Conference PaperPDF Available

Parametric Study of Honeycomb Composite Structure Using Open Source Finite Element Software

Conference Paper

Parametric Study of Honeycomb Composite Structure Using Open Source Finite Element Software

Abstract and Figures

This paper deals with the parametric optimisation of a simply supported sandwich panel made of honeycomb composite structure using sequential quadratic programming SQP. The panel consists of aluminum honeycomb sandwiched between two orthotropic fibre glass faces. The parameters studied are fibreglass thickness, tf, honeycomb height, h, and honeycomb wall thickness, tc. The objective was to minimise weight to bending stiffness ratio by using the nonlinear MATLAB function fmincon, considering the maximum central displacement and intercellular buckling as the constraints. Following this, a static structural analysis was conducted on the optimised structure using the open source finite element solver CalculiX and Salome Platform software for preprocessing. The maximum displacement of the honeycomb panel was found less than the displacement serviceability limit state. Preliminary results show that composite honeycomb structures can be optimised yielding low weight to bending stiffness ratio using SQP method and CalculiX for design evaluation. Keywords: Parametric optimisation; Sequential quadratic programming; CalculiX; Salome Platform; Honeycomb composites
Content may be subject to copyright.
2019 UKACM Conference City, University of London
1
PARAMETRIC STUDY OF HONEYCOMB COMPOSITE STRUCTURE
USING OPEN SOURCE FINITE ELEMENT SOFTWARE
*Ahmed H. Abdulaziz1,2, Mohammed Hedaya1, John P. McCrory2, Karen M. Holford2,
Adel Elsabbagh1
1Design and Production Engineering Department, Faculty of Engineering,
Ain Shams University, Abbaseya, Cairo, Egypt, 11517
2School of Engineering, Cardiff University, Wales, United Kingdom, CF24 3AA
* ahesham@eng.asu.edu.eg
Summary
This paper deals with the parametric optimisation of a simply supported sandwich panel made
of honeycomb composite structure using sequential quadratic programming SQP. The panel
consists of aluminum honeycomb sandwiched between two orthotropic fiberglass faces. The
parameters studied are fibreglass thickness, tf, honeycomb height, h, and honeycomb wall
thickness, tc. The objective was to minimise weight to bending stiffness ratio by using the
nonlinear MATLAB function fmincon, considering the maximum central displacement and
intercellular buckling as the constraints. Following this, a static structural analysis was
conducted on the optimised structure using the open source finite element solver CalculiX and
Salome Platform software for preprocessing. The utmost displacement of the honeycomb
panel was desirably less than the serviceability limit. Preliminary results show that composite
honeycomb structures can be optimised yielding low weight to bending stiffness ratio using
SQP method and CalculiX for design evaluation.
Keywords: Parametric optimisation; Sequential quadratic programming; CalculiX; Salome
Platform; Honeycomb composites
Introduction
In the wind turbines industry, blade materials must have a low weight to bending stiffness ratio
for optimal aerodynamics. Aluminum honeycomb can play a vital role in manufacturing longer
wind turbine blades with fibre glass as outer skin due to the cost benefit when compared with
using carbon fibre composites alone. This study proposes a parametric optimisation using
Sequential Quadratic Programming algorithm SQP, which can be used in MATLAB’s fmincon
function to minimise weight to bending stiffness. This function deals with nonlinear constrained
convex objective functions with linear/nonlinear equalities and inequalities. To evaluate the
optimum values, structural analysis using finite element method was carried out using the open
source finite element solver CalculiX. CalculiX has many interesting features such as wide
compatibility with open source CAD modelling and mesh generating softwares such as Salome
platform, FreeCad and GMSH. Further, it is extremely versatile as is it can be modified using
Python programming on Linux platform. For instance, recently Genao et al [1] have proposed
a framework to merge Calculix FE solver with NASA’s Micromechanics Analysis Code MAC to
promote multiscale analysis of the composite materials effectively. Galehdari et al [2] have
optimised honeycomb structural parameters using SQP and genetic algorithm for minimising
the weight to absorbed energy ratio to increase the crashworthiness. Park et al [3], have
conducted structural linear analysis on a cantilever model and sliding contact analysis using
CalculiX and Code_Aster comparing the results favourably with ANSYS commercial FE
software. Therefore, in this paper, Salome platform was used for meshing the honeycomb
composite structure and CalculiX FE solver was used for conducting structural analysis.
Methodology
The common failure modes of sandwich structures may happen due to severe shear force,
intercellular buckling, core crushing, delamination in case of orthotropic composite facets,
2019 UKACM Conference City, University of London
2
shear crimping and punching shear [4]. The sandwich panel dimensions width, b, and length,
l, are 0.2m× 0.2m respectively, and the honeycomb top/bottom faces are fibre glass with
thickness, tf, honeycomb height, h, and with wall thickness, tc. The sandwich panel is treated
as a shell structure considering the length/width are significantly larger than the height [5]. The
top/bottom faces consist of three laminates with a combined thickness of tf mm, and a
[0o/90o/0o] layup meaning that the in-plane/bending deformations are decoupled. The fibre
glass composite micromechanics properties are computed using the Halpin-Tsai empirical
approach. Moreover, the research methodology workflow is presented in Figure 1.
Figure 1: Block diagram of the research methodology
According to Bitzer [6] the equivalent bending stiffness of honeycomb sandwich panel  can
be computed using Eq. (1).
where; E1 is longitudinal Young’s modulus of faces and Ec is the honeycomb Young’s modulus,
is equal to (1-and are Poisson’s ratio in longitudinal and transverse directions of
composite layer, is (1-
is Poisson’s ratio of aluminum. The weight is      
  where, g is gravity acceleration, b is breadth, l is length and  is
honeycomb density and is top/bottom face material density. Fmincon function in MATLAB
ustilises sequential quadratic programming SQP algorithm to obtain the optimum minimum
value. Therefore, the objective function is to minimise weight to bending stiffness which is
formulated as in Eq. (2)


