Finite element modeling method for transient dynamics of reusable launch vehicle landing impact

Abstract

The present invention relates to a transient dynamic finite element modeling method for landing impact of a reusable launch vehicle, comprising the following steps: input of launch vehicle model related parameters; finite element modeling; model assembly connection; time step and mass scaling control; calculation result evaluation and calculation result evaluation post-processing; and formal calculation according to development needs using the final modified finite element model. This method is used to establish a nonlinear finite element analysis model of landing impact of a reusable launch vehicle, and the credibility of the calculation results is ensured by performing numerical stability checks and precision checks on the calculation results. Comparative analysis shows that this method is mature and reliable, can provide priori guidance for the design improvement of the vertical return landing recovery scheme of a reusable launch vehicle and the prediction of the dynamic environment, and has a high engineering application value.

Description

Technical Field

[0001] The invention belongs to the technical field of dynamic finite element modeling technology, and specifically relates to a transient dynamic finite element modeling method for landing impact of a reusable launch vehicle. Background Art

[0002] During the vertical return landing impact of a reusable launch vehicle, the rocket body and landing cushion system need to withstand a large impact load in a very short time. Whether they can withstand this transient impact dynamic environment is the key to the success of the launch vehicle's soft landing. Therefore, it is necessary to predict the rocket body landing impact dynamic environment in the early design stage in order to formulate the design and test conditions of the compartment and equipment.

[0003] The study of dynamics can be divided into two aspects: experimental methods and dynamic simulation. The experimental method is often not adopted in the early stage of design due to its disadvantages such as high cost and long cycle. In the early stage of design, dynamic simulation is generally used to simulate and conduct dynamic analysis of the landing impact of the launch vehicle under a variety of typical extreme working conditions to obtain the mechanical environment boundaries of each compartment and the single machine and equipment in the cabin of the launch vehicle in the landing and recovery mission profile. Typical dynamic simulation methods are mainly divided into the following categories: a) multi-rigid body dynamics simulation; b) rigid-flexible coupling dynamics simulation; c) full flexible body finite element simulation. The first two dynamic simulation methods are widely used, and the modeling is relatively simple. They are generally suitable for dynamic problems with low speed and small deformation. When there are many flexible bodies in the model, and it is necessary to pay attention to problems such as high-speed impact and large deformation of flexible bodies, the calculation results are quite different from the actual results, which have certain limitations. The fully flexible body finite element simulation method is used to replace the actual structure with finite elements, and the landing impact process of the reusable launch vehicle is fully flexible. Finite element modeling and simulation prediction can better simulate the contact, large deformation and large displacement problems in the landing impact process (involving material nonlinearity, contact nonlinearity and geometric nonlinearity). The credibility and accuracy of the calculation results are relatively the highest. However, this method has the highest modeling difficulty, large amount of calculation, time-consuming and labor-intensive, and low engineering application value. Summary of the invention

[0004] In view of the defects of existing technologies and the needs of engineering applications, this paper combines the structural characteristics of the reusable launch vehicle itself, the dynamic characteristics of the landing impact, and draws on the application cases of impact dynamics simulation in the aerospace field to explore a finite element modeling method for the transient dynamics of the landing impact of a reusable launch vehicle.

[0005] The present invention provides a finite element modeling method for transient dynamics of landing impact of a reusable launch vehicle, wherein the launch vehicle comprises a rocket body, a tail section and landing legs provided with a buffer connected in sequence, and comprises the following steps:

[0006] Input of launch vehicle model related parameters;

[0007] Finite element modeling, including:

[0008] Structural meshing, structural simulation, the body structure of the reusable launch vehicle is modeled by finite element in a three-dimensional + one-dimensional manner. The mesh model of the entire rocket is established based on the geometric data of the entire rocket and the mass center of mass parameters. The tail of the rocket including the tail section and landing legs is simulated using three-dimensional shell elements and solid elements, and the body above the tail is simulated using one-dimensional beam elements;

[0009] Buffer simulation: The geometric shape of the buffer is modeled by three-dimensional shell elements according to the actual structure, and the physical parameters of its materials are assigned according to the actual manufacturing materials. The buffer structure is equivalent to a theoretical analysis model, which is specifically a three-dimensional shell element model + column hinge + spring unit + damping unit. The three-dimensional shell element model is used to simulate the structural shape and the structural stiffness when it is not deformed, the column hinge is used to simulate the relative motion relationship, the spring unit is used to simulate the mechanical properties, and the damping unit is used to simulate the mechanical properties;

