MATS23702
An Introduction to Modelling in Abaqus
Tutorial 2
In the last workshop, you have been introduced to Abaqus, and now have
some experience of setting up and running mechanical simulations. In this
workshop, you will be given a problem to model with only a limited number of
instructions. You will be asked to generate a suitable simulation, and compare
the results of your simulation against theory and experiment.

You will also be asked to perform a mesh sensitivity study on your Abaqus
model – sometimes the result of an FE simulation can change depending on
the mesh size, and a mesh sensitivity study can help you understand when
this is happening.

You may find it useful to look back at the previous tutorial if you are unsure
how to set up your model.

You should work individually for this tutorial.

There will be a preliminary report for this tutorial, and also a longer written
report. The details of the longer written report are given at the end of this
tutorial document.

You are not expected to finish this tutorial in only one three-hour
session – it may take more time than this!


Learning Outcomes:
By the end of this tutorial, you should be able to:
• Use Abaqus to create a model of three-point bending with only limited
guidance.

• Extract model prediction data from Abaqus and compare it against
experimental data.





1 Problem Definition

Your task is to set up and run an Abaqus FE simulation of a polymer beam
undergoing three-point elastic bending. The experimental set up is shown in
the schematic, and photo, below:






A video of the bend test is provided on Canvas, together with the
experimental data obtained. The polymer used was high-density
polyethylene (HDPE).

The test was performed such that a load was applied at the centre of the
beam, which induced a vertical displacement of the centre point, denoted .
It is your task to produce a model of this three-point bending scenario
that predicts the load vs. displacement behaviour.

You will set up your model in a very similar way to that in the previous
tutorials. However, in addition you will perform a mesh sensitivity analysis
on your model, before comparing your results to theory and experiment.


To create and run the simulation, you will need to:

• Create the beam and test fixture parts
• Create the material file for the beam
• Assign section properties to the beam
• Assemble the model
• Define the analysis steps
• Create the surfaces to use in contact interactions
• Define contact between regions of the model
• Apply boundary conditions and loads to the assembly
• Mesh the assembly
• Create and submit a job
• View and record the results of your analysis
• Vary the mesh size and re-run your model to determine mesh
sensitivity

Some instructions for each of these tasks are given in the following sections.

Please refer to the Tutorial 2 - Supplementary Guidance document for
further information on the specific tasks in Abaqus.


2 Create the Model Parts

1. Create the jig pieces and beam parts, with dimensions as shown in the
schematic above. The beam should be a 3D deformable extrusion, whilst
the jig parts can be made as a 3D discrete rigid extruded shell.

• All the jig pieces have the same geometry. Hence, you only need to
create one part for this (you’ll just make three instances of it).

2. Partition your beam (find under Tools) into quarters as shown below.
This will help when you come to applying boundary conditions later.




3. Add a Datum point (find under the Tools menu) at the centre of the top of
the beam – this is where the top jig piece will first make contact with the
beam.

4. Add two Datum points to the bottom surface of the beam, where the
centre of the jig pieces will first contact the beam.

5. Add a Datum point at the middle of the curved surface of your jig piece
(where it will first touch the beam).

6. Add a Reference Point (find under Tools menu) at some corner of your jig
piece that is away from the contact surface.


Note 1: You need to define a reference point on any rigid body in order to
apply constraints to it (i.e., to prevent its movement in particular directions).

Note 2: You could have proceeded with this simulation without generating the
parts of the three-point bending jig. You could have simulated their effect
reasonably well simply by applying loads to the beam at given points.
However, you’re asked to generate these parts here to try out your CAD skills.


3 Generate the Material

Unlike metals, polymers exhibit non-linear elastic behaviour – their stress vs.
strain curves are often not straight lines in the elastic regime. A tensile
engineering stress vs. engineering strain curve was measured for the HDPE
material used in the bend test, and is shown below, along with a photograph
of the experimental set-up. Even though this behaviour was almost entirely
elastic (i.e. reversible), pronounced non-linear behaviour is seen.





