Characterization of sandwich materials – Nomex-Aramid carbon fiber performances under mechanical loadings: Nonlinear FE and convergence studies

3.1 Mechanical testing aims

Laboratory testing was used to determine the maximum strength of the sandwich structure. From this test, how much damage occurs to the sandwich structure when given a flexural load and the stages of the damage process were identified. These data were then used to validate the calculation results with numerical simulations, as well as to determine the actual characteristics of the material used in FEM.

3.2 Specimen preparation

The specimen materials utilized in this investigation were made from commercially available materials. P.T. Justus Kimiaraya provided the epoxy resin with hardener, known as “Epocshon A and B.” The carbon fiber was provided by Easy Composite Co Ltd., while the core used Nomex® Aramid honeycomb. Table 2 shows the details of the specification and its attributes. Figure 2 shows the schematic dimension of the Nomex^® Aramid honeycomb.

Figure 2

Schematic dimension of the Nomex^® Aramid honeycomb for a 5 mm depth.

3.3 Specimen manufacture

The specimen was prepared throughout the production process using the hand lay-up technique. During the procedure, each ply was handled exclusively by hand and stacked layer by layer to the required thickness. This was accomplished by sequentially stacking layers of 0/90 directional carbon fiber, −45/45 directional carbon fiber, 0/90 directional carbon fiber, and honeycomb core for the first step of the manufacturing. During the interlayer preparation process, the resin and hardener mixture was poured (in a 2:1 solution ratio) and pushed using a roller to ensure the resin was disseminated evenly and equally. The curing process was then performed after all the composite materials had been sequentially placed. Vacuum was used during the curing process to reduce the specimen’s porosity. At room temperature, the curing process was completed in 10 h.

The preparation of the composite layer for the second stage continued after the progress was accomplished in the first stage. All these layers were layered above the honeycomb, with the addition of a carbon layer arrangement in the 0/90 direction, followed by the −45/+45 direction, and finally, the 0/90 direction. Similar to the previous step, this also included the addition of resin and hardener. Additionally, a vacuum operation was carried out once the preparation was completed to lower the porosity of the specimen. Figures 3–7 show the detailed plan of the composite layers. Specifically, Figure 7 shows that there were foam/air bubbles frozen on the right side of the specimen, proving that the vacuum process can lift the air trapped in the resin.

Figure 3

Schematic of the composite layer specimen manufacturing for the first step.

Figure 4

The vacuum operation during the curing process for the first stage.

Figure 5

Schematic of the composite layer specimen manufacturing for the second step.

Figure 6

The vacuum operation during the curing process for the second stage.

Figure 7

Specimen material after the curing process before the cut using a waterjet cutting machine. Foam/air bubbles frozen on the right side of the specimen are seen (red arrow), proving that the vacuum process can lift the air trapped in the resin.

To comply with the American Society for Testing and Materials (ASTM) D7264 test guidelines, the specimen was divided into six parts using a waterjet cutting machine once the curing procedure was completed. This technique cuts the specimens with the least amount of precision feasible while minimizing harm to the specimen. Figure 8 shows the specimen after the waterjet cutting process.

Figure 8

Sandwich structure specimen ready for testing.

3.4 Mechanical testing setup and results

The three-point bending test was carried out using the ASTM D7264 standard test method, which is a test standard for polymer composite matrices. The test procedure requires that the entire length of the specimen is 20% longer than the length of the supporting span. To comply with this standard, the length of the specimen used was 250 mm, with a support span of 200 mm. The tests were carried out using the RTF 2410 test machine made by A&D Japan. This machine had an accuracy of ±0.5% with a sampling rate of 1 ms to improve testing accuracy. Figure 9 shows the laboratory testing setups. A loading speed of 1 mm·min⁻¹ was used during the testing procedure. The specimen immediately ceases loading if it fails or breaks. Table 3 displays the test’s results.

Figure 9

Laboratory testing setup.

Based on the testing results in Table 3, the average maximum point load was 189.26 N with a maximum point stress for facing of 238.06 MPa. Then, the average breaking point was obtained at a 6.8 displacement. Stress was obtained using Eq. (5), which is obtained from the ASTM C393 procedure [26].