[0010] Impact ground simulation, which can be set to rigid ground or concrete ground according to analysis needs;

[0011] Model assembly connection, connection simulation, connection and assembly between the various structures of the launch vehicle are carried out according to the structural characteristics of the launch vehicle itself and the actual connection form. The connection inside the rocket body includes two categories: bolt connection and hinge connection. Rigid units are used to simulate the bolt connection between various structural parts, and hinges are used to simulate the relative motion relationship between various structural parts.

[0012] Model contact settings, contact simulation, use symmetric penalty function contact algorithm, do not define repeated or overlapping contacts at any time and under any circumstances, and there is no initial penetration and interference in the model;

[0013] Hourglass control parameter setting,The method adopted for hourglass control is: using uniform mesh division as much as possible, and combining,applying hourglass control to the specified structure separately and increasing the model stiffness locally;

[0014] Time step and quality scaling control:

[0015] The time step is determined by explicit integration, i.e., the central difference method. When solving a specific problem, the time step must be less than the critical time step Δtmin determined by the nature of the equation to be solved, i.e., the Courant condition, which requires that the overall mass increase percentage of the model should be controlled within 5%.

[0016] Evaluation of calculation results:

[0017] After completing the construction of the overall landing impact finite element model of the launch vehicle, a preliminary evaluation of the overall simulation calculation results is carried out. The specific steps are as follows:

[0018] Complete the numerical stability check to determine whether the numerical stability of the calculation results meets the requirements;

[0019] Check the accuracy of calculation results to determine whether the numerical accuracy of the calculation results meets the requirements;

[0020] Post-processing of calculation results evaluation,

[0021] If both numerical stability and numerical accuracy meet the requirements, the calculation results are considered to be credible, and the finite element model is used to carry out formal calculations according to the research needs;

[0022] If one of the numerical stability and numerical accuracy does not meet the requirements, the calculation result is judged to be unreliable. Then, according to the modeling process, the mesh quality, contact parameters, connection settings, hourglass control parameters, time step and mass scaling control parameters are checked one by one until the problem is finally located. After modifying the relevant parameters of the model, the calculation is resubmitted, and the process of numerical stability check and calculation result accuracy check is repeated until the numerical stability and accuracy of the final calculation result meet the requirements. The calculation result is judged to be credible, and the final modified finite element model is used to carry out formal calculations according to research and development needs.

[0023] Furthermore, in the connection simulation, the specific connection simulation content is as follows:

[0024] The rocket body includes an instrument compartment section provided with a single-machine mounting plate, an engine compartment section provided with an engine mount and an engine, and a rear transition section, wherein the rear transition section is connected to the tail section, and the landing legs provided with foot pads are connected to the outer wall of the tail section through upper and lower lugs, and rigid units are used to simulate bolt connections between the upper and lower lugs and the tail section, between the tail section and the rear transition section, between the engine and the engine mount, and between the single-machine mounting plate and the inner wall of the instrument compartment section of the rocket body;

[0025] The relative motion relationship between the landing legs and the upper and lower ears (pieces) is simulated using a rotary joint;

[0026] The relative motion relationship between the landing legs and the foot pads is simulated using a spherical joint.

[0027] Furthermore, the specific definitions of various contacts of the contact simulation are as follows: the whole arrow itself defines a global single-sided contact to simulate the contact between various structural parts inside the arrow body during the landing process. The contact includes all structural parts except the landing ground and the acceleration sensor.

[0028] A surface-to-surface contact pair is defined between the landing legs and the landing ground to simulate the dynamic contact between the legs and the ground.

[0029] Furthermore, the specific content of the symmetric penalty function contact algorithm is:

[0030] To simulate the dynamic contact and relative sliding between the launch vehicle and the ground, at each time step, we first check whether each slave node penetrates the main surface. If not, no processing is done on the node. If penetration occurs, a large interface contact force is introduced between the node and the penetrated main surface, and its magnitude is proportional to the penetration depth and the stiffness of the main surface.

