Honeycomb sandwich panel finite element fine modeling method and system for strength check

Abstract

The invention provides a honeycomb sandwich panel finite element fine modeling method and system for strength checking, and the method comprises the steps: building a honeycomb sandwich panel fine finite element model, the step of establishing the fine finite element model of the honeycomb sandwich panel comprises the steps of analyzing the composition and stress characteristics of the honeycomb sandwich panel, formulating a failure mode and a modeling criterion, simplifying and cleaning a three-dimensional geometric model, simulating and meshing the simplified three-dimensional geometric model, and simulating the cementing assembly relation of each element of the honeycomb sandwich panel. Material parameters are obtained, physical attributes are created, and boundary conditions are simulated; solving and calculating the fine finite element model of the honeycomb sandwich panel; and checking and indicating the strength according to a strength criterion. According to the method, the fine finite element model of the honeycomb sandwich plate is established based on the product composition and stress characteristics, and the technical effects of highly restoring the actual product technical state, accurately predicting and evaluating the strength characteristics and the failure mode of the honeycomb sandwich plate and guiding spacecraft structure design and weight reduction work are achieved.

Description

Technical Field

[0001] This invention relates to the field of spacecraft structure technology, specifically to a finite element fine modeling method and system for honeycomb sandwich panels oriented towards strength verification. Background Technology

[0002] In spacecraft structural design, honeycomb sandwich panels are widely used in various space structures due to their lightweight and high strength properties. To ensure that honeycomb sandwich panels meet strength requirements in actual working environments, accurate strength verification is essential. The finite element method, as an important tool in modern computational mechanics, plays a crucial role in the strength analysis and prediction of honeycomb sandwich panels.

[0003] In the prior art, patent document CN202011262400.1 discloses a finite element modeling method for honeycomb sandwich panels, which equates the honeycomb core to an orthogonal anisotropic homogeneous plate and the skin to an isotropic plate. This method is suitable for the study of honeycomb sandwich panel raw material level, but the model ignores components such as embedded frames, foaming adhesive, and scraping sheets, as well as their connection relationships, resulting in a significant difference from the honeycomb sandwich panel structure products actually used in aerospace engineering.

[0004] Patent document CN202210048940.2 provides a method and system for rapid extraction of shell simulation models based on satellite cabin structure, but this method focuses on improving modeling efficiency by using digital means, without making improvements to the model itself or the calculation accuracy.

[0005] Patent document CN202210650144.6 proposes a system-level method for designing honeycomb sandwich panels, which automatically creates high-quality mesh elements. However, this method focuses on rapidly generating finite element meshes for the honeycomb core and does not solve the problem of connection and assembly between the honeycomb core and other components.

[0006] Patent document CN202410265159.X proposes a method for calculating the vibration response of a honeycomb sandwich panel. It determines the free vibration equation based on the strain energy and kinetic energy of the upper and lower fiber layers and the honeycomb layer, and then calculates the vibration response. However, this method focuses on the mathematical modeling and equation derivation of the vibration problem of the honeycomb sandwich panel, and belongs to basic theoretical research.

[0007] Patent document CN201210035017.1 proposes a method for calculating the natural frequency of a honeycomb sandwich structure. This method involves measuring the bending stiffness of the honeycomb sandwich panel and the shear modulus of the core layer, then substituting these measurements into a formula to calculate the natural frequency. However, this method is not suitable for strength verification of honeycomb sandwich panels.

[0008] In summary, given the problems of the existing technologies, researching a fine finite element modeling method and system for strength verification of honeycomb sandwich panels has become a critical task that urgently needs to be addressed. Summary of the Invention

[0009] To address the shortcomings of existing technologies, the purpose of this invention is to provide a finite element fine modeling method and system for strength verification of honeycomb sandwich panels.

[0010] The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification provided by the present invention includes the following steps: Step S1, establishing a fine finite element model of the honeycomb sandwich panel based on its composition and stress characteristics; Step S2, solving and calculating the fine finite element model of the honeycomb sandwich panel; Step S3, performing strength verification prediction based on strength criteria.

