Numerical simulation method of impact guided wave response of composite thin-walled structures

Abstract

The application discloses a numerical simulation method of impact wave response of a composite thin-walled structure, comprising the following steps: constructing a geometric model; performing mesh division on the model; giving material properties to each part of the model; setting impact boundary conditions; setting the interaction of each part; setting analysis steps and output; and submitting calculation. The method considers piezoelectric effect and material damping characteristics, simulates the wave response of the composite thin-walled structure under impact through finite element software, can be used for revealing the impact wave response mechanism of the composite thin-walled structure and influencing factors, and has a promoting effect on the development of the impact monitoring technology of the composite structure based on the piezoelectric sensor.

Description

TECHNICAL FIELD

[0001] The application belongs to the field of structural health monitoring, and relates to a numerical simulation method for impact wave response of a composite thin-walled structure. BACKGROUND

[0002] Carbon fiber composites have been widely used in the fields of aviation, aerospace, rail transportation and wind power due to their superior specific strength, specific stiffness, strong designability and excellent fatigue resistance. However, the composite material has a natural defect in impact resistance. Due to the laminated structure, the composite material is prone to delamination damage when impacted by external objects. Delamination damage can significantly reduce the mechanical properties of the structure. For example, the largest delamination damage caused by tool drop during maintenance can reduce the compressive strength of the structure by 40%, and the delamination damage is invisible to the naked eye. Therefore, strict monitoring of the initiation and propagation process of delamination damage is the key to ensuring the safety of the structure.

[0003] Impact passive monitoring technology based on piezoelectric sensors is an online monitoring technology. A certain number of piezoelectric sensor networks are arranged on the surface of the structure. When an impact event occurs, the voltage signal generated by the piezoelectric effect of the piezoelectric sensor is obtained, and then the signal is extracted for feature extraction, and a specific algorithm is used to predict the impact position and impact energy, thereby providing support for the health maintenance of the composite structure. In order to ensure the reliability of the monitoring, the impact passive monitoring technology based on piezoelectric sensors usually needs to be verified by a large amount of experimental data. However, the carbon fiber composite structure is often expensive, and it is difficult to reuse after damage caused by impact, and the experimental cost is huge. In addition, the experiment can only obtain the guided wave response signal of the structure caused by impact, and cannot reveal the generation mechanism and influencing factors of the guided wave response of the composite structure under impact from the principle, thereby hindering the in-depth understanding of the impact guided wave signal of the composite structure and restricting the theoretical research and engineering application of the impact monitoring technology of the composite structure. In order to overcome this difficulty, it is necessary to develop a numerical simulation technology for the impact guided wave response of the composite structure with high fidelity. SUMMARY

[0004] The purpose of the present application is to at least solve one of the problems existing in the prior art, and to provide a numerical simulation method, device and / or system for the impact guided wave response of a composite structure with high fidelity.

[0005] To this end, some embodiments of the present application provide a numerical simulation method for impact wave response of a composite thin-walled structure, which comprises the following steps: establishing a geometric model, wherein the geometric model comprises a composite thin-walled structure model part, a piezoelectric sensor array model part comprising a plurality of piezoelectric sensor model parts, and an impact object model part; the piezoelectric sensor model parts in the piezoelectric sensor array model part are uniformly distributed on the surface of the composite thin-walled structure model part; a layer of glue layer model part is arranged between each piezoelectric sensor model part and the composite thin-walled structure model part; dividing the model parts of the geometric model into finite element grids, including setting the grid elements of the composite thin-walled structure model part as three-dimensional solid or shell elements, setting the grid elements of the impact object model part as three-dimensional solid elements, and setting the grid elements of each piezoelectric sensor model part as piezoelectric elements; defining the material direction of the composite thin-walled structure model part and giving it orthogonal anisotropic material properties; giving the glue layer model part and the impact object model part corresponding linear elastic isotropic material properties; giving the piezoelectric sensor model part the parameters of piezoelectric material; setting the boundary conditions of the composite thin-walled structure model part, and simulating the impact process by applying a certain initial velocity to the impact object model part; setting the binding constraint between the piezoelectric sensor model part and the composite thin-walled structure model part, setting the contact action between the impact object model part and the composite thin-walled structure model part, and introducing a suitable friction coefficient; using implicit dynamic analysis steps, wherein the time step is set according to the required sampling frequency, the nodes on the upper surface of each piezoelectric sensor model part are set as monitoring points to output the voltage response of the impact process, and the voltage signals of all nodes on the upper surface of each piezoelectric sensor model part are calculated based on the voltage response output by each monitoring point, and the average voltage signal of all nodes of one piezoelectric sensor model part is obtained by taking the average value of the voltage signals of all nodes of the piezoelectric sensor model part.

