 Prepared 3D CAD model of honeycomb in SolidWorks; studied structural behavior for static and dynamic loading  Performed mesh refinement, verification, validation and error analysis for the FEA

1. 1
Finite Element Analysis of Aluminum Honeycomb Subject to
Compression Loads
Udayan Ghosh (uID: u1138967)
ME EN 6510 Project Report
Fall 2017
University of Utah
Salt Lake City, UT, 84112, USA
udayan.ghosh@utah.edu
December 15, 2017
Abstract:
Honeycomb structure is widely found in nature: plants, animals and even human cells. This structure is
regarded as one of the most stable structures with optimal coverage. Aluminum honeycomb is
lightweight and has high strength to weight ratio. Additionally, it is a good energy absorber. Study of the
behavior of aluminum honeycomb can help us to determine its extensive use as a structural component
in various engineering fields. In this project, the mechanical characteristics of Aluminum Hexagonal
Honeycomb structure will be analyzed under compression loading conditions using ABAQUS. The model
will be validated using experimental data. For the validation purpose, honeycomb will be considered as
uniform having cell size as 9.525 mm and single wall thickness as 0.0762 mm for a total dimension of
90*90*50 mm3
. This is named as H42 with specification of 4.2-3/8-5052-.003N according to the
manufacturer. The validated model is used to investigate the deformation due of compression.
Keywords: Honeycomb, Numerical Simulation; FEA; ABAQUS.
1. Introduction:
Honeycomb structure is mainly hexagonal comb
like structure which is commonly found in beehive.
It is a widely popular structure for structural
analysis due to its high strength, yet low weight
property. Honeycomb can be made of various
types of materials based on the purpose of its use.
However, for structural purposes, most commonly
used material is Aluminum. Aluminum
honeycombs are mainly used to aerospace and
automotive engineering field where both the
structural integrity and light-weight property is
highly valued. In sandwich structures, honeycomb
is widely used.
Different studies have been conducted to analyze

2. 2
the impact of different loading conditions both
experimentally and numerically to understand
and predict the performance and integrity of
Aluminum honeycomb structures. Ashab et al. [1]
have performed only experimental analysis of
aluminum honeycomb for both dynamic out of
plan indentation and compression load for three
types of honeycomb structure of different cell
size and wall thickness. They have also highlighted
on energy absorption for both loading conditions.
Gibson [2]
et al. analyzed that the mechanism of
deformation in honeycomb structures of elastic
bucking. Xinyang et al.[3]
have run their numerical
finite element analysis for thermoplastic
honeycomb under compression. Their
investigated structure had material property of
ThermHex(R)
. They have tried to develop a
method for nonlinear analysis considering the FE
linear buckling analysis. Moreover, they have
considered the tilting of the honeycomb cells.
Jeom et al [4]
showed their work both theoretically
and experimentally. They have performed three-
point bending, axial compression and lateral
crushing loads for their experimental purpose and
found that cell thickness plays an important role
to delay the deformation due to three point
buckling. They have also looked into the effect of
core height for compressive test and found that it
is a crucial parameter. D. Ruan et al. [5]
have
worked on numerical simulation using Abaqus for
in plane dynamic crushing of the honeycomb.
They investigated modes and plateau stresses
creating a relation among those and wall
thickness and impact velocity. M. Yamashita and
M. Gotoh [6]
have completed their investigation
both numerically (using DYNA3D) and
experimentally (using drop-hammer apparatus)
for various cell specifications considering
compression of Aluminum Honeycomb. Lingling
Hu et al. [7]
focused their research on the impact
of the angle of the cell wall both experimentally
and numerically. They concluded that the
optimum cell wall angle is 450
which gives the
optimal crushing strength. Dong Ruan et al. [8]
have performed FEA of Aluminum Honeycombs
using ANSYS/LS-DYNA considering dynamics
indentation and compression loads and compared
them with experimental values. As dynamic
indentation has not been widely explored, they tried
to concentrate on it more. They have reported that
with the increase of t/l ratio, plateau stress,
dissipated energy, and tearing energy increases and
also proposed an empirical formula for the tearing
energy per unit fracture area in terms of strain rate
and relative density of honeycombs. M. Zarei
Mahmoudabadi, and M. Sadighi [9]
studied the metal
honeycomb under the impact of Quasi-Static Loading
and proposed a modification to Wierzbicki’s [10]
model by comparing results with experimental data.
