Defining sections

A section contains information about the properties of a part or a region of a part. The information required in the definition of a section depends on the type of region in question. For example, if the region is a deformable wire, shell, or two-dimensional solid, you must assign a section to that region that provides information about the region's cross-sectional geometry. Likewise, a rigid region requires a section that describes its mass properties. Most sections must refer to a material name. Beam sections must also refer to a profile name.

When you assign a section to a part, Abaqus/CAE automatically assigns that section to each instance of the part. As a result, the elements that are created when you mesh those part instances will have the properties specified in that section.

Sections are named and created independently of any particular region, part, or assembly. You can assign a single section to as many different regions as necessary. You can use the Property module to create solid sections, shell sections, beam sections, fluid sections, and other sections.

Solid sections

Solid sections define the section properties of two-dimensional, three-dimensional, and axisymmetric solid regions.

  • Homogeneous solid sections. Homogeneous solid sections consist of a material name. In addition, if the section will be used with a two-dimensional region, you must also specify the section thickness. (You have the option of specifying a plane stress or plane strain thickness even if the section will be assigned to a three-dimensional region. Abaqus/CAE ignores the thickness information if it is not needed for the region type.)

    For more information, see Creating homogeneous solid sections.

  • Generalized plane strain sections. Generalized plane strain sections consist of a material name, thickness, and wedge angles about the global 1- and 2-axes. You can assign generalized plane strain sections only to two-dimensional planar regions.

    For more information, see Creating generalized plane strain sections.

  • Eulerian sections. Eulerian sections consist of a list of material names. This list specifies all of the materials that can be present in an Eulerian domain. You can assign Eulerian sections only to Eulerian parts.

    For more information, see Creating Eulerian sections. For an overview of Eulerian analyses, see Eulerian analyses.

  • Composite solid sections. Composite solid sections consist of layers of materials. For each layer of material, you must specify a material name, thickness, and orientation.

    For more information, see Creating composite solid sections.

  • Electromagnetic solid sections. Electromagnetic solid sections are valid for electromagnetic models and consist of a material name. In addition, if the section will be used with a two-dimensional region, you must also specify the section thickness. (You have the option of specifying a plane stress or plane strain thickness even if the section will be assigned to a three-dimensional region. Abaqus/CAE ignores the thickness information if it is not needed for the region type.)

    For more information, see Creating electromagnetic solid sections.

Shell sections

Shell sections define the section properties of shell regions. Shells model structures in which one dimension (the thickness) is significantly smaller than the other two dimensions and in which the stresses in the thickness direction are negligible. You can define one or more layers of reinforcement (rebar) in shell sections. For more information, see Understanding rebar in shell sections.

  • Homogeneous shell sections. Homogeneous shell sections consist of a shell thickness, material name, section Poisson's ratio, and optional rebar layers. You can choose to provide the section property data before the analysis or to have Abaqus calculate (integrate) the cross-sectional behavior from section integration points during the analysis. If the latter is chosen, options are provided to control the section integration and temperature variation through the thickness.

    For more information, see Creating homogeneous shell sections.

  • Composite shell sections. Composite shell sections consist of layers of materials, a section Poisson's ratio, and optional rebar layers. For each layer of material, you must specify a material name, thickness, and orientation. You can choose to provide the section property data before the analysis or to have Abaqus calculate (integrate) the cross-sectional behavior from section integration points during the analysis. If the latter is chosen, options are provided to control the section integration and temperature variation through the thickness.

    For more information, see Creating composite shell sections.

  • Membrane sections. Membranes represent thin surfaces in space that offer strength in the plane of the surface but have no bending stiffness. Membrane sections consist of a material name, membrane thickness, section Poisson's ratio, and optional rebar layers.

    For more information, see Creating membrane sections.

  • Surface sections. Surface sections represent surfaces in space that have no inherent stiffness and behave like membrane elements with zero thickness. Surface sections consist of optional rebar layers.

    For more information, see Creating surface sections.

  • General shell stiffness sections. General shell stiffness sections allow you to define a shell's mechanical response by directly specifying the stiffness matrix and thermal expansion response. General shell stiffness sections consist of a section stiffness matrix and scaling moduli. Optionally, you can also specify a thermal expansion coefficient and thermal stresses in the section.

    For more information, see Creating general shell stiffness sections.

Beam sections

Beams are used in two and three dimensions to model slender, rod-like structures that provide axial strength and bending stiffness. Beams represent structures in which the cross-section is assumed to be small compared to the length. You can assign beam sections only to wire regions. In addition, you must assign a beam section orientation to all regions with beam sections.

  • Beam sections. Beam sections consist of a section Poisson's ratio and a reference to a profile. Additional information is required depending on whether you choose to calculate (integrate) the section stiffness either before or during analysis.

    For information on profiles, see Defining profiles. For more information on beam sections, see Creating beam sections.

  • Truss sections. Trusses, like beams, are used in two and three dimensions to model slender, rod-like structures that provide axial strength but no bending stiffness. Truss sections consist of a material name and cross-sectional area.

    For more information, see Creating truss sections.

You can use the part display options to view an idealized representation of the beam or truss profile along the wire region. For more information, see Controlling beam profile display.

Other sections

Other sections you can create include gasket sections, cohesive sections, acoustic infinite sections, and acoustic interface sections.

  • Gasket sections (Abaqus/Standard analyses only). Gaskets model thin sealing components that are positioned between structural components. Gasket sections are used to provide pressure-closure behaviors for sealing components. Gasket sections consist of a material name, initial gasket thickness, initial gap, initial void, and cross-sectional area.

    For more information, see Creating gasket sections and Gaskets.

  • Cohesive sections. Cohesive sections are used to model finite thickness adhesives, negligibly thin adhesive layers for debonding applications, as well as gaskets. No specialized gasket behavior (typically defined in terms of pressure versus closure) is available. Cohesive sections consist of a material name, response, initial thickness, and out-of-plane thickness.

    For more information, see Creating cohesive sections and Adhesive joints and bonded interfaces.

  • Acoustic infinite sections. Acoustic infinite sections are used to model an acoustic medium undergoing small pressure changes involving exterior domains. Acoustic infinite sections consist of an acoustic medium material name. In addition, if the section will be used with a two-dimensional region, you must also specify the section thickness. (You have the option of specifying a plane stress or plane strain thickness even if the section will be assigned to a three-dimensional region. Abaqus/CAE ignores the thickness information if it is not needed for the region type.)

    For more information, see Creating acoustic infinite sections.

  • Acoustic interface sections. Acoustic interface sections are used to couple an acoustic medium to a structural model. Acoustic interface sections consist of an acoustic medium material name. In addition, if the section will be used with a two-dimensional region, you must also specify the section thickness. (You have the option of specifying a plane stress or plane strain thickness even if the section will be assigned to a three-dimensional region. Abaqus/CAE ignores the thickness information if it is not needed for the region type.)

    For more information, see Creating acoustic interface sections.

Warning:

The type of section that you assign to a part must be consistent with the element type that you assign to instances of that part in the Mesh module. For example, if you assign a truss section to a wire part in the Property module, you should assign a truss element type (and not a beam element type) to any instances of that part in the Mesh module.