you 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

<!-- source-page: 179 -->

![](images/page-179_af7b4665dfa0a0cd12382e3c75c4876942d0f2e6e86b7bf14bd7b0eb37c498f3.jpg)

<details>
<summary>text_image</summary>

1
2
3
4
</details>

Figure 2.2.4–2 “Isoparametric” rebar directions in a distorted three-dimensional shell or membrane element (dashed lines indicate rebar directions).

(“Nodal thicknesses,” Section 2.1.3), this distance is 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,” Section 2.8.1), this distance is scaled by the ratio of the element thickness defined by the distribution to the default thickness. If the shell has a composite section whose layer thicknesses are defined with distributions (“Distribution definition,” Section 2.8.1), this distance is scaled by the ratio of the sum of the element layer thicknesses defined by the distributions to the sum of the default layer thicknesses.

Input File Usage: Use the following option to define isoparametric rebars in three-dimensional shell elements:

\*REBAR, ELEMENT=SHELL, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC

Use the following option to define isoparametric rebars in general membrane elements:

\*REBAR, ELEMENT=MEMBRANE, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC

# Defining skew rebars in three-dimensional shell and membrane elements

Skew rebars need not be similar to an element edge; they can lie at any prescribed angle from the local 1-axis. The direction of the rebars must be defined in one of two ways, as indicated in Figure 2.2.4–3:

1. The rebars can be defined relative to the default projected local coordinate system (see “Conventions,” Section 1.2.2).   
2. The rebars can be defined relative to a user-defined local coordinate system (see “Orientations,” Section 2.2.5).

<!-- source-page: 180 -->

![](images/page-180_9f5dea31343bcf24c0d64a7f88ea6450870f4f23062cb932dfbf314ab71385b6.jpg)

<details>
<summary>text_image</summary>

Projected local surface directions
or user-defined local
surface directions
n
2
1
Skew angle, α
</details>

Figure 2.2.4–3 “Skew” rebar in a three-dimensional shell or membrane.

The orientation definition that can optionally be associated with a shell or membrane section definition has no influence on the rebar angular orientation definitions. If the shell or membrane is curved in space, the local 1-direction will vary across the element and the skew rebar will also vary accordingly.

For shell elements the definition of a local coordinate system using distributions (“Distribution definition,” Section 2.8.1) has no influence on the rebar angular orientation definitions.

If the rebar cross-sectional area is A, the rebar spacing, s, should be given so that the thickness of the equivalent “smeared” layer of reinforcing is $t = A / s$ .

# Defining skew rebars relative to the default projected local coordinate system

To define skew rebars relative to the default projected local coordinate system, you specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing in the plane of the shell, s; 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); and the angle , in degrees, between the default local 1-direction and the rebars. See “Conventions,” Section 1.2.2, for a definition of the default projected local directions on a surface in space. If the shell’s thickness is defined by nodal thicknesses (“Nodal thicknesses,” Section 2.1.3), the rebar position in the thickness direction 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,” Section 2.8.1), the rebar position in the thickness direction is scaled by the ratio of the element thickness defined by the distribution to the default thickness. A positive angle defines a rotation from local direction 1 to local direction 2 around the element’s normal direction. For example, in a membrane the following data would result in the rebar definition shown in Figure 2.2.4–4: A=0.05, s=0.1, and =45.

When a user-defined local orientation definition is not used to define the angular orientation of the rebar and the normal to the shell is nearly parallel to the global 1-axis, the local 1-axis may change significantly within an element or from one element to the next (see “Conventions,” Section 1.2.2).
