This section describes the standard beam sections that are available in Abaqus/Standard and Abaqus/Explicit for use with beam elements. A subset of the standard beam sections is available for use
with frame elements in Abaqus/Standard. General (nonstandard) beam cross-sections can be defined as described in Choosing a Beam Cross-Section.
The arbitrary section type is provided to permit modeling of simple, arbitrary,
thin-walled, open and closed sections. You specify the section by defining a series of
points in the thin-walled cross-section of the beam; these points are then linked by
straight line segments, each of which is integrated numerically along the axis of the
section so that the section can be used together with nonlinear material behavior. An
independent thickness is associated with each of the segments making up the arbitrary
section.
Warping effects are included when an arbitrary section is used with open-section beam
elements (available only in Abaqus/Standard).
An arbitrary section can be used only with beams in space (three-dimensional models).
An arbitrary section should not be used to define closed sections with branches,
multiply connected closed sections, or open sections with disconnected regions.
For each individual segment of an arbitrary section there is no bending stiffness
about the line joining the end points of the segment. Thus, an arbitrary section
cannot be made up of only one segment.
Geometric Input Data
First, give the number of segments, the local coordinates of points
A and B, and the thickness of the segment
connecting these two vertices. Then, proceed by giving the local coordinates of point
C and the thickness of the segment between points
B and C, followed by the local coordinates of
point D and the thickness of the segment between points
C and D, and so on. An arbitrary section can
contain as many segments as needed. All coordinates of section definition points are given
in the local 1–2 axis system of the section.
The origin of the local 1–2 axis system is the beam node, and the position of this node
used to define the section is arbitrary: it does not have to be the centroid.
Defining a Closed Section
A closed section is defined by making the starting and end points coincident. Only
single-cell closed sections can be modeled accurately. Closed sections with fins (single
branches attached to the cell) cannot be modeled with the capability in Abaqus.
Defining an Arbitrary Section with Discontinuous Branches
If the arbitrary section contains discontinuous sections (branches), a section with
zero thickness should be used to return from the ending point of the branch to the
starting point of the subsequent section. This zero thickness section should always
coincide with a nonzero thickness section. For an example of an I-section defined using
this method, see Buckling analysis of beams.
Default Integration
A three-point Simpson integration scheme is used for each segment making up the section.
For more detailed integration, specify several segments along each straight portion of the
section.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
The vertices of the section.
Temperature and Field Variable Input at Specific Points through Beam Sections
Integrated during the Analysis
Give the value at each vertex of the section (points A,
B, C, D in the figure).
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points in each wall that is parallel to the 2-axis.
This number must be odd and greater than or equal to three.
Beam in space: Give the number of points in each wall that is parallel to the 2-axis,
then the number of points in each wall that is parallel to the 1-axis. Both numbers must
be odd and greater than or equal to three.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: 4 corners (points 1, 5, 9, and 13 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Give the value at each of the points shown below.
Temperature Input for a Frame Section
Constant temperature throughout the element cross-section is assumed; therefore, only one
temperature value per node is required.
Defining a channel section is not supported in Abaqus/CAE.
Geometric Input Data
l, h, , , , , , o
You can specify l and o to
place the origin of the local cross-section anywhere on the local 1- and local 2-axes. In
the figure above, a negative value of l implies that the origin of
the local cross-section is below the lower edge of the bottom flange, which might be
required when constraining a beam stiffener to a shell. A negative value of
o implies that the origin of the local cross-section is on the left
of the leftmost outer edge of a channel web, which might be required when applying loads
through the section shear center.
Beam in space: 3 points radially, 8 circumferentially (17 total; trapezoidal rule).
Integration point 1 is situated at the center of the beam and is used for output purposes
only. It makes no contribution to the stiffness of the element; therefore, the integration
point volume (IVOL) associated with this
point is zero.
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: A maximum of 9 points are permitted.
Beam in space: Give an odd number of points in the radial direction, then an even number
of points in the circumferential direction.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: On the intersection of the surface with the 1- and 2-axes (points 3, 7,
11, and 15 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Give the value at each of the points shown below.
Temperature Input for a Frame Section
Constant temperature throughout the element cross-section is assumed; therefore, only one
temperature value per node is required.
Defining a hat section is not supported in Abaqus/CAE.