(2)
The nonlinear constraints of the design are displacement and intercellular buckling. The
displacement at the panel centre should not exceed span/100. The displacement of the panel
at the centre can be computed by Lèvy’s single series as shown in Eq. (3)
  
 
(3)
Since the panel is square of side , Eq. (3) can be re-written as given in Eq. (4) [7], and the
intercellular buckling load must be less than critical value as computed in Eq. (5).
  
 (span/100 = 2mm)
(4)
   

(5)
where k is 5.75, Es is the honeycomb Young’s modulus, The upper/lower limits of the design
variables are tabulated in Table 1. SQP function tolerance is 10-6.
Table 1: Optimisation design variables with upper/lower bounds
 
 


(1)
2019 UKACM Conference City, University of London
3
Design Variable
x (1)
x (2)
x (3)
Geometric Parameter
Upper bound
0.002
0.010
0.001
Lower bound
0.0015
0.001
0.0001
As a side note, the positive definite Hessian matrix is a measure of function convexity over the
domain [8]. Therefore, the eigenvalues of the Hessian have been computed and they are
positive. After computations, a local minimum that satisfies the nonlinear constrains has been
detected. Further, the variations of weight to bending stiffness ratio according to different
honeycomb height and faces thickness are plotted in Figure 2. The eigen values of the Hessian
matrix are computed. The iterations stopped as the objective function is non-decreasing in the
feasible region. The buckling load factor (BLF)has been computed (i.e.  /) and it
is larger than 1 which indicates safety of the honeycomb cell wall under buckling.
Figure 2: Weight to bending stiffness ratio for different height and face thickness
The optimum values are tabulated in Table 2. Furthermore, the MATLAB script used to obtain
this result is provided at the end of this paper.
Table 2: Honeycomb optimum values
tf (m)
H(m)
W (N)
Deq(N.m)
W/ Deq
(N/N.m)
Intercellular
Critical
Buckling (N)
Buckling
Load
Factor
0.0020
0.0100
3.31564
5.8898e+03
5.6295e-04
1599.4
1.6
Finite Element Model
To evaluate the optimisation results, a honeycomb composite panel of zero thickness is
processed in Salome Platform and meshed with “S6” and “S8R” shell elements [9] using
Netgen 1D-2D option with maximum length 3 mm and minimum length 1.5 mm. Further, for
better accuracy in solution, second order approximation for the meshing process is followed.
However, care must be taken in meshing process as unlike commercial softwares, node-to-
node connectivity is not assured for multiple surfaces automatically. Therefore, the sandwich
panel must be partitioned into multiple shells and edges to assure the nodal connectivity. Yet,
after partitioning it, the honeycomb core and top/bottom faces must be grouped as well the two
edges at the bottom face to form the elemental and nodal groups which will be used later for
2019 UKACM Conference City, University of London
4
materials definitions and boundary conditions in CalculiX. The mesh is saved as .unv file to
obtain a Python code of elements data. Afterwards, unical mesh converter in CalculiX is used
to convert the (.unv) mesh file into input deck for further finite element analysis. Figure 3a)
presents a block diagram of the FE process and 3b) shows the meshed honeycomb panel. It
consists of 18,309 quadrangle elements “S8R” and 2,863 triangular elements “S6”. These
elements expand to 3D quadratic brick elements and 3D wedge elements in modelling the
top/bottom composite faces .
Figure 3: a) Finite element steps, b) Honeycomb Meshing in Salome Platform
The lateral concentrated force 5,000 N is positioned at the centre of the panel and structural
static analysis is conducted. The maximum central deflection is 1.31 mm as shown in Figure
4a. Compared to serviceability limit (i.e. span/100) which has been utilised within the
optimisation, the utmost deflection obtained by CalculiX for the panel is desirably less. It is
noteworthy to mention that in CalculiX section definition, the shell elements after expanding to
build the required thickness may intersect at the corners as shown in Figure 4b. This
intersection is dependent on the shell offset value and its normal direction whether negative or