Wang et al. [11]
investigated on axial impact of
honeycomb under high speed impact values both
experimentally (using their own experimental set-up)
and numerically (using ANSYS and LS-DYNA). During
simulation, they have presented the effect of
element size for the honeycomb. Moreover, they
have highlighted the velocity sensitivity of
honeycomb and found that honeycomb maintains a
power law on specific load against impact velocity.
In the present project, numerical simulation is
performed using ABAQUS to study the impact of out
of plane compression load over the Aluminum
honeycomb of thin wall. Previous experimental data
available, full-scale models of honeycombs were
considered for verification. The verified FE models
are then used for further investigation.
2. Finite Element Model Set-up:
In this project, Finite Element Analysis is performed
for Aluminum Honeycomb for compression load.
Generally, honeycomb has hexagonal structure. In
natural honeycomb, both regular and irregular
hexagons are found. For some structures both
regular and irregular shaped hexagons form the
whole structure.
2.1 Geometry Preparation:
In most of the structural purposes, regular hexagonal
honeycomb core is used; especially in the sandwich
panels. For this project, the honeycomb’s each cell
dimension specifications are given in Table 1. The
physical illustration of the conventional dimensions is
shown in Figure 01. The dimensions of each

3. 3
honeycomb are same and have a height (h) of 0.05m
[1]
. The in plane dimension of honeycomb sample is
0.092 m * 0.087 m for compression test (Figure 03).
Table 01: Specifications of aluminum honeycomb[8]
Type Material
Description
Cell Size
(D)
(mm)
Single
Wall
Thickness
(t) (mm)
H42 4.2-3/8-
5052-0.003N
9.525 0.0762
Figure 01: Dimensions of honeycomb. a)
honeycomb’s orientation and direction of
compression load. b) Thickness and angular
dimension of honeycomb. c) Cell size (D)
Figure 02: Solidworks drawing and dimension
specifications.
The relation between the cell size and the length of
cell edge (l) is . To construct the whole
geometry, Solidworks was used first for the 3D
modeling. At first, a 2D drawing was created using
wall thickness specifications and cell size. As we
considered regular honeycomb, hexagons with inner
angle 1200
was drawn first. This model with
dimensions is shown in Figure 02.
Figure 03: Compelte rectangular honeycomb model.
The Honeycomb had dimension of 0.09 m * 0.09m. The
structure in that experiment had extensions of single
wall thickness in all sides of the honeycomb. For this
project, then single wall extensions are reduced and
only honeycombs are considered for the analysis
purpose. Figure 03 shows the whole model without
extended single wall in every side except two single
walls at two opposite end of the strucutre. It was
considered to make the whole strucuture a rectangle.
The complete structure has a total number of 90 regular
hooneycombs altogether. The outer most honeycombs
parallel to plane 6, has single wall thickness at their
outer most wall. Apart from this, double wall thickness
is employed for all honeycombs. Although the extended
single wall was considered in the experiment because of
its specifications according to the manufacturer, during
this project, for numerical analysis, those walls are
excluded due to its little significance of carrying
compression loads as they have very little length
compared to the whole structure.
2.2 Material Specification:
Hexagonal aluminum honeycombs are lightweight and
good energy absorber. The plastic deformation is its
main energy absorption zone [1]
. However, physical
experiments have been conducted for both elastic and
plastic deformation of the aluminum honeycomb. Dong
Ruan et al. [8]
has studied their model considering
kinematic hardening for elasto-plastic material using
ANSYS. In this project, the honeycomb is considered as
elasto- plastic.

4. 4
Material specifications are given in the Table 02. The
values of constants are taken from the conventional
material properties of aluminum.
Beyond the elastic region, material behavior
becomes nonlinear and it starts to behave in-
elastically. Stiffness of the member changes which
depends on material behavior called elasto-plastic.
Figure 04 shows the regions. An increase in yield
stress is referred as work hardening and decrease is
regarded as work softening. Based on diagram,
Figure 04: Material nonlinear behavior.
