Impact Dynamic Analysis and Rubber Impact-Resistant Design of a Launcher

,


Introduction
Te impact resistance of naval ships has attracted increasing research attention as an important index to evaluate their vitality [1].Te transient noise caused by the impact force of a weapon launch can expose the position of submarines during wartime, which can have fatal consequences.Terefore, it is necessary to examine and improve the transient noise control technology to realize the combination of acoustic stealth and combat functionality [2,3].Lai et al. [4]and Kuang et al. [5] enhanced the hydraulic mechanism design of the lifting and closing device of a naval ship, successfully reducing the impact force of the drag reduction plate on the hull structure.Wang et al. [6] performed a fnite element numerical simulation of the submarine cabin structure to obtain the law of impact spectrum variation with mass and stifness of naval ship equipment in diferent connection modes, revealing the limitations of the dynamic design analysis method (DDAM) commonly used for naval vessels.It is common to use rubber materials in military equipment to generate a considerable amount of internal friction during the deformation process, absorbing the kinetic energy of impact to reduce the transient impact force [7,8].Zhao et al. [9] established the constitutive relation of rubber bufer components through static and dynamic load experiment and analyzed the impact of rubber bufer component of a sniper grenade launcher on its fring performance using Adams software.Li et al. [10] applied fnite element calculation and analysis to the impact problem presented by the projectile ejection device with a rubber cushion and examined its dynamic structural strength.Li [11] adopted the fnite element method to establish a mechanical model of a composite material launcher while analyzing and evaluating its dynamic performance in a launch state.Ravishankar et al. [12,13] conducted fnite element modeling for ballistic impact behavior of sandwich structures made of diferent composite materials, pointing out that the energy absorption capacity of glass-rubberepoxy sandwich was highest among the natural rubber and glass-epoxy.
Te rubber collision and impact-resistant structure is not limited to the military feld but is also widely used in civil engineering.For example, using the fnite element method, Yuan et al. [14] studied the infuence of the rubber-damping layer thickness on the damping characteristics of rock arch structures under an explosion load.Liu et al. [15] designed a fexible box structure, an anticollision device for the bridge pier protection of ships.Tis device could efectively absorb a signifcant amount of impact energy, reduce the impact reaction force, improve the anticollision ability of vessels, protect the bridge and ship, and reduce losses due to accidents.Chen et al. [16] used the honeycomb structure composed of corrugated steel pipes as the anticollision structure of bridge piers, and verifed the efectiveness of the design through test methods.Zeng et al. [17] calculated the dynamic response of train tracks.Xu et al. [18] used the fnite element method and a genetic algorithm to optimize the energy absorption rate of the rubber ring bufer at the junction of a locomotive under impact load.Lu et al. [19] established a multidegree of the freedom dynamic model for the hinged foating structure with rubber cushion, and studied its hydrodynamic response, the results show that the strength of the rubber cushion designed meets the allowable stress of the material.
Wang et al. [20] studied the impact of aircraft landing on airborne equipment and analyzed the diferences between the impact characteristics of two types of engines.Luo et al. [21] conducted numerical simulation on the dynamic characteristics of the shield tunnel under aircraft taxiing load to obtain a reasonable range of taxiing speed and tunnel depth.
Most of these studies utilized dynamic software to simplify and resolve the impact problem in the impact-resistant structures of large equipment according to their impact characteristics [22].Based on this, and targeting the impact response of the drag reduction plate on the hull of the ship when the launching and closing device is opened, this study extracted the main vibration components during the impact response process to establish an efective mechanical model of a single degree of the freedom system.Furthermore, it combined theoretical analysis and fnite element calculations, studied the load and dynamic response characteristics of the impact-resistant structure under impact load, and created the impact spectrum curves with diferent load times.In addition, a simplifed fnite element model was established based on the dynamic response characteristics, impact spectrum, and rubber material performance tests, while the rubber impact-resistant pad size was designed to meet the strength requirements.Tis study provides a new possibility for resolving the collision challenge presented by launchers.