[0031] Furthermore, the calculation formula of the time step in the time step and quality scaling control is:

[0032]

[0033] Where: L—characteristic length of the unit;

[0034] c — wave propagation speed,

[0035] α—A coefficient related to the element size (beam element, shell element, solid element, etc.).

[0036] The calculation time step is proportional to the element size and the root mean square of the material density, and inversely proportional to the root mean square of the elastic modulus.

[0037] Furthermore, the specific content of completing the numerical stability check is as follows:

[0038] Whether the calculation ends normally according to the set time;

[0039] Carefully observe the simulation deformation animation to see if there are any flying nodes;

[0040] When there is no external energy input, the total energy conservation is calculated and the total energy change should not exceed 3%.

[0041] Furthermore, the specific contents of the calculation result accuracy check are as follows:

[0042] The hourglass energy and interface contact slip energy should be much smaller than the internal energy, and the contact energy should be greater than zero;

[0043] Check the total mass added by the calculated model. The mass increase percentage should not exceed 3%. Check whether the mass increase of each component is normal.

[0044] Carefully check the simulation deformation animation to make sure there is no penetration between contacting parts;

[0045] Determine the mesh size to accurately simulate structural deformation;

[0046] Make sure the results are physically correct: cross-check nodal accelerations and section forces, internal energy, stresses, and strains;

[0047] Analyze the calculation stability and consistency of similar calculation conditions of the same model, and whether they are sensitive to certain parameters.

[0048] The method of the present invention comprehensively considers the structure of the landing buffer system, buffer flexibility, dynamic response characteristics and contact factors. Based on transient response analysis, a set of transient dynamic finite element modeling methods for reusable launch vehicle landing impact with a buffer soft landing design system is explored, and this method is used to establish a nonlinear finite element analysis model of reusable launch vehicle landing impact. The reliability of the calculation results is ensured by performing numerical stability and accuracy checks on the calculation results. Comparative analysis shows that this method is mature and reliable, and can provide prior guidance for the design improvement and dynamic environment prediction of the vertical return landing recovery of reusable launch vehicles, and has high engineering application value. BRIEF DESCRIPTION OF THE DRAWINGS

[0049] Figure 1 It is a schematic diagram of the process of the present invention;

[0050] FIG2( a ) is a schematic diagram of a three-dimensional model of a reusable launch vehicle;

[0051] Figure 2(b) is a schematic diagram of the three-dimensional model of the tail section and the landing main support leg and a schematic diagram of the output cross-sectional force position of the landing main support leg and the tail section;

[0052] Figure 3 It is a schematic diagram of the simplified finite element model of the buffer theory structure level;

[0053] Figure 4 It is a schematic diagram of the overall energy curve of the model;

[0054] Translation from top to bottom: external force work (gravity), hourglass energy (the line labeled 42 is close to the zero axis because its value is relatively small), internal energy, kinetic energy, the one starting with liding is the sliding interface energy, contact energy, buffer spring damping energy, total energy;

[0055] Figure 5(a) is a schematic diagram of the force output curve of the landing main leg section;

[0056] FIG5( b ) is a schematic diagram of the force curve of the arrow body cross section;

[0057] Figure 6 (a) is a stress cloud diagram of the tail section stress distribution;

[0058] Figure 6(b) is a schematic diagram of the unit stress time history condition at the maximum stress point of the tail section;

[0059] Among them, 1-rocket body, 11-instrument compartment, 12-attitude control compartment, 13-front transition section, 14-oxidizer fuel tank and inter-tank compartment, 15-rear transition section, 2-tail section, 21-upper support ear upper end surface cross-sectional position, 22-lower support ear upper end surface cross-sectional position, 3-landing main support leg, 31-upper support ear (piece), 32-lower support ear (piece), 33-landing main support leg cross-sectional position, 34-buffer, 35-foot pad, 311-partition, 312-outer tube, 313-inner tube, 301-column hinge, 302-spring unit + damping unit. DETAILED DESCRIPTION

[0060] like Figure 1 , which is a flow chart of a transient dynamic finite element modeling method for a reusable launch vehicle landing impact according to an embodiment of the present invention.

[0061] An embodiment of the present invention provides a finite element modeling method for transient dynamics of landing impact of a reusable launch vehicle, which uses pre-processing software to model and solve, and post-processing software to complete numerical stability checks and calculation result accuracy checks based on calculation data results.

