Thin-wall shell welding seam dynamic modeling method based on common shell unit

Abstract

The invention relates to the technical field of weld joint dynamic modeling, in particular to a thin-wall shell weld joint dynamic modeling method based on a common shell unit, which comprises the following steps of: S1, dispersing the middle surface of a welding part by a global shell grid, and simulating a weld joint by using a CSE instead of a rigid connection unit; s2, simplifying the modeling process of the CSE by adopting a grid common node processing method; s3, constructing an interface shell unit to replace part of GSM on the two sides of the welding area, and achieving the grid consistency requirement; s4, the CSE welding seam modeling method is applied to welding of the thin-wall shell for dynamic simulation analysis; and S5, performing result verification and adjustment on the data obtained by simulation in the step S4. According to the method, the ISE unit is introduced to meet the grid consistency requirement of the non-matched connection interface; building a weld joint dynamic model based on a CSE and RE modeling method, and carrying out dynamic simulation analysis and experimental research; the problem that the finite element analysis accuracy is affected due to the fact that an existing connecting unit cannot accurately simulate the real characteristics of weld joints is solved.

Description

Technical Field

[0001] The invention relates to the technical field of weld dynamics modeling, and in particular to a thin-wall shell weld dynamics modeling method based on common shell element (CSE). Background Art

[0002] Complex mechanical structures are composed of independent parts and connections between parts, such as welding, bolts, bonding, riveting and other joints. The large number and wide distribution of joints in the mechanical mechanism have a great influence on the stiffness and deformation of the overall mechanical structure. Therefore, the accuracy of joint modeling is the key and important prerequisite for the analysis and prediction of structural dynamic performance. For welded shells with a large number of welds, due to the limitations of the connection unit itself, its dynamic model cannot reflect the true characteristics of the welds and will bring a large amount of computational workload. Therefore, an accurate and efficient weld modeling method is urgently needed to realize the accurate construction of the dynamic model of the welded shell.

[0003] Commonly used modeling forms for welded joints are spot welding modeling and weld modeling. Spot welding modeling is mainly achieved through a variety of simplified finite element models, such as shell element model, umbrella beam model, beam-shell combination model and solid nugget model. Zhang et al. used shell element and solid element to simulate spot welding and proposed a hybrid structural stress method to evaluate the fatigue of complex spot welding structures. Ertugrul et al. used a multi-axial low-cycle fatigue analysis method to conduct fatigue analysis tests on a spot welding specimen and compared the accuracy of spot welding simulation by umbrella beam model, solid element model and combination model. The results showed that the modeling accuracy of umbrella beam model was low, the robustness of solid model was the worst, and the modeling accuracy and robustness of combination model were the highest. Therefore, the combination model is widely used in the analysis of spot welding structures. Thuan et al. used elastic beam elements to connect the spider shell mesh representing the nugget area to simulate spot welding, and applied interface shell element (ISE) to connect the mismatched interface between the local spider mesh and the global mesh of the plate to improve the mesh quality, effectively alleviating the lateral shear and membrane locking phenomenon of ISE. However, the above methods have high requirements on the mesh consistency of the welding area. Weld modeling is mainly based on connection element simulation. Among them, the solid element has great advantages in reflecting weld details, improving model stability and evaluating local stress fields, but it often requires the refinement of the mesh in the welding area. To avoid refining the mesh, a simpler rigid beam element (RBE2) or shear flexible beam element (CWELD) can be used to simulate the weld, but the mesh quality in the welding area is required to be high. The above studies all show that the solid element can better reflect the actual state and characteristics of the weld, but the modeling and calculation workload is large, which affects the calculation efficiency; while the modeling efficiency of the beam element is higher, but its cross-sectional parameters (shape, eccentricity, etc.) are somewhat arbitrary, which cannot truly reflect the characteristics of the weld material and will also lead to inaccurate dynamic analysis results. Summary of the invention

[0004] The purpose of the present invention is to provide a thin-walled shell weld dynamic modeling method based on common shell element (CSE), aiming at the problem that the rigid element (RE) used in weld dynamic modeling cannot accurately simulate the real characteristics of the weld, thus affecting the accuracy of finite element analysis; the present invention uses CSE to assign weld material and thickness attributes to simulate its real characteristics, and performs mesh common node processing to simplify the CSE modeling process; introduces interface shell element (ISE) with an arbitrary number of nodes to optimize mesh consistency to form a high-quality mesh in the weld joint area. On this basis, a welded thin-walled shell is used as the application object, and a weld dynamic model is constructed based on the CSE and RE modeling methods, and dynamic simulation analysis and experimental research are carried out.

[0005] Rigid element (RE) and adhesive element (AE) are common forms of simulating welds. Among them, RE is a beam element with a simple structure and easy to create, but it cannot be assigned material properties; AE is an entity element that can reflect the material and structural characteristics of welds, but when there are a large number of welds, the model construction efficiency is low, and the analysis and calculation workload is large. However, CSE is a shell element, which is easy to build a model. Assigning it material and thickness properties can truly reflect the characteristics of the weld. Compared with the above-mentioned connection elements, CSE can not only improve the modeling efficiency, but also simulate welds more realistically. On this basis, for different connection interfaces and welding methods of different materials, mesh common node processing and mesh consistency optimization methods can be used to simplify the CSE modeling process and improve modeling efficiency.