The data for this test in text format is available on Canvas.

The stresses that your beam will experience in this simulation should be
small, less than 15 MPa.

1. Estimate the Young’s modulus of the HDPE that would be most
appropriate for the bend test simulation, and use this to create the material
file.

2. Use a Poisson’s ratio of 0.4 (or another one of similar size you find in from
another source, HDPE is usually in the range 0.4 to 0.45).

4 Define and Assign a section


1. Define a homogeneous solid Section with the properties of the HDPE
you just entered.

2. Assign the Section to the beam (in the Model Tree expand the beam part
and look for Section Assignments).

• A set is created at the same time (see the prompt window). It’s called
Set-1 by default, but you may wish to change this name.

• The beam will go an aqua colour when it has been assigned properties.

5 Assemble the model


To assemble the model, you need to first create instances of the parts
required, then position the parts appropriately.

1. Create one instance of your beam piece to start with (dependent or
independent, it doesn’t matter here).

2. Create one instance of the jig piece.

3. Position the first jig piece by using the Datum points and the Constraint
→ Coincident Point tool. You could also apply further constraints if you
wish (for instance, you could constrain certain edges of the jig and beam
to be parallel, to ensure the correct loading geometry).

4. Create two further instances of the jig piece, and position as appropriate.

• You may need to rotate the jig pieces. To do this, use the Rotate
Instance tool

5. Create a new Set that includes only the reference point on the top jig
piece. This reference point should be added only in the Assembly
container within the model tree.


6 Define your analysis steps


Before you apply loads or boundary conditions to the model or define contact
within the model, you must define the different steps in the analysis. Once the
steps are created, you can specify in which steps loads, boundary conditions,
and interactions should be applied.

The analysis that you perform on the beam-bending model will consist of an
initial step (as generated by Abaqus automatically) and two general analysis
steps:


• In the first general analysis step you allow contact to become
established. You will ensure boundary conditions and contact
interactions are active in this step.

• In the second general analysis step you will apply a displacement to
the top jig piece of the model to simulate the three-point bending.

• You will need to toggle Nlgeom on in both the contact and
displacement (loading) steps so that Abaqus can use your input
material data correctly.

1. Create the contact analysis step. This should be a Static, General step
with an initial increment size of 0.1.

2. Create a load step, with the same settings, apart from using an initial
increment size of 0.001 (this will help you ensure that the initial
movement of the top jig piece is not too large).


7 Request output


1. As you did in the previous tutorial, change the F-Output-1 settings such
that outputs are only recorded at the Last increment of the contact step,
but every step in the loading step.

2. Accept the default output variables selected for each step.

3. You need to record the load-displacement behaviour of the top jig piece.
To do this, in the History Output Requests, create a new output in the
loading step.

• For Domain, select Set, and select the reference point on the top jig.

• Select the output variables associated with displacement in the
appropriate direction (it will be either U1, U2 or U3 along X, Y or Z
respectively).
• Select the output variable associated with the reaction force in the
appropriate direction (it will be either RF1, RF2 or RF3 along X, Y or Z
respectively).


8 Define contact between regions of the model


Interactions are objects that you create to model mechanical relationships
between surfaces that are in contact or closely spaced. Remember that mere
physical proximity of two surfaces on an assembly is not enough to
indicate any type of interaction between the surfaces.

You will need to define the contact interactions between each of the three jig
pieces and the beam. You will assume there is no friction present between the
jig pieces and the beam.

1. Create an Interaction property (contact type). Select Mechanical →
Tangential Behavior and accept Frictionless.

2. Create the three surface-to-surface interactions from the contact step
onwards. Make sure the jig piece is the master surface and the beam the
slave (the master surface should always be the less-deformable one).



9 Apply boundary conditions and loads

Apply the following constraints from the contact step onwards:

1. Constrain the two bottom jig pieces to be fixed in space and not rotate
(Displacement/Rotation = 0).

• You will need to apply the boundary condition to the reference points
on each of the jig pieces.