[0006] In some embodiments, the composite thin-walled structure model part is a flat plate or a stiffened wall plate, and the configuration and geometric size thereof are determined according to actual requirements; the piezoelectric sensor array model part is formed by regularly arranging a plurality of identical piezoelectric sensor model parts; and the shape and size of the impact object model part are determined according to actual conditions.

[0007] In some embodiments, the size of the grid element of the composite thin-walled structure model part is determined according to the wavelength of the impact stress wave, and the grid element of the piezoelectric sensor model part is refined in the thickness direction.

[0008] In some embodiments, the size of the grid element of the composite thin-walled structure model part is set to arrange ten grid nodes on the minimum wavelength.

[0009] In some embodiments, the potential of the lower surface of the piezoelectric sensor model part is set to zero.

[0010] In some embodiments, the boundary conditions include clamped or pinned boundary conditions.

[0011] In some embodiments, the parameters of the piezoelectric material assigned to the piezoelectric sensor model part include elastic constants, piezoelectric constants and dielectric constants, which satisfy the piezoelectric effect equation therebetween.

[0012] In some embodiments, damping is introduced in the composite material model part and the glue layer model part for simulating energy dissipation.

[0013] In some embodiments, Rayleigh damping is set for the composite thin-walled structure model part and the glue layer model part to simulate the energy attenuation behavior thereof during impact; the damping coefficients are solved for finite element software analysis.

[0014] The numerical simulation method of the composite thin-walled structure impact guided wave response provided by the present application has at least one of the following beneficial effects: by constructing a composite thin-walled structure impact monitoring numerical simulation model based on a piezoelectric sensor, the guided wave response signal of the composite thin-walled structure under different impact conditions is simulated, which can greatly reduce the time and cost of composite structure impact test; more importantly, the numerical method is not affected by the production process, environment and other factors of the sensor, and is more conducive to revealing the guided wave response mechanism of the structure impact and its influencing factors. BRIEF DESCRIPTION OF DRAWINGS

[0015] Figure 1a A schematic diagram of a composite thin-walled structure impact monitoring numerical simulation model based on a piezoelectric sensor;

[0016] Figure 1b A schematic diagram of a composite thin-walled structure impact monitoring numerical simulation model based on a piezoelectric sensor; Figure 1a An enlarged side view of part A in FIG. 8;

[0017] Figure 2 A schematic diagram of the piezoelectric effect of a piezoelectric sensor;

[0018] Figure 3 A schematic diagram of the relationship between the natural angular frequency of the structure and the damping ratio in Rayleigh damping;

[0019] Figure 4 A schematic diagram of a composite stiffened panel impact monitoring based on a piezoelectric sensor;

[0020] Figure 5 A comparison diagram of the normalized amplitude of the time domain signal of the fifth sensor in simulation and experiment;

[0021] Figure 6 Figure 5 is a comparison chart of normalized root mean square sequences of time domain signals of the fifth sensor in simulation and experiment;

[0022] Figure 7 Figure 6 is a comparison chart of time domain characteristics-wave arrival times of all sensors in simulation and experiment;

[0023] Figure 8 Figure 7 is a comparison chart of frequency domain characteristics of signals of the fifth sensor in simulation and experiment;

[0024] Figure 9a and Figure 9b Figures 8 and 9 are time-frequency spectrograms of signals of the fifth sensor in simulation and experiment, respectively. DETAILED DESCRIPTION

[0025] In order to make the technical solutions and advantages of the present application clearer, the technical solutions of the present application will be described in detail below with reference to the drawings.

[0026] Step 1: constructing a composite thin-walled structure impact monitoring geometric model in finite element software Abaqus.

[0027] This step specifically includes: as shown in Figure 1a , Figure 1b is a geometric model for monitoring impact guided wave response of a composite thin-walled structure based on a piezoelectric sensor, which includes a composite thin-walled structure 10, a piezoelectric sensor array 20 and an impact object 30. The composite thin-walled structure model part can be a flat plate or a stiffened wall plate, and its configuration and geometric size are determined according to actual requirements; the piezoelectric sensor array model part is composed of a plurality of identical piezoelectric sensor model parts arranged according to certain rules and uniformly distributed on the surface of the thin-walled structure model part; as shown in Figure 1b in order to simulate the actual sensor bonding conditions, a layer of adhesive 40 is added between the piezoelectric sensor model part and the thin-walled structure model part; the shape and size of the impact object model part are determined according to actual conditions.

