Nonlinear Elastic Plastic Finite Element Analysis of U-Shaped Plate (2D and 3D)

Nonlinear Elastic plastic finite element
analysis of U-shaped plate (2D and 3D)
J. Smith
School of Engineering
[e-mail]
ABSTRACT: In the current study, a finite element study has been performed on a U-shaped
plate using both 2D plane stress as well as 3D approach using Abaqus software. An
elastic-plastic nonlinear material behavior is considered. It was concluded from the
analysis that structure has a collapse load of ~43000 N as obtained from 3D analysis.
Comparison of numerical and analytical calculations also compares well and values are
discussed in the results.
KEY WORDS: finite element analysis, material nonlinearity
Introduction
Finite element analysis is a very
important, fast and cheaper tool to assess
performance of various designed
structures for intended loading
(Gunwant, 2013). Conventional
approach of designing product uses
analytical methods (1D calculations) to
assess displacements and stresses in
components which sometimes could be
misleading. The shape of the
components are approximated with
several primitives for analytical
component which might not capture the
accurate performance (Khatawate,
2016). Moreover, design of systems and
assemblies becomes more complicated,
needing more design iterations and
costly because of experiments performed
(Kannan, 2015).
In the current study, a U-shaped plate
has been analyzed using finite element
method in Abaqus software. The
analysis is done considering both types
of element which are 2D (plane stress)
and full 3D. The aim of the current
study is following:
1. Performing a non-linear elastic
plastic analysis to assess collapse
load in U-shaped plate
2. Comparison of Collapse loads as
obtained from 2D and 3D
analysis
Finite Element Model
In this section, finite element model
prepared for the analysis of U-shaped
plate is explained. Abaqus software has
been used for the current finite element
analysis. Used steps in terms of
geometry, mesh, loading and boundary
conditions are explained in the current
section.
Symmetry
1

The prepared model for the current
analysis of U-Shaped plate is shown in
figure 1. The dimensions of the model
are taken as per the drawing schematic
which is shown in figure 2.
As per the last 3 digits of student number
which are 937, following are the
dimensions taken for figure 2:
X = 1.5 + 0.001*937 = 2.437 mm
t = 5X = 5*2.437 = 12.185 mm
10X = 10*2.437 = 24.37 mm
20X = 20*2.437 = 48.74 mm
40X = 40*2.437 = 97.48 mm
Figure 1: Prepared U-Shaped plate model in
Abaqus software for both 2D and 3D finite
element analysis
Considering the only geometric shape of
the U-shaped plate, a symmetry can be
considered at the middle of the middle
portion of the plate. Looking at loads
and boundary conditions, the left hand
side is applied with a fixed (all 6 degrees
of freedom) boundary condition while
right side is applied with a roller support
(5 degrees of freedom constrained,
horizontal motion free). Since it is not
symmetric, hence it was decided to
perform a full geometry analysis.
Figure 2: Prepared U-Shaped plate model in
Abaqus software for both 2D and 3D finite
element analysis
Choice of elements
In the current section, used elements for
both 2D as well as 3D analysis are
discussed. As shown in figure 3, the 3D
element used in Abaqus tool is C3D8R
which is an 8 node 3D element with
reduced integration scheme. This is a
linear element i.e. no middle node
present in the element.
Figure 3: Settings of 3D element – C3D8R used
for 3D analysis of U-shaped plate in Abaqus
2

Figure 4: Settings of 2D element – S4R used for
2D analysis of U-shaped plate in Abaqus
For 2D analysis, used element type is
shown in figure 4 which is S4R. It is a
quad element with 4 nodes and uses
reduced integration scheme.
More than element type, the accuracy
depends on the mesh density if it is
enough to capture the non-linear
behavior of the plate.
Material properties
In the current section, material properties
used in the current analysis are
explained. The material used is mild
steel sheet or low carbon steel which is
widely used for manufacturing in
automotive industry. Following are the
material properties as listed in Table 1
for the material.
Table 1: Material properties of low carbon steel
as used in current analysis
Type of property Value
Elastic Modulus 210 GPa
Poisson’s ratio 0.33
Yield strength 270 MPa
Plastic Strain 0.15 (15%)
For the material property definition in
Abaqus, both elastic as well as plastic
definition is used. The defined material
property is shown in figure 5.
Constraints
In this section, loading and boundary
conditions applied in Abaqus model are
discussed. For the definition of boundary
condition, the schematic shown in figure
2 is used. The defined boundary
conditions in Abaqus are shown in figure
6 for 2D analysis and figure 7 for 3D
analysis.
The left hand side of the U-plate is
applied with ‘encastre’ i.e. all 6 degrees
of freedome are constrained while right
hand side is applied with displacement
and rotation constraints with
displacement in x-direction to be free i.e.
roller support.
Figure 5: Material card as defined in Abaqus to
perform both 2D as well as 3D analysis
3