positive.
Figure 4: a) Maximum central displacement of the simply supported panel, b) the shell
elements corner intersection after expanding
Conclusions
In conclusion, the honeycomb composite panel has been optimised using sequential quadratic
programming. The ratio of weight to bending stiffness is minimised considering the intercellular
buckling and lateral deflection as the main constraints functions. The optimum geometric
parameters are the faces thickness, core height and core thickness. After the optimisation, a
a) b)
a) b)
2019 UKACM Conference City, University of London
5
numerical model is processed and meshed with S8R/S6 shell elements in Salome platform
then a structural static analysis has been carried out in the open source finite element solver
CalculiX. Overall, it is demonstrated that coding with CalculiX is flexible nevertheless care must
be taken in the section definition. Mainly, the shell element offset and normal direction because
the results are dependent on them. The maximum displacement retrieved from CalculiX was
1.31 mm which is less than the limiting value specified in SQP optimisation. Future research
should be devoted to couple the SQP optimisation code within Salome Python code of the
geometry/mesh to be processed after that in Calculix input deck. In addition, optimisation of
honeycomb composite structure might prove an important area for future optimisation research
so it is recommended that another optimisation technique such as Method of Moving
Asymptotes MMA or Genetic algorithms is used and all optimisation results are examined.
Acknowledgements
This research is carried out within the PhD project entitled “Investigation of Honeycomb
Composite Structure for Wind Turbine Blades with Acoustics Emissions Damage Assessment
funded by Newton-Mosharafa Fund in Egypt, I.D: (NMJ 3/18). Many thanks to Prof Otto Ernst
Bernhardi in Karlsruhe University of Applied Sciences, Germany, Hossem Elnachmie and
Haoluan Li in Cardiff University for recommendations and discussions about some technical
issues encountered in finite element modelling and optimisation.
References
1
F. A. Yapor Genao, E. J. Pineda, B. A. Bednarcyk and P. A. Gustafson, "Integration of
MAC/GMC into CalculiX, an open source finite element code," in AIAA SciTech Forum,
San Diego, California, 7-11 January 2019.
2
S. Galehdari, M. Kadkhodayan and S. Hadidi-Moud, "Analytical, experimental and
numerical study of a graded honeycomb structure under in-plane impact load with low
velocity," International Journal of Crashworthiness, vol. 20, no. 4, pp. 1754-2111, 2015.
3
S. K. Park, D.W. Seo, H. Jeong and M. Kim, "Performance evaluation of open-source
structural analysis solver, CalculiX and Code_Aster, for linear static and contact
problems," ICIC Express Letters , vol. 12 , no. 7, pp. 655-662, 2018.
4
G. Lubin, Handbook of Composites, Springer Science & Business Media , 2013.
5
T. Kubiak, Static and Dynamic Buckling of Thin-Walled Plate Structures, Lodz, Poland:
Springer, 2013.
6
T. N. Bitzer, Honeycomb Technology: Materials, Design, Manufacturing, Applications
and Testing, Springer Science & Business Media, 2012.
7
S. P. Timoshenko and S. Woinowsky-Krieger, Theory of Plates and Shells, Singapore:
Mcgraw-Hill Inc., 1959.
8
A. Messac, Optimization in Practice with MATLAB® for Engineering Students and
Professionals, Cambridge: Cambridge University Press, 2015.
9
E. J. Barbero, Finite Element Analysis of Composite Materials using Abaqus, Taylor and
Francisn Group, 2013.
MATLAB M-script
%This code is written to perform
parametric optimisation using SQP
algorithm-All dimensions are in SI-
units~~After reading left hand
column to its end, continue reading
ub= [0.002,0.010,0.001];
nonlcon = @Constrains;
x0 = [0.0018,0.002,0.0002] ;
%Initialisation point
2019 UKACM Conference City, University of London
6
from top of right column to its
end. ~~File 1 consists of 3
sections. File 2 presents
constraints functions
% File 1-Section 1: Halpin-Tsai
empirical approach for
micromechanics computations &
parameters definition
clc
rhof = 1800 ; % Faces density
rhos = 2700; % Aluminum density
% Material is Al honeycomb
L=0.2; % length