4.1 Flowchart and research procedures

The methodology in this study began by studying previous studies on a sandwich structure. Then, we proceeded with specimen manufacturing using the vacuum molding method. The next step was mechanical testing, which was carried out to obtain the maximum flexural strength from the sandwich structure through three-point bending. The strength obtained was mainly used to find material properties from the sandwich structure constituents. The method used for material calibration was mix and match. The author made a matrix derived from the material properties of both parts collected from various articles. Then, one by one, it was tried until the maximum flexural strength was found to be similar to the mechanical results. Next, the study continued with parametric studies using material properties that were obtained. Parametric studies included four tests (three-point bending, tensile test, compression test, and torsional test) and two core variations (geometry and material). The study proceeded with mesh convergence studies to determine how the mesh’s effect changes the specimen’s maximum strength. In addition, convergence studies were also conducted to determine the mesh configuration suitable for use in future studies. Figure 10 is the methodological scheme used in this study.

Figure 10

Methodology schematic of the present study.

4.2 Finite element method

FInite element method started with specimen modeling with a size that was obtained, both from the producer datasheet and direct measurement. Figure 11 shows a general-size drawing of the sandwich structure. The core had a 5 mm thickness, a core cell of 6.5 mm long, 5 mm wide, and a wall thickness of 0.11 mm. The facing consisted of three layers of carbon fiber cloth, with each layer having a 0.1 mm thickness. Carbon fiber modeling used composite ply in the lamina feature. The size of the overall specimen length and width will be presented in the testing procedure and boundary conditions because each test has different requirements.

Figure 11

Cell size and sandwich thickness.

This section also discusses mesh configuration, interaction, and material properties. Honeycomb modeling used the Fusion 360 framework while facing modeling used the ABAQUS Framework. A tie constraint was used to model the bonding of the facing and core parts. This constraint connected nodes from honeycomb as slaves and surfaces from facing as masters. The constraint tie was used to ensure the relationship between the facing and core was inseparable so that the strength of the material could be calculated in perfect conditions.

4.2.1 Mesh configuration

Mesh configuration is important because it defines the material behavior. Both core and facing parts used the S4R meshing type. The author used a shell in this study to speed up computation and facilitate the modeling of Hashin damage (HSNCRFT) on the facing, which was a carbon fiber. The facing part of the sandwich had a mesh size of 1 mm, and the core part was 2.25 mm. This difference in size is shown in Figure 12. This mesh configuration was chosen because of fast computing time. Computing time will significantly increase as the meshing becomes smaller. Also, for this size, a small margin of error comparing smaller mesh sizes was achieved. Results from smaller meshing were not significantly different from this meshing configuration.

Figure 12

Mesh difference between facing and core part of sandwich modeling.

4.2.2 Material configuration

4.2.2.1 Nomex honeycomb

Nomex-Aramid honeycomb was used as a core filling because it mainly had a small density, and its honeycomb shape naturally had good strength. Nomex-Aramid had material properties as shown in Table 4 (ρ – density, E – Young’s modulus, ν – Poisson’s ratio, G – shear modulus). The material properties were referred to as local material direction (1 = X, 2 = Y, 3 = Z). These material properties were obtained from the study of Roy et al. [11]. This study investigated the individual strengths of the Nomex-Aramid honeycomb. These material properties had been through benchmarking with three-point bending mechanical testing and achieved good margin results.

Table 4

Material properties of the Nomex-Aramid honeycomb [11]

ρ (g·cm−3)	E 1 (MPa)	E 2 (MPa)	E 3 (MPa)	ν1 (−)	ν2 (−)	ν3 (−)	G 1 (MPa)	G 2 (MPa)	G 3 (MPa)
0.64	5,200	4,400	4,400	0.24	0.24	0.24	1,400	1,400	1,400

4.2.2.2 Carbon fiber

Carbon fiber is a material with a high strength-to-weight ratio [27], which indicates carbon fiber has very high strength and is very lightweight. This makes carbon fiber very suitable for use as a facing of sandwich structures. Material properties are needed for parameters in numerical simulation. The Young’s modulus of the carbon fiber was obtained from the carbon fiber datasheet provided by the manufacturer (Torayca, United States). The shear modulus and Poisson’s ratio were obtained from Isbilir and Ghassemieh [28]. These material properties are shown in Table 5 (ρ – density, E – Young’s modulus, ν – Poisson’s ratio, G – shear modulus). The material properties were referred to as local material direction (1 = X, 2 = Y, 3 = Z). The arrangement of material properties has been through benchmarking and has achieved good margin results compared to real three-point bending mechanical testing. As stated before, in real specimens, carbon fiber consists of three plies arranged in (0/90/+45/−45/0/90) configuration for overall good mechanical properties [29].

