#### Abstract

Explosion load studies are an essential part of shield engineering design. This is especially true for explosion-proof plates, which are used in order to reduce the impact of explosions, which have the potential to cause substantial damage to structural elements. The purpose of this study is to detail the explosion phenomenon and the response of sandwich panel structures under explosive loading. The finite element method (FEM) is used to model the dynamic structural response to explosions. Explicit finite element modeling and analysis are performed using ABAQUS CAE software. An air explosion simulation code is used to determine the blast load on the lower skin plate of a test panel on a typical armored personnel vehicle. Structural analysis is carried out with respect to displacement, von-Mises stress, and internal kinetic energy. Three variations of explosive loads are considered in the simulation in order to better compare the responses of the structures. Three different design variants and materials are considered, including honeycomb, stiffener, and corrugated geometric models and mild steel, medium carbon steel, and alloy steel materials. The results provided by this study pave the way toward the development of guidelines for the design of lightweight structural reinforcement elements.

#### 1. Introduction

A blast load is a load applied to a structure or object from a blast wave, which is described by a combination of overpressure and impulse or duration. In cases of uncontrolled unloading, such as IEDs, explosive loading is generated from explosives with a payload weight (kg) and type determined directly by the explosive device. During the detonation of high explosives [1], a blast wave is generated, impacting the structure through the application of incident overpressure (Pso) [2] which, in turn, is reflected back from the structure in the form of reflected excess pressure (PCa) [3, 4].

Research on the response of the geometric structure of a plate to impact and various active loads [5–13], including air blast loading, has been carried out over the past few decades. Explosive loading due to landmines and improvised explosive devices (IEDs) poses a significant threat to military vehicles and civilian infrastructure. According to the Landmine Monitor report, the number of victims from the use of landmines and improvised explosive devices (IEDs) in 2020 increased by 20%, compared to the previous 12 months as a result of the “increased armed conflict and contamination” of land with improvised mines. More than 7000 people were killed or injured in 54 countries and territories [14]. This highlights the need for better mine-resistant vehicles, especially for peacekeepers. Efforts have been made to improve the response of civil structures and transport vehicles to blast loads in order to address the risks involved. It is essential to understand the loads caused by the explosion and the damage to the structure. With proper engineering and the selection of materials with higher strength and hardness (which is useful in ballistic applications), the ability of the designed structure to respond to explosions will increase [15, 16]. Thus, the investigation of the use of layered structures as a means to withstand blast loads resulting from explosions has become more significant.

Several types of studies on air blasts using both software and experimental simulations have been carried out, as there are limitations to each method. Experimental, numerical, and analytical methods have been utilized to study the impact of air blasts. In order to understand the safety of structures under blast waves, it is essential to describe and define some basic and relevant concepts. The concept of an explosion describes a rapid phenomenon of physical, chemical, or nuclear conservation, in which the transformation of potential energy into mechanical and thermal work cannot be separated. This work is carried out by expanded gas, which is compressed during the phenomenon [17]. Sandwich structures can dissipate considerable amounts of energy and can generate large plastic deformation under impact/explosion loads; therefore, they have been widely used in various fields, including aerospace, marine, and railway engineering. Xue and Hutchinson compared the performance of metal sandwich panels under pulsed blast loads with solid panels made of the same material and weight. The results demonstrated that the sandwich panels outperformed the solid panels, especially concerning water spray [18]. Dharmasena et al. conducted explosion tests to study the dynamic response of square honeycomb core sandwich and solid panels. The results indicated that the honeycomb sandwich panels produced less deflection than solid panels of the same mass [19]. Zhu and Khanna conducted air-jet experiments to study the dynamic response of honeycomb sandwich panels. The results showed that the thickness of the panel and the core density significantly affect the deformation/failure mode [20].

Several studies have shown that the structural configuration of sandwich panels still needs to be optimized, in terms of their function in resisting air blasts. Markose and Rao have proposed an APV hull plate optimization method using a single panel and mild steel materials to resist the effects of air blast loads [21]. Plate geometries limited to single flat plates, commonly used materials, and explosion loads limited to small loads are critical for technological advancement, especially that of armored vehicles. Our focus and key contribution in this study are that we use the more complex geometric variations (honeycomb, stiffeners, and corrugations), materials with better properties (mild steel, medium carbon steel, and alloy steel), and higher blast loads (21 kg, 28 kg, and 35 kg) for comparison. We use the CONWEP system in the ABAQUS CAE software to investigate the dynamic response of sandwich panels under blast load. The interaction between the blast wave and the plate, as well as the displacement mode, stress mode, and internal energy, is considered in the experiment. Numerical simulations are also carried out, in order to study the sandwich panel response process.