• Note in the prompt window that a set is created automatically when you
create the constraint. Rename the set as appropriate.

• Hold [shift] to select more than one object.

2. Constrain the beam, as appropriate, to stop it slipping out of position. This
may take some thought (hint: use the lines created by the partition).

3. Constrain the top jig piece to only move in the vertical direction also (and
no rotation).

4. From the load step onwards, apply a displacement of 2.5 mm to the top jig
in the appropriate direction (probably this will be the negative y-direction).
Again, you do this by applying the movement to the reference point.

• If any of the other parts get in the way of selecting, you can go into the
Assembly → Instances section of the Model Tree and hide them
temporarily.



10 Mesh the beam


Select the Parts container → your beam:

1. Check the Mesh → Mesh Controls. Make sure Hex is the default
Element Shape selection and Structured is the default Technique
selection.
2. In the Element Type dialog box, check the Incompatible modes option to
change the element type to C3D8I. Retain all other default values. (C3D8I
are good for beam bending, and C3D8R can also be used, but you could
also switch to quadratic elements – these are more expensive
computationally, but more accurate in general. See more details here:
http://50.16.225.63/v6.14/books/usb/default.htm\
3. Seed the part with a global size of 2 and mesh it.

For the jig pieces:

4. Seed the parts will a mesh size of 0.5 or smaller (you can do this without
impacting computing times significantly, since they are not solid objects).


11 Creating and submitting a job


Create and submit the job!



12 View results and export simulation data


1. Right click on the job and select Results.

2. Select to plot the results as contours on the parts.

3. From the top menu bar, select Animate → Time History to view the
animation of your simulation.

4. To export data from the model, you first need
to create the appropriate XY data:

• Double click on XYData in the Results
Tree. Select ODB history output (the
results are saved in an output database
.obd file).

• Find the Reaction force for the top jig
reference point (i.e., the load). Click Plot to
view the data graphically, then click Save
As… to save the data (this had not been
exported yet). Do the same for the Spatial
Displacement for the top jig reference point.

• Double click on XYData in the Results Tree.
Select Operate on XY Data.

• Under Operators, select combine(X,X). Select
the displacement data first to make this the X-axis
data, then click the reaction force data to plot this
on the Y-axis. Click Plot Expression to see this
data, then click Save As… to save the data.

• To export the data, go to Report → XY…, select
the data you just created and click Apply. This will append your data to
an .rpt file in the directory you’re saving your Abaqus files.

• If you get an error doing
this, select to use the XY
plot in current viewport
and click Apply.





13 Perform a mesh sensitivity analysis


The results obtained from FEM simulations can sometimes vary significantly
with mesh size. In order to judge the impact of mesh size, a mesh
sensitivity study can be performed, in which the mesh size is varied and
results are compared against each other. Generally it will be the case that, as
the mesh size decreases, the results obtained will converge to a constant
value, such that a further decrease in mesh size makes little appreciable
difference. Very small mesh sizes can take a long time to run, so it is
advantageous to use the largest mesh size that gives the most consistent
result.

1. Assess the results obtained for smaller mesh sizes, try 1 mm and 0.5 mm
to begin with.

• Save the load vs displacement curves (see procedure in Section 13)
for each of the mesh sizes.

2. Plot and compare these in an appropriate software package (e.g. Excel).

• Do they compare well? Do you think that decreasing the mesh size
further will improve your results significantly? If so, try it! Note


14 Further Tips

How to open your data in Excel:

1. If you follow the instructions given in the Tutorial 3 script, Abaqus exports
your data as a .rpt file. This is exported to your working directory.

2. If you’re struggling to find where the .rpt file is, go into Abaqus and click
File > Set Work Directory. You should be able to see where the file has
been exported to (e.g. C:\work).

3. Open up Excel. Click Open, find the working directory. Select the type of
file you can open to All Files (not just Excel files). You should now be able
to see the .rpt file. Open it.