Table 5

Material properties of the carbon fiber [27,28,29]

ρ (g·cm−3)	E 1 (MPa)	E 2 (MPa)	ν1 (−)	G 12 (MPa)	G 23 (MPa)	G 31 (MPa)
1.76	135,000	8,200	0.3	4,500	4,500	3,000

The Hashin damage criterion was used in this study. The detailed parameters of the Hashin damage criterion used in this study are presented in Table 6 (S _t = tensile strength, S _c = compressive strength, S _s = shear strength, G _ft = tensile fracture energy, G _fc = compressive fracture energy). These criteria had been through benchmarking and had achieved good margin results compared to real three-point bending mechanical testing.

Table 6

Hashin criterion and damage evolution parameters [30]

Parameter	Value
S t1 (MPa)	2,471
S t2 = S t3 (MPa)	62
S c1 (MPa)	2,597
S c2 = S c3 (MPa)	190
S s1 = S s2 = S s3 (MPa)	81
G ft1 (N·mm−1)	95
G fc1 (N·mm−1)	103
G ft2 (N·mm−1)	0.2
G fc2 (N·mm−1)	0.2

The damage stabilization of 0.001 was adopted in this study, which provided good results and faster numerical simulation. Also, the smaller the damage stabilization number, the time needed for numerical simulation time increased substantially [30].

4.2.2.3 Lamina configuration

Lamina configuration is a setting that defines fiber composite orientation. Carbon fiber composite consists of three plies. The first ply is 0/90, the second ply is 45/−45, and the third ply is 0/90. In ABAQUS framework, modelling all plies as one direction is needed. Therefore, from original three plies, it is needed to break down into six plies. Figure 13 shows the configuration of lamina for carbon fiber composite. The direction for lamina setting was 0/90/45/−45/0/90.

Figure 13

Lamina configuration.

4.2.2.4 Hanshin failure criterion

The Hashin damage criterion is based on the work of Hashin and Rotem [3,31]. Hashin proposed a single equation to predict the damage initiation of the composite. The present work used Hashin damage as one of its parameters and there were four possible failure modes with four corresponding indexes: F f t = fiber breakage in tension (Eq. (1)), F f c = fiber buckling in compression (Eq. (2)), F m c = matrix cracking in tension (Eq. (3)), and F m c = matrix crushing in compression (Eq. (4)). Damage initiation occurs when any of the indexes exceeds 1.0 [30]. The following equation shows the previously stated possible failure:

(1) F f t = σ 11 s t 1 2 + α σ 12 s s 12 2 ≤ 1.0 and σ 11 ≥ 0 ,

(2) F f c = σ 11 S c 1 2 ≤ 1.0 and σ 11 < 0 ,

(3) F m t = σ 22 s t 2 2 + σ 12 s s 12 2 ≤ 1.0 and σ 22 ≥ 0 ,

(4) F m c = σ 22 2 S s 23 2 + S c 2 2 S c 23 2 − 1 σ 22 s c 2 + σ 12 s s 12 2 ≤ 1.0 and σ 22 < 0 ,

where σ 11 , σ 22 , and σ 12 are applied stresses, and α (0 ≤ α ≤ 1.0) is the coefficient of shear stress ( σ 12 ) contribution to fiber breakage in tension creation. In the ABAQUS framework [32,33], the Hashin damage initiation criterion can be conjugated with damage evolution, which is based on four fracture energies (longitudinal/transverse tensile fracture energy and longitudinal/transverse compressive fracture energy) [3]. The detailed parameters of this damage evolution are listed in Table 6.

4.3 Boundary conditions

The boundary conditions of each numerical simulated mechanical test are based on standard procedures used in real-condition mechanical testing. These testing procedures play a vital role in determining the specimen size, which then affects how boundary conditions are created in numerical simulation. In addition, this procedure is also a reference in calculations used in determining the stress of the test specimen. These are expected to increase the accuracy of numerical simulation results. There are four numerical simulated mechanical tests in the present study: three-point bending, tensile test, compression test, and torsional test.

4.3.1 Three-point bending

Three-point bending boundary conditions are made based on ASTM D7264. The schematic of boundary conditions is shown in Figure 14. The load was placed on arrows marked with the letter P, while the support span was placed on P/2. The length of the support span was 200 mm, the overall length of the modeling was 254 mm, and the overall length of the model must be 20% longer than the support span [25]. The details of model dimensions are shown in Figure 15. Based on the test procedure, the boundary conditions of three-point bending simulation were designed and shown in Figure 16.

