Beam elements are 1D elements used to model 3D structures in a computationally efficient manner. They are commonly used in industries like construction, bridges, transportation and more. The document outlines the process for modeling with beam elements which includes defining the geometry, beam properties like element type, cross section, material and meshing the geometry. It specifically recommends using BEAM188 and BEAM189 elements and describes how to define standard and custom cross sections. The steps for applying loads, solving, and reviewing results are also provided. An example problem is included to demonstrate modeling a frame structure with various beam elements and cross sections.

2.  Beam elements are line elements used to
create a one-dimensional idealization of a 3-
D structure.
 They are computationally more efficient than
solids and shells and are heavily used in
several industries:
◦ Building construction
◦ Bridges and roadways
◦ People movers (trams,
railcars, buses)
◦ Etc.

3.  A brief introduction to beam modeling via the
following topics:
A. Beam Properties
B. Beam Meshing
C. Loading, Solution, Results

4.  The first step in beam modeling, as with any
analysis, is to create the geometry — usually
just a framework of keypoints and lines.
 Then define the following beam properties:
◦ Element type
◦ Cross section
◦ Material

5. Element Type
 Choose one of the following types:
◦ BEAM188 — 3-D, linear (2-node)
◦ BEAM189 — 3-D, quadratic (3-node)
 ANSYS has many other beam elements, but
BEAM188 & 189 are generally recommended.
◦ Applicable to most beam structures
◦ Support linear as well as nonlinear analyses, including
plasticity, large deformation, and nonlinear collapse
◦ Ability to include multiple materials to simulate layered
materials, composites, reinforced sections, etc.
◦ Ability to create “user defined” section geometry
◦ Easy to use, both in preprocessing and postprocessing
phases

6. Cross Section
 To completely define a BEAM188
or 189 element, you also need to
specify its cross section
properties.
 The BeamTool provides a
convenient way to do this.
◦ Preprocessor > Sections > Common
Sectns...
◦ Select the desired shape, then enter
its dimensions.
◦ Press the Preview button to view the
shape, then OK to accept it.
◦ If there are multiple cross sections,
specify a different section ID number
(and an optional name) for each.

7.  A sample preview (SECPLOT) of an I-beam cross section is shown
below.
 In addition to the predefined cross-section shapes, ANSYS allows
you to create your own, “user-defined” shape by building a 2-D
solid model.
 You can save user-defined
sections as well as standard
sections with the desired
dimensions in a section
library for later use.
 See Chapter 15 of the ANSYS
Structural Analysis Guide for
more information.

8. Material Properties
 Both linear and nonlinear material properties are
allowed.
 After all beam properties are defined, the next step
is to mesh the geometry with beam elements.

9.  Meshing the geometry (lines) with
beam elements involves three main
steps:
◦ Assign line attributes
◦ Specify line divisions
◦ Generate the mesh
 The MeshTool provides a
convenient way to perform all three
steps.

10. Step 1: Line Attributes
 Line attributes for beam meshing consist of:
◦ Material number
◦ Section ID
◦ Orientation keypoint
 Determines how the cross section is oriented with
respect to the beam axis.
 Must be specified for all cross-section types.
 A single keypoint can be assigned to multiple lines (i.e,
no need to specify a separate keypoint for each line).
 Each end of a line can have its own orientation
keypoint, allowing the cross section to be “twisted”
about the beam axis.

11.  Examples of using orientation keypoints:

12.  To assign line attributes, use the “Element
Attributes” section of the MeshTool (or select
desired lines and use the LATT command).
Pick lines
Additional
attributes for
BEAM188 & 189

13. Step 2: Line Divisions
 For BEAM188 and 189 elements, a single
element spanning the entire beam length is
not recommended.
 Use the “Size Controls” section of the
MeshTool (or the LESIZE command) to specify
the desired number of line divisions.

14. Step 3: Generate the Mesh
 First save the database (Toolbar > SAVE_DB or
SAVE command).
 Then press the Mesh button in the MeshTool (or
issue LMESH,ALL) to generate the mesh.
Pick lines

15.  To see the cross-section shape in the element
display, activate the element shape key:
◦ Utility Menu > PlotCtrls > Style > Size and Shape…
◦ Or /ESHAPE,1

16.  After beam meshing is completed, the next
step is to apply loads and solve.

17.  Typical loading for beam models consists of:
◦ Displacement constraints
 applied at keypoints or nodes
◦ Forces
 applied at keypoints or nodes
◦ Pressures
 load per unit length
 applied on element faces
 Solution > Apply > Pressures > On Beams
 Or SFBEAM command
◦ Gravity or rotational velocity
 acts on entire structure

18.  To obtain the solution:
◦ First save the database.
◦ Then solve. (Or write the loads to a load step file and
solve all load steps later.)
 Results review is the same as for other stress
analyses:
◦ View the deformed shape
◦ Check reaction forces
◦ Plot stresses and strains
 The main advantage of BEAM188 and 189 is that with the
element shape key activated (/ESHAPE,1), stresses can be
directly viewed on the elements (similar to solids and shells).

19.  Demo:
◦ Resume frame.db (contains lines, kp’s, loading, element type, material, and two cross
sections)
◦ Plot the two cross section already defined (SECPLOT,1 & 2)
◦ Define a third cross section using the BeamTool:
 ID=3: Name = peak, Sub-type = box (hollow rectangle), W1=6, W2=6;
T1=T2=T3=T4=0.25
◦ Bring up MeshTool, GPLOT, then assign the following line attributes:
 Sloping lines: mat=1, secnum=3, orientation KP = topmost KP (#100)
 Left vertical lines: mat=1, secnum=2, orientation KP = #102
 Right vertical lines: mat=1, secnum=2, orientation KP = #101
 Left & front horizontal lines: mat=1, secnum=1, orientation KP = #1
 Right & back horizontal lines: mat=1, secnum=1, orientation KP = #3
◦ Specify size=20 on all lines
◦ Save, then LMESH,ALL; then EPLOT with /ESHAPE,1
◦ Constrain the 4 bottom keypoints in all DOFs and apply a force of -10,000 lb in the fy
direction on keypoint #9
◦ Solve, then review results: deformed shape (animate), reaction forces, SX stresses (= axial +
bending). Select elements with section ID=3 and replot stresses. Repeat for ID=2.
October 30, 2001
Inventory #001571
5-19

20.  This workshop consists of the following
problem:
W4. Building Frame
Please refer to your Workshop Supplement for
instructions.
October 30, 2001
Inventory #001571
5-20