#### 2. Literature Review

##### 2.1. Air Blast Loading

A blast wave consists of a high-intensity pressure front, propagating outward from the center of the explosive into the surrounding air. As the shock wave expands, its amplitude decreases, its duration increases, and its detonation velocity decreases [22, 23]. Figure 1 shows a typical pressure curve for an explosion in free air. The shock wave is characterized by two phases: an overpressure phase and a low-pressure phase. The positive phase is characterized by a sudden linear increase in pressure at the peak of the pressure front, followed by an exponential drop back to standard atmospheric pressure (*P*_{O}), which is then followed by a suction phase, in which the air is absorbed and a partial vacuum is formed [22].

It can be seen, from Figure 1, that the maximum negative overpressure (*P*_{S}^{−}) is much smaller than the maximum positive overpressure (*P*_{OP}), and its limit is 1 atm (≈0.1 MPa). However, the duration of the negative phase is 2 to 3 times longer than that of the positive phase [24]. Generally, blast design standards and manuals include the IS 6922 Bureau of Indian Standards (BIS) and TM 5-855-1. The U.S. Department of Defense recommends using only the positive pressure phase of blast loads in structural analysis and design, assuming that the negative pressure phase is generally much weaker, and does not significantly affect the structural response/damage [25, 26].

The time history of the blast wave pressure can be formulated using the modified Friedlander equation:where *p*_{o} is the ambient pressure, *t* is the overall duration, *t*_{A} is the arrival time, *t*_{o} is the positive phase duration, and *θ* is the time decay constant [27]. The peak pressure of the blast wave (*P*) can be written using the following equation:where *K* is an explosive material parameter, *m* is the explosive mass, and *r* is the stand-off distance [28]. The imparted impulse (*I*) is obtained by integrating the pressure acting with respect to the time duration of the loading:where *p* represents the applied pressure due to the blast loading function in CONWEP and *t*_{o} is the duration of loading.

##### 2.2. FEM Explicit Dynamic Simulation

In ABAQUS/Explicit models, the explicit integration uses center interpolation (i.e., H). At time *t*, when the dynamic equilibrium condition is satisfied, the nodal force (external force *P* minus internal force *I*) can be calculated by multiplying the mass matrix *M* by the acceleration matrix:

When increasing from the initial time *t*, the acceleration can be calculated as follows:

As the lumped mass matrix is always used in the explicit integration algorithm, the acceleration can be obtained directly without solving the equations. The acceleration of a given node can be determined using only the nodal mass and nodal force, which can significantly reduce the computation time. Assuming that the acceleration remains constant for a particular time increment, the increase in velocity can be calculated using central interpolation. The velocity at the midpoint of the current time increment is obtained by adding the velocity increment to the velocity at the midpoint of the previous time increment:

The deformation at the end of the time increment can be calculated by integrating the velocity:

The stability of the explicit procedure is conditional; that is, the time increment cannot exceed the t_{stable} constraint, which can be estimated by the following equation:

Modeling using explicit time integration is limited by the Courant–Friedrichs–Levy condition [29]. This condition implies that the time step is limited, so a disturbance (e.g., stress wave) cannot travel further than the smallest characteristic element dimension in the mesh in a single time step. Thus, the time step criterion for solution stability is calculated as follows:where *dt* is the time increment, *dx* and *dy* are the characteristic dimensions of an element, and *c* is the local speed of sound in an element. Based on this condition, one can conclude that a smaller mesh size implies smaller time steps and, consequently, longer calculation time.

##### 2.3. CONWEP (Conventional Weapons Effects Program)

An appropriate choice for numerical simulation analysis of the fluid-structure interaction problem under air blast loading is to utilize CONWEP’s built-in explosion generation function. CONWEP uses an empirical equation to calculate the shock wave pressure acting on a surface [21]. In the CONWEP approach, the explosion will produce a pressure wave, as shown in Figure 1.

