Study of Influential Factors of the Vibration Modal of the Rocket Equipment Bay and Structural Improvement Based on Finite Element Analysis

In this paper, the study focuses on influential factors of the vibration modal of the equipment bay of a carrier rocket and the structural improvement of the equipment bay by using finite element modal analysis. The finite element analysis focuses on the influences of the mass of the inertial bracket, the thickness of parts of the inertial bracket, and the stringer thickness on the first modal frequency of the equipment bay. As the analytical results show, the vibration displacement of mounting panels can be greatly reduced when the equipment bay is added with mass, and the vibration of the equipment bay with mass mainly occurs on the inertial bracket (without mass, the maximum vibration displacement occurs on the mounting panel); the top surface thickness of the inertial bracket has the maximum influence on the first modal frequency of the equipment bay, the stringer thickness and the side thickness of the inertial bracket have relatively high influence on the first modal frequency, the rib thickness of the inertial bracket has relatively low influence on the first modal frequency, and the beam thickness of the inertial bracket has the minimum influence on the first modal frequency.


Introduction
The equipment bay is an extremely important bay section of a carrier rocket, in which most of the rocket's instruments are mounted.The equipment bay has strict requirements for vibratory frequency.It requires a relatively high frequency of the first modal for avoiding sympathetic vibration and a relatively small vibration amplitude of its mounting panels.In the design of the equipment bay, finite element analysis is used to ensure that the structure of the equipment bay satisfies the requirements.Some applications of finite element analysis in simulation analyses of rockets have been presented.Choi et al. [1] evaluated the structural integrity and weight of the rocket motor with a hemispherical dome by analyzing the improved 2-D axisymmetric finite element model.Engberg and Korde [2] verified the possibility of 3-D full-scale finite element modeling by analyzing the two-dimensional finite element acoustic model of the fairing of a launch vehicle.Mahyari et al. [3] established a finite element model of the launch vehicle tank to analyze the effectiveness of the rotor crusher in reducing the critical height of propellant.Schwane and Xia [4] established a finite element model of the rocket engine nozzle to calculate the lateral load generated by the nozzle.Mense et al. [5] studied the thermal response of unprotected structural steel under solid rocket propellant flame by finite element thermal analysis.Howard et al. [6] verified the effect of the absorber in the rocket structure by analyzing the finite element model of the rectangular plate.Salvador and Xu [7] established a twodimensional finite element model of the rocket burner with electrodes to analyze the influence of an electric field on flame combustion stability.Sim et al. [8] established finite element modeling techniques for computational modal analyses by considering the liquid propellant and flange joints of launch vehicles.Baldesi [9] introduced some studies that the dynamics analyses of various types of launch vehicles were executed by using finite element analysis.Hutchinson and Olds [10] estimated the structural weight of the propellant tank of a rocket by establishing a simplified beam finite element model.Marimuthu and Rao [11]carried out dynamic analysis of the open cylindrical storage tank of a launch vehicle by means of finite element dynamic analysis.Roh and Kim [12] solved the trajectory optimization problem of a multistage launch vehicle by using an indirect time finite element method.Li and Zhang [13] researched the connection strength and slip characteristics of the rocket bolt by using finite element analysis.Elhefny and Liang [14] built a 2-D axisymmetric rocket gas turbine disk model to analyze the stress of the gas turbine disk.Zhang and Jiang [15] simulated the flight response of a rocket sled by using finite element coupling mechanical analysis.Chandana et al. [16] analyzed six mode shapes of the launch vehicle payload fairing structure by finite element analysis.
However, these studies focus on the application of finite element analysis in the simple rocket part structure, and the exhibit of finite element analysis in the complex rocket structures is less.This paper will present the vibration modal analysis of an equipment bay that has 7 parts and 572 thousand elements.The materials of the equipment bay include aluminum alloy, cast iron, carbon fiber composite laminates, and honeycomb sandwich.The parts in the finite element model of the equipment bay are linked by adhesive contacts, including in total 13 contact bodies that mutually adhere with each other.And the influence of some structural parameters of the equipment bay on its first modal and the structural improvement of the equipment bay will be investigated.