[0006] In order to achieve the above technical objectives and the above technical effects, the present invention is implemented through the following technical solutions:

[0007] A thin-walled shell weld dynamics modeling method based on ordinary shell elements includes the following steps:

[0008] S1: The global shell mesh (GSM) discretizes the mid-surface of the weldment, and CSE replaces RE to simulate the weld;

[0009] S2: The grid common node processing method is used to simplify the CSE modeling process;

[0010] S3: Construct ISE to replace part of the GSM on both sides of the welding area to achieve the mesh consistency requirement of the non-matching connection interface;

[0011] S4: Apply the above CSE weld modeling method to the welded thin-walled shell (WTWS) for dynamic simulation analysis;

[0012] S5: Verify and adjust the simulation results obtained in S4.

[0013] Furthermore, the step S1 specifically includes: importing the three-dimensional model of the WTWS into HyperMesh, extracting the midsurface of the solid model using the midsurface command, and discretizing the midsurface using the automesh command to form a GSM;

[0014] Through the HyperMesh ruled command, a CSE is constructed in the welding area in the middle of the weldment GSM to simulate the weld;

[0015] The thickness property of the weld is set through the HyperMesh property card, and the material properties of the weld are set through the material card, such as density, Poisson's ratio, elastic modulus, etc. Finally, the above cards are assigned to CSE to simulate the real characteristics of the weld.

[0016] Furthermore, the step S2 specifically includes:

[0017] The mesh of the matching connection interface at the edge of the welding area meets the consistency requirements and can be directly processed for common nodes. However, the non-matching connection interface requires GSM optimization before CSE modeling and common node processing can be performed.

[0018] The non-matching connection interface will cause the GSM to fail to meet the mesh consistency requirements due to the inconsistency between the mesh size and the weldment size. As a result, when constructing CSE and mesh common node processing, the shell mesh will be distorted or even unable to form in the welding area due to the unequal number of meshes or nodes. Usually, it is improved by refining the mesh, which will undoubtedly increase the workload of finite element construction and analysis calculation;

[0019] To avoid the above-mentioned problem of increased workload, a special shell element (ISE) can be introduced to process the mesh at the edge of the welding area to ensure that the GSM at the edge has an equal number of nodes, thereby meeting the mesh consistency requirements. Only after the GSM on both sides of the welding area meet the mesh consistency requirements, use the replace command of HyperMesh to merge the mesh nodes corresponding to the CSE and GSM. The CSE and GSM are merged into one mesh to simplify the modeling process of the CSE.

[0020] Furthermore, the step S3 specifically includes:

[0021] ISE is a polygonal variable-node shell element with an arbitrary number of nodes. It improves mesh quality by giving a consistent shape function at the interface of mismatched meshes to connect different independently designed meshes. Its shape function can be represented by a piecewise bilinear function:

[0022]

[0023] Wherein, d=2 / (n-3) indicates that the node spacing is equal, and when n=4, the shape function of ISE becomes a standard quadrilateral bilinear shape function.

[0024] ISE is used to replace some GSM on both sides of the welding area of ​​the non-matching connection interface. On the basis of not refining the mesh, the nodes of ISE are adjusted to make the meshes on both sides of the welding area have equal number of nodes to meet the mesh consistency requirements. This avoids the problems existing in CSE construction and mesh common node processing of non-matching interfaces.

[0025] Furthermore, the step S4 specifically includes:

[0026] The finite element model of WTWS was constructed by RE modeling method and CSE modeling method for dynamic simulation analysis. The natural frequency and modal vibration shape of the structure were obtained by modal analysis, and the frequency response function curve of the structure was obtained by harmonic response analysis.

[0027] Furthermore, the modal analysis specifically includes: performing modal analysis on the WTWS to obtain the structural natural frequency and the corresponding modal vibration shape. The upper annular surface of the WTWS is milled at a low speed, with the main rotation speed concentrated in the range of 300rpm to 600rpm. The excitation frequency is relatively low, so the analysis focuses on the low-order frequency range of the structure, that is, the response modes and vibration shapes of the first 10 orders. Based on ANSYS WORKBENCH, modal parameter identification and vibration shape prediction analysis are performed on the finite element models established by different methods.

[0028] The harmonic response analysis specifically includes: based on modal analysis, a harmonic response analysis is performed on the WTWS structure to study the dynamic response of the structure to external excitation. According to the modal analysis results, the four maximum deformation points are set as measuring points to obtain a good dynamic response, and a multi-point excitation and single-point vibration pickup experimental scheme is adopted. One of the measuring points is selected as the pickup point, and the remaining points are selected as the excitation points, and the excitation force is set to a transient excitation of 2N. According to the set load application method and the boundary conditions of the tooling fixture, a harmonic response analysis is performed based on ANSYS WORKBENCH to obtain the frequency response function of the measuring point in the three directions of X, Y, and Z to the excitation response. After completion, the pickup point is updated, and the above process is repeated to obtain the origin excitation frequency response curve of the measuring point in three directions.