Figure 14

Three-point bending testing setup illustration (in mm) [25].

Figure 15

Model dimensions for three-point bending numerical simulation (in mm) [26].

Figure 16

Boundary conditions for three-point bending.

Eq. (5) was used to calculate the facing bending stress of the specimen model and was obtained from ASTM C393. This equation was chosen to calculate only the facing bending stress [26]. The overall sandwich stress cannot be calculated because the sandwich structure thickness in the present study was not the same along the length.

(5) σ = PL 2 t ( d + c ) b ,

where σ is the facing bending stress (MPa); b is the width of the beam (mm); P is the applied force (N); d is the sandwich thickness (mm); L is the support span (mm); t is the thickness of the facing (mm); and c is the core thickness (mm).

The pin shown in letter A is a fixed support span that held the model when the bending test was carried out. On point A, an encase setting was applied where U ₁ = U ₂ = U ₃ = UR ₁ = UR ₂ = UR ₃ = 0 to simulate the static pin on the model. Meanwhile, point B was given a displacement control setting in the U ₂ direction as long as −15 mm to simulate the bending loading on the model. For the interaction between the jig and the specimen, interaction properties were used with a friction coefficient of 0.2.

4.3.2 Tensile test

Boundary conditions for tensile testing were made in accordance with the ASTM D3039 procedure. The specimen size, clamp size, and testing setup were obtained from this procedure. The overall model length is 254 mm, and the clamp length is 50 mm [34]. The designed boundary conditions for the tensile simulation is presented in Figure 17. Meanwhile, the stress calculation (Eq. (6)) was used only to calculate the facing stress of the sandwich structure, as mentioned previously. Eq. (6) was used to calculate the stress load on the facing part of the sandwich structure. This equation was obtained from ASTM C 364 and deemed suitable for sandwich structure application.

(6) σ = P max [ w ( 2 t fs ) ] ,

where σ is the stress (MPa); P _max is the max point load (N); w is the specimen width (mm); and t _fs is the single-facing thickness (mm).

Load modeling is detailed in Figure 17. Clamp modeling used the coupling feature on carbon fiber facing. Letter A, shown in Figure 17, was given displacement control with U ₂ as long as 10 mm to simulate tensile loading on the model, and Letter B was given boundary with U ₁ = U ₂ = U ₃ = UR ₁ = UR ₂ = UR ₃ = 0 to simulate the static clamp on the model. F is the direction of the loading.

Figure 17

Boundary conditions for the tensile test.

4.3.3 Compression test

Boundary conditions for compression testing were made in accordance with ASTM D6041 [35]. The compression test aims to test the overall edgewise strength of the sandwich material under compression loading. The detailed boundary condition setup is shown in Figure 18. The overall model length was 155 mm and was clamped on both sides, where F is the loading direction. The detailed model dimensions are shown in Figure 19. The dimensions of the sandwich material modeling were 155 mm long, 25 mm wide, and 5.6 mm thick. As stated before, the procedure from real mechanical testing was used to mimic real testing scenarios to increase numerical simulation accuracy.

Figure 18

Boundary conditions for the compression test.

Figure 19

Model dimensions (in mm) for the compression test [35].

The detailed boundary conditions for the compression test are shown in Figure 19. The clamp was modeled with coupling features on carbon fiber facing 65 mm from each end of the model. Point A was given displacement control as long as −10 mm in the U ₂ direction to simulate compression loading on the model. Point B was given a boundary setting with U ₁ = U ₂ = U ₃ = UR ₁ = UR ₂ = UR ₃ = 0 to simulate the static clamp on the model. F is the loading direction.

4.3.4 Torsional test

Torsional test boundary conditions are made in accordance with the study of Li et al. [14]. In this study, mechanical testing and numerical simulation were carried out. The dimensions of the model were 270 mm long, 70 mm wide, and 5.6 mm thick (Figure 20). Clamp modeling used coupling features that took place on the carbon fiber facing 20 mm from each end of the model. Point A in Figure 21 was given a displacement control in the UR ₂ direction as large as 4 rad, which was to simulate torque loading on the model. Point B was given a boundary setting (U ₁ = U ₂ = U ₃ = UR ₁ = UR ₂ = UR ₃=0) to simulate the static clamp that held the specimen.

Figure 20

Specimen dimensions for torsional testing (in mm) [14].

Figure 21

Boundary conditions for torsional testing.