4. The Text Import Wizard opens. The data in the .rpt is delimited by a space
(i.e., a space separates the columns). Accept the delimited option
highlighted, and on the next screen click the box next to Space. Accept
everything else and finish.

5. Your data should be displayed. If you have multiple sets of data, it’s
because you’ve exported your data on multiple occasions, and Abaqus
has simply appended it to the .rpt file.




If your data looks orders of magnitude out compared to my test data, make
sure you're using the correct units for the Young's modulus you input (see bit
on units in Tutorial 1).

If your plots show a different slope (i.e., a negative gradient, rather than
positive like my experimental results), this is simply because we have defined
our directions differently (e.g., my positive is your negative). You can flip your
results in Excel if you want.



15 Preliminary Report

You should submit one screenshot and one file to Canvas.
1. A screenshot of your von Mises contour plot when the beam is in
its position of maximum bending (best pasted into a Word
document)

2. Your Abaqus CAE file (.cae) for the beam bending model.
Upload this onto Canvas by the date specified in the assignment.
To take a screenshot, you might wish to use the Snipping Tool, which is
activated using the Windows + Shift + S key combination. Paste this into
Word for easy viewing on Blackboard.

Continue to Section 16 for details of the written report…

Assessment criteria
Your submission will be marked /3, according to the following:
• 3 marks: full submission, correct.
• 2 marks: full submission, but with significant errors.
• 1 marks: partial submission (e.g., only the contour plot).
• 0 marks: no submission.
16 Written report - assessment brief

As part of your assessment for this course, you are asked to write and submit
individually a report giving details of the simulation you created above and its
results.

It should compare your simulation results to the experimental results for the
beam bending you simulated, which are shown in the graph below (data for
this available on Blackboard), and offer explanations for any discrepancies.

Your report should be no more than 3000 words, and no more than 8
pages including all figures, references and appendices. Font size no
smaller than 11.

You need to upload your report via Canvas by the specified date.
Please read all the information and guidance below.



You can split up your report into the following sections. The report should be
written in the style of a standard lab report (see further guidance on BB for
this):

• Introduction and Aims. Provide a brief introduction to FE modelling
and the problem you are trying to solve.

• Simulation Set Up. Assume your reader is an experienced Abaqus
user – what important information would you need to convey in order
for them to recreate your simulation? You do not need to give lots of
detail here - no ‘this button was clicked’, ‘that button was clicked’ etc.
This should be written in the past tense, in the same style as you would
for a standard lab report.
• Results. Describe your results and present your figures (graphs, etc).
Remember to provide text describing your results.

• Discussion. Discuss possible reasons for what your results shows.

• Summary. Give a brief summary of the findings of your investigation.
Include only the key points.


There is an analytical theory (i.e., an equation) that describes the force vs.
deflection behaviour of a beam undergoing three-point bending. You may
wish to find out what this is and compare your simulation results to it, as well
as to the experimental results.

Assessment criteria

Marks will be awarded according to the following:

• Introduction and Aims (10%): Whether you have provided a brief
introduction explaining the aims of your work.

• Simulation Set Up (15%): Whether you have provided the reader with
sufficient information to recreate your model (in the simulation set up
section).

• Model and Tutorial Execution (15%): Whether you have completed
the tasks outlined in the tutorial script, created a working and
representative FE model, and presented evidence of these.

• Results (20%): Whether you have presented your results in an
appropriate and coherent manner.

• Discussion (30%): The quality of your discussions, including
comparisons of model results to the experimental results and theory.

• Presentation and Writing (10%): The structure of your report and the
quality of writing, as well as the presentation of your report, including
the quality of figures.

See the rubric at the end of this document.






17 Learning Outcomes Assessed:

• Create a basic linear elastic finite-element model in Abaqus for a
simple loading scenario.

• Describe the creation of your model so others can understand your
approach and accurately reproduce it.