[0028] Step 2: meshing the model.

[0029] This step specifically includes: meshing the model in the finite element software, setting the mesh elements of the composite thin-walled structure model part 10 as three-dimensional entities or shell elements, setting the mesh elements of the impact object model part 30 as three-dimensional entity elements, and setting the mesh elements of the piezoelectric sensor model part 20 as piezoelectric elements. In order to accurately simulate the propagation of guided waves in the composite thin-walled structure model part 10, the grid size L of the composite thin-walled structure model part 10 should be determined according to the wavelength of the impact stress wave. In order to meet the calculation accuracy and reduce the calculation amount, it can be generally set to be arranged with 10 nodes at the minimum wavelength λ min , i.e.

[0030] L = λ min / 10 (1)

[0031] For Figure 1b The grid size of the composite thin-walled structure model part 10 is set to 1 mm, which generally meets the requirements.

[0032] In some embodiments, to ensure the simulation accuracy of the piezoelectric sensor model part 20, the grid of the piezoelectric sensor model part is refined in the thickness direction.

[0033] Step three: Assign material properties to each component of the model.

[0034] This step specifically includes defining the material direction of the composite thin-walled structure model part 10, assigning orthotropic material properties, and assigning corresponding linear elastic isotropic material properties to the adhesive layer model part 40 and the impactor model part 30.

[0035] The piezoelectric sensor model part 20 is assigned parameters such as elastic constants, piezoelectric constants, and dielectric constants of piezoelectric materials, which satisfy the following piezoelectric effect equation:

[0036]

[0037] In the above formula, δ is stress, ε is strain, E e is electric field intensity, D e is electric displacement, is the elastic constant matrix, is the piezoelectric constant matrix, is the transpose matrix of, ξ ε is the dielectric constant matrix.

[0038] As shown in Figure 2 , the polarization direction of the piezoelectric sensor model part 20 is defined as the thickness direction.

[0039] Rayleigh damping parameters are set for the materials of the composite thin-walled structure model part 10 and the adhesive layer model part 40 to simulate the energy attenuation behavior of the composite thin-walled structure model part and the adhesive layer model part during the impact process. The application of Rayleigh damping in the finite element software is realized by setting damping coefficients α and β. Then the damping coefficients α and β are solved through the following steps.

[0040] Rayleigh damping assumes that the damping matrix of the structure is a combination of the mass matrix and the stiffness matrix, i.e.:

[0041] [C] = α[M] + β[K] (3)

[0042] Where [C] is the damping matrix, [M] is the mass matrix, and [K] is the stiffness matrix.

[0043] In Rayleigh damping, the natural angular frequency of the structure and the damping ratio satisfy the following relationship:

[0044]

[0045] in, and These represent the mass proportional component and the stiffness proportional component, respectively, where ω is the natural angular frequency of the structure and ξ is the damping ratio. Their relationship curves are shown below. Figure 3 As shown. The natural angular frequency ω of the structure is known. m and ω n With the corresponding damping ratio ξ m and ξ n Substituting these values ​​into the above equation, we obtain two systems of linear algebraic equations concerning the damping coefficients α and β, from which we can solve for α and β:

[0046]

[0047] Step 4: Set the boundary conditions for structural impact.

[0048] This step specifically includes: the boundary conditions of the composite material thin-walled structure model 10 have a significant impact on the reflection of impact stress waves and should be set according to the actual situation, generally using fixed or hinged boundary conditions. The impact process is simulated by applying a certain initial velocity to the impact model 30; the initial velocity can be calculated based on the impact energy. In some embodiments, to obtain better impact simulation results, only the displacement degree of freedom in the initial velocity direction of the impact model 30 is retained. In some embodiments, to facilitate the extraction of the voltage signal from the piezoelectric sensor model 20, the potential of the lower surface of the piezoelectric sensor model 20 is set to 0.

[0049] Step 5: Set up the interactions between the parts.

[0050] This step specifically includes: setting binding constraints between the piezoelectric sensor model part 20 and the composite material thin-walled structure model part 10; setting contact between the impactor model part 30 and the composite material thin-walled structure model part 10; and introducing a suitable friction coefficient through a penalty function.

[0051] Step Six: Set up the analysis steps and output.

[0052] This step specifically includes: employing an implicit dynamic analysis step suitable for simulating the piezoelectric effect, where the step size Δt must satisfy the following relationship:

[0053] Δt≤L min / c L (6)

[0054] In the above formula, L min is the minimum size of the unit grid of the thin-walled structure model part, c L is the wave velocity of the longitudinal wave in the impact stress wave.