5.1 Three-point bending

Three-point bending was done to estimate the flexural strength and fracture characteristics from flexural loading. Numerical simulation shows that failure in sandwich construction began from the skin that had direct contact with the indenter (upper skin). The core and lower skin remained intact when the whole model reached its maximum strength.

Generally, when a model is given a bending load, the failure starts from the lower part of the model (lower skin). However, in the case of carbon fiber Nomex-Aramid honeycomb sandwich construction, the damage that occurred during the bending load started from the upper skin (Figure 22). This phenomenon was due to the huge difference in the strength and density between the skin and core. Because of this difference, the loading from the indenter cannot be distributed throughout the model, and the stresses will accumulate on the upper skin, thus failing in the first place. After the upper skin fails, the core will bear the load and experience damage, and at a certain point, after the load has accumulated, the lower skin will eventually fail.

Figure 22

Simulation results of the three-point bending.

Figure 23 shows the numerical simulation results and detailed Hashin damage criterion contour. It can be seen that the specimen had several strength peaks. This phenomenon occurred because the failure of the composite ply did not occur at the same time, but its failure occurred separately in accordance with the load in every ply. When displacement reached 6.3 mm (Figure 23, point A), the global loading occurred where the whole model bore the load. The composite structure has shown the germ of failure at this period, although the total breakdown was not imminent. This instance can be seen in Figure 22: 0° ply with F f c type (fiber buckling in compression). Next, with a displacement of 7.5 mm (Figure 23, point B). The model reached ultimate stress with 258 MPa. Also, at this point, the failure of 45° ply occurred with F m c (matrix crushing in compression) type. The transition between global loading to local loading had occurred. From this point, the distribution of stress was becoming smaller in size. This phenomenon was the nature of heterogenic material. Finally, at a displacement of 12.7 mm (Figure 23, point C), the failure occurred at 0° ply with F f t (fiber breakage in tension) type. The matrix on the composite is a substance that bonded fiber together as a filler between those fibers. Thus, under certain loading, those matrixes always fail first. After the failure of the matrix, the fiber will endure the loading until its break. Therefore, the matrix on B always failed first before the fiber on C. Failure on C is marked by the decrease in the model strength. Also, at this point, the local loading that the model experienced was becoming worse. This instance was proved by facing and core contours that showed more red color in smaller areas.

Figure 23

Hashin damage criterion and damage evolution of the specimen in three-point bending’s numerical simulation.

The stress shown in Figure 23 is the stress that occurs on the facing part of the sandwich structure (facing stress). The facing stress was used to represent the whole model strength and calculated using Eq. (5). Facing stress was directly affected by the failure both on the core and facing (Hashin damage). Figure 24 shows the correlation between the facing stress and Hashin damage criterion. In the case of bending loading, the Hashin criterion had a direct correlation with facing stress. Proven failure on facing (fiber compression and matrix compression failure) had caused the model to fail, which was marked by steep decreases in facing stress. Figure 24 shows the effect of facing failure on the overall sandwich strength under loading bending.

Figure 24

Correlation between Hashin damage and model facing stresses under bending loading (A: facing failure, and B: core crushing under bending loading).

Mesh convergence studies showed a relationship between the number of elements and the maximum point load of the specimen. A mesh convergence study was carried out by changing the mesh sizing on the facing part (carbon fiber) of the specimen. The results showed an exponential graph. A drastic decrease occurred in the range of 680 (mesh size, 3 mm) to 2,873 elements (mesh size, 1.5 mm). After increasing the number of elements to 6,350 (mesh size, 1 mm) onward, the chart began to show a downward trend. From Figure 25, it can be concluded that the mesh convergence of three-point bending occurred on a 1 mm mesh with a number of elements of 6,350 elements and had a maximum point load of 205 N.

Figure 25

Mesh convergence of the three-point bending’s numerical simulation result.