The Dynamic Model Analysis of the Drag
Reduction Plate of the Launcher 2.1.Impact Load Analysis.Figure 1 shows a schematic diagram of a naval ship launcher.Te cover plate could be hydraulically opened, and the drag reduction plate, driven by the crank connection mechanism, could rotate while the stopper was attached to the hull.Te drag reduction plate consumed kinetic energy via the collision stopper, and the angular velocity was reduced to zero to open the launcher in place.Te drag reducer plate weighed about 300 kg.Since the stopper impact time was short, this could be regarded as the transient impact load on the stopper, with a contact area of 1200 mm 2 .In order to avoid the stress singularity of the connection part and ensure the accuracy, the part of the hull structure connecting the impact-resistant structure is taken into account, and the connection part of the hull can be regarded as a fxed boundary.Figure 2 shows the size of the stopper and its base.Tis transient impact caused two types of damage.First, the signifcant short-term impact caused the dynamic response of the structure to exceed the yield strength, which could lead to local structural stress failure.Second, the signifcant transient vibration and noise caused by considerable impact force could easily expose the position and attack intention from the side.
To further examine the impact on the system, a 511F05 dynamic force sensor was installed at the impact location to test the force signal (Figure 3).Te collected impact forcetime history curve of the stopper is shown in Figure 4(a).After the impact force was restored to zero, it turned negative, indicating that the drag reduction plate rebounded after impacting the hull structure.Since the rebound disappeared within 3 s, and the maximum value of the rebound force was one order lower than the maximum value of the impact force, the collision could be described as in a completely inelastic state, that is, the rebound action did not require consideration [23].Due to the short duration of the impact force, the impact load was approximated via the triangular load for theoretical analysis, as shown in Figure 4(b).
Te triangular load can be described mathematically as follows: where F 0 � 15 kN, t 1 � 0.125 s, and t 2 � 0.635 s.

Analysis of the Inherent System Characteristics and the
Static Mechanics Calculation.Te impact-resistant structure composed of the stopper and the base was considered the vibration system, while the connection between the bottom of the base and the hull was regarded as the fxed support.Te free vibration of the structure was calculated via fnite element software, using common carbon steel as the impact- Te frst-order natural frequency calculated by the fnite element method (FEM) was f 1 � 993.02Hz, that is, the frstorder vibration period was about 0.001 s.Te impact load duration was much longer than the frst-order vibration period of the system.Terefore, the vibration system will likely produce only frst-order vibration at the impact force and can be treated as a single-degree-of-freedom system.Te static analysis of this system was performed using fnite element software.A static force with a size of F 0 was applied to the force surface of the impact load of the stopper, while the center point of the dynamic load action surface was considered the equivalent displacement point.Te deformation vector diagram is shown in Figure 6, with an equivalent displacement of x 0 � 0.2 mm.Te equivalent stifness and mass of the system were calculated according to the abovementioned expression of the frst-order natural frequency was . Te equivalent stifness was k � F 0 /x 0 � 7.04 × 10 7 N/m, and the equivalent mass was m � 1.81 kg.After grid independence analysis, the maximum stress value and location are obtained by using the optimal mesh strategy with acceptable calculation speed and accuracy.As shown in Figure 7, the maximum stress occurred at the middle of the connection, which is 188.3MPa.

Te Analytical Solution and Finite Element Analysis of the Impact Vibration Response. Te dynamics analysis in this
paper is likely to exhibit only low modal response.For this case, the use of implicit unconditional stabilization algorithms is usually preferred over conditional stabilization algorithms [24].Terefore, an implicit direct algorithm was used to perform the matrix iteration using the Newton-Rapson method to ensure calculation accuracy.Eight time steps of 0.12588 ms were set in each vibration period, respectively.Te computing platform consisted of four cores and a 3.2 GHz processor, while the computing time was 3.5 h.Te center point of the action surface of the force was considered the reference point to calculate its acceleration curve with time, as shown in Figure 8. Due to the infuence of structural damping, the variation in the acceleration response caused by the impact was attenuated in three time periods (0 < t < 0.125 s, 0.125 s < t < 0.635 s, and 0.635 s < t < 1 s).In addition, during the frst two periods, the structure was subjected to diferent external loads, while no external forces were evident in the third period.Terefore, the three periods showed diferent attenuation trends.
Fourier transform analysis was performed on the vibration curves of the three stages (as shown in Figure 9), showing that the system only has one resonant frequency point, namely 993.01 Hz, which is highly consistent with the frst-order natural frequency (993.02Hz), of the impactresistant structure and verifes the accuracy of the implicit direct calculation method.It also indicated that the impact response analysis of the stopper and base system could be considered a Kelvin-Voigt single-degree-of-freedom model under this transient impact load, as shown in Figure 10, where c represented the damping coefcient of the system.
Te HHT [24] integration algorithm is adopted in the implicit solution method, which has no numerical dissipation for the low frequency response [25].As shown in