Finite Element Model of the Equipment Bay
The equipment bay includes 7 major parts such as the skin, upper-end frame, lower-end frame, supporting plate, mounting panel, circular frame, and inertial bracket, as shown in Figure 1.The skin is a reinforced cylindrical shell structure, with an outer diameter of 3000 mm and an overall height of 650 mm.It includes a cylindrical shell, stringer, window, and window cover.The skin is made of aluminum alloy.The function of stringers is to enhance the bearing capacity of the cylindrical shell, and the role of windows is to facilitate the installation and maintenance of equipment.The window includes a big window and a small window.The big window is a 300 mm × 300 mm square frame, and the small window is a 200 mm × 200 mm square frame.The lower-end of all the windows is 260 mm away from the lower-end of the skin.The location of the window on the skin is shown in Figure 2. Windows 1, 2, 3, and 4 are big windows and Windows 5 and 6 are small windows.The symmetry axis of Windows 1 and 4 coincides with the vertical symmetry axis.The symmetry axis of Window 3 coincides with the horizontal symmetry axis.The angle between the symmetry axis of Window 2 and the vertical symmetry axis is 45 °and the angle between Windows 5 and 6 and the horizontal symmetry axis is 20 °.The stringers have two types of cross sections, as shown in Figure 3.The parameters of the I-type stringer are H 1 = 25 mm, W 1 = 20 mm, t 1 = 1.5 mm, and t 2 = 1.5 mm.The parameters of the II-type stringer are H 2 = 25 mm, W 2 = 20 mm, W 3 = 20 mm, and t 3 = 1.5 mm.The number of I-type stringers and II-type stringers is 12 and 76, respectively.The cylindrical shell is simulated with a shell element of which the thickness is 1 mm.The stringer is simulated with a beam element.The skin finite element model is shown in Figure 4.In the figure, the 3-D beam is the result of the 3-D display of the 1-D beam element.The left and right sides of the window are reinforced by two I-type beams.The cylindrical shell of the skin is linked with stringers and a window cover by using merging nodes.
The inertial bracket is used to control the overall dynamic characteristics, which is made of cast iron as a whole.The finite element model of the inertial bracket is shown in Figure 5.In the figure, all the elements are plate shell elements.The top surface and rib have a thickness of 3.5 mm, the side surface and beam have a thickness of 2 mm, and the top surface and rib, top surface and beam, and rib and beam have the conodes on their intersection.The rib, beam, top surface, and side surface in the inertial bracket are linked with merging nodes, while the inertial bracket is linked with the skin and circular frame by adhesive contact.For the   International Journal of Aerospace Engineering successful setting of the adhesive contact, the distance between shell elements must be considered or the offset of the shell element is set or the distance between surfaces should be calculated when establishing the surfaces.
The supporting plate is used to support the mounting panel, and it is made of carbon fiber composite laminates.The stacking sequence of the laminates is [45/0/-45/90] 3S .Each layer has a thickness of 0.125 mm.The shell element is used for simulating the supporting plate.The finite element model of the supporting plate is shown in Figure 6.The blue surface of the supporting plate is in contact with the mounting panel, and its red surface and yellow surface are in contact with the skin and the circular frame, respectively.
The circular frame is used to enhance the stiffness and strength in the circumference direction of the skin.The finite element model of the circular frame is shown in Figure 7.The red surface of the circular frame is in contact with the skin, and its blue surface and yellow surface are in contact with the mounting panel and the supporting plate, respectively.The mounting panel is of a honeycomb sandwich.The upper and lower faces are carbon fiber laminates.The stacking sequence is [45/0/-45/90] S .Each layer has a thickness of 0.125 mm.The middle sandwich is a 10 mm aluminum honeycomb.One 17-layer laminate is used to simulate the honeycomb sandwich.The mounting panel is in contact with the supporting plate and circular frame.The upper-end frame and lower-end frame are used to enhance the stiffness and strength of the upper and lower ends of the skin and are used to link the equipment bay with other bay sections, and their cross sections are both the "L" shape.The upper-end frame and the lower-end frame are in contact with the upper and lower ends of the skin, respectively.The overall finite element model of the equipment bay is shown in Figure 8.The model includes 4 materials: aluminum alloy, cast iron, CFRP (carbon fiber-reinforced polymer) tape, and aluminum honeycomb.Aluminum alloy and cast iron are isotropic materials, and the CFRP tape and aluminum honeycomb are 2-D orthotropic materials; their characteristics are shown in Table 1.
The parts of the equipment bay are linked by adhesive contact.In the finite element model, it is necessary to define the contact body and contact table.In the model, 13 contact bodies are defined in total: the portion of mounting panel that contacts with the circular frame is defined as Contact body 1, the portion of the mounting panel that contacts with the supporting plate is defined as Contact body 2, the portion of the inertial bracket that contacts with the skin is defined as Contact body 3, the portion of the inertial bracket that contacts with the circular frame is defined as Contact body 4, the portion of the skin that contacts with the upper-end frame is defined as Contact body 5, the portion of the skin that contacts with the lower-end frame is defined as Contact body 6 (the portion contacts also with the inertial bracket and supporting plate), the portion of the skin that contacts with the circular frame is defined as Contact body 7, the portion of the upper-end frame that contacts with the skin is defined as Contact body 8, the portion of the lower-end frame that contacts with the skin is defined as Contact body 9, the circular frame is defined as Contact body 10, the portion of the supporting plate that contacts with the mounting panel is defined as Contact body 11, the portion of the supporting plate that contacts with the skin is defined as Contact body 12, and the portion of the supporting plate that contacts with the circular frame is defined as Contact body 13.The two contact bodies in mutual contact are classified as the master and the slave.One contact body can be taken as the salve once only but as the master for n times.The contact table of the 13 contact bodies in mutual contact is shown in Table 2, where S represents the slave, M represents the