5.2 Tensile loading

Tensile test numerical simulation was done to estimate the sandwich structure's tensile strength and also to study the sandwich structure behavior under tensile loading. Under tensile loading, facing (carbon fiber composite) will be experiencing a total failure. When this occurs, all of the tensile force will be borne by the sandwich structure core (Nomex-Aramid). Numerical simulation results from the sandwich structure carbon fiber Nomex-Aramid honeycomb under tensile load are shown in Figure 26 ( F f t = fiber breakage in tension, F m t = matrix cracking in tension and S = stress). This Hashin damage criterion was obtained by using parameters in ABAQUS in accordance to Eqs. (1)–(4), and the parameters are listed in Table 6. At a displacement of 2.1 mm (Figure 26, point A), the failure in carbon fiber plies with 90° and 45° occurred, with matrix failure under tensile loading type failure. At this point, the carbon fiber facing was still intact. At a displacement of 2.9 mm (Figure 26, point B), the model had reached an ultimate strength of 970 MPa. At this point, the failure of the remaining carbon fiber plies occurred. The failure occurred in 0° and −45° fiber orientation with fiber failure under tensile load type. In this instance, the facing (carbon fiber) had completely failed, and all remaining loading was borne by the core (Nomex Aramid). At a displacement of 4.2 mm (Figure 26, Point C), the load transition from facing to the core occurred. This instance was marked by a steep drop in the tensile strength of the model, but the model did not completely fail (reaching 0 strength). This phenomenon showed that the sandwich structure of the carbon fiber Nomex-Aramid honeycomb was resilient.

Figure 26

Hashin damage criterion and damage evolution of the specimen in the tensile test’s simulation.

The stress shown in Figure 26 is the stress that occurs on the facing part of the sandwich structure (facing stress). The facing stress was used to represent the whole model strength and calculated using Eq. (6). Facing stresses were directly affected by failure both on the core and facing (Hashin damage criterion). Figure 27 shows the correlation between the facing stress and Hashin damage criterion. In the case of tensile loading, the Hashin criterion had a direct correlation with facing stress. There were two face sheet failures that met its criterion: the matrix failure under tensile loading and fiber breakage under tensile loading. Matrix failure did not affect the overall strength of the sandwich structure, but fiber failure did. The failure on facing (fiber tensile and matrix tensile failure) had caused the model to fail, which was marked by steep decreases in the facing stress.

Figure 27

Correlation between the Hashin damage and model facing stresses under tensile loading (A: matrix failure under tensile loading, B: fiber breakage under tensile loading, and c: core bears all tensile loading).

The matrix on the composite is the substance that bonds the fiber together as a filler between those fibers. Thus, under certain loading, those matrixes always fail first. After the failure of the matrix, fibers will endure the loading until its break. Therefore, the matrix failed first before the fiber did. Figure 27 shows the effect of facing failure on the overall sandwich strength under loading bending.

The mesh convergence study was conducted on the tensile test by changing the mesh size of the facing part in specimen modeling. The results of the mesh convergence study are shown in Figure 28. The tensile tests mesh convergence occurred in exponential graphs where the maximum stress on the number of elements 824 (mesh size 4 mm) to 3,450 (mesh size 1 mm) still increased significantly. Then, the chart began to show a constant trend on the number of elements 4,554 (mesh size 0.75) onward. It can be concluded that in the tensile test, the numerical simulation mesh convergence occurred on the mesh size of 0.75 with 4,554 elements. The maximum point load occurred when the mesh convergence was 14,450 N.

Figure 28

Mesh convergence study of the tensile test’s simulation.

5.3 Compression loading

A compression test was performed to estimate the maximum compression strength of the sandwich structure. In addition, the characteristics of the sandwich against compressive load can also be known. The results of the stress vs displacement graph and damage evolution for facing and core parts are shown in Figure 29. It was known from compression numerical simulation results that the maximum compressive strength of the model was 266 MPa, which occurred at 0.125 mm displacement. At this point (Figure 29, point A), failure at the core occurred, causing the model to buckle. At this point, there was no sign of Hashin damage initiation meeting its criterion. Model failure had occurred sideways because there was a limitation from the carbon fiber facing to move in the longitudinal direction. This limitation was due to the difference in mechanical properties between the carbon fiber facing and Nomex-Aramid core (carbon fiber is way stiffer than Nomex-Aramid). Therefore, in order to receive compressive load, the model started to buckle in the lateral direction (sideways). This movement was more obvious in the displacement range of 0.6–2.85 mm (Figure 29, points B and C).

Figure 29

Results of the compression test’s simulation.

