Blog

Blog

Modeling Reinforcement in Abaqus

 

When modeling concrete, in most situation you probably need to define steel reinforcement to follow tensional behaviour of the structure. In general, you have two options:

-Modeling reinforcements as individual parts such as solids or beams or trusses and adding them to the main concrete made part. This can be done by using embedded region constraint.

-Using Rebar layers concept in Abaqus, which is the best way to model concrete reinforcement. Here we introduce the second method.

Here we will learn:

Rebar element concept in Abaqus to define reinforcements.

Defining rebar layers in Abaqus/CAE

How to use rebars for shell and membrane (structural) elements.

How to use rebars for continuum (solid) elements

Using structural elements to specify rebar layers

We can define reinforcement in structural elements (shell, membrane, and surface elements) by directly specifying a rebar layer in the element.

If you do not know the difference of shell and membrane elements, look at this Q&A:

Surface elements do not have any element properties other than the rebar layer. In other words, they are used primarily just as place-holders for rebar layers.

Defining Reinforcement in Abaqus, Structural and solidWhat is Rebar layer?

Rebar layers are used for modeling uniaxial reinforcement in shell, membrane and surface elements. Their material properties are independent of those of the underlying elements. The rebar layer volume is not subtracted from the volume of the element to which the rebar layer is added. Thus, rebar layers should be used only when the volume fraction of reinforcement is small. Such as with reinforced concrete where the volume fraction of the rebar is between 1% and 4%).

We can define as many different combinations and orientations of rebar layers as are needed within a single element. They have material properties that are distinct from those of the underlying or host element.

Defining rebar layers in Abaqus/CAE

When you create homogeneous shell sections, composite shell sections, membrane sections, or surface sections, you can define one or more layers of reinforcement (rebar) by using the Rebar Layers option.

1. From the Options field of the shell, membrane, or surface section editor, click Rebar Layers… icon. 

The Rebar Layers dialog box appears.

Specify the type of rebar geometry.

    • Choose Constant for a constant rebar spacing.
    • Choose Angular if the rebar spacing varies as a function of radial position in a cylindrical coordinate system.

2. In the table, enter a row of data for each rebar layer:

    • Name: the name of the rebar layer (to identify the layer in the list of section points when post processing in Visualization module).
    • Material: the name of the material forming the rebar layer. Click the arrow that appears to display the list of available materials, and select the material you created before forming the rebar layer.
    • Area: the cross-sectional area per bar.
    • Spacing: the rebar spacing in the plane of the section. For angular rebar spacing, specify the spacing angle in degrees.
    • Orientation: the angular orientation of the rebar (in degrees) relative to the 1-direction of the rebar reference orientation.
    • Position (not applicable for membrane/surface): the position in the shell thickness direction measured from the middle surface of the shell.

Specifying rebar geometry

We always define the rebar geometry with respect to a local coordinate system. The rebar geometry can be constant or vary as a function of radial position in a cylindrical coordinate system. In each case, you must specify the spacing, s, and the angular orientation, α, of the rebar with respect to this local system.

Output for rebar elements

Abaqus/CAE supports visualization of rebar layer orientations and results in rebar layers. Output of variables such as stresses and strains at the rebar integration points is available on a layer-by-layer basis. Remember to request outputs for rebars when defining a step:

Using Rebar layers in Solid elements

When defining reinforcement in a solid concrete part, we follow this procedure:

1. Using structural elements to specify rebar layers

To use rebar layers later for solid elements, first we specify either membrane or surface elements with rebar layers.

2. Embedding structural elements in Solid elements

Then, we use embedded element constraint to reinforce solid elements. In this technique, we embed either surface or membrane elements reinforced with rebar layers in the solid host elements, in an arbitrary manner such that the two meshes need not match. Use Embedded region constraint to accomplish:

When selecting Whole Model, Abaqus searches the elements in the vicinity of the embedded elements for elements that contain embedded nodes. After that, the embedded nodes are constrained by the response of these host elements. To preclude certain elements from constraining the embedded nodes, you can define a host element set (Select Region).

Using Embedded element constrain for rebars in solid

Quiz Time!

  1. We can embed rebar elements directly in continuum elements. (True/False)
  2. The rebar layer volume is subtracted from the volume of the element added to. (True/False)
  3. Abaqus/CAE supports visualization of results in rebar layers. (True/False)
  4. We define must the position of the rebars in the thickness direction for shell/membrane elements (True/False)
  5. The rebar can have material properties that are distinct from those of the underlying element. (True/False)
  6. The rebar geometry can vary as a function of circumferential position in a cylindrical coordinate. (True/False)
  7. Stresses and strains at the rebar integration points are available in results by default. (True/False)

Eager to hear from You…

Any complication or other questions? Feel free to comment here…

You can also send any new questions from the Questions and Answers page. Just find that blue Ask Question button at the top right corner…


Leave a Reply

Shopping cart
Sidebar