w=0.2; % breadth
g=9.81; % Gravity acceleration
E=60e9;
Ef = 73.1e9; %Fibre glass Young's
modulus
Em = 3.45e9;
vf=0.55; %volume fibre fraction
vm=0.45 ; % volume matrix fraction
uf = 0.22; % poisson ratio
fiberglass
um = 0.33; % poisson ratio Epoxy
Gf = 30e9; %Shear rigidity of fibre
Gm = 1.25e9 ; %Epoxy shear rigidity
v12 = uf*vf + um*vm ;
v21 = v12;
k = 0.9;%k:fibre misalignment
factor
E1 =k*(Ef*vf+Em*vm);%Longitudinal
Young's modulus
zeta = 2;
etae = ((Ef/Em)-1)/((Ef/Em)+zeta);
E2 = Em*(1+zeta*etae*vf)/(1-
etae*vf);%Longitudinal Young's
modulus
etaG= ((Gf/Gm)-1)/((Gf/Gm)+zeta);
G12 = Gm*(1+zeta*etaG*vf)/(1-
etaG*vf);
lambda = 1-v12*v21 ;
v_Al = 0.3 ; %Poisson ratio Al
lambdac = 1-v_Al;
s=0.0064;%Side length of cell
%File 1-Section 2:Optimisation
Formulation
f=@(x)2*g*w*L*(rhof*x(1)+(x(2)*x(3)
*rhos/(s*(3^0.5))))/(((E1*x(1)*(x(2
)+x(1))^2/(2*lambda))
+(E1*x(1)^3/(6*lambda))+(E*x(3)^3/(
12*lambdac))));
A =[];
b = [];
Aeq = [];
beq = [];
lb =[0.0015,0.001,0.0001];
options =
optimoptions('fmincon','Algorithm','
sqp','Display','iter') ;
[x,fval,exitflag,output,lambda,grad,
hessian]=fmincon(f,x0,A,b,Aeq,beq,lb
,ub,nonlcon,options);
disp (hessian);
e = eig(hessian);
[~,r] = chol(hessian);
disp (e)
disp (x)
M=2*g*w*L*(rhof*x(1)+(x(2)*x(3)*rhos
/(s*(3^0.5))));
K = M/fval ;% stiffness at optimum
point
% File 1-Section 3: 3D plot of the
variables and corresponding
objective function
tf1 = linspace(0.001,0.009,10) ;
h1 = linspace(0.005,0.05,10) ;
tc1 = linspace(0.0001,0.009,10);
[XX,YY] = meshgrid(tf1,h1);
[VV] = meshgrid(tc1);
WW =
2*g*w*L.*(rhof*XX+(YY.*VV*rhos./(s*(
3^0.5)))); %Weight at optimum point
; %Weight
DD =(E1*XX.*(YY+VV).^2/ 2*0.9274)
+(E1*XX.^3/(6*0.9274))+(E*VV.^3/(12*
0.7));
Func = WW./DD ;
[FF] = meshgrid(Func);
%plot objective function vs design
variables core height&face thickness
figure
set(gcf, 'PaperPosition', [0 0 4
4]);
C = contourf(XX,YY,Func);
clabel(C,'FontSize',12)
xlabel('Faces Thickness in
m','FontSize',12,'Color','k');
ylabel('Honeycomb Height in
m','FontSize',12,'Color','k' );
%File-2:Constraints.m File
function [c,ceq] = Constrains(x)
%Displacement at centre due to 5000
N concentrated force
c(1)=0.00406*5000*0.2^4/((3.758175e1
0*x(1)*(x(2)+x(1))^2/(2*0.9274))
+(3.758175e10*x(1)^3/(6*0.9274))+(6e
10*x(3)^3/(12*0.7)))-
0.002;%deflection
c(2) = 1000 -(5.75*60e9*x(3)^3/((1-
0.3^2)*0.0064)); %intercellular
buckling acting force on the side
ceq = [];
end
... The glass fibre top and bottom plates consisted of 5 laminates each [0 o /90 o ] 5s and total thickness is 2.5 mm per plate and the honeycomb core height was 10 mm. Further details on the specimen structure design and optimisation is provided in the study of Abdulaziz et al 6 . The glass fibre plate was manufactured by vacuum resin infusion technique. ...
Conference Paper
Full-text available
The objective of this article is to study in detail the acoustic emission wave propagation in a complex sandwich structure panel by utilising artificial Hsu-Nielsen acoustic emission sources. The sandwich panel consists of aluminium honeycomb core placed between two unidirectional glass fibre laminated plates. In order to study the effects of a bonded honeycomb core, artificial acoustic emission sources were generated on the top of a glass fibre laminated plate alone, at different angles relative to the fibre direction then repeated on the sandwich panel to find the change in (i) attenuations, (ii) wave velocities and (iii) frequencies of propagating acoustic emission waves. The attenuation of the waves increases after bonding the honeycomb in some directions. As an example, in direction 30o, the attenuation coefficient increases significantly from 5.252 dB/m to 10.27 dB/m whereas in 15o the change is small from 5.256 dB/m to 5.994 dB/m. On the other hand, the average velocity of acoustic emission in the plate has increased from 3527.02 m/s to 3836.85 m/s after bonding the honeycomb. However, in some other directions such as 0o direction, the average velocity has significantly reduced from 4028.41 m/s in the fibre glass laminated plate to 3637.36 m/s. Finally, wavelet transformation has been carried out on the waves in all directions and it is found that the active frequencies in the glass fibre laminated plate and the sandwich panel are in range from 30 kHz to 130 kHz. The results show that the presence of a bonder honeycomb core contributes significantly in changing to the acoustic emission propagation characteristics in the laminated glass fibre plates.