The Hashin damage criterion under a compression load is shown in Figure 30 ( F f t = fiber breakage in tension, F f c = fiber buckling in compression, F m t = matrix cracking in tension, and F m c = matrix crushing in compression). This Hashin damage criterion was obtained by using parameters in ABAQUS in accordance to Eqs. (1)–(4), and the parameters are listed in Table 6. Despite having a compressive load, there was a certain area of the composite that experienced tensile failure. This phenomenon was due to buckling failure that was experienced by the whole model. In F m c 90° orientation, buckling epicenter (Figure 32) was experiencing matrix compression failure, and the rest of ply was experiencing matrix cracking in tension failure ( F m t ). This was due to the compressive load concentrating at a single point (buckling epicenter). On the contrary to 90° fiber orientation, the 0° fiber orientation was experiencing fiber breakage in tension ( F f t ) failure in buckling epicenter and the rest of the ply was experiencing fiber compressive buckling failure ( F f c ) (Figure 30). This phenomenon underlined the difference between the fiber orientations under compressive loading. There were several plies of the composite that did not experience failure; for these reasons, the compressive strength of the model remained high after reaching the ultimate strength.

Figure 30

Hashin damage contour under compression.

The stress shown in Figure 29 was the stress that occurred on the facing part of the sandwich structure (facing stress). The facing stress was used to represent the whole model strength and calculated using Eq. (6). Facing stress was directly affected by failure both on the core and facing (Hashin damage criterion). Figure 31 shows the correlation between the facing stress and Hashin damage criterion. In the case of compression loading, the Hashin criterion did not correlate with the failure of the model. The failure of the model was due to core buckling. This buckling is clearly shown in Figure 32 (compression). Because of this buckling, the local stress arose and caused facing to bear excessive loading on those buckling epicenters, thus failing. Facing failure still affected the overall strength of the model. As shown in Figure 31 (point B), the failure on facing with matrix under tensile loading type caused a drop in facing stress. Figure 31 shows the effect of the core and facing failure on the overall sandwich strength under compressive loading.

Figure 31

Correlation between the Hashin damage and model facing stresses under tensile loading (A: core buckling had occurred, and B: MTCRT affecting drop on facing stress).

Figure 32

The deployed model is under compressive loading.

The mesh convergence on compression test modeling was done by changing the mesh size on the facing part (carbon fiber lamina) of the sandwich structure. The meshing size in the study was 5–0.25 mm. The Y-axis contains the maximum load (N). The results of the convergence study (Figure 33) showed a drastic reduction in the maximum compression load in the number of mesh elements from 507 (mesh size 2 mm) to 2,640 (mesh size, 0.625 mm). The chart shows a constant trend in the number of elements from 3,800 (mesh size, 0.5 mm) onward. From this finding, it can be concluded that the mesh convergence for compression numerical simulation occurred for a mesh size of 0.5 mm with 3,998 elements. The maximum compression load was observed when mesh convergence was 2623.97 N.

Figure 33

Mesh convergence study of the compression test’s simulation.

5.4 Torsional loading

Torsional tests were performed to estimate the maximum twisting strength of the sandwich structure. The characteristics of the sandwich structure, when subjected to twisting loads, can also be found through this experiment. The torsional numerical simulation results showed that the model could withstand torsional load as large as 88.9 N m at 1.34 rad, which indicates that the sandwich material had good torsional properties. In torsional loading, the model experienced two phases: the global load and the local load. In the global load phase, the facing part of the sandwich is still intact. This facing part distributed load on the entire model (Figure 34, points A and B). After the model reached the maximum strength (circa 1.34 rad), failure on the carbon fiber facing occurs (Figure 34, point C). This occurrence was observed with a steep decrease in the torsional strength. This strength decreased due to facing failure after the facing could no longer distribute the load on the entire model when the local load had arisen. This local load destroyed the core part because of its centralized (localized) force (Figure 34).

Figure 34

Results of the torsional test’s simulation.

Hashin damage failure in the carbon fiber composite under a torsional load is shown in Figure 35 (Hashin damage failure at the end of numerical simulation). Basically, composite failure occurred in all plies of the composite, but the location and type of failure were different. In one ply, two types of failure can occur that are different in places. In general, failure in a composite occurred in the middle section because of excessive compressive load (Figure 30, F m c 0, 45) and the side section of the composite experienced a tensile load (Figure 30, F m t 90, −45). When the model reached 1.34 rad (Figure 35), it was estimated that the material had totally failed. Only the 90° ply held the torsional load. Because of this instance and core failure, the torsional load is concentrated in this fault.

Figure 35

Hashin failure criterion of the carbon fiber composite under torsional loading.

The stress shown in Figure 36 shows that the torque occurred on the whole model of the sandwich structure. The torque was used to represent the whole model strength extracted directly from the simulation. The torque was directly affected by failure both on the core and facing (Hashin damage criterion). Figure 36 shows the correlation between the torque and Hashin damage criterion. In the case of torsional loading, the Hashin criterion did not correlate with the failure of the model. The failure on facing came first before the model did. The failure of the model was mainly because the core was crushed by two face sheets under a torsional load. Figure 36 shows the effect of core and facing failure on the overall sandwich strength under torsional loading.