The structural interactions are described numerically using the CONWEP (conventional weapons effects program) payload property available in the ABAQUS software, considering the mass of TNT to describe the explosive charge [30]. The CONWEP algorithm, developed by Kingery and Bulmash, calculates the angle of incidence by combining the value of the reflected pressure (normal incident) and the value of the incident pressure (side on incidence). The following equation can be used to calculate the pressure:where *R* is the stand-off distance, which refers to the distance from the center of the explosion to the target structure, and the greater the stand-off distance, the less structural damage from the blast wave can be expected. *R* can be easily expressed as follows:

Furthermore, is the weight of the explosive charge. The total air blast overpressure (*P*_{total}) can be determined by combining the angle of incidence (*θ*), depending on the incident overpressure (*P*_{io}) and reflected overpressure (*P*_{ro}) [31], as follows:where *P*_{so} represents the peak incident pressure (subscripts have been used to denote the peak incident pressure and side pressure [32]), *P*_{o} represents the ambient pressure, *t*_{a} indicates the arrival time of the shock wave propagating to the target structure, *t*_{o} is the time duration of the positive phase, *β* is a dimensionless decay coefficient that depends on the shape of the shock wavefront [33], and *γ* is the ratio of the specific heat of air.

##### 2.4. Johnson–Cook Model

In cases such as those considered here, TNT is usually modeled using the Johnson–Cook model. An elastoplastic material model was used with Johnson–Cook strain hardening and damage initiation. This model has been widely used in engineering, due to its simple form and few parameters [34]. The Johnson–Cook strain rate dependence assumeswhere is the yield stress at nonzero strain rate, is equivalent plastic strain rate, is the reference strain rate, is the static yield stress, and is the ratio of the yield stress at nonzero strain rate to the static yield stress.

The equivalent von-Mises yield stress can, therefore, be expressed as follows:where *A*, *B*, *n*, *C*, and *m* are material parameters, and *T* is expressed as follows:where *T* is the material temperature (*K*), *T*_{m} is the melting temperature of the material, and *T*_{r} is the room temperature.

The damage initiation and evolution can also be modeled by the Johnson–Cook approach [35]. The damage is based on the value assumed by a variable *D*, defined as follows:where is the equivalent plastic strain and is the equivalent strain required to fracture. Fracture occurs when *D* becomes 1. The general form of the fracture strain is given as follows [35]:where is defined as , with denoting the average normal stresses and denoting the von-Mises equivalent stress. D_{1}–D_{5} are material parameters, obtained experimentally.

##### 2.5. Sandwich Panel

A sandwich structure is a structure that connects two surface layers (top and bottom) to a core in the middle [36], in order to achieve load transfer between components, which is usually used for objects that require specific standards. For example, a racing car must have the characteristics of low weight and rapid acceleration, as well as high resistance in the event of an accident [37].

Sandwich structures are also used in ships, airplanes, and various other structures. Applying the core structure helps to reduce material waste while reducing component weight. It can also increase the specific strength with the least amount of material used, increasing the structure’s capacity [38]. Figure 2 shows the general structure of a sandwich panel. An air blast test is one way to understand the performance of sandwich panels under dynamic load conditions. The finite element codes allow for simulations under such dynamic conditions to be carried out without the need for destructive air blast experiments [15, 39].

##### 2.6. State-of-the-Art

Research on sandwich panel structures with various configurations has been carried out before as summarized in Table 1. Pan et al. have simulated a U-shaped thin-walled steel plate with GFRP (glass fiber-reinforced plastic) honeycomb filler against a pendulum impact. The results indicated that the protective structure, designed with a thin-walled steel plate and fiber composite material, has good collision safety [40]. Wowk et al. have simulated an aluminum sandwich panel with different honeycomb core configurations and impact parameters. The experimental and numerical results demonstrated that the cellular core configuration did not significantly influence the core damage depth [41]. Luo et al. have simulated a sandwich panel with in-plane honeycombs in low-to-medium impact tests. It was found that the sandwich panels with in-plane honeycomb cores presented an elongated and stable plateau stage, with deeper and larger indentation profiles but smaller global deflections, compared to out-of-plane cores [42]. Liu et al. have simulated a U-type corrugated sandwich panel with the quasi-static compression load. The results indicated that the compression process occurs in three stages in the sandwich panel structure [27]. Khaire et al. have simulated a Honeycomb core cylindrical sandwich panel under ballistic impact. In the simulation, it was found that the transverse deflection of the hind forewings was highest, while the transverse deflection of the rear surface decreased with increasing cell wall thickness and facial skin thickness [43].