[0062] The launch vehicle includes a rocket body, a tail section and a landing leg with a buffer connected in sequence. The landing leg is connected to the outer wall of the tail section. The modeling and solving using pre-processing software includes the following steps:

[0063] Input of relevant parameters of the launch vehicle model; relevant parameter input includes the overall parameters of the rocket, theoretical appearance drawing, 3D CAD model, load and boundary conditions;

[0064] Finite element modeling software is used for modeling and solving, and finite element modeling includes:

[0065] Structural meshing, structural simulation, the body structure of the reusable launch vehicle is modeled by finite element in a three-dimensional + one-dimensional manner. The mesh model of the entire rocket is established based on the geometric data of the entire rocket and the mass center of mass parameters. The tail of the rocket including the tail section and landing legs is simulated using three-dimensional shell elements and solid elements, and the body above the tail is simulated using one-dimensional beam elements;

[0066] FIG2(a) is a schematic diagram of a three-dimensional model of a reusable launch vehicle; FIG2(b) is a schematic diagram of a three-dimensional model of a tail section and landing legs; Figure 3 This is a schematic diagram of the simplified finite element model of the buffer;

[0067] Buffer simulation: The buffer is the main energy-absorbing structure during the landing impact of the launch vehicle. Accurately simulating the relative motion relationship and mechanical properties of the buffer during the landing process is the key to accurately predicting the landing impact dynamics environment.

[0068] The relative motion relationship between the upper sleeve (outer sleeve) and the lower sleeve (inner sleeve) of the buffer during landing can be simulated by an equivalent column hinge. The mechanical properties of the buffer itself are mainly reflected in the spring vibration reduction characteristics and the damping vibration reduction characteristics. Therefore, the physical model of the buffer can be considered to be a superposition of a spring oscillator model and a damping oscillator model. Finally, the buffer structure can be equivalent to a theoretical analysis model of a three-dimensional shell unit model (simulating the structural shape and structural stiffness when not deformed) + column hinge (simulating relative motion relationship) + spring unit (simulating mechanical properties) + damping unit (simulating mechanical properties), as shown in Figure 3. After comparison and verification, this equivalent simulation method can not only accurately reflect the motion relationship of the buffer during the landing impact process, but also accurately examine its mechanical properties during the landing impact process. Figure 3 The middle column hinge + spring unit + damping unit overlap together.

[0069] The geometric shape of the buffer is modeled with three-dimensional shell elements according to the actual structure, and its material physical parameters are assigned according to the actual manufacturing materials.

[0070] Impact ground simulation, which can be set to rigid ground or concrete ground according to analysis needs;

[0071] Model assembly and connection: connect and assemble the various structures of the launch vehicle according to the structural characteristics of the launch vehicle itself and the actual connection form;

[0072] Connection simulation: The connections inside the rocket body include bolt connections and hinges. For the impact of the launch vehicle landing at a low speed, it can be assumed that the bolts and nuts of the main structural connections will not deform during the collision. In short, rigid units are used to simulate the bolt connections between the various structural parts, and hinges are used to simulate the relative motion relationship between the various structural parts.

[0073] In the connection simulation, the specific connection simulation contents are as follows:

[0074] The rocket body sequentially comprises an instrument compartment section provided with a single-machine mounting plate, an attitude control compartment section, a front transition section, an oxidant-combustion compartment section, and a rear transition section, wherein the rear transition section is connected to the tail section, an engine mount and an engine are mounted in the tail section, and a landing leg provided with a foot pad is connected to the outer wall of the tail section through an upper support ear and a lower support ear, and rigid units are used to simulate bolt connections between the upper support ear and the lower support ear and the tail section, between the tail section and the rear transition section, between the engine and the engine mount, and between the single-machine mounting plate and the inner wall of the instrument compartment section of the rocket body;

[0075] The relative motion relationship between the landing legs and the upper and lower ears (pieces) is simulated using a rotary joint;

[0076] The relative motion relationship between the landing legs and the foot pads is simulated using a spherical joint.