[0011] Preferably, a refined finite element model of the honeycomb sandwich panel is established based on its composition and stress characteristics, including: Step S11, analyzing the composition and stress characteristics of the honeycomb sandwich panel; Step S12, formulating failure modes and modeling criteria based on the stress characteristics of the honeycomb sandwich panel; Step S13, simplifying and cleaning the three-dimensional geometric model of the honeycomb sandwich panel; Step S14, simulating and meshing the simplified three-dimensional geometric model; Step S15, simulating the adhesive assembly relationship of each component of the honeycomb sandwich panel; Step S16, using the material parameters of each component measured in the furnace test piece, obtaining material modulus and strength data, and assigning them to each component to create physical properties; Step S17, substituting the refined finite element model of the honeycomb sandwich panel into the finite element model of the entire spacecraft, connecting it with the structural components of adjacent honeycomb sandwich panels, accurately simulating the boundary conditions of the refined finite element model of the honeycomb sandwich panel, and applying displacement constraints and loads for calculation under the finite element model of the entire spacecraft.

[0012] Preferably, the calculation of the fine finite element model of the honeycomb sandwich panel includes: performing buckling analysis on the fine finite element model of the honeycomb sandwich panel to obtain the critical load coefficient, performing static analysis to obtain the static stress in use, performing frequency response analysis to obtain the dynamic stress in use, and calculating the safety margin based on the stress in use.

[0013] Preferably, the strength verification prediction is performed according to the strength criteria, including: the strength criteria include the critical load factor criterion, the allowable stress criterion, and the safety margin criterion; the critical load factor criterion is that the critical load factor is greater than 2; the allowable stress criterion includes that the stress used for aluminum alloy materials is less than the allowable stress of 255 MPa, the stress used for magnesium alloy materials is less than the allowable stress of 120 MPa, the shear stress used for foamed adhesive is less than the allowable stress of 3.5 MPa, and the stress used for quasi-isotropic carbon fiber materials is less than the allowable stress of 450 MPa; the safety margin criterion includes that the safety margin for carbon fiber composite materials is greater than 0.25, and the safety margin for metallic materials is greater than 0.

[0014] Preferably, the analysis of the composition and stress characteristics of the honeycomb sandwich panel includes: the honeycomb sandwich panel is a composite material structure product composed of upper and lower panels, honeycomb core, embedded parts, embedded frames, reinforcing sheets and scraping sheets, which are bonded together by adhesive; the stress characteristics of the honeycomb sandwich panel are that the upper and lower panels, embedded frames, reinforcing sheets and scraping sheets bear in-plane tensile force, compressive force and bending moment, while the honeycomb core and embedded parts bear transverse shear force.

[0015] Preferably, based on the stress characteristics of the honeycomb sandwich panel, failure modes and modeling criteria are formulated, including: the failure modes of the honeycomb sandwich panel include overall instability, local instability of the panel, local instability of the honeycomb core, shear failure of the honeycomb core, crushing failure of the honeycomb core, plastic deformation of the panel, and cracking of the foam adhesive; the modeling criteria include accurately simulating each load-bearing component and the bonding assembly relationship, reflecting the stress transmission characteristics of the product, and comprehensively predicting the failure modes of the honeycomb sandwich panel.

[0016] Preferably, the simplification and cleaning of the three-dimensional geometric model of the honeycomb sandwich panel includes: using three-dimensional design software to reasonably simplify and clean the three-dimensional geometric model of the honeycomb sandwich panel, including deleting only the secondary geometric features of each load-bearing element and retaining the main geometric features of each load-bearing element, wherein the secondary geometric features include small openings and rounded corners on each load-bearing element; cutting the panel and honeycomb core according to the geometric and material properties of the three-dimensional model, and supplementing the pre-embedded parts and the foam around the embedded frame.

[0017] Preferably, the simplified three-dimensional geometric model is simulated and meshed, including: importing the simplified and cleaned three-dimensional geometric model into finite element simulation analysis software, selecting appropriate elements for simulation based on the geometric characteristics and stress characteristics of each component, and independently performing mesh generation. Among them, the upper and lower panels, reinforcing plates, and embedded frames are typical thin-walled structures, which are simulated using triangular and quadrilateral shell elements, while the honeycomb core, embedded parts, foam adhesive, and scraper are simulated using pentahedral and hexahedral solid elements.

[0018] Preferably, simulating the adhesive assembly relationship of each component of the honeycomb sandwich panel includes: simulating the adhesive assembly relationship of each component of the honeycomb sandwich panel using an adhesive contact method, creating interface units on the contact boundaries of each component, calculating the contact stiffness matrix based on the penalty factor and assigning it to the interface units, and then bonding each component together.