It can be concluded that research on the sandwich structure has not yet fully developed, as studies focused on the phenomenon of sandwich panel strength through a parametric study approach are still lacking. In this research, we examine the effect of geometric variations on the performance of a hull plate structure under blast loads, considering the critical role of the hull plate in military vehicles and civilian infrastructure.

#### 3. Benchmark and Mesh Strategy

##### 3.1. Geometrical Model

The geometry of the simulated disk used for the benchmark analysis was 2.5 m × 2.5 m × 0.016 m (Figure 3). The geometry was adopted from the study by Markose and Rao [21], which refers to Yuen et al. [44], containing the dimensions of the Casspir armored personnel vehicle. The explosion is considered to come from a mine located 0.41 m below the surface of the central hull. Two convergence studies were performed on a 180° plate subjected to a 21 kg TNT load.

##### 3.2. Mesh Strategy

The mesh size of a finite element model is also an essential factor affecting the numerical results, which should be small enough to allow the impacted structure to deform to its natural shape. However, very high-density meshes can significantly increase the computational resource requirements and, thus, modest cell mesh sizes are desirable. Therefore, a sensitive mesh size analysis was performed to obtain reasonable impact performance for the energy-absorbing structure [40].

The steel plate was modeled using first-order solid elements C3D8R (continuum three-dimensional 8-node reduced integration), which have minimal shear and volume locking effect. Solid elements are preferred over less time-consuming (i.e., shell) elements, as the limitations imposed by Mindlin shell theory can be avoided. The mesh size in the simulation model (Figure 4) varied, with element sizes of 0.01 m and 0.02 m.

##### 3.3. Benchmarking Result

We compared the midpoint displacement values obtained in our numerical simulation with those obtained by Markose and Rao [21], as presented in Figure 5. The simulation and comparison data indicate that our result was very similar to the reference, thus validating the method we used.

#### 4. Finite Element Configuration and Setting

##### 4.1. Blast Test Arrangement

The explosion was assumed to come from a land mine located at a distance of 0.41 m directly below the bottom surface of the hull. We tested detonated TNT masses of 21 kg, 28 kg, and 35 kg. In this study, the mesh used was 0.01 m and the time step was 0.2 s. The simulation was performed by determining the weight of the TNT payload, the distance of the target from the center of the blast, and the geometry of the sandwich panel surface. The CONWEP explosion simulation code was then used to calculate the pressure distribution and impulse loads due to the blast load on sandwich panel surfaces with various properties.

The plates had fixed boundary conditions along the two sides parallel to the centerline, while the two remaining sides were left unconstrained (Figure 6). Symmetric boundary conditions were used, where suitable.

##### 4.2. Design Variation

We considered three variations for the core model of the sandwich panels simulated in this study (Table 2): honeycomb, stiffener, and corrugated. The thickness was used to adjust the structural weight ratio. Table 2 provides geometric descriptions of the core plates. Solid plates, as skin (top and bottom), with 0.006 m thickness were joined to cores with structural weight adjustment using eight-point continuum-3D solid elements with reduced integration (C3D8R).

##### 4.3. Material Properties

Various materials and shapes can be used as energy-absorbing structures. Steel exhibits ductile and stable plastic mechanism behavior and provides a controlled and stable failure mode during the impact energy absorption process [45]. The material chosen for benchmark object simulation was mild steel, characterized by *E* = 203 GPa, = 0.3, and *ρ* = 7850 kg/m^{3}. Markose and Rao [21], referring to Iqbal et al. [46], have characterized mild steel and evaluated all material parameters in the Johnson–Cook elastoplastic model. The constants A, B, *n*, C, *m*, and *ε*_{0} are material-dependent parameters, which can be determined from empirical fitting to yield stress data. The obtained parameters were verified through finite element simulations in ABAQUS.

The first material used was the same as the material used in the benchmark paper: mild steel. Mild steel, as presented in Figure 7, is a type of low-carbon steel. Although the range varies, depending on the source, the amount of carbon normally found in mild steel is between 0.05% and 0.25% by weight. An example of a mild steel material is ASTM A36. The properties of the used material are provided in Table 3.