[0077] Model contact settings, contact simulation, contact is one of the most complex issues in collision models. How to accurately simulate the contact problem between different objects directly determines the predictive ability of the simulation results. The difficulties in contact processing in collision analysis include: contact between metal materials and non-metallic materials; contact between edges and corners between complex parts. Therefore, a reasonable and efficient dynamic contact-interface algorithm must be used when modeling, and the corresponding specifications must be followed to ensure the stability of the contact and reasonable contact behavior.

[0078] Key points for contact simulation in reusable launch vehicle landing impact simulation modeling: Use symmetric penalty function contact algorithm, do not define repeated or overlapping contacts at any time and under any circumstances, and there is no initial penetration and interference in the model, because initial penetration may change the buckling mode of the structure, and initial interference may produce completely wrong results;

[0079] Commonly used contact types can be divided into three categories: single-sided contact, point-surface contact, and surface-surface contact.

[0080] The main contacts of the reusable launch vehicle landing impact simulation modeling are defined as:

[0081] The whole arrow defines a global single-surface contact to simulate the contact between the internal components of the arrow body during landing. This contact includes all components except the landing ground and acceleration sensor.

[0082] A surface-to-surface contact pair is defined between the landing legs and the landing ground to simulate the dynamic contact between the legs and the ground.

[0083] Specifically, the symmetric penalty function contact algorithm is as follows:

[0084] The symmetric penalty function contact algorithm can be used to more accurately simulate the dynamic contact and relative sliding between the launch vehicle and the ground. The basic analysis principle is: at each time step, first check whether each slave node penetrates the main surface. If not, no processing is performed on the slave node. If penetration occurs, a large interface contact force is introduced between the slave node and the penetrated main surface. Its magnitude is proportional to the penetration depth and the stiffness of the main surface, which is called the penalty function value. Its physical meaning is equivalent to placing a normal spring between the slave node and the penetrated main surface to limit the penetration of the slave node into the main surface. The so-called symmetric penalty function method refers to processing all the main nodes according to the above steps, and its algorithm is the same as that of the slave node. The symmetric penalty function method is simple to program, rarely excites the zero-energy mode of the grid, and has no noise. The size of the penalty function value is limited by stability. If obvious penetration is found in the calculation, the penalty function value can be enlarged or the time step can be reduced to adjust.

[0085] The finite element model of landing impact of reusable launch vehicle adopts symmetric penalty function contact algorithm. The calculation results show that the dynamic contact effect is good, the total interface slip energy is less than 5% of the total energy, and the calculation results are valid.

[0086] The hourglass mode is also called the zero-energy mode. In the process of solving the explicit dynamics analysis, in order to reduce the calculation cost, the single-point integration mode is usually used for shell elements and solid elements in the finite element modeling process. The solid elements and shell elements with a single integration point are prone to form zero-energy modes during the deformation process, which is mainly manifested as a natural oscillation that is much shorter than the cycle of all structural responses. The mesh deformation presents a jagged shape, which is called hourglass deformation. The hourglass deformation in the solution process must be effectively controlled to ensure the correctness of the analysis.

[0087] Generally speaking, when using reduced integration elements in an explicit dynamic analysis, a total hourglass energy not exceeding 10% of the total energy is considered an acceptable analysis result.

[0088] Hourglass control includes hourglass control parameter settings, such as local model stiffness. Specifically, hourglass control adopts the following methods: First, use uniform mesh division as much as possible. Generally speaking, overall mesh refinement will significantly reduce the impact of hourglass;

[0089] The second method is to apply hourglass control to the specified structure separately and increase the model stiffness locally. This is a commonly used and effective hourglass control method. The reusable launch vehicle landing impact finite element model mainly adopts the hourglass control method combining the first and second methods. After calculation verification, the overall hourglass control effect of the model is good, and the total hourglass energy is less than 3% of the total energy. The calculation result is valid.

[0090] Time step and quality scaling control:

[0091] The time length of the simulated landing process is the iteration step. The time step is determined by explicit integration, i.e., the central difference method. When solving a specific problem, the time step must be less than the critical time step Δtmin determined by the nature of the equation to be solved, i.e., the Courant condition, which requires that the overall mass increase percentage of the model should be controlled within 5%.

[0092] Specifically, the calculation formula of the time step in the time step and quality scaling control is:

[0093]

[0094] Where: L—characteristic length of the unit;

[0095] c — wave propagation speed,

[0096] α—A coefficient related to the element size (beam element, shell element, solid element, etc.).