[0019] This invention also provides a finite element fine modeling system for honeycomb sandwich panels oriented towards strength verification. This system can be implemented by executing the steps of the finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification. That is, those skilled in the art can understand the finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification as a preferred embodiment of the finite element fine modeling system for honeycomb sandwich panels oriented towards strength verification. The system includes: The fine modeling module establishes a fine finite element model of the honeycomb sandwich panel based on its composition and stress characteristics. The solution calculation module performs solution calculations on the fine finite element model of the honeycomb sandwich panel; The strength verification prediction module performs strength verification prediction based on the strength criteria.

[0020] Compared with the prior art, the present invention has the following beneficial effects: Honeycomb sandwich panels, widely used in aerospace engineering, are lightweight composite material structures with complex composition and anisotropy. In practical applications, these panels face complex boundary conditions and numerous failure modes, making strength characteristic analysis and prediction a challenge in spacecraft design. This invention proposes a universally applicable finite element modeling method that can accurately predict and evaluate the strength characteristics of honeycomb sandwich panels, guiding spacecraft structural design and weight reduction efforts.

[0021] Traditional finite element models for honeycomb sandwich panels are overly simplified, neglecting load-bearing components such as embedded parts and expanding foam. This results in significant discrepancies between the model and the actual product's technical condition, leading to coarse analysis results, large errors in strength verification, and inaccurate failure mode predictions. The refined finite element modeling method proposed in this invention considers the actual composition of the honeycomb sandwich panel product, ensuring that all load-bearing components are represented in the finite element model. The model highly replicates the actual product's technical condition, resulting in reliable analysis results and accurate failure mode predictions. Attached Figure Description

[0022] Other features, objects, and advantages of the present invention will become more apparent from the following detailed description of non-limiting embodiments with reference to the accompanying drawings: Figure 1 This is a flowchart of a finite element fine modeling method for honeycomb sandwich panels for strength verification, provided in an embodiment of the present invention.

[0023] Figure 2a A three-dimensional geometric model and composition diagram of a spacecraft honeycomb sandwich panel provided for an embodiment of the present invention.

[0024] Figure 2b A three-dimensional geometric model and composition diagram of a spacecraft honeycomb sandwich panel with a hidden panel provided for an embodiment of the present invention.

[0025] Figure 3 Fine finite element model of spacecraft honeycomb sandwich panel provided in embodiments of the present invention Figure 4 The finite element model of the entire spacecraft, including a fine finite element model of a honeycomb sandwich panel, is provided for embodiments of the present invention.

[0026] Figure 5 The buckling contour map provided for an embodiment of the present invention.

[0027] Figure 6 The static stress cloud diagram provided for the embodiments of the present invention.

[0028] Figure 7 The dynamic stress cloud diagram provided for the embodiments of the present invention.

[0029] Figure 8 Safety margin cloud map provided for embodiments of the present invention.

[0030] icon: 1-Top panel; 2-Reinforcing sheet; 3-Scraping blade; 4-Honeycomb core; 5-Embedded frame; 6-Embedded parts; 7-Expanding foam; 8- Bottom panel. Detailed Implementation

[0031] The present invention will now be described in detail with reference to specific embodiments. These embodiments will help those skilled in the art to further understand the present invention, but do not limit the invention in any way. It should be noted that those skilled in the art can make several changes and improvements without departing from the concept of the present invention. These all fall within the protection scope of the present invention.

[0032] Figure 1 A flowchart illustrating a finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification, as provided in an embodiment of the present invention, is shown below. Figure 1 As shown, it includes three steps: detailed modeling, solution calculation, and verification prediction.

[0033] Step 1: Detailed modeling, including the following sub-steps: S101, Analysis of product composition and stress characteristics.