Shock and Vibration
Figure 11, the results of fnite element calculation show that the dissipated energy ALLVD is always zero with time, and the total strain energy ALLIE reaches the peak when the impact force is at its maximum, which exactly verifes the above views of the literature [25].Terefore, the real structural damping coefcient can be extracted from the attenuation curve of acceleration by the FEM model.
Amplitude attenuation curves, A1, A2, and A3, are ftted in Figure 12, which shows that the attenuation coefcients of the three curves were exceedingly close.Due to the external force interference in A1 and A2 stages, the curve A3 was used to calculate the damping coefcient of the system.
Under the triangular load in equation ( 1), the displacement response of the damped single-degree-of-freedom system is solved according to the Duammel integral.Te system response under the action of the microimpulse F(τ)dτ is as follows:

Shock and Vibration
Ten, in the frst stage (0 < t < t 1 ), we have Te equation mentioned above was integrated to obtain the following: Since and 1 − 2ζ 2 are approximately equal to 1. Equation ( 4) can be simplifed as follows: In the second stage, (t 1 < t < t 2 ), there are Te equation was integrated to obtain the following: Since ζ 2 (ζ � 0.0021) is a tiny value, both and 1 − 2ζ 2 are approximately equal to 1. Equation ( 7) can be simplifed as follows: In the third stage (t > t 2 ), there is Te equation mentioned above was integrated and simplifed to obtain the following: After solving the equation mentioned above, the response of the single-degree-of-freedom system under the impact load can be expressed as follows: 6 Shock and Vibration x st ω n t 1 − t 2  ω n t − ω n t 2 − 2ζ  + x st 2ζe −ζω n t ω n t 1 cos ω n t − x st e −ζω n t ω n t 1 sin ω n t, where x st is the static displacement under static load F 0 , and x st � F 0 /k.Te analytical solution of displacement on the center point (equivalent displacement point) of the stopper contact surface under impact load was compared with the fnite element numerical solution, as shown in Figure 13.Te trend of displacement variation with time derivated by the Kelvin-Voigt single-degree-of-freedom model is highly consistent with that by the fnite element implicit solution, and the maximum displacement obtained by both methods occurs at 0.125 seconds, with a diference of 2.3%, which verifes the accuracy of the theoretical model.

Analysis of the Infuence of the Excitation Duration on the
Dynamic Response of the System.Te natural vibrational circular frequency of the system was ω n � 6239.3 rad/s, and the natural period was T ≈ 0.001 s.When the excitation force was applied to the system as a dynamic load, it produced a certain dynamic load efect.Assuming that the ratio of the rising time t 1 and the falling time t 2 − t 1 of the exciting force was certain, then t 2 − t 1 /t 1 � 0.635 − 0.125/0.125� 4.08, while the maximum change law value of the dynamic system response at an excitation duration t 2 /T ratio and the frstorder vibration period T of the system were examined as variables.Take the ratio of maximum displacement to static displacement α � x max /x st as the ordinate and t 2 /T as the abscissa to draw the impact spectrum curve under dynamic load.Te calculation results are shown in Figure 14.When t 2 /T approached zero, the dynamic amplifcation coefcient α approached zero; when t 2 /T �1.45, α reached the maximum value of 1.7; and when t 2 /T exceeded 5, the dynamic amplifcation coefcient α gradually tended toward 1.When the load duration is much smaller than the frst-order vi-bration period of the system, that is, t 2 /T tends to zero, in other words, the excitation frequency is much larger than the frst-order natural frequency of the system, the broadband response of the vibrational system may be excited, it cannot be regarded as a single-degree-of-freedom system.Terefore, the impact spectrum curve is not considered in the range when t 2 /T is much less than 1.
Te duration ratio t 2 /T of the impact load on the stopper and the base to the natural vibration period of the system studied in this study is 577, which is far greater than 5. Terefore, the dynamic displacement of the stopper tended to the static displacement, that is, the impact load has no amplifcation efect on the system response.Since the maximum stress was directly related to the structural deformation, the deformation and stress distribution of the structure under the transient impact load was regarded as the deformation under static load.According to the calculation results obtained in Section 2.2, the maximum stress of the structure was 188.3 MPa, which occurred at the middle of the connection between the base and the hull.
Terefore, although the impact load did not dynamically amplify the system, according to the design specifcations GJB/Z 21A-2001, the maximum generated stress still exceeded the allowable stress value of [σ c ] � 0.3 × 355 MPa � 106.5 MPa.Consequently, laying rubber impact-resistant mats on the impact surface of the stopper to reduce the transient impact force is commonly used in engineering to reduce vibration and avoid local stress excess.Te impact load generated by the rigid contact between the drag reduction plate and the stopper verifed that the dynamic amplifcation factor equaled 1.According to the law of the impact spectrum presented in Figure 14, the t 2 /T ratio increased after the rubber pads were laid, and the dynamic amplifcation factor was closer to 1, which could still be regarded as a static problem.