Figure 6: Loads and boundary conditions as
applied on U-shaped plate for 2D analysis
Figure 7: Loads and boundary conditions as
applied on U-shaped plate for 3D analysis
Loads are applied onto the U-shaped
plate at the left as well right hand side.
Since we do not know the failure or
collapse load of the U-shaped structure,
a 25000 N was applied on each end of
the arms. In the analysis, the virtual time
at which the strain completely crosses
the middle portion of the U-shaped plate,
according to that, the collapse load is
estimated.
Mesh density
In this section, the mesh density used in
2D as well as 3D analysis of U-shaped
plate is discussed.
For 2D finite element analysis, the used
mesh density with quad elements is
shown in figure 8 for U-shaped plate.
For 3D finite element analysis, the used
mesh density with quad elements is
shown in figure 9 for U-shaped plate. It
is very necessary for the mesh density to
be fine enough so as to make the output
results independent of it.
Figure 8: Loads and boundary conditions as
applied on U-shaped plate for 3D analysis
Figure 9: Loads and boundary conditions as
applied on U-shaped plate for 3D analysis
For the current study, 3 different mesh
sizes were analyzed for both 2D as well
as 3D analysis so as to compare and
study the effect of mesh size variation of
the stress outputs. It was observed that
with a global mesh size of 2 mm, the
mesh appears to be converged. From the
calculated stress numbers, it was
observed that if the mesh density is
reduced further below 2 mm, the change
in stress numbers are less than 3% for
both 2D as well as 3D analysis hence
mesh size of 2 mm is decided to be
converged.
Output requests
4

In this section, output data requests in
Abaqus software are discussed. The load
step created in Abaqus is ‘static, general’
for which total virtual simulation time
defined is 1. While analysis is run and
solved, different solved field variables
like displacements, stresses and strains
need to be stored. In Abaqus, user need
to define which variables to store in the
result, at which locations and at what
solution time. This keeps the solution
file size limited but at the same time, it
captures all the required necessary data
which is needed for post-processing.
In the current case, displacements (all 3
directions), stresses (principal and
equivalent), strains (elastic and plastic)
are all needed and stored by default in
the field output created with the load
step. It is shown in figure 10. Field
outputs are usually taken for the whole
model so as to be able to plot the
contours of stress, displacement etc.
Figure 10: Field output as created in Abaqus for
whole element to take relevant field variables in
output results (.odb) file
For history output, a separate request is
created in Abaqus. Since we need to
know the stress-displacement curves of
the locations where loads are applied, it
is a good practice to create a set and
define a history output corresponding to
it. In the current Abaqus model, the set
for loading locations are created in the
name of ‘Load1’ and ‘Load2’ for both
the locations. The created history output
is shown in figure 11.
Figure 11: History output as created in Abaqus
for whole element to take relevant field variables
in output results (.odb) file
Results
In this section, the obtained results from
the finite element analysis are presented.
There are 2 different analysis that are
performed which is in 2D and 3D for the
current study. The results from 2D
analysis are discussed first followed by
results of 3D analysis.
5

The displacement plot obtained from 2D
analysis is shown in figure 12. The stress
distribution after the structure collapse is
shown in figure 13. The strain plot is
shown in figure 14. It is shown by 3
different plots, the first plot correspond
to the simulation at onset of plastic
deformation in the middle region of the
U-shaped plate. The second plot is when
plastic deformations in the middle
portion of the plate progress half way to
the centre line of the plate and third plot
is when the middle portion of the plate
becomes fully plastic (plastic
deformation reaches centreline of the
plate), resulting in plastic collapse load
Figure 12: Displacement plot from 2D analysis
of U-shaped plate in Abaqus
Figure 13: Stress plot from 2D analysis of U-
shaped plate in Abaqus
Figure 14: Strain plot from 2D analysis of U-
shaped plate in Abaqus, first at the onset of
plastic deformation, second when plastic strain
reaches midway, third when plastic deformation
reaches centerline of middle portion
The displacement plot obtained from 3D
analysis is shown in figure 15. The stress
distribution after the structure collapse is
shown in figure 16. The strain plot is
shown in figure 17. It is shown by 3
different plots similar to strain plots for
2D analysis.
Figure 15: Displacement plot from 3D analysis
of U-shaped plate in Abaqus
Figure 16: Stress plot from 3D analysis of U-
shaped plate in Abaqus
6