[0055] Since the impact stress wave propagates in the composite material with dispersion, the wave velocity changes all the time, and it is difficult to determine the analysis step length according to the above relationship. The following criteria can be generally used:

[0056] Δt = 1 / (20f max ) (7)

[0057] In the above formula, f max is the maximum frequency of the stress wave, which can be determined by experiment.

[0058] All nodes on the upper surface of the piezoelectric sensor model part 20 are set as monitoring points, and the voltages of these monitoring points are output.

[0059] Step seven: submitting calculation and analyzing the calculation results

[0060] This step specifically includes: submitting the finite element software for calculation. After the calculation is completed, the voltage signals of all nodes on the upper surface of the piezoelectric sensor model part are obtained, the average value thereof is taken to obtain the average voltage signal of the piezoelectric sensor model part, and then advanced signal processing means are used to analyze and extract the characteristics of the signal.

[0061] Embodiment:

[0062] Based on the above method of the application, the impact wave response of the composite stiffened panel is simulated, and the impact monitoring experiment is carried out based on the piezoelectric sensor and the composite stiffened panel with the same parameters. Figure 4 The principle diagram of the simulation and the experiment. In the simulation and the experiment, the overall size of the stiffened panel is 700mm*450mm, the material is carbon fiber / epoxy composite material, the skin thickness is 1mm, the skin layer mode is [45 / 90 / -45 / 0] s , four T-shaped ribs are pasted on the skin, the rib span is 130mm, the thickness is 2mm, and the rib layer mode is [45 / 0 / -45 / 90 / 0 / 45 / -45 / 0] s . The piezoelectric sensor used in the experiment is a P-51 type piezoelectric ceramic disc with a diameter of 8mm and a thickness of 0.25mm. Twelve piezoelectric sensors P1 to P12 are arranged on the surface of the stiffened panel to form a monitoring network, the horizontal spacing of the sensors is 160mm, and the vertical spacing is 130mm. The composite stiffened panel is fixed at both ends, and a drop hammer impact device is used to impact it.

[0063] As Figure 5The figure shows the impact of the punch on the composite stiffened panel with an energy of 2J. The figure shows the time-domain signal of the fifth sensor in the simulation and the experiment, i.e. Figure 4 The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals.

[0064] The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals. Figure 6 The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals. Figure 7 The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals.

[0065] Figure 8 The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals.

[0066] Figure 9a The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals. Figure 9b The figure shows the comparison of the normalized amplitude of the time-domain signal of the sensor at point P5 in the simulation and the experiment. It can be seen that the trends of the two signals are in good agreement, and both have two obvious peaks in front of the signals.

[0067] In summary, the impact guided wave signals obtained by the piezoelectric sensor model part in the simulation and the piezoelectric sensor in the experiment are highly consistent in the time domain, the frequency domain, and the time-frequency domain, thereby verifying the effectiveness of the numerical simulation method of the application.

[0068] The specific structural and functional details disclosed herein are merely representative for purposes of describing exemplary embodiments of the present application. However, the present application can be embodied in many alternatives, and should not be construed as limited to the embodiments set forth herein.

[0069] It should be understood that although the terms "first", "second" and the like can be used herein to describe various elements, these elements should not be limited by these terms. These terms are only used to distinguish one element from another. For example, a first element could be termed a second element, and, similarly, a second element could be termed a first element without departing from the scope of the exemplary embodiments. The term "and / or" as used herein includes any and all combinations of one or more of the associated listed items.

[0070] The terminology used herein is for the purpose of describing particular embodiments only and is not intended to be limiting of example embodiments. As used herein, the singular forms "a", "an" and "the" are intended to include the plural forms as well, unless the context clearly indicates otherwise. It will be further understood that the terms "comprises" and / or "comprising," when used in this specification, specify the presence of stated features, integers, steps, operations, elements, and / or components, but do not preclude the presence or addition of one or more other features, integers, steps, operations, elements, components, and / or groups thereof.

[0071] It should also be noted that in some alternative implementations, the functions / acts / steps noted in the figures can occur out of the order noted in the figures. For example, two figures shown in succession can in fact be executed substantially concurrently or can sometimes be executed in the reverse order, depending upon the functionality / acts / steps involved.

[0072] Moreover, the foregoing description of embodiments of the present application is by way of example only, and other embodiments of the present application are within the scope of the present application.