Material behavior can be divided into three main
parts. i. perfectly plastic; ii. Elasto-plastic
(hardening); iii. Elasto-plastic (Softening). As the
large plastic deformation in hexagonal honeycomb
is the main energy absorption region, elasto plastic
material model is chosen for this project. Elasto-
plastic strain hardening has two types of
characteristics - 1. Isotropic 2. Kinematic. Here we
have considered it as isotropic hardening
Table 02: Material properties of aluminum
honeycomb[8]
Mass
Density
Young’s
Modulus(E)
Poisson’s
Ratio (υ)
Yield
Stress(σ)
2780
kg/m3
73 GPa 0.33 280
MPa
For the plastic zone, due to its non-linearity, data is
collected for Yield stress vs Plastic Strain from the
standard material property for AL 2024-T351 Alloy.
This is a widely used alloy in various industry.
Table 03: Data for plastic region[13]
Yield Stress (Pa) Plastic Strain
280000000 0
291521000 0.00323599
323634000 0.00617938
355590000 0.0130631
388551000 0.0231783
411518000 0.0333928
429860000 0.0489437
453156000 0.0717011
477319000 0.100551
495990000 0.128281
510955000 0.155988
524274000 0.188516
533454000 0.223694
539880000 0.25169
543760000 0.279305
546202000 0.305118
2.3 Boundary Conditions:
For compression test in the physical specimen [1]
, the
honeycomb specimen was placed on a fixed plate and
crushed by an upper plate at a constant speed. The
speed of the upper plate ensured displacement for
certain time intervals. As the hexagonal structure of
aluminum honeycomb is velocity sensitive [11]
, it is
important to choose the velocity for the simulation. In
this project, the velocity is chosen as 5 mm/s based on
the experimental data[1]
.
In present FE project, boundary constrains are applied
to make the lower plane rigid. For lower plane of the
honeycomb, all degrees of freedom were kept fixed. For
loading criterion, out of plane compression load is
considered by constructing velocity constraint.

5. 5
The direction of the compression is shown in Figure
05 and Figure 06 shows 3D model of Aluminum
Honeycomb after applying all the boundary
conditions.
Figure 05: Direction of out of plane compression
over the honeycomb.
Figure 06: Aluminum Honeycomb (3D) after
applying all boundary constraints
2.4 Meshing:
For the simulation of the aluminum, choice of mesh
element type and element size is very important.
The increased number of element ensures the
accuracy of the analysis. However, at the same time,
it increases the time required for the analysis which
eventually affects the cost of the analysis. Thus, in
FE analysis, choosing the right size of the element is
one of crucial parts to ensure both accuracy and
optimization of analysis run time.
In this project, the geometry is complex and it
requires more attention while meshing. The
thickness of the wall is very thin and at the joints of the
honeycomb hexagons, little triangle forms which makes
the choice of element more difficult. It is difficult to
select only one type of element for the whole
geometry. Before meshing, at first nodes are assigned
to the whole honeycomb. For this project, global size
was taken as 0.7mm. Using this value, a total of 357552
nodes is distributed over the whole honeycomb
structure.
For meshing the honeycomb, a combination of
hexahedral and wedge element is considered. For
better accuracy with less analysis time, hexahedral
elements are best choice. However, for complex
geometry where local partition thus local meshing is
required, a combination of hex and other elements are
considered. While using ABAQUS, hex dominated
element shape was chosen due to the complexity of
hexagon’s geometry at the six sharp edges. Table 04
presents the specification of element shapes used for
meshing.
Table 04: Element shape specification.
Element
Type
Element
Shape
Geometric
Order
Number
of
Elements
C3D8 Hexahedral Linear 174092
C3D6 Wedge Linear 17040
Here, C3D8 stands for 8 nodes linear brick and C3D6
stands for 6 node linear triangular prisms.
Geometric order of the element is chosen based on the
analysis type. Although Quadratic order gives better
result, it is mainly useful when rotation is considered
[12]
. For this project, Linear order gives the satisfactory
result without increasing simulation time like quadratic
order. As optimization is also another prime concern of
FE analysis, the choice of element order was crucial for
this project. Aluminum has good elasto-plastic behavior
and keeping our goal in mind, 3D stress family is
selected for this project.