[0097] The calculation time step is proportional to the element size and the root mean square of the material density, and inversely proportional to the root mean square of the elastic modulus.

[0098] The display dynamics analysis software will check all units when calculating the time step, and the calculation time step of the entire finite element model depends on the time step of the smallest unit. When the quality of the model is not good, especially when there are many small units, the calculation cost will increase exponentially. In order to reduce the amount of calculation, it is necessary to manually control the calculation time step. At this time, without changing the finite element model, increase the calculation time step. From the above time step calculation formula, it can be seen that the unit size, material density, or elastic modulus can be changed. For the initialized finite element calculation model, all unit sizes cannot be changed and the elastic modulus remains unchanged (the real elastic modulus needs to be used in the calculation), so the unit density can only be changed in the end, which will eventually lead to an increase in the overall mass of the model. This is why changing the time step is also called mass scaling.

[0099] Generally speaking, mass scaling is only applied to units that are smaller than the specified time step. The time step can be controlled manually. In the display dynamics analysis software, by specifying the actual calculation step, the program automatically increases the density of the corresponding unit. Although the use of mass scaling can significantly reduce the solution time, it should be noted that the increase in density of some units will lead to an increase in the overall mass of the model. When the inertial effect of the model needs to be considered, the percentage of increased mass should be controlled, that is, the time calculation time step cannot be set arbitrarily. In general, the percentage increase in the overall mass of the model should be controlled within 5%.

[0100] The final calculated mass increase percentage of the reusable launch vehicle landing impact finite element model is 0.35%, which shows that the time step of the calculation model is set reasonably and the mass scaling level is well controlled.

[0101] Evaluation of calculation results:

[0102] After completing the construction of the overall landing impact finite element model of the launch vehicle, conduct a preliminary evaluation of the overall simulation calculation results, and use CAE post-processing software to complete the numerical stability check and calculation result accuracy check based on the calculation data results to ensure the credibility of the calculation results. The specific steps are to set up at least one typical calculation condition based on the project development background; conduct a preliminary check on the calculation file under the typical condition, complete the numerical stability check, and determine whether the numerical stability of the calculation results meets the requirements;

[0103] Specifically, the specific contents of completing the numerical stability check are as follows:

[0104] Whether the calculation ends normally according to the set time;

[0105] Carefully observe the simulation deformation animation to see if there are any flying nodes;

[0106] When there is no external energy input, the total energy conservation is calculated and the total energy change should not exceed 3%. Figure 4 , Figure 4 It is a graph made by CAE post-processing software based on the calculation data results. Figure 4 The curve in the figure is the curve of energy change over time. The order from top to bottom in the box is: 41-external work (gravity), 42-hourglass energy (the line is close to the zero axis, i.e. the horizontal axis, because the value is relatively small), 43-internal energy, 44-kinetic energy, 45-the one starting with liding is the sliding interface energy, i.e. the contact energy, 46-buffer spring damping energy, 47-total energy; it can be seen from the figure that the total energy has almost no change after 150ms, which meets the requirement that the total energy change should not exceed 3%.

[0107] Check the accuracy of calculation results to determine whether the numerical accuracy of the calculation results meets the requirements;

[0108] Specifically, the specific contents of the calculation result accuracy check are as follows:

[0109] The hourglass energy and the interface contact slip energy should be much smaller than the internal energy, and the contact energy should be greater than zero (see Figure 4 , Figure 4 The number starting with 45-liding is the sliding interface energy (i.e. contact energy);

[0110] Check the total mass added to the calculated model. The percentage of increased mass should not exceed 3%. The model calculation quality check is shown in Table 1. Mass scaling, i.e., initial mass increase and final mass increase, is related to the time step setting, which is the issue of mass scaling.

[0111] Check whether the mass increase of each component is normal;

[0112] Table 1

[0113] Contents of Model Calculation Quality Inspection Check Data Values Remarks Model Calculation Quality 6004.1 kg Initial Mass Increase 63.27 kg Percentage of Initial Mass Increase 1.054％ Final Mass Increase 68.94 kg Percentage of Final Mass Increase 1.148％

[0114] Carefully check the simulated deformation animation to make sure there is no penetration between contacting parts; in the CAE post-processing software, you can manually judge and set the deformation magnification factor, which is very easy to identify.