Figure 36

Correlation between Hashin damage and the facing stress under tensile loading (A: facing failure).

Mesh convergence on torsional numerical simulation was done by changing the mesh size on the facing part of the sandwich structure (carbon fiber), and the core part remained constant (2.25 mm in size). The variant of mesh sizing ranged from 6 to 0.5 mm. The y-axis of mesh convergence used the reaction moment at a 0.004 increment time. This method was used because reaching the failing point for all of the numerical simulations could take days for just one numerical simulation. This method was deemed accurate because the difference in strength at the failing point can be seen even on the first increment. The results of the convergence study (Figure 37) showed a drastic reduction in the torsional load in the number of mesh elements from 552 (mesh size, 6 mm) to 4,725 (mesh size, 2 mm). The chart shows a constant trend in the number of elements from 18,900 (mesh size, 1.0 mm) onward. From this finding, it can be concluded that mesh convergence for torsional numerical simulation occurred at a mesh size of 1.0 mm with 18,900 elements. The number of elements for the torsional load at 0.004 rad was 127.71.

Figure 37

Mesh convergence study of the torsional test’s simulation.

5.5 Geometrical change study

The study was conducted by changing the geometrical shape of the sandwich core into an octagonal, which was previously a hexagonal honeycomb. Two numerical simulations were carried out to study the differences between the two, namely the flexural strength from three-point bending. The mesh configuration (1 mm facing and 2.25 mm core) and material properties had the same configuration between the geometries. This study was conducted to underline the geometric effect on the overall strength of the sandwich material. The difference in the material core is shown in Figure 38.

Figure 38

The size difference for core shapes.

A three-point bending comparison was carried out to determine the effect of differences in the core geometry on the flexural strength of the sandwich material as a whole. Figure 39 compares the results of three-point bending tests from both geometries. The octagonal specimen had a higher maximum flexural strength (349 MPa) when compared to the hexagonal variant (254 MPa). This phenomenon was caused by the difference in the core cell size in octagonal and hexagonal variants. This difference increased the strength of the facing and could minimize the local stress that occurred in the sandwich structure. With minimal local stress, the fundamental weakness of the heterogeneous materials can be overcome by decreasing the core cell size of the sandwich core. This phenomenon was caused by the difference in the size of the core cell. The core with an octagonal shape had a smaller cell size compared with that with a hexagonal shape. Thus, the octagonal shape had a larger area for transferring the load from the upper skin to lower skin. This difference can be clearly seen in Table 7.

Figure 39

Comparison between the hexagonal and octagonal cores in the three-point bending test’s simulation.

5.6 Material variation study

Material variation studies were conducted to determine the effect of material changes on the strength of the sandwich structure. In this study, conducted by changing the material properties of the core sandwich, three variants were compared, namely Nomex-Aramid, which was the main material, aluminum, and stainless steel. The mesh size was the same in each material, namely 1 mm for the facing size and 2.25 mm for the core size. This was done to emphasize experiments on the effect of the core material on the overall strength of the sandwich structure. Three-point bending was used to test the differences between the three materials. The test results (Figure 40) found that the sandwich structure with a stainless steel core had the largest ultimate facing flexural stress of 411.4 MPa, followed by aluminum with a strength of 321.2 MPa, and finally, Nomex-Aramid with a strength of 258 MPa.

Figure 40

Comparison of the numerical results: material changes in the three-point bending test.

The replacement of the core material significantly impacted changes in the facing flexural stress of the sandwich structure. This is evidenced in Figure 40. The higher the strength of the core, the higher the strength of the facing flexural strength, which also improved the overall strength of the sandwich structure. The order of stiffness of the material was Nomex-Aramid (the weakest), aluminum, and stainless steel (the strongest). The test results were also similar for stiffness order. The Young’s modulus of the core sandwich also affected the stiffness of the overall sandwich structure. The stiffer the core, the stiffer the sandwich structure. The three materials had a similar graphic shape with one main peak and several follow-up peaks, which is the nature of the sandwich structure. The assessment and characterization introduced in this work can be recommended to be used for other composite materials, for example, bio-material-based composites from sea sand [36,37], Cantala [38,39], Salacca Zalacca [40,41], egg shells [42,43,44], and hybrid and core materials [45,46,47].