The Rubber Impact-Resistant Mat Size Design
Since the impact response in this paper was a linear dynamic problem, the linear relationship between the displacement and stress of the stopper could be established.Te force and deformation of the stopper conformed to Hooke's law, and the maximum stress caused by unit deformation was as follows: Ten, on the condition that the vibration system composed of the stopper and the base met the allowable stress scale, the allowable displacement of the equivalent displacement point on the stopper was as follows: After the rubber pad was laid on the surface of the stopper, as shown in Figure 15, the bottom area of the rubber block was the same as the contact area between the drag reduction plate and the stopper, which was A � 1200 mm 2 .A thicker rubber block d absorbed more impact kinetic energy.However, if the rubber was too thick, the height of the drag reduction plate increased after it was opened and in place, possibly afecting the launching channel of the 8 Shock and Vibration weapon.After the drag reduction plate is opened and in place, the height of the rubber pad should be less than 5 mm to ensure the normal launch of the weapon.

Acquisition of the Property Parameters of the Rubber
Materials.Tis study installed a rubber impact-resistant mat on the surface of the stopper.Because the mass of the drag reduction plate of the launcher was relatively large and the momenta of the contact with the stopper were substantial, a rubber material with a Shore hardness of 65 and density of 1630 kg/m 3 was selected while comprehensively considering its deformation potential energy and impact resistance.
To accurately describe the mechanical properties of the rubber material and facilitate calculation and analysis, dumbbell-shaped rubber specimens were created, and their tensile capacity was tested according to the determination procedures of GB/T528-2009.Specimen length l � 25 mm, width b � 6 mm, and thickness d � 2 mm.Te loading force at both ends of the specimen varied with the elongation, as shown in Figure 16.Te axial force and deformation were transformed to obtain the nominal stress (σ � F/bd, where F is the axial force) and the nominal strain (ε � z/l, where z is the deformation).Te stress-strain curve obtained by the experiment was ftted using the Mooney-Rivlin model on the fnite element calculation platform ABAQUS, yielding an excellent general consistency, as shown in Figure 17.Te

Te Finite Element Analysis of the Simplifed "Rubber
Impact-Resistant Mat + Collider" Model.Te reasonable thickness of the rubber impact-resistant mat was determined via fnite element analysis after obtaining the material property parameters.Te impact process fulflled the conservation of the momentum, while the integration of the impact load presented in Section 2.1 over time yielded an impulse of I � 4762.5 kg•s.Actual ship measurements revealed that when the drag reduction plate collided with the stopper, the linear velocity of the drag reduction plate was V 0 � 0.438 m/s.Terefore, the efective mass of the collision was m 0 � 10873.3kg.In the fnite element calculation, the actual geometric size of the collider did not need to be expressed, requiring only the unstructured mass m 0 and initial velocity V 0 .Te collision mechanics model is shown in Figure 18.At 40 mm × 30 mm, the bottom area of the collider and rubber block was the same, while the bottom of the rubber block was fxed.Te fnite element calculation defned the tangential frictionless and normal elastic contact, while a display algorithm was adopted, with a calculation and analysis time of 0.02 s, a quadcore CPU, a main frequency processor of 3.2 GHz, and a calculation time of 63 s.
Rubber blocks of diferent thicknesses were selected for the fnite element calculation, while the maximum resultant force on the contact surface between the rubber blocks and the stopper was extracted, as shown in Table 1.Te rubber impact-resistant mat absorbed more impact kinetic energy as the rubber pad thickness increased, while the force transferred to the stopper gradually decreased.However, when the thickness exceeded 12.5 mm, the decreasing trend diminished.Te power was divided by the equivalent stifness k of the system consisting of the stopper and the