• Discuss the limitations of finite element models, and reasons for
discrepancies between model and experiment.

• Present the results of finite element simulations in a coherent manner.

• Write reports of sufficient quality for industry.


18 Other general considerations:

• The style of your report should be similar to your experimental lab
reports – e.g., the simulation set up paragraph should be written in the
past tense.

• You should make sure the scales on your graphs and other results are
readable.

• You should label all your figures (e.g., Figure 1), and refer to all of them
from your text.

• You should always define any acronyms (e.g., FEM) at the first point of
use.

• There should be a space between numbers and their units, as well as
between different units. For example: 600 m s-1, not 600ms-1

• Think about how many decimal places (or significant figures) it is
appropriate to quote your results in. Do not present the same results in
both tabular form and in graphical form – choose one or the other.

• You should NOT copy work from other sources, including other
students – the work should be entirely your own. If information
has been gathered from outside sources, it should be referenced
appropriately.





0 Not present
10%
Very poor
20%
Very poor
30%
Poor
40%
Satisfactory
50%
Satisfactory
60%
Good
70%
Very good
80%
Excellent
90%
Outstanding
100%
Flawless
Introduction
and Aims
(10%)
No introduction
and aims are
provided.
There is barely
any
introduction
and no aims are
listed.
Significant
errors/
omissions
present.
There is a
limited
introduction
and a partial
list of aims,
with significant
errors/
omissions.
The
introduction
and aims are
more
substantial, but
poor overall,
with significant
errors/
omissions.
Reasonable
introduction
and aims are
provided, but
with significant
errors/
omissions.
Reasonable
introduction
and aims are
provided, but
with some
errors/
omissions.
Introduction
and aims are
good, with
minor errors/
omissions.
Introduction
and aims are
very good, with
minor errors/
omissions.
Introduction
and aims are
very good, with
very minor
errors/
omissions.
Introduction
and aims are
outstanding,
with very
minor errors/
omissions.
Introduction
and aims are
flawless, with
no errors/
omissions.
Simulation
Set up (15%)
No
methodology is
provided.
There is barely
any
methodology
described, with
significant
errors/
omissions.
There is a
limited
methodology
section, with
significant
errors/
omissions.
The
methodology
section is
relatively
substantial, but
overall poor,
with significant
errors/
omissions.
Reasonable
methodology
section is
provided, but
with significant
errors/
omissions.
Reasonable
methodology
section is
provided, but
with some
errors/
omissions.
Methodology
section is good,
with minor
errors/
omissions.