For hex elements, regular formulation is considered.
Hybrid formulation is mainly used for incompressible or
almost incompressible material [12]
. In this project,
aluminum holds good compressible property. Reduced
formulation is omitted because it uses only one

6. 6
integration point instead of eight. This impacts the
accuracy of the numerical analysis in a great
amount.
Figure 07: Aluminum Honeycomb after meshing.
Figure 07 shows the honeycomb structure after
meshing. The meshed structure has a total number
of 3909087 elements. Close up element shapes are
shown in Figure 08. Figure 08(a) shows the close up
of the hex element and figure 08(b) shows the
wedge elements at the connecting edge of the
hexagonal honeycombs. A close inspection of Figure
08(b) shows that at the connecting edge, there are
three closely assembled nodes which form a shape
of triangle.
(a) (b)
Figure 08: (a) Hexahedral brick element; (b) Wedge
element at the connecting edge of hexagons.
The quality of the mesh is analyzed using ABAQUS
verification tool. The aspect ratio is our main concern
while verifying the quality of the mesh. It is general
convention that an aspect ratio around 1 indicates
better quality of the meshing. Table 05 shows the
aspect ratio for each element type.
Table 05: Verification of the quality of mesh
Element Type Total Number
of Element
Average
Aspect Ratio
Hexahedral 3829833 4.69
Wedge 79254 4.77
In meshing of the aluminum, the worst aspect ratio for
hex element is 9.45 and for wedge element, it is 9.24.
Inspecting all elements, there was no analysis error and
the percentage of analysis warning was 0.74%.
Considering all these facts, it can be concluded that the
combination of both hexahedral and wedge elements
maintains the integrity of the meshing.
2.5 Convergence Study
For any Finite Element Analysis (FEA), convergence
study is an important consideration because it is crucial
to optimize the computational cost by minimizing the
simulation run time and ensuring maximum accuracy at
the same time. By convergence study, it is possible to
choose the optimum element size for the mesh. There
are mainly two methods for convergence study – i) h-
method ii) p-method. In “h-method”, the element size is
increased/decreased i.e. one element breaks into two
small elements as such. In “p-method”, instead of
increasing/decreasing element, the integration point is
increased in each element by choosing the quadratic
element formulation. For this project, both “h-method”
has been performed to observe and understand how
convergence affects the overall study. As previously
mentioned that for this project quadratic elements are
not considered because this project does not include
rotation, “p-method” convergence has been ignored.
For “h-method” convergence test, different element
size has been considered and the maximum von mises
stress has been studied to observe the change in values.

7. 7
Table 06 presents the data of stress for different
element size and Figure 09 shows the convergence
graphically.
Table 06: Data for “h-method” convergence
Type of
Element
Element
Size
Total
Element
Number
Stress
(MPa)
Linear
0.7 191132 810.8
1 90250 819.4
1.2 74730 821.8
1.4 52416 831.5
2 29117 838.2
3 14246 825.8
Figure 09: “h-method” convergence
Observing the graph, it is visible to understand how
the mesh element size is converging with the
reduced size of the element. By reducing the size of
the element, the element number has been
increases which ensured more accuracy in the
project. However, after a certain iterations, reducing
the element size does not affect the change in
result; thus we conclude mesh has converged. In
Figure 09, we observe larger element size showed
large fluctuations in values but for smaller element,
it is opposite.
2.6 Error Analysis:
For error analysis, Richardson Extrapolation method is
used to find the exact solution for a certain node. In this
project data has been extracted for a certain node over
all the models of different mesh refinement. As the
stress concentration is highest at the lower plane of the
honeycomb, a node has been picked from the lower
plane and data for that particular node has been
extracted for all cases. From Richardson extrapolation,
we get equation 1. Using this equation for three points,
two equations can be formed. By solving these two
equations for three element size, exact solution for that
particular node can easily be extracted.
Here, “f” denotes the value of consideration and m, n
denotes total element size. “α” is a constant which
depends on the order. Table 07 shows represent data
for error analysis. The comparison between exact
solution and the FE analysis result has also been shown.
Figure 10 shows the relation between errors decreasing
with increase in element number.