The next material considered was medium carbon steel. Medium carbon steel is a material with a carbon content of around 0.3–0.8%, with microstructure that is harder and stronger. The high amount of carbon makes this steel more responsive to various heat treatment processes, improving its mechanical properties. An example of medium carbon steel material is AISI 1040. The properties of the used material are given in Table 4.

The last material used was alloy steel. Alloy steel may include any of several elements: molybdenum, manganese, nickel, chromium, vanadium, silicon, and boron. These alloying elements increase the strength, hardness, wear resistance, and toughness of the material. The amount of alloying elements can vary between 1 and 50%. Alloy steels can be classified into low-alloy steels and high-alloy steels. The boundary between low- and high-alloy steel is generally accepted as 5% of alloying element. An example of an alloy steel material is AISI 4340. The properties of the used material are provided in Table 5.

#### 5. Results and Discussion

The results of 27 air blast test simulations, considering variations in core design, materials, and weight of TNT, in terms of midpoint displacement, stress contours, and internal energy, are investigated in the following sections:

##### 5.1. Midpoint Displacement

The simulated core compression process is shown in Figures 8–10, which demonstrates the case when a blast wave is applied to the lower skin. Considering the short time of action and the high shock frequency of the explosion, it only takes a few milliseconds from zero to maximum load. The stress-strain behavior of the structure under the action of the shock wave is positively correlated with the rate of action of the shock wave. Explosive propagation will spread to all sides after the explosion occurs. Under the unimpeded influence, the explosion wave would form a spherical wave array and spread outwards. As the blast point is relatively short (i.e., 0.41 m from the bottom layer), the short first contact with the bottom layer will increase the pressure, produce a reflected wave, and propagate over the distance. The first buckling occurs on the underside (affected side), and the bevel bends towards the inner side. Figures 11–13 show the displacement-time curves of the structure affected by the explosion. The highest deflection was located right in the center of the lower skin, closest to the blast source. However, the bevel near the top remained almost in its original state. During the movement of the lower skin, failure occurred at the bottom of the bevel, while the bevel near the top moves outward. Then, the core bent from the center to the limit, and the compression gradually reached a maximum. The dynamic global response of the core was then initiated. When the core reached maximum deflection, it started to vibrate.

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

The displacement value decreased farther away from the center of the plate. It can be seen that the effect of geometric variation on the collision response was very influential. It can be seen that, at time *t* = 0.01 s, displacement was at its highest, after which global deformation began to occur. When the face sheet reached maximum deflection, the whole plate vibrated, then returned to the static state. As can be seen from these profiles, the stiffener core model showed better maximum displacement, in comparison with the other panels.

In the contour image, it can be seen that the boundary edge also experienced movement; this was due to the boundary conditions that we used, which also affect the structure’s response. However, there were some different contour results, especially at the low TNT load of 21 kg and with the medium carbon steel and alloy steel materials. For the corrugated geometry model, the maximum point occurred on the front and back of the plate; this was possible because there were several significant differences in the properties of the existing material.

At a load of 21 kg, the honeycomb model obtained the best results with alloy steel material, at . The stiffener model also obtained the best results with alloy steel material, with . Finally, the corrugated model also obtained the best results with alloy steel material, where *m*. The worst results for all models were obtained when considering mild steel material.

At a load of 28 kg, again, the honeycomb, stiffener, and corrugated models all obtained the best results with alloy steel material (, 0.186 m, and 0.207 m, respectively). Meanwhile, the worst results for all models were obtained with the mild steel material.

Finally, for the highest TNT load (35 kg), the stiffener, honeycomb, and corrugated models all obtained the best results with alloy steel material (, , and , respectively). Again, the worst results were obtained with the mild steel material; in particular, for the corrugated model, .

After 0.01 s, it can be seen that the plates presented a spring-back phenomenon, which occurred before the structures produced a permanent response, as shown in terms of multiple peaks, indicating a weakening trend. In the simulation results, it can be seen that the displacements in the honeycomb, stiffener, and corrugated models with medium carbon steel and alloy steel materials at low loads were not apparent, due to significant differences in the properties of these materials; therefore, we included yield stress in the analysis, such that the properties could be clearly determined under high-load conditions.