Figure 17: Strain plot from 2D analysis of U-
shaped plate in Abaqus, first at the onset of
plastic deformation, second when plastic strain
reaches midway, third when plastic deformation
reaches centerline of middle portion
Discussion
In the current section, the obtained
results are discussed, compared and
inferences are drawn.
From the 2D analysis, strain plots at
different levels of strain are obtained and
compared. It was observed that the for
onset of plastic deformation, total
simulation time was 0.6 hence applied
load is 50000*0.6 = 30000 N. For the
plastic deformation to reach middle of
the plate, it is 0.8 hence applied load is
50000*0.8 = 40000 N and finally for the
structure to collapse, total simulation
time was 0.9065 hence applied load is
50000*0.9065 = 45325 N.
From the 3D analysis, It was observed
that the for onset of plastic deformation,
total simulation time was 0.57 hence
applied load is 50000*0.57 = 28500 N.
For the plastic deformation to reach
middle of the plate, it is 0.8 hence
applied load is 50000*0.77 = 38500 N
and finally for the structure to collapse,
total simulation time was 0.9065 hence
applied load is 50000*0.865 = 43250 N.
It can be observed that shell or 2D
modeling slightly over estimates the
stiffness of the structure and hence
provides comparatively higher collapse
load value. From the analysis, it can be
concluded that 3D analysis is
comparatively more accurate but
simulation time needed for 3D analysis
is approximately 30 minutes while 2D
analysis took 3 minutes.
Accuracy of the analysis is also
governed by the mesh density which is
already converged and type of element.
From the analytical calculation, for onset
of plasticity, Equation 1 can be used.
From the analytical calculation, for
partial plasticity, Equation 2 can be used
and for collapse load, equation 3 can be
used.
, (1)
, (2)
, (3)
Where h and b are beam dimensions, and
other is yield stress.
Hence
Onset of plasticity =
270 x (48.74) x 12.185/6 = 26725 N
For Partial plasticity =
270 x (48.74) x 12.185 x 11/48 =
36747.3 N
For collapse load =
270 x (48.74) x 12.185/4 = 40088 N
7

It can be seen that analytically calculated
loads correlates well with numerical
results.
Conclusion
Following are the obtained conclusions
based on the analysis study:
1. From the 2D analysis, for onset
of plastic deformation, applied
load is 30000 N. For the plastic
deformation to reach middle of
the plate, applied load is 40000 N
and finally for the structure to
collapse, applied load is 45325
N.
2. From the 3D analysis, for onset
of plastic deformation, applied
load is 28500 N. For the plastic
deformation to reach middle of
the plate, applied load is 38500 N
and finally for the structure to
collapse, applied load is 43250
N.
3. From analytical solution, for
onset of plastic deformation,
applied load is 26725 N. For the
plastic deformation to reach
middle of the plate, applied load
is 36747 N and finally for the
structure to collapse, applied load
is 40088 N.
4. Analytical solution and
numerical solution compares
well
5. 3D approach is found to be more
accurate as compared to 2D
approach for numerical analysis.
Declaration
I declare that this document contains
less than 15 pages.
I declare that I will submit this work
as a PDF document.
I declare that the file size of the
submitted PDF document is below 3Mb.
<Insert student signature>
References
1. Khatawate, Vinayak & Dharap, M.A.
& Moorthy, R.I.K.. (2016). Stress
and strain concentration factors for
flat plate with opposite side U-
shaped notches under tension.
International Journal of Design
Engineering. 6, 173-179.
2. I., Vimal Kannan. (2015).
Comparative study of stress analysis
on notched plates between analytical
and Finite Element Solutions.
International Journal of Engineering
and Innovative Technology (IJEIT).
121-131.
3. Gunwant, Dheeraj. (2013). Stress
and Displacement Analysis of a
Rectangular Plate with Central
Elliptical Hole. International Journal
of Engineering and Innovative
Technology (IJEIT). 211-223.
8