Table 07: Error Comparison
Element
Size
Total
Element
Number
Exact
Solution
Stress
From
Simulation
Percentage
Error (%)
0.7 191132
586.1
586.7 0.09
1 90250 619.95 5.76
1.4 52416 645.14 10.05
3. Verification and validation:
In the project, models have been created based on the
experiment of Ashab et el [1, 8]
. During the compression
experiment they have used two plates on both side of
the honeycomb to apply the displacement uniformly.
Moreover, they have performed the test for bilinear
kinematic hardening material model. They have
805
810
815
820
825
830
835
840
0 50000 100000 150000 200000 250000
Stress
Number of Elements
Graph of Convergence Test

8. 8
calculated plateau stress and dissipated energy for
tearing. During experiment, a gap of 1 mm was kept
between honeycomb and the both plates to reduce
the effect of instant initial loading. The
displacement was performed at a speed of 5 ms-1
in
varying step up to 38 mm. However, this project
differs from the experimental procedure in many
ways. As the primary assumptions and the material
model vary in great extent, exact validation using
experimental data is quite difficult to achieve.
Figure 10: The change in error due to increase in
element number
However, to perform approximate validation, a
particular case for kinematic hardening is performed
for single loading of 5ms-1
. To reduce the
computational cost coarse mesh is used. For this
particular case the element size 2.5 is taken. These
assumptions evidently show great fluctuations from
expected value. From the experiment, plateau stress
was observed as 1.64 MPa and for this case,
maximum von mises stress observed as 0.66 MPa
which has a difference of 59.7%. The large error is
quite expected for this analysis due to all the
assumptions made on the process. Later, for
validation, volume, area of the top surface and mass
has been calculated manually. As the velocity load
has not been applied using any rigid wall system, it
was difficult to know exact contact force. Using
element number and total stress in Z axis, average
values are calculated and using mass, area and
volume, stress is calculated and compared. The
average stress was 0.601Mpa and stress from
theory was 0.695 which differs by 13.52%.
4. Result and Discussion:
The deformation due to the impact of velocity has been
observed. Table 08 shows the displacement of the
honeycomb. It can be observed that the maximum
impact occurs at the top surface of the honeycomb and
this impact affects the displacement in all direction. In
figure 11, it can be observed that the maximum
deformation occurs at the red marked zone and the
upper half of the honeycomb minimize the impact of
the load by deformation. The hexahedral structure of
the honeycomb works as a great shock absorber here.
Table 08: Displacement of Honeycomb
Displacement
X-axis
mm
Displacement
Y-axis
mm
Displacement
Z-axis
mm
Node No 2689 299 4699
Maximum 5.15 5.81 18.32
Minimum -5.15 -5.81 -5.00
Total 0.652 0.327 653
Figure 11: Deformed Honeycomb
Figure 12: Both deformed and undeformed honeycomb
0
2
4
6
8
10
12
0 50000 100000150000200000250000
PercentageError
Number of Element
Error Percentage Vs Element Number

9. 9
For a single node, the stress-strain relation has also
been observed. Figure 13 shows the plot of stress-
strain relation. As honeycomb has good shock
absorption capability, the linear relation between
plastic strain and plastic dissipated energy density
from figure 14 can be observed.
Figure 13: Stress-strain curve.
Figure 14: Plastic strain vs plastic energy density
Compression loading as velocity was changed
(0.5m/s and 1m/s) and deformation at each load
velocity is observed. Displacement magnitude
increases with the increase in velocity.
Figure 15: Relation of Velocity and displacement.
With the increase in velocity, the changes in Von mises
stress have also been studied. From figure 16, it can be
observed that increase in load velocity causes linear
increase in von mises stress.
Figure 16: Relation of velocity vs Von mises Stress
From this study, different compression loading and their
impact on deformation and stress is clearly
understandable. The linear relation among them agrees
with the theory.
5. Conclusion:
The main objective of this project was to understand
the use and impact of Finite Element Method in
engineering analysis. It was important to understand
the effect of element size, element formulation, gauss
integration point etc. on the FE analysis result to
understand and evaluate the outcome better. As FE
analysis gives us an approximation of different criterion,
to make a decision based on this result, it is of great
importance to understand the theory of Finite Element
Method to know how much this result is reliable.