From the results of the simulation with the variations, it can be seen that the alloy steel material obtained the best results on average, with minimum displacement of the objects. In the second place, there was medium carbon steel, while the worst performing was mild steel. The geometric model that obtained the best average results, in terms of lower skin displacement, was stiffener. However, in terms of further observations regarding the effect of the air blast charge on the lower skin hull plate, it may be possible that the upper skin displacement presents a different order, regarding the best geometric model, due to the shape of the core layer affecting the energy absorption. This is important to consider, as the upper skin is a plate, which is directly related to the object (vehicle).

##### 5.2. Stress Contour

Snapshots of the von-Mises stress contours are shown in Figures 14–16, while the von-Mises stress distributions at the time of the collision are shown in Figures 17–19. It can be seen, from these figures, that the stress patterns of the honeycomb and stiffener panels were similar, while that of the corrugated panel differed. The contour depends on the interaction between the bottom layer and the core, which is affected by the formation of the core’s geometry using the weight ratio method. The reflected wave ring on the panel is affected by the panel boundary effect and is related to the blast wave generated at the center of the panel. In the explosion generated by the CONWEP model, the air blast is concentrated at the center of the panel and gradually spreads across the panel.

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

It can be seen that the stress response to the air blast in each model at the bottom of the plate was very similar. With each additional load, the area experiencing stress increased, proving that, as the load increases, the affected area also increases. This can be seen from the color of the existing structure: blue denotes lower von-Mises stress, while red indicates higher von-Mises stress. The stress contour results also showed that the occurrence of maximum stress in the boundary area, caused by the boundary conditions used.

Stress is something that fluctuates and, so, its distribution at a certain point in time cannot be representative of the entire process. Therefore, we also provide graphs of the time history of the von-Mises stress values:

At a load of 21 kg, the honeycomb, stiffener, and corrugated models all obtained the highest von-Mises stress value with the alloy steel material ( Pa, Pa, and Pa, respectively). Meanwhile, the lowest results for all models were obtained with the mild steel material.

At a load of 28 kg, the honeycomb model obtained the highest von-Mises stress with the medium carbon steel material, at Pa. Meanwhile, in the stiffener and corrugated models, the maximum value was obtained with the alloy steel material ( Pa and Pa, respectively). Again, the lowest results for all models were obtained with the mild steel material.

At a load of 35 kg, the honeycomb and corrugated models obtained the highest von-Mises stress with medium carbon steel material ( Pa and respectively). Meanwhile, for the stiffener model, the maximum value was obtained with the alloy steel material ( Pa). Once more, the lowest results for all models were obtained with the mild steel material.

The simulation results indicated that the von-Mises stresses for honeycomb, stiffener, and corrugated models with mild steel, medium carbon steel, and alloy steel materials well defined the stress obtained with each geometric model and material used. The data show that the stress was at its maximum after the TNT had detonated and the shock wave hit the hull plate. The results demonstrated that mild steel has less fluctuations in stress (i.e., tending to be flat), when compared to the other materials. This was due to the fact that there are several significant differences in the properties of the considered materials, as previously mentioned.

Stress variations can vary, depending on how many step times are considered in the sample. The graphs above considered a time step of 0.01 s, in order to measure the maximum von-Mises stress. It can be seen that all materials and models had almost the same trend in their stress history. After reaching a peak, the stress immediately decreased, with vibration occurring at the following step time. The stress behavior of the objects in this simulation can be determined through analysis of the necessary conditions, including the magnitude of the blast load, the thickness of the hull plate, the modulus of elasticity, and the Poisson ratio.

##### 5.3. Structure Internal and Kinetic Energy

Energy output is often an important part of ABAQUS/Explicit analysis. Comparisons between the various components of energy can be used to help evaluate whether an analysis produces an appropriate response. The components and their abbreviation are summarized in Table 6.