[0115] Determining the size of the mesh can accurately simulate structural deformation; from the perspective of the entire system, the size of the mesh is determined according to the size of the specific component. The smaller the size of the component, the smaller the mesh size.

[0116] Determine that the calculation results are consistent with physical phenomena: cross-check the node acceleration and section force (see Figure 5 (a) main leg 51a-X1 section force, 52a-X2 section force, 53a-Y1 ​​section force, 54a-Y2 section force, X1 and X2 represent two main legs symmetrical with the axis of the arrow body, Y1 and Y2 represent the other two main legs symmetrical with the axis of the arrow body; Figure 5 (b) 51b-section force near the upper ear of the arrow body, 52b-section force near the lower ear of the arrow body), internal energy, stress (see Figure 6 (a) stress distribution of the tail section of the arrow body, and Figure 6 (b) unit stress time history condition at the maximum stress point of the tail section of the arrow body) and strain;

[0117] Analyze the calculation stability and consistency of similar calculation conditions of the same model, and judge the stability and consistency by comparing the calculation results of similar calculation conditions; analyze whether it is sensitive to certain parameters, such as the friction coefficient, change the value of the friction coefficient, and compare the changes in the corresponding calculation results to judge whether it is sensitive;

[0118] Post-processing of calculation results evaluation,

[0119] If both numerical stability and numerical accuracy meet the requirements, the calculation results are considered to be credible, and the finite element model is used to carry out formal calculations according to the research needs;

[0120] If one of the numerical stability and numerical accuracy does not meet the requirements, the calculation result is judged to be unreliable. Then, according to the modeling process, the mesh quality, contact parameters, connection settings, hourglass control parameters, time step and mass scaling control parameters are checked one by one until the problem is finally located. After modifying the relevant parameters of the model, the calculation is resubmitted, and the process of numerical stability check and calculation result accuracy check is repeated until the numerical stability and accuracy of the final calculation result meet the requirements. The calculation result is judged to be credible, and the final modified finite element model is used to carry out formal calculations according to research and development needs.

Claims

1. A finite element modeling method for transient dynamics of landing impact of a reusable launch vehicle, wherein the launch vehicle comprises a rocket body, a tail section and landing legs provided with a buffer connected in sequence, Features The following steps are included Input of launch vehicle model related parameters; Finite element modeling, including: Structural meshing, structural simulation, the rocket body structure of the reusable launch vehicle is modeled by finite element in three-dimensional and one-dimensional ways. The full rocket mesh model is established according to the full rocket geometry data and mass center parameters. The rocket tail including the tail section and landing legs is simulated by three-dimensional shell elements and solid elements, and the rocket body above the tail is simulated by one-dimensional beam elements. Buffer simulation: The geometric shape of the buffer is modeled by three-dimensional shell elements according to the actual structure, and the physical parameters of its materials are assigned according to the actual manufacturing materials. The buffer structure is equivalent to a theoretical analysis model. The theoretical analysis model is specifically a three-dimensional shell element model, a column hinge, a spring unit and a damping unit. The three-dimensional shell element model is used to simulate the structural shape and the structural stiffness when it is not deformed, the column hinge is used to simulate the relative motion relationship, the spring unit is used to simulate the mechanical properties, and the damping unit is used to simulate the mechanical properties; Impact ground simulation, which can be set to rigid ground or concrete ground according to analysis needs; Model assembly connection, connection simulation, connection and assembly between the various structures of the launch vehicle are carried out according to the structural characteristics of the launch vehicle itself and the actual connection form. The connection inside the rocket body includes two categories: bolt connection and hinge connection. Rigid units are used to simulate the bolt connection between various structural parts, and hinges are used to simulate the relative motion relationship between various structural parts. Model contact settings, contact simulation, use symmetric penalty function contact algorithm, do not define repeated or overlapping contacts, and there is no initial penetration and interference in the model; Hourglass control parameter setting,The method used for hourglass control is: using uniform mesh division, and combining,applying hourglass control to the specified structure separately and increasing the model stiffness locally; Time step and quality scaling control: The time step is determined by explicit integration, i.e., the central difference method. When solving a specific problem, the time step must be less than the critical time step Δtmin determined by the nature of the equation to be solved, i.e., the Courant condition, which requires that the overall mass increase percentage of the model should be controlled within 5%. Evaluation of calculation results: After completing the construction of the overall landing impact finite element model of the launch vehicle, a preliminary evaluation of the overall simulation calculation results is carried out. The specific steps are to complete the numerical stability check to determine whether the numerical stability of the calculation results meets the requirements; Check the accuracy of calculation results to determine whether the numerical accuracy of the calculation results meets the requirements; Post-processing of calculation results evaluation, If both numerical stability and numerical accuracy meet the requirements, the calculation results are considered to be credible, and the finite element model is used to carry out formal calculations according to the research needs; If one of the numerical stability and numerical accuracy does not meet the requirements, the calculation result is judged to be unreliable. Then, according to the modeling process, the mesh quality, contact parameters, connection settings, hourglass control parameters, time step and mass scaling control parameters are checked one by one until the problem is finally located. After modifying the relevant parameters of the model, the calculation is resubmitted, and the process of numerical stability check and calculation result accuracy check is repeated until the numerical stability and accuracy of the final calculation result meet the requirements. The calculation result is judged to be credible, and the final modified finite element model is used to carry out formal calculations according to research and development needs.