In this project, effect of only compression load has been
observed on deformation of honeycomb. For different
loading condition, the behavior of honeycomb should
change and it can be observed further. By reproducing
this project for bilinear kinematic hardening material
model and introducing plates as indenter, it could be
validated accurately. Moreover, dynamic loading can be
applied to study the characteristics of honeycomb.
0.00E+00
2.00E+08
4.00E+08
6.00E+08
8.00E+08
1.00E+09
0 2000 4000 6000
Displacement
Velocity(mm/s)
Velocity vs Displacement Magnitude
7.66E+08
7.67E+08
7.68E+08
7.69E+08
7.70E+08
7.71E+08
0 2000 4000 6000
VonMisesStress
Velocity(mm/s)
Velocity vs Von Mises Stress

10. 10
References:
[1] Ashab, A.; Ruan, D.; Lu, G.; Xu, S.; Wen, C. Experimental
investigation of the mechanical behavior of aluminum
honeycombs under quasi-static and dynamic indentation.
Mater. Des. 2015, 74, 138–149.
[2] L.J. Gibson, M.F. Ashby, G.S. Schajer, C.I. Robertson, The
mechanics of twodimensional cellular materials, Proc. Royal
Soc. London. A. Math. Phys. Sci. 382 (1782) (1982) 25–42.
[3] Fan X., Verpoest I., Vandepitte D. (2005) Finite Element
Analysis on Out-of-Plane Compression Properties of
Thermoplastic Honeycomb. In: Thomsen O., Bozhevolnaya E.,
Lyckegaard A. (eds) Sandwich Structures 7: Advancing with
Sandwich Structures and Materials. Springer, Dordrecht
[4] Jeom Kee Paik, Anil K Thayamballi, Gyu Sung Kim, The
strength characteristics of aluminum honeycomb sandwich
panels, In Thin-Walled Structures, Volume 35, Issue 3, 1999,
Pages 205-231, ISSN 0263-8231.
[5] D Ruan, G Lu, B Wang, T.X Yu, In-plane dynamic crushing of
honeycombs—a finite element study, In International Journal of
Impact Engineering, Volume 28, Issue 2, 2003, Pages 161-182,
ISSN 0734-743X.
[6] M. Yamashita, M. Gotoh, Impact behavior of honeycomb
structures with various cell specifications—numerical simulation
and experiment, In International Journal of Impact Engineering,
Volume 32, Issues 1–4, 2005, Pages 618-630, ISSN 0734-743X.
[7] Hu, L.; You, F.; Yu, T. Effect of cell-wall angle on the in-plane
crushing behaviour of hexagonal honeycombs. Mater. Des.
2013, 46, 511–523
[8] Ashab, A.s.m., et al. “Finite Element Analysis of Aluminum
Honeycombs Subjected to Dynamic Indentation and
Compression Loads.” Materials, vol. 9, no. 3, Apr. 2016, p. 162.,
doi:10.3390/ma9030162.
[9] M. Zarei Mahmoudabadi, M. Sadighi, A theoretical and
experimental study on metal hexagonal honeycomb crushing
under quasi-static and low velocity impact loading, In Materials
Science and Engineering: A, Volume 528, Issue 15, 2011, Pages
4958-4966, ISSN 0921-5093.
[10] T. Wierzbicki, Crushing analysis of metal honeycombs.
International Journal of Impact Engineering 1, 1983, 157–174.
[11] Wang, Z.; Tian, H.; Lu, Z.; Zhou,W. High-speed axial impact
of aluminum honeycomb—Experiments and simulations.
Compos. Part B Eng. 2014, 56, 1–8.
[12] ABAQUS (2011) `ABAQUS Documentation', Dassault
Systèmes, Providence, RI, USA.
[13] Kalyanasundaram, Anand, et al. “Stress Strain Curves:
Aluminum.” ICME,HPC, Cooperative Computing Group at Center
for Advanced Vehicular Systems at Mississippi State University.,
29 Apr. 2015, 14:15, icme.hpc.msstate.edu/mediawiki/index.php/
SSC_Aluminum:_Al_2024-T351_alloy