[0034] Specifically, the spacecraft honeycomb sandwich panel is a typical composite material structure product, as shown in Figure 2. It consists of components such as the upper panel 1, reinforcing sheet 2, scraper 3, honeycomb core 4, embedded frame 5, pre-embedded part 6, foam adhesive 7, and lower panel 8. The overall thickness of the panel is 15mm~30mm. The upper panel 1 and lower panel 8 are usually made of M55J carbon fiber composite material or aluminum alloy material with a thickness of 0.3mm. The reinforcing sheet 2 is made of T800 carbon fiber composite material with a thickness of 0.2mm~0.8mm. The scraper 3 is a 2mm aluminum alloy sheet. The honeycomb core 4 is a regular hexagonal aluminum alloy foil with a side length of 5mm, a wall thickness of 0.03mm, and a height of 14.1mm~29.1mm. The embedded frame 5 is a carbon fiber or magnesium alloy frame with a wall thickness of 1.5mm. The embedded part 6 is an aluminum alloy or magnesium alloy cylinder with a diameter of Φ20mm and a height of 14.1mm~29.1mm. The foaming adhesive 7 is J78D2 adhesive. All components are bonded together with adhesive.

[0035] The stress characteristics of honeycomb sandwich panels are that the upper and lower panels, embedded frames, reinforcing plates and scraping plates mainly bear in-plane tensile force, compressive force and bending moment, while the honeycomb core and embedded parts mainly bear transverse shear force.

[0036] S102, Failure Mode and Modeling Criteria Development.

[0037] Specifically, the main failure modes of honeycomb sandwich panels include overall instability, local instability of the panel, local instability of the honeycomb core, shear and crushing failure of the honeycomb core, plastic deformation of the panel, and cracking of the foam adhesive. The criteria for detailed modeling are to ensure that the model highly replicates the actual technical condition of the product, accurately simulates the various load-bearing components and adhesive bonding relationships, reflects the product's stress transmission characteristics, and comprehensively predicts all of the aforementioned failure modes.

[0038] S103, 3D geometric model simplification and cleanup.

[0039] Specifically, the 3D geometric model of the honeycomb sandwich panel is simplified and cleaned using 3D design software (such as PROE). Only minor geometric features such as small openings and rounded corners on each load-bearing element are deleted, while the main geometric features of each load-bearing element are retained. The panel and honeycomb core are cut according to the geometric and material properties, and the pre-embedded parts and foam around the frame are added.

[0040] S104, Component Simulation and Mesh Generation.

[0041] The simplified and cleaned 3D geometric model of S103 was imported into finite element simulation analysis software (such as Patran / Nastran). Appropriate elements were selected for simulation based on the geometric characteristics and stress features of each component, and mesh generation was performed. The upper and lower panels, reinforcing plates, and embedded frames, being typical thin-walled structures, were simulated using triangular and quadrilateral shell elements (mesh size 10mm~50mm), while the honeycomb core, embedded parts, foam adhesive, and scraper blades were simulated using pentahedral and hexahedral solid elements (mesh size 1mm~5mm).

[0042] Through the above steps, the simplified and cleaned 3D geometric model is imported into the finite element modeling software. Appropriate elements are selected to simulate each load-bearing element independently without considering the coordination of element types and sizes. The finite element mesh generation is free and flexible, enabling efficient and rapid modeling.

[0043] S105, Simulation of component bonding assembly relationship.

[0044] Since the honeycomb sandwich panel has many components, and the element types and sizes of each component are different, the finite element mesh cannot be coordinated and unified. Therefore, the glued contact method is used to simulate the glued assembly relationship. That is, interface elements are created on the contact boundary of each component, and the contact stiffness matrix is ​​calculated based on the penalty factor and then assigned to the interface element to glue the components together.

[0045] Through the above steps, the units of each load-bearing element are connected by adhesive contact method, restoring the adhesive assembly relationship between each load-bearing element of the honeycomb sandwich panel, and the product's stress and force transmission path are accurately simulated.

[0046] S106, Material Parameter Acquisition and Property Creation.

[0047] Specifically, material parameters of each component are measured using in-furnace specimens to obtain data such as material modulus and strength, which are then assigned to each component to create physical properties. A detailed finite element model of the honeycomb sandwich panel is shown below. Figure 3 As shown.

[0048] S107, Boundary condition simulation.

[0049] Specifically, the refined finite element model of the honeycomb sandwich panel is substituted into the overall finite element model of the spacecraft, connected with adjacent structural components such as honeycomb sandwich panels, to accurately simulate the boundary conditions of the refined finite element model of the honeycomb sandwich panel. Displacement constraints and loads are then applied to the overall spacecraft model for calculation. The overall finite element model of the spacecraft containing the refined finite element model of the honeycomb sandwich panel is shown below. Figure 4 As shown.