Shock and Vibration
base according to Hooke's law to obtain the equivalent displacement at the center of the force surface.Furthermore, when the thickness exceeded 12.5 mm, the equivalent displacement was below the allowable displacement of 0.12 mm.Consequently, the equivalent displacement of the stopper with a rubber thickness of 11.6 mm was equal to the permissible displacement by interpolation.Terefore, in order to meet the requirements of the design specifcations, the thickness of the rubber impact-resistant mat laid on the stopper should exceed 11.6 mm. Figure 19 shows the displacement clouds of the four impact-resistant pads at maximum deformation.Meanwhile, the deformation rates of the rubber impact-resistant pad with diferent thicknesses in the thickness direction were all about 20%.
To satisfy the requirement of a rubber pad thickness below 5 mm after opening the drag reduction plate in place, that is, the height of the portion exceeding the stopper should be less than 5 mm, it is compressed.On condition that the stopper stifness was not afected, a groove with a depth of 5 mm was added downward along the normal direction of the contact surface, as shown in Figure 20.Terefore, according to the 20% rubber deformation rate calculation, the thickness of the rubber mat should be less than 12.5 mm to meet the requirements.In summary, the thickness of the rubber impact mat should be 11.6 mm < d < 12.5 mm.

Conclusions
Tis paper combines theoretical derivation and fnite element analysis to examine the load and dynamic response characteristics of the impact-resistant structure of the launching and closing device of a certain type of weapon under an impact load.Te size design of the rubber impactresistant mat is accomplished based on these characteristics, and the conclusions are drawn as follows:  (1) Te frst-order vibration period (0.001 s) of the impact-resistant structure consisting of the stopper and the base is much lower than the duration of the impact load.Terefore, the system only produces low-order vibration deformation under the impact load, which is verifed via highly accurate implicit fnite element dynamic calculations.Te damping coefcient of the structure is obtained according to the displacement response attenuation curve, while the equivalent stifness of the frst-order vibration is obtained through static calculation.
(2) Since the stopper and base of the impact-resistant structure under the impact load only exhibit frstorder vibration deformation, the dynamic response analysis is considered a Kelvin-Voigt single-degree-of-freedom model.Consequently, the analytical solution of the displacement response of the single-degree-of-freedom system is derived, and the accuracy of the theoretical derivation is verifed via comparison with the fnite element results.(3) Te impact spectrum curve of the system at diferent impact load duration is obtained according to the theoretical formula.For both the rigid and fexible contact containing rubber mat, the dynamic amplifcation coefcient is close to 1, the stress and deformation of the stopper is in accordance with Hooke's law, and the local strength can be checked as a statics issue, which greatly reduces the computational cost.(4) A simplifed collision model is established for rubber pads with diferent thicknesses, followed by fnite element calculations.According to Hooke's law, a rubber mat thickness range of 11.6 mm < d < 12.5 mm adequately meets the specifcation requirements for a normal weapon's launch.

2
Shock and Vibration resistant structure material, with an elastic modulus of 210 GPa, Poisson's ratio of 0.3, yield stress of 355 MPa, and a density of 7850 kg/m 3 .Te geometric parameters are shown in Figure 2, and the fnite element mesh is shown in Figure 5.

Figure 6 :
Figure 6: Te deformation vector diagram of the impact-resistant structure under static force.

Figure 19 :Figure 20 :
Figure 19: Displacement nephogram of rubber impact pads with diferent thicknesses at maximum deformation.

Table 1 :
Te calculation results of the force and equivalent displacement at diferent rubber block thicknesses.