Claims

1. A numerical simulation method for the impact wave response of a thin-walled composite material structure, characterized in that: The method includes the following steps: A geometric model is established, comprising a composite material thin-walled structure model, a piezoelectric sensor array model comprising multiple piezoelectric sensor model parts, and an impactor model part; wherein, the piezoelectric sensor model parts in the piezoelectric sensor array model part are uniformly distributed on the surface of the composite material thin-walled structure model part; and an adhesive layer model part is provided between each piezoelectric sensor model part and the composite material thin-walled structure model part. The geometric model is divided into finite element meshes, including setting the mesh elements of the composite material thin-walled structure model to three-dimensional solid or shell elements, setting the mesh elements of the impactor model to three-dimensional solid elements, and setting the mesh elements of each piezoelectric sensor model to piezoelectric elements. Define the material orientation for the composite thin-walled structure model and assign it orthotropic material properties; assign corresponding linear elastic isotropic material properties to both the adhesive layer model and the impactor model; assign piezoelectric material parameters to the piezoelectric sensor model. The boundary conditions of the composite material thin-walled structure model are set, and the impact process is simulated by applying an initial velocity to the impact object model, wherein the initial velocity is calculated based on the impact energy. A binding constraint is set between the piezoelectric sensor model part and the composite material thin-walled structure model part, a contact interaction is set between the impactor model part and the composite material thin-walled structure model part, and a friction coefficient is introduced through a penalty function; An implicit dynamic analysis step is employed, wherein the time step is set according to the required sampling frequency, and nodes on the upper surface of each piezoelectric sensor model portion are set as monitoring points to output their voltage response to the impact process; and The voltage signal of all nodes on the upper surface of each piezoelectric sensor model part is calculated based on the voltage response output of each monitoring point. The average voltage signal of the piezoelectric sensor model part is obtained by taking the average value of the voltage signals of all nodes of a piezoelectric sensor model part. The parameters assigned to the piezoelectric material in the piezoelectric sensor model include the assignment of elastic constant, piezoelectric constant, and dielectric constant, such that they satisfy the following piezoelectric effect equation: In the formula, For stress, In response, For electric field strength, For electric displacement, The elastic constant matrix, The piezoelectric constant matrix, for The transpose of the matrix, Here is the dielectric constant matrix; Damping is introduced into the composite material thin-walled structure model and the adhesive layer model to simulate energy dissipation; Rayleigh damping was applied to both the thin-walled composite material structure model and the adhesive layer model to simulate their energy attenuation behavior during impact; the damping coefficient was then solved using the following steps. and For use in finite element software analysis: In the Rayleigh damping, the natural angular frequency of the structure and the damping ratio satisfy the following relationship: ,in, The natural angular frequency of the structure, Given the damping ratio and the structure's natural angular frequency. and With the corresponding damping ratio and Substituting these values ​​into the above equation, we obtain the damping coefficient. and Two systems of linear algebraic equations Thus, the solution is obtained. and .

2. The numerical simulation method for the impact wave response of a thin-walled composite material structure according to claim 1, characterized in that: The composite material thin-walled structure model part is a flat plate or a stiffened wall panel, and its configuration and geometric dimensions are determined according to actual needs; the piezoelectric sensor array model part is composed of several identical piezoelectric sensor model parts arranged in a regular manner; the shape and size of the impactor model part are determined according to actual conditions.

3. The numerical simulation method for the impact wave response of a thin-walled composite material structure according to claim 1, characterized in that: The size of the mesh cells in the composite material thin-walled structure model is determined according to the wavelength of the impact stress wave, and the mesh cells in the piezoelectric sensor model are refined in the thickness direction.

4. The numerical simulation method for the impact guided wave response of a thin-walled composite material structure according to claim 3, characterized in that: The mesh element size of the composite thin-walled structure model is set to be within the minimum wavelength. Ten grid nodes are arranged on top.

5. The numerical simulation method for the impact guided wave response of a thin-walled composite material structure according to claim 1, characterized in that: Set the potential of the lower surface of the piezoelectric sensor model part to zero.

6. The numerical simulation method for the impact guided wave response of a thin-walled composite material structure according to claim 1, characterized in that: The boundary conditions include fixed or hinged boundary conditions.

7. The numerical simulation method for the impact guided wave response of a thin-walled composite material structure according to claim 3, characterized in that: wherein, The step size of the implicit dynamics analysis step Satisfying Relationship: ,in, This refers to the minimum size of the mesh element in the composite material thin-walled structure model. The step size is determined by the wave velocity of the longitudinal wave in the impact stress wave; or by using the following criteria: ,in, The maximum frequency of the stress wave is denoted as .

Images