Vibration Modal Analysis of Equipment Bay
The boundary conditions of the modal analysis of equipment bay are as follows: all freedoms of the nodes on the horizontal surface of the upper-end frame are restricted and all freedoms of the nodes on the horizontal surface of the lower-end frame are restricted.The first modal frequency of the equipment bay obtained by the finite element modal analysis is 52.487Hz.The vibration shape is shown in Figure 9.The location of maximum vibration displacement is on the corner of the mounting panel, with the maximum value of 60.2 mm.Because the equipment is installed on the mounting panel and its excessive vibration displacement may cause damage to the equipment, it is necessary to reduce its vibration displacement.On the top surface of the inertial bracket, add three 20 kg masses, of which each represents the instrument with corresponding quality.The mass is defined with a 0D quality element, which is linked to the relevant nodes on the top surface by RBE3 (Rigid Body Element, Form3), as shown in Figure 10.With the masses added, the first modal frequency of the equipment bay is 28.816Hz, and the vibration shape is shown in Figure 11.The area with relatively high vibration displacement is mainly on the inertial bracket,   4 International Journal of Aerospace Engineering with the maximum value as 5.32 mm (being 8.8% of the maximum value before the mass is added).The vibration displacement of the two corners of the mounting panel is also relatively high.In order to reduce further the vibration displacement of the mounting panel, one supporting plate is added at the two sides of the mounting panel, so that the first modal frequency of the equipment bay becomes 29.615 Hz, with the vibration shape as shown in Figure 12.The area with relatively high vibration displacement is mainly on the inertial bracket, with the maximum value as 5.19 mm.In order to simulate more truly the vibration of the equipment bay in the rocket, extend the upper end and lower end of the skin by 200 mm (to reduce the influence of the boundary effect on the result).The first modal frequency of the extended equipment bay is 26.855Hz; the vibration shape is shown in Figure 13.The area with relatively high vibration displacement is mainly on the inertial bracket, with the maximum value as 5.38 mm.
From the foregoing finite element analysis, it is known that the vibration of the equipment bay with the mass mainly occurs on the inertial bracket and its surrounding area, and thus, the influence of the following parameters on the first modal frequency of the equipment bay is further studied: the bracket top surface (as shown in Figure 14         From the foregoing figures and data, it is known that T 1 has the maximum influence on the first modal frequency of the equipment bay, the frequency increases with the increasing T 1 , T 3 and T 5 have a relatively high influence on the first modal frequency of the equipment bay, the frequency increases as they increase, T 2 has a relatively low influence on the first modal frequency of the equipment bay, and T 4 has a minimum influence on the first modal frequency of the equipment bay.Thus, the vibration of the inertial bracket is simplified as the superimposition of two simple circumstances: Rod L is composed of Rod 1 and Rod 2. The shape of Rod L before the application of force is shown in Figure 20(a).When the stiffness of Rod 2 is very high and the stiffness of Rod 1 is relatively low, the shape of Rod L under the effect of Force F is shown in Figure 20(b), with Rod 2 not deformed and Rod 1 bending downward.When the stiffness of Rod 1 is very high and the stiffness of Rod 2 is relatively low, the deformation of Rod L under the effect of Force F is shown in Figure 20(c), with Rod 1 not deformed and Rod 2 bending.However, since the stiffness of Rod 1 and the stiffness of Rod 2 will not differ much, the deformation of Rod L under the effect of Force F is the composition of two circumstances, as is consistent with the vibration of the inertial bracket (Rod 1 is equivalent to the top surface and Rod 2 is equivalent to the side surface).The first modal deformation of the top surface and side surface of the inertial bracket is shown in Figure 21.The comparison of the top surface and side surface before and after deformation proves the result of such composition.
Optimize comprehensively T 1 , T 2 , T 3 , T 4 , and T 5 , with the optimizing target: under the condition that the first modal frequency of the equipment bay is more than 26 Hz, the weight of the equipment bay structure is the minimum.First, according to the influence of T 1 , T 2 , T 3 , T 4 , and T 5 on the first modal frequency of the equipment bay, adjust their changing range: the changing range of T 1 is 3-4.5 mm, the changing range of T 2 is 2-3.5 mm, the changing range of T 3 is 2-3 mm, the changing range of T 4 is 1-2 mm, and the changing range of T 5 is 1.2-2 mm.The result of comprehensive optimization is 3.2 mm for T 1 , 2 mm for T 2 , 2.1 mm for T 3 , 1 mm for T 4 , and 1.4 mm for T 5 , the weight of the equipment bay is 162.8 kg, decreasing by 4.9 kg as compared with the initial weight.