Article
Full-text available
Given the significance of energy absorption in various industries, light shock absorbers such as honeycomb structure under in-plane and out-of-plane loads have been in the core of attention. The purpose of this research is the analyses of graded honeycomb structure (GHS) behaviour under in-plane impact loading and its optimisation. Primarily, analytical equations for plateau stress and specific energy are represented, taking power hardening model (PHM) and elastic-perfectly plastic model (EPPM) into consideration. For the validation and comparison of acquired analytical equations, the energy absorption of a GHS made of five different aluminium grades is simulated in ABAQUS/CAE. In order to validate the numerical simulation method in ABAQUS, an experimental test has been conducted as the falling a weight with low velocity on a GHS. Numerical results retain an acceptable accordance with experimental ones with a 5.4% occurred error of reaction force. For a structure with a specific kinetic energy, the stress-strain diagram is achieved and compared with the analytical equations obtained. The maximum difference between the numerical and analytical plateau stresses for PHM is 10.58%. However, this value has been measured to be 38.78% for EPPM. In addition, the numerical value of absorbed energy is compared to that of analytical method for two material models. The maximum difference between the numerical and analytical absorbed energies for PHM model is 6.4%, while it retains the value of 48.08% for EPPM. Based on the conducted comparisons, the numerical and analytical results based on PHM are more congruent than EPPM results. Applying sequential quadratic programming method and genetic algorithm, the ratio of structure mass to the absorbed energy is minimised. According to the optimisation results, the structure capacity of absorbing energy increases by 18% compared to the primary model.
Conference Paper
An analysis framework is presented that makes multiscale analysis of composite structures available using the open-source FEA solver package CalculiX CrunchiX (CCX). At the center of this framework is the coupling of the Finite Element Analysis - Micromechanics Analysis Code (FEAMAC) library from NASA’s Micromechanics Analysis Code with Generalized Method of Cells (MAC/GMC) to allow micromechanics analysis. The results show that the proposed coupling can be used with appropriate care for multiscale FEA simulations of composite materials. The largest error reported in this validation was in a four-point bend test specimen with an error of less than 1% difference in the maximum deflection of the beam.
Article
This paper evaluates simulation results obtained using CalculiX and Code-Aster, which are open-source structural analysis solvers for modeling and simulation (M&S). Linear static analyses are conducted with a pipe model under a pressure load and a cantilever model under a remote force. Contact analyses are tested using a two-beam model with tie, sliding and general contact conditions. Outputs obtained using CalculiX and Code-Aster agree well with those of the commercial software, ANSYS. These results suggest that CalculiX and Code-Aster are reliable, and can be used to improve efficiency of product development in manufacturing and engineering.
Chapter
The method proposed and explained below allows one to determine critical loads, natural frequencies and coefficients of the equation describing the postbuckling equilibrium path for thin orthotropic plates or girders, columns and beams composed of flat orthotropic plates (walls). This method also allows one to analyse a dynamic response of the plate structure subjected to pulse loading. Taking the deflections as a function of time and applying the relevant dynamic buckling criteria, it is possible to determine the dynamic critical load.