[0050] By substituting the detailed model of the honeycomb sandwich panel into the overall finite element model of the spacecraft through the above steps, and connecting it with the adjacent structural components, the analysis and calculation are performed in the state of the whole spacecraft rather than in the state of a single panel, making the boundary condition simulation more reasonable.

[0051] Step 2: Solve the calculation.

[0052] Specifically, in order to comprehensively verify the strength of the honeycomb sandwich panel, buckling analysis is carried out to obtain the critical load coefficient, static analysis is carried out to obtain the static stress in use, frequency response analysis is carried out to obtain the dynamic stress in use, and then the safety margin is calculated based on the stress in use. Figure 5 For the curved cloud pattern, Figure 6 This is a static stress contour map. Figure 7 For dynamic stress contour plot, Figure 8 For safety margin cloud map.

[0053] Step 3: Verify the prediction.

[0054] Specifically, criteria such as critical load factor, allowable stress, and safety margin are proposed to provide a comprehensive and complete strength verification of honeycomb sandwich panels.

[0055] Among them, the critical load factor criterion is: critical load factor > 2; Allowable stress criteria: The service stress (Mises) of aluminum alloy materials is less than the allowable stress of 255 MPa; the service stress (Mises) of magnesium alloy materials is less than the allowable stress of 120 MPa; the service shear stress of foam is less than the allowable stress of 3.5 MPa; and the service stress (Mises) of quasi-isotropic carbon fiber materials is less than the allowable stress of 450 MPa.

[0056] Safety margin criteria: Safety margin for carbon fiber composites > 0.25, safety margin for metallic materials > 0.

[0057] This invention also provides a finite element fine modeling system for honeycomb sandwich panels oriented towards strength verification. This system can be implemented by executing the steps of the finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification. That is, those skilled in the art can understand the finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification as a preferred embodiment of the finite element fine modeling system for honeycomb sandwich panels oriented towards strength verification. The system includes: The fine modeling module establishes a fine finite element model of the honeycomb sandwich panel based on its composition and stress characteristics. The solution calculation module solves and calculates the fine finite element model of the honeycomb sandwich panel; The strength verification prediction module performs strength verification prediction based on the strength criteria.

[0058] Those skilled in the art will understand that, besides implementing the system and its various devices, modules, and units provided by this invention in the form of purely computer-readable program code, the same functions can be achieved entirely through logical programming of the method steps, making the system and its various devices, modules, and units of this invention function in the form of logic gates, switches, application-specific integrated circuits, programmable logic controllers, and embedded microcontrollers. Therefore, the system and its various devices, modules, and units provided by this invention can be considered as a hardware component, and the devices, modules, and units included therein for implementing various functions can also be considered as structures within the hardware component; alternatively, the devices, modules, and units for implementing various functions can be considered as both software modules implementing the method and structures within the hardware component.

[0059] Specific embodiments of the present invention have been described above. It should be understood that the present invention is not limited to the specific embodiments described above, and those skilled in the art can make various changes or modifications within the scope of the claims, which do not affect the essence of the present invention. Unless otherwise specified, the embodiments and features described in this application can be arbitrarily combined with each other.

Claims

1. A finite element fine modeling method for honeycomb sandwich panels for strength verification, characterized in that, include: Step S1: Based on the composition and stress characteristics of the honeycomb sandwich panel, establish a refined finite element model of the honeycomb sandwich panel; Step S2: Solve the fine finite element model of the honeycomb sandwich panel; Step S3: Perform strength verification and prediction based on strength criteria.

2. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 1, characterized in that, Based on the composition and stress characteristics of the honeycomb sandwich panel, a refined finite element model of the honeycomb sandwich panel is established, including: Step S11: Analyze the composition and stress characteristics of the honeycomb sandwich panel; Step S12: Based on the stress characteristics of the honeycomb sandwich panel, formulate failure modes and modeling criteria; Step S13: Simplify and clean up the three-dimensional geometric model of the honeycomb sandwich panel; Step S14: Simulate and mesh the simplified 3D geometric model; Step S15: Simulate the adhesive bonding assembly relationship of each component of the honeycomb sandwich panel; Step S16: Measure the material parameters of each component using the furnace-fed specimen, obtain the material modulus and strength data, and then assign them to each component to create physical properties; Step S17: Substitute the fine finite element model of the honeycomb sandwich panel into the finite element model of the entire spacecraft, connect it with the structural components of the adjacent honeycomb sandwich panel, accurately simulate the boundary conditions of the fine finite element model of the honeycomb sandwich panel, and apply displacement constraints and loads to the finite element model of the entire spacecraft for calculation.

3. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 1, characterized in that, The calculation of the fine finite element model of the honeycomb sandwich panel includes: Buckling analysis was performed on the refined finite element model of the honeycomb sandwich panel to obtain the critical load coefficient, static analysis was performed to obtain the static stress, frequency response analysis was performed to obtain the dynamic stress, and the safety margin was calculated based on the stress.

4. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 1, characterized in that, The strength verification prediction based on the strength criterion includes: The strength criteria include the critical load factor criterion, the allowable stress criterion, and the safety margin criterion; The critical load coefficient criterion is that the critical load coefficient is greater than 2; The allowable stress criteria include: the allowable stress for aluminum alloy materials is less than 255 MPa, the allowable stress for magnesium alloy materials is less than 120 MPa, the allowable stress for foamed adhesive is less than 3.5 MPa, and the allowable stress for quasi-isotropic carbon fiber materials is less than 450 MPa. The safety margin criteria include a safety margin greater than 0.25 for carbon fiber composite materials and a safety margin greater than 0 for metallic materials.

5. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 2, characterized in that, The analysis of the composition and stress characteristics of the honeycomb sandwich panel includes: The honeycomb sandwich panel is a composite material structure product consisting of upper and lower panels, honeycomb core, embedded parts, embedded frames, reinforcing sheets and scraping sheets, which are bonded together with adhesive. The stress characteristics of the honeycomb sandwich panel are that the upper and lower panels, embedded frames, reinforcing plates and scraping plates bear in-plane tensile force, compressive force and bending moment, while the honeycomb core and embedded parts bear transverse shear force.

6. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 2, characterized in that, The failure modes and modeling criteria are formulated based on the stress characteristics of the honeycomb sandwich panel, including: The failure modes of the honeycomb sandwich panel include overall instability, local instability of the panel, local instability of the honeycomb core, honeycomb core shearing, honeycomb core crushing failure, plastic deformation of the panel, and cracking of the foam. The modeling criteria include accurately simulating the relationships between load-bearing components and adhesive bonding, reflecting the stress transmission characteristics of the product, and comprehensively predicting the failure modes of the honeycomb sandwich panel.

7. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 2, characterized in that, The simplification and cleanup of the three-dimensional geometric model of the honeycomb sandwich panel includes: The three-dimensional geometric model of the honeycomb sandwich panel is simplified and cleaned up using three-dimensional design software, including deleting only the secondary geometric features of each load-bearing element and retaining the main geometric features of each load-bearing element. The secondary geometric features include small openings and rounded corners on each load-bearing element. Cut the panels and honeycomb cores according to the geometric and material properties of the 3D model, and supplement the pre-embedded parts and the foam around the frame.

8. The finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 2, characterized in that, The simulation and mesh generation of the simplified 3D geometric model includes: The simplified and cleaned 3D geometric model was imported into the finite element simulation analysis software. Appropriate elements were selected for simulation based on the geometric characteristics and stress characteristics of each component. Mesh generation was carried out independently. The upper and lower panels, reinforcing plates, and embedded frames are typical thin-walled structures and were simulated using triangular and quadrilateral shell elements. The honeycomb core, embedded parts, foam adhesive, and scraper were simulated using pentahedral and hexahedral solid elements.

9. A finite element fine modeling method for honeycomb sandwich panels oriented towards strength verification according to claim 2, characterized in that, The simulation of the adhesive bonding assembly relationship of the various components of the honeycomb sandwich panel includes: The adhesive contact method is used to simulate the adhesive assembly relationship of each component of the honeycomb sandwich panel. Interface units are created on the contact boundaries of each component. The contact stiffness matrix is ​​calculated based on the penalty factor and then assigned to the interface units to bond the components together.

10. A fine-grained finite element modeling system for strength verification of honeycomb sandwich panels, characterized in that, include: The fine modeling module establishes a fine finite element model of the honeycomb sandwich panel based on its composition and stress characteristics. The solution calculation module performs solution calculations on the fine finite element model of the honeycomb sandwich panel; The strength verification prediction module performs strength verification prediction based on the strength criteria.

Images