Results and Discussion
Before inertial bracket is added with mass, the vibration of the equipment bay occurs mainly on the mounting panel, and the maximum vibration displacement is 60.2 mm; after the inertial bracket is added with mass, the vibration of the equipment bay occurs mainly on the inertial bracket, and the maximum vibration displacement is 5.32 mm (being 8.8% of the maximum value before mass is added), and with the inertial bracket added with mass, the maximum vibration displacement of the equipment bay is significantly reduced.By adding two supporting plates on both sides of the mounting panel, it can reduce effectively the vibration displacement of the mounting panel.In the further study, it is observed that the influence of the inertial bracket top surface thickness on the first modal frequency of the equipment bay is the highest.The influence of the inertial bracket side surface thickness and stringer thickness on the first modal frequency of the equipment bay is relatively high.The influence of the inertial bracket rib thickness on the first modal frequency of the Figure 19: Influence of the stringer thickness on the first modal frequency of the equipment bay.International Journal of Aerospace Engineering equipment bay is relatively low, and the influence of the inertial bracket beam thickness on the first modal frequency of the equipment bay is the lowest.The vibration of the inertial bracket can be simplified as the deformation of Rod L (when the force is applied to Rod L).In engineering, the stiffness and vibration of the inertial bracket top surface (equivalent to Rod 1 of Rod L) is mostly studied, while the stiffness and vibration of the inertial bracket side surface (equivalent to Rod 2 of Rod L) is less studied.The analysis proves that studies on the stiffness and vibration of the top surface and side surface are all extremely important.The result of the comprehensive optimization of the equipment bay is 3.2 mm for T 1 , 2 mm for T 2 , 2.1 mm for T 3 , 1 mm for T 4 , and 1.4 mm for T 5 ; the weight of the equipment bay is 162.8 kg, decreasing by 4.9 kg as compared with the initial weight.

Conclusions
It can greatly reduce the vibration displacement of mounting panels when the inertial bracket is added with mass, and the vibration of the equipment bay with mass mainly occurs on the inertial bracket (without mass, the maximum vibration displacement occurs on the mounting panel).The top surface thickness of the inertial bracket has the maximum influence on the first modal frequency of the equipment bay, the stringer thickness and the side thickness of the inertial bracket have relatively high influence on the first modal frequency, the rib thickness of the inertial bracket has relatively low influence on the first modal frequency, and the beam thickness of the inertial bracket has the minimum influence on the first modal frequency.These results can be used to improve the equipment bay structure and decrease the weight of the equipment bay.

Figure 1 :Figure 2 :
Figure 1: Geometry of the equipment bay.

2
Cross section of II-type stringer

Figure 3 :Figure 4 :
Figure 3: Cross sections of I-type stringer and II-type stringer.

Figure 5 :
Figure 5: Finite element model of the inertial bracket.

Figure 6 :
Figure 6: Finite element model of the supporting plate.

Figure 7 :
Figure 7: Finite element model of the circular frame.
(a)) thickness T 1 , the bracket rib (as shown in Figure 14(b)) thickness T 2 , Lower-end frame Upper-end frame (a) Overall finite element model of the equipment bay (vertical view) Overall finite element model of the equipment bay (upward view)

Figure 8 :
Figure 8: Overall finite element model of the equipment bay.

Figure 9 :Figure 10 :Figure 11 :
Figure 9: First modal shape of the equipment bay.

Figure 12 :Figure 13 :
Figure 12: First modal shape of the equipment bay (with additional supporting plates).

Figure 15 :
Figure 15: Influence of the inertial bracket top surface thickness on the first modal frequency of the equipment bay.

Figure 16 :
Figure 16: Influence of the inertial bracket rib thickness on the first modal frequency of the equipment bay.

7
International Journal of Aerospace Engineering 1 mm, the frequency is 26.331Hz.When T 5 is 2 mm, the frequency is 27.128 Hz.

Figure 21 :
Figure 21: First modal deformation of the top surface and side surface of the inertial bracket.

Table 2 :
Contact table of 13 contact bodies.
Figure 17: Influence of the inertial bracket side surface thickness on the first modal frequency of the equipment bay.