Geometric Input Data
l, h, b, , , , ,
By allowing you to specify l, the origin of the local cross-section
axis can be placed anywhere on the symmetry line (the local 2-axis). In the above figure a
negative value of l implies that the origin of the local
cross-section axis is below the lower edge of the bottom flanges, which may be needed when
constraining a beam stiffener to a shell.
Beam in space: 3 points in each wall segment (12 total)
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points along the section wall, moving in the second
beam section axis direction. This number must be odd and greater than or equal to three.
Beam in space: Give the number of points in each wall segment. This number must be odd
and greater than or equal to three.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: Vertices (points 1, 3, 5, 7, 9, and 11 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
By allowing you to specify l, the origin of the local cross-section
axis can be placed anywhere on the symmetry line (the local 2-axis). In the above figures
a negative value of l implies that the origin of the local
cross-section axis is below the lower edge of the bottom flange, which may be needed when
constraining a beam stiffener to a shell.
Defining a T-Section
Input File Usage
Set and or and to zero to model a T-section.
Abaqus/CAE Usage
Property module: Create Profile: T
Default Integration (Simpson)
Beam in a plane: 5 points (one in each flange plus 3 in web)
Beam in space: 5 points in web, 5 in each flange (13 total)
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points in the second beam section axis direction.
This number must be odd and greater than or equal to three.
Beam in space: Give the number of points in the lower flange first, then in the web, and
then in the upper flange. These numbers must be odd and greater than or equal to three in
each nonvanishing section.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Flanges (points 1 and 5 above for default integration).
Beam in space: Ends of flanges (points 1, 5, 9, and 13 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Give the value at each of the points shown below.
For a beam in space the temperature is first interpolated linearly through the flanges
based on the temperature at points 1 and 2, and then 4 and 5, respectively. It is then
interpolated parabolically through the web.
Temperature Input for a Frame Section
Constant temperature throughout the element cross-section is assumed; therefore, only one
temperature value per node is required.
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points in the second beam section axis direction.
This number must be odd and greater than or equal to three.
Beam in space: Give the number of points in the first beam section axis direction, then
the number of points in the second beam section axis direction. These numbers must be odd
and greater than or equal to three.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: End of flange along positive local 1-axis; section corner; end of flange
along positive local 2-axis (points 1, 5, and 9 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Give the value at each of the points shown below.
Pipe Section (Thin-Walled)
Pipe cross-sections can be associated with beam, pipe, or frame elements.
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give an odd number of points in the radial direction, then an odd number
of points (greater than or equal to 5) in the circumferential direction.
Beam in space: Give an odd number of points in the radial direction, then an even number
of points (greater than or equal to 8) in the circumferential direction.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top on the pipe midsurface (points 2 and 14 above for default
integration).
Beam in space: On the intersection of the pipe midsurface with the 1- and 2-axes (points
2, 8, 14, and 20 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points in the second beam section axis direction.
This number must be odd and greater than or equal to five.
Beam in space: Give the number of points in the first beam section axis direction, then
the number of points in the second beam section axis direction. These numbers must be odd
and greater than or equal to five.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: Corners (points 1, 5, 21, and 25 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
Give the value at each of the points shown below.
Temperature Input for a Frame Section
Constant temperature throughout the element cross-section is assumed; therefore, only one
temperature value per node is required.
By allowing you to specify d, the origin of the local cross-section
axes can be placed anywhere on the symmetry line (the local 2-axis). In the above figures
a negative value of d implies that the origin of the local
cross-section axis is below the lower edge of the section. This may be needed when
constraining a beam stiffener to a shell.
Default Integration (Simpson)
Beam in a plane: 5 points
Beam in space: 5 × 5 (25 total)
Nondefault Integration Input for a Beam Section Integrated during the Analysis
Beam in a plane: Give the number of points in the second beam section axis direction.
This number must be odd and greater than or equal to five.
Beam in space: Give the number of points in the first beam section axis direction, then
the number of points in the second beam section axis direction. These numbers must be odd
and greater than or equal to five.
Default Stress Output Points If a Beam Section Integrated during the Analysis Is
Used
Beam in a plane: Bottom and top (points 1 and 5 above for default integration).
Beam in space: Corners (points 1, 5, 21, and 25 above for default integration).
Temperature and Field Variable Input at Specific Points for Beam Sections Integrated
during the Analysis