2. The dynamic finite element modeling method according to claim 1, It is characterized in that In the connection simulation, the specific connection simulation contents are as follows: The rocket body includes an instrument compartment section provided with a single-machine mounting plate, an engine compartment section provided with an engine mount and an engine, and a rear transition section, wherein the rear transition section is connected to the tail section, and a landing leg provided with a foot pad is connected to the outer wall of the tail section through an upper support ear and a lower support ear, and rigid units are used to simulate bolt connections between the upper support ear, the lower support ear and the tail section, between the tail section and the rear transition section, between the engine and the engine mount, and between the single-machine mounting plate and the inner wall of the instrument compartment section of the rocket body; The relative motion relationship between the landing legs and the upper and lower lugs is simulated using a rotary joint; The relative motion relationship between the landing legs and the foot pads is simulated using a spherical joint.

3. The dynamic finite element modeling method according to claim 1, It is characterized in that The specific definitions of various contacts in the contact simulation are as follows: the whole arrow itself defines a global single-sided contact to simulate the contact between the internal structural parts of the arrow body during the landing process. This contact includes all structural parts except the landing ground and the acceleration sensor. A surface-to-surface contact pair is defined between the landing legs and the landing ground to simulate the dynamic contact between the legs and the ground.

4. The dynamic finite element modeling method according to claim 3, It is characterized in that The specific content of the symmetric penalty function contact algorithm is: To simulate the dynamic contact and relative sliding between the launch vehicle and the ground, at each time step, we first check whether each slave node penetrates the main surface. If not, no processing is done on the slave node at that location. If penetration occurs, a larger interface contact force is introduced between the slave node and the penetrated main surface, and its magnitude is proportional to the penetration depth and the stiffness of the main surface.

5. The dynamic finite element modeling method according to claim 1, It is characterized in that The calculation formula of the time step and the time step in the quality scaling control is: Where: L—characteristic length of the unit; c — wave propagation speed, α—Coefficient related to the unit size. The unit is a beam unit, a shell unit, or a solid unit. The calculation time step is proportional to the unit size and the root mean square of the material density, and inversely proportional to the root mean square of the elastic modulus.

6. The dynamic finite element modeling method according to claim 1, Features The specific contents of completing the numerical stability check are as follows: Whether the calculation ends normally according to the set time; Carefully observe the simulation deformation animation to see if there are any flying nodes; When there is no external energy input, the total energy conservation is calculated and the total energy change should not exceed 3%.

7. The dynamic finite element modeling method according to claim 1, Features The specific contents of the calculation result accuracy check are as follows: The hourglass energy and interface contact slip energy should be much smaller than the internal energy, and the contact energy should be greater than zero; Check the total mass added by the calculated model. The mass increase percentage should not exceed 3%. Check whether the mass increase of each component is normal. Carefully check the simulation deformation animation to make sure there is no penetration between contacting parts; Determine the mesh size to accurately simulate structural deformation; Make sure the results are physically correct: cross-check nodal accelerations and section forces, internal energy, stresses, and strains; Analyze the calculation stability and consistency of similar calculation conditions of the same model, and whether they are sensitive to certain parameters.

Images