ENGN 1750: Advanced Mechanics of Solids

Introduction to Abaqus: Trusses

1 Introduction
A major goal of this course is to gain a proficiency with the use of the finite-element method
(FEM) in solid mechanics. Broadly-speaking, the finite-element method is simply a numer-
ical technique for solving partial differential equations. The governing equations of solid
mechanics lend themselves particularly well to this technique, and by the end of the 1970s,
enabled by the advent of digital computing, the application of FEM to solid mechanics had
revolutionized the field. Prior to this development, the field was primarily the domain of
advanced specialists and mathematicians, since, as we shall see later in the course, by-hand,
analytical solutions quickly become quite complex in all but the simplest of geometries. The
use of FEM has placed the full power of solid mechanics in the hands of a broad community
of engineers for use in everyday design.
It will take the majority of the semester to cover the mathematical foundations of solid
mechanics and the theory behind the finite-element method in lecture. Therefore, for the
sake of efficiency, we will undertake in parallel a series of exercises to develop a familiarly
with using a commercial FEM program. By the end of the semester, you should have a
fluency with the program as well as a knowledge of what is going on “under the hood.” In
this course, we will be using the FEM program Abaqus. Abaqus is one of the major FEM
codes used in industry and research (others you might encounter are ANSYS, LS-DYNA,
Nastran, COMSOL, or ADINA) and was developed by Brown PhD graduates David Hibbett
and Paul Sorensen along with Bengt Karlsson in the 1970s. It has since been acquired by
the French company Dassault Systemès, but Abaqus headquarters remains in Providence to
this day.

2 Using the finite element method

Performing a finite-element analysis consists of three stages: (1) Pre-processing, (2) Process-
ing, and (3) Post-processing, each discussed below:

(1) Pre-processing: In this stage, one sets up a model prior to running the calculation.
It involves specifying geometry, material behavior, boundary conditions, and loading,
as well as discretizing the analysis domain into many smaller elements, called the
mesh. Setting up a model and troubleshooting errors is a skill, requiring practice.
We will utilize the Abaqus graphical environment, called CAE, or “Complete Abaqus
Environment,” for preprocessing.

(2) Processing: The calculation is actually performed in this stage. For the user of the
program, it is a “black box” operation. When a job is submitted, Abaqus will run it
and inform the user whether the analysis completed successfully or not. We will learn
the theory behind this step later in the course.

1
 (3) Post-processing: In this stage, the calculation results are displayed. Typical simulations
results for the types of analyses we will be running are displacement, strain, and stress
fields. It is crucial to always cast a skeptical eye towards your simulation results and
ask yourself whether they make sense or not. Never blindly trust the simulation output.

When progressing through these stages, one navigates Abaqus/CAE through the use of
the module menu, which is followed sequentially. The modules, in order, are (1) Part, (2)
Property, (3) Assembly, (4) Step, (5) Interaction, (6) Load, (7) Mesh, (8) Optimization, (9)
Job, and (10) Visualization. (The sketch module is supporting, and we won’t be making use
of it in our exercises.) The basic use of each module is explained below:

(1) Part: The Part module allows for the drawing of parts, be they 1-D, 2-D, or 3-D. It
operates much like any CAD program. You may create many parts for use in your
analysis, but for the time being, we will only create one part per model.

(2) Property: This module allows for the definition of material behavior. For the bulk of
the course, we will focus on the simplest material behavior: isotropic, linear elasticity,
but Abaqus has an extensive library of material models. This module also allows for
the specification of cross-sectional areas and profiles for analyses involving trusses or
beams.

(3) Assembly: Here, one would assemble the parts constructed in the part model into a
single assembly. Since we will only be considering a single part, this step is quite simple
for our present purposes.

(4) Step: Specify the analysis type. We will mainly be performing “Static” analyses,
meaning there in no contribution from inertia. This is the “bread-and-butter” analysis
type in Abaqus, but the Abaqus analysis library is vast, allowing for the study of wave
propagation, stress-temperature effects, instabilities, and much more physics. This
module is also where one specifies the desired outputs.

(5) Interaction: For problems involving contact, the details of the contact problem are
specified here. We will come back to this module in the last assignment.

(6) Load: Specify boundary conditions – both displacement boundary conditions as well
as force/pressure boundary conditions. An important module, and the first place to
look for errors if an analysis unexpectedly fails.

(7) Mesh: Break the part into elements. These elements are the fundamental units of
the numerical technique. We will get into the precise details of what these elements
mean and do later in the course. For truss problems, each member should be a single
element.

(8) Optimization: For performing a topology optimization analysis. We will not be using
the optimization module in this course.

(9) Job: This step is where pre-processing ends and processing begins. Simply to create
the job and tell the computer to calculate the solution!

2
(10) Visualization: Provided the job completes successfully, you may view the simulation
results in this module. This module encompasses all of post-processing. Here, we can
view quantities, such as displacement, strain, and stress.

2.1 Units in Abaqus

It is important to note that Abaqus has no built-in set of units. It is up to the user to choose
a consistent set of units for dimensional quantities and stick with it. In this exercise, we will
use standard SI units.