Methodology
section is very
good, with
minor errors/
omissions.
Methodology
section is
excellent, with
very minor
errors/
omissions.
Methodology
section is
outstanding,
with very
minor errors/
omissions.
The
methodology
section is
flawless.
Model and
tutorial
execution
(15%)
No evidence of
a correct and
working model
is provided.
None of the
tasks in the
tutorial (e.g.,
mesh
sensitivity
analysis) have
been
completed.
Very limited
evidence of a
correct and
working model
is provided.
None of the
tasks in the
tutorial (e.g.,
mesh
sensitivity
analysis) have
been
completed.
Limited
evidence of a
correct and
working model
is provided.
Significant
issues with the
model may be
apparent. Very
few of the tasks
in the tutorial
(e.g., mesh
sensitivity
analysis) have
been
completed.
Relative
substantial
evidence of a
correct and
working model
is provided.
Some issues
with the model
may be
apparent. A few
of the tasks in
the tutorial
(e.g., mesh
sensitivity
analysis) have
been
completed.
Reasonable
evidence of a
correct and
working model
is provided.
Some minor
issues with the
model may be
apparent. A few
of the tasks in
the tutorial
(e.g., mesh
sensitivity
analysis) have
been
completed.
Reasonable
evidence of a
correct and
working model
is provided.
Some minor
issues with the
model may be
apparent. Most
of the tasks in
the tutorial
(e.g., mesh
sensitivity
analysis) have
been
completed.
Good evidence
of a correct and
working model
is provided. No
issues with the
model are
apparent. Most
of the tasks in
the tutorial
(e.g., mesh
sensitivity
analysis) have
been
completed.
Very good
evidence of a
correct and
working model
is provided. No
issues with the
model are
apparent. All of
the tasks in the
tutorial (e.g.,
mesh
sensitivity
analysis) have
been completed
to a high
standard.
Excellent
evidence of
correct and
working model
is provided. No
issues with the
model are
apparent. All of
the tasks in the
tutorial (e.g.,
mesh
sensitivity
analysis) have
been completed
to a very high
standard.
Outstanding
evidence of
correct and
working model
is provided. No
issues with the
model are
apparent. All of
the tasks in the
tutorial (e.g.,
mesh
sensitivity
analysis) have
been completed
to a
exceptionally
high standard.
The model is
flawless, as are
all the tasks
that have been
asked for (e.g.,
mesh
sensitivity
analysis).
Results
(20%)
No results are
provided.
There are
barely any
results
presented.
Significant
errors/
omissions
present.
There is limited
set of results
presented, with
significant
errors/
omissions.
The results
section is
relatively
substantial, but
overall poor,
with significant
errors/
omissions.
Reasonable
results section
is provided, but
with significant
errors/
omissions.
Reasonable
results section
is provided, but
with some
errors/
omissions.
Results section
is good, with
minor errors/
omissions.
Results section
is very good,
with minor
errors/
omissions.
Results section
is excellent,
with very
minor errors/
omissions.
Results section
is outstanding,
with very
minor errors/
omissions.
The results
section is
flawless.
Discussion No discussion
is provided.
There is barely
any discussion
There is a very
limited
The discussion
is relatively
Reasonable
discussion is
Reasonable
discussion is
Discussion is
good, with
Discussion is
very good, with
Discussion is
excellent, with
Discussion is
outstanding,
The discussion
is flawless.
(30%) of results, with
significant
errors/
omissions. No
mention of
sources of
uncertainty/
error/model
improvements.
discussion,
with significant
errors/
omissions.
Very limited
discussion of
sources of
uncertainty/
error/model
improvements.
substantial, but
overall poor,
with significant
errors/
omissions.
Some
discussion of
sources of
uncertainty/
error/model
improvements.
provided, but
with significant
errors/
omissions.
Some
discussion of
sources of
uncertainty/
error/model
improvements.
provided, but
with some
errors/
omissions.
Discussions of
sources of
uncertainty/
error/model
improvements.
minor errors/
omissions.
Discussions of
sources of
uncertainty/
error/model
improvements.
minor errors/
omissions.
Discussions of
sources of
uncertainty/
error/model
improvements.
very minor
errors/
omissions.
Discussions of
sources of
uncertainty/
error/model
improvements.
with very
minor errors/
omissions.
Discussions of
sources of
uncertainty/
error/model
improvements.
Presentation
and Writing
(10%)
The document
is unreadable.
The document
is very poorly
presented.
Almost all the
writing and
figures are
unclear and/or
inappropriate.
The document
is very poorly
presented.
Most of the
writing and
many of the
figures are
unclear and/or
inappropriate.
The document
is poorly
presented.
Much of the
writing and
many of the
figures are
unclear and/or
inappropriate.
The document
is reasonably
well presented.
A few sections
of the writing
and a few of the
figures are
unclear and/or
inappropriate.
The document
is presented
satisfactorily. A
few sections of
the writing or a
few of the
figures are
unclear and/or
inappropriate.
The document
is well
presented.
Most of the
writing and
figures are
clear and
appropriate.
The document
is very well
presented. All
of the writing
and figures are
clear and
appropriate.
The document
is presented
excellently. All
of the writing
and figures are
clear and
appropriate.
The document
presentation is
outstanding.
All of the
writing and
figures are
clear and
appropriate.
The
presentation
and writing is
flawless.


学霸联盟