Figures 20–22 show that, after the blast wave loading had completed, the plate began to vibrate, where the kinetic energy of ALLKE increased and the strain energy of ALLSE began to decrease. The strain energy was greatest when the plate had deformed the most, and least when the plate was vibrating at other times. The plastic strain energy of ALLPD reached a steady state and increased with time. The kinetic energy diagram indicates that a second expansion of the plastic strain energy occurred as the plate recovered from its maximum deformation. Therefore, plastic deformation after blast wave loading was observed. In ABAQUS, the deformation of an hourglass-shaped element is controlled by the quantity ALLAE (virtual strain energy). The results demonstrate that the plastic deformation corresponds to the deformation of the structure when the internal energy dissipates, and the total internal energy itself is much higher than the sum of the elastic strain energies. Therefore, it can be concluded that the virtual strain energy in this analysis is a type of quantum energy, including dissipative energy and elastic strain energy. ALLIE is the total internal strain energy (ALLSE + ALPD + ALLAE), including all internal energies [49].

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

**(a)**

**(b)**

**(c)**

It can be seen, from the simulation results, that the internal and kinetic energy presented a similar trend, as they should. However, in some simulations (i.e., medium carbon steel and alloy steel materials in honeycomb, stiffener, and corrugated models at low loads of 21 and 28 kg), different trends were observed up to 0.2 s, as ALLAE, ALLIE, and ALLPD continued to increase. This was due to the significant differences in the properties of these materials, including the yield stress. The trend was expected to be clearly seen at the highest TNT load; however, at the highest TNT load, all geometric models presented the same graphic pattern. In the perfectly formed graph, the history patterns of medium carbon steel and alloy steel, to be precise; it can be seen that ALLIE has a steeper turning point, compared to that with mild steel.

From the figures, it can be seen that the honeycomb model had the highest maximum average values of ALLAE and ALLIE, the stiffener model had the highest maximum average values of ALLKE and ALLPD, and the corrugated model had the highest maximum average value on ALLSE. This can be more clearly seen at the highest load of TNT (35 kg), where ALLAE and ALLIE for the honeycomb model with alloy steel material are 707,672 J and 2,075,160 J, respectively; ALLKE and ALLPD in the stiffener model with the same material were 742,631 J and 1,357,130 J, respectively; ALLSE of the corrugated model with the same material was 180,238 J.

#### 6. Conclusions

In this study, a numerical investigation of the dynamic response and internal kinetic energy of sandwich panels with various structural and material combinations was carried out. In particular, simulations were carried out using three different variations of the core geometry (honeycomb, stiffener, and corrugated), through equations using structural weights. We found that using a sandwich panel structure with stiffener or honeycomb core geometry can provide an appropriate means to increase the structural resistance against explosions, serving as an exciting innovation or a substitute for the conventional (i.e., corrugated) form. Their structural performance was found to be more effective, in terms of minimizing the damage caused by explosion loads. Simulation was carried out with several variations, including the different geometric core models with mild steel, medium carbon steel, and alloy steel materials. The test was conducted using the CONWEP method in the ABAQUS software, considering free air blast under a TNT load of 21 kg, 28 kg, or 35 kg. In this simulation, we assessed the impact of the free air blast on the hull plate, in terms of displacement, von-Mises stress, and internal kinetic energy.

The simulation results indicated each structural variation’s ability to withstand the free air blast load. It can be seen from the displacement results that sandwich plates with a core stiffener form were more effective in resisting the various blast loads. We also obtained the best displacement results when using the alloy steel material. It was concluded that a stiffener geometric model with an alloy steel material provides the best combination of shape and material.

The stiffener model obtained the best results regarding the maximum displacement of the lower skin; however, for the upper skin, it was found that the honeycomb had the best displacement results, demonstrating that the honeycomb core model provided the best energy absorption. The simulation results showed that the von-Mises stress of honeycomb, stiffener, and corrugated models with mild steel, medium carbon steel, and alloy steel materials well defined the stress for each geometric model and material used. The resultant graphs showed that all of the combinations experienced a point of maximum stress right after the explosion load, while experiencing vibrations afterward.

For optimal results, the core structure must provide the necessary supporting stiffness to spread the impact forces at the contact points throughout the structure. More complex core, material, and corner models may be considered in further research, in order to enhance the model strength while developing advanced lightweight designs.

#### Data Availability

The data used to support the findings of this study are included within the article.

#### Conflicts of Interest

The authors declare that they have no conflicts of interest.

#### Acknowledgments

This research was funded by the Universitas Sebelas Maret under funding scheme Kolaborasi Internasional (KI-UNS) with contract/grant no. 254/UN27.22/PT.01.03/2022. The grant is gratefully acknowledged by the authors.