2.2 Abaqus documentation

The Abaqus documentation is helpful for when you get stuck or want to utilize a feature
with which you are unfamiliar. It is quite comprehensive – a hard copy of the documentation
fills an entire shelf. The easiest way to find the information you need is to go to “Help ⇒ On
context” and then click on any piece of the Abaqus/CAE environment. The corresponding
page of documentation explaining that feature will then open. To simply search the entire
documentation go to “Help ⇒ Search & Browse Manuals.”

3 An illustrative example
The goal of the first exercise is to give an introduction to building models in Abaqus in the
context of a simple mechanics problem – a truss. Consider the following simple truss:

'()*+,"-+.//0/,-1.2"
%" &"

!" #" $"

Figure 1: A simple statically-determinant truss.

All joints are frictionless pins, and all members have the same length, which we take to be
L = 1 m. Likewise, all members have a square cross-section with w = 0.05 m and are made
of steel, so that E = 210 GPa and ν = 0.3. A downward load of P = 10 kN is applied at
pin B. Since the truss is statically-determinant, it is straightforward to calculate the forces

3
in each of the members:
√ √
√ 3,
PAD = PCE = −P/ PAB = PBC √
= P/(2 3),
PBD = PBE = P/ 3, PDE = −P/ 3,

where a negative force indicates that the member is in compression. Using Castigliano’s
theorem (which we will learn about later in the course), we may calculate the downward
vertical displacement of point B as
11P L
δB = .
6EA
In this exercise, we will perform a numerical analysis of this truss and verify against the
analytical results to convince ourselves of the effectiveness of the method.

3.1 Model definition and analysis

Below is an outline of the steps for performing the analysis in Abaqus/CAE:

(1) Part:

- Part ⇒ Create
- Select 2D Planar, Deformable, Wire, and Approximate size: 2
- Sketch the part as pictured in Fig. 1 and click Done

(2) Property:

- Material ⇒ Create
- Mechanical ⇒ Elasticity ⇒ Elastic
- Enter the material properties for steel and click OK
- Section ⇒ Create
- Beam ⇒ Truss ⇒ Continue
- Enter the cross-sectional area and click OK
- Assign ⇒ Section
- Select the entire part and click Done/OK

(3) Assembly:

- Instance ⇒ Create ⇒ OK

(4) Step:

- Step ⇒ Create ⇒ Static/General ⇒ Continue ⇒ OK

(5) Interaction: None

(6) Load:

4
 - BC ⇒ Create ⇒ Mechanical ⇒ Displacement/Rotation ⇒ Continue ⇒ Select
point A and click Done ⇒ Enter U1=U2=0 and click OK
- BC ⇒ Create ⇒ Mechanical ⇒ Displacement/Rotation ⇒ Continue ⇒ Select
point C and click Done ⇒ Enter U2=0 and click OK
- Load ⇒ Create ⇒ Mechanical ⇒ Concentrated Force ⇒ Continue ⇒ Select point
B and click Done ⇒ Enter CF2 and click OK

(7) Mesh:

- Make sure Object is set to Part.

- Mesh ⇒ Element Type ⇒ Select the entire part and click Done ⇒ Family: Truss
⇒ Click OK
- Seed ⇒ Edges ⇒ Select entire part and click Done ⇒ Method: By number ⇒
Number of elements: 1 ⇒ Click OK
- Mesh ⇒ Part ⇒ Yes

(8) Optimization: None

(9) Job:

- Job ⇒ Create ⇒ Continue/OK

- Job ⇒ Submit ⇒ Job-1
- When the job successfully completes: Job ⇒ Results ⇒ Job-1

(10) Visualization:

- Examine contour plots of displacement (U1 and U2) and stress (S11).
- Probe quantitative results at specific points of the model:
Tools ⇒ Query ⇒ Probe values
- Verify that the calculated results match their analytical counterparts. Repeat the
calculation for P = 50 kN and verify.

Note on managers: Most of the menus encountered above have a “manager” associated
with them, which you may find useful. These managers allow you to create, edit, rename,
and delete the feature of interest. How you choose to navigate CAE is, in the end, a matter
of taste.

5
 ENGN 1750: Advanced Mechanics of Solids
Abaqus Assignment 1
Due: Monday, September 29, 2014 OR Thursday, October 2, 2014 (in class)

Consider the following three trusses:

P/4
'"

P/2
(" &" L
P/4 L
!" #" $" 2
%"

L L L

P/4
("

P/2
)" '" L
P/4 L
$" 2
!" #" %"
&"

3L/4 3L/4 3L/4 3L/4

P/4
("

P/2
)" '" L
P/4 L
!" #" $" %" 2
&"

3L/4 3L/4 3L/4 3L/4

As in the class exercise, all members have a square cross-section with w = 0.05 m and are
made of steel. All joints are frictionless pins. Take L = 1 m. The truss is subjected to forces
as shown in the schematics. The forces are applied perpendicularly to the side CDE of each
truss structure. The truss is considered to fail when the magnitude of stress in any of its
members reaches a value of 250 MPa (compressive or tensile), and we denote the value of P ,
at which the first truss member fails as Pmax .
1. Using Abaqus, determine the value of Pmax and the member that fails first for each
truss.
2. Calculate the mass of each truss. Based on the maximum allowable load and mass of
each truss structure, which design would you recommend? Justify your choice.