[0029] Furthermore, the step S5 specifically includes:

[0030] The dynamic response of the structure under the excitation of the hammer is obtained through the modal experiment of the hammer method to obtain the accurate modal parameters of the structure, and the dynamic performance of the structure is analyzed and optimized. First, the excitation signal is filtered and denoised with the help of the data acquisition system to eliminate noise interference. Then, the important parameters such as the natural frequency, damping ratio and stiffness of the structure are extracted through the spectrum analysis and modal identification algorithm of the data processing module. Finally, the experimental results are used to guide the modification of the theoretical model to make the finite element model more perfect and reasonable.

[0031] Beneficial effects of the present invention:

[0032] Rigid element (RE) and adhesive element (AE) are common forms of simulating welds. Among them, RE is a rigid element with a simple structure and easy to create, but it cannot be assigned material properties; AE is an entity element that can reflect the material and structural characteristics of welds, but when there are a large number of welds, the model construction efficiency is low, and the analysis and calculation workload is large. However, CSE is a shell element, which is easy to build a model. Assigning it material and thickness properties can truly reflect the characteristics of the weld. Compared with the above-mentioned connection elements, CSE can not only improve the modeling efficiency, but also simulate welds more realistically. On this basis, for different connection interfaces and welding methods of different materials, mesh common node processing and mesh consistency optimization methods can be used to simplify the CSE modeling process and improve modeling efficiency.

[0033] Based on the construction of the above weld dynamic model, the thickness property of the weld is set through the HyperMesh property card, and the density, Poisson's ratio, elastic modulus and other parameters are set through the material card to ensure that the physical properties of the weld can be accurately reflected in the finite element model. This method avoids the problem that the connection unit cannot reflect the material and structural characteristics of the weld, thereby improving the accuracy of weld modeling and making the dynamic characteristics of the weld closer to the actual situation.

[0034] The present invention aims at matching the connection interface, and the GSM on both sides of the welding area meets the mesh consistency requirements. The ruled command of HyperMesh can be used to construct a high-quality CSE in the welding area in the middle of the welded part GSM to simulate the weld. If the weld and the welded plate have the same material and thickness properties, the replace command of HyperMesh is used to merge the mesh nodes corresponding to the CSE and GSM. The CSE and GSM are merged into one mesh to simplify the modeling process of the CSE. This processing method not only simplifies the modeling process, but also avoids the formation of low-quality rectangular shell meshes at the edges of the welding area. The consistency and quality of the mesh are maintained, while improving the overall quality of the finite element model.

[0035] The present invention is aimed at non-matching connection interfaces, and the GSM on both sides of the welding area does not meet the grid consistency requirements. Directly constructing CSE to simulate the weld by the above method can easily lead to CSE grid distortion or even failure to form CSE due to the unequal number of GSM grids and nodes on both sides of the welding area. In addition, the above problems can be avoided by mesh refinement, but it undoubtedly increases the workload of model construction and analysis and calculation. Therefore, ISE is used to replace part of the GSM on both sides of the welding area, and the number of grid nodes on both sides of the welding area is equal by adjusting the number of nodes of ISE. On the basis of not refining the grid, the consistency requirements of the grid are met, and the mesh quality problem of CSE caused by unequal number of nodes is avoided.

[0036] ISE is a polygonal variable node shell element with an arbitrary number of nodes. It improves the mesh quality by giving a consistent shape function at the mismatched mesh interface to connect different independently designed meshes. This optimization method effectively solves the common node mismatch problem in traditional methods, improves the mesh quality in the weld area, and makes the finite element model more accurate and stable overall.

[0037] By adopting the CSE modeling method of the present invention, the predicted value of the natural frequency of the shell obtained by finite element analysis is closer to the experimental value, the overall change trend of the frequency response curve is consistent with the modal test results, and the experimental value at the peak and trough has a small deviation from the predicted value, which proves the high accuracy of the method in predicting dynamic characteristics. In addition, this method can be applied to the modeling of similar welded thin-walled structures, and has good promotion and engineering application value. Through dynamic simulation analysis and experimental verification of WTWS, the results show that the relative error between the predicted value of the structural natural frequency obtained by the CSE modeling method and the experimental value is small, the average value of the relative error of the first 10 orders is 2.51%, and the relative error of the last 8 orders is less than 3.75%. This method shows higher accuracy and consistency in the prediction of dynamic characteristics. Furthermore, this method is not only suitable for specific thin-walled welded shells, but can also be promoted to finite element modeling analysis of similar large thin-walled welded parts, and has good promotion and engineering application value. This method can provide a strong guarantee for structural performance analysis and prediction in engineering practice, and can be widely used in different types of thin-walled welded structures.

[0038] Of course, any product implementing the present invention does not necessarily need to achieve all of the advantages described above at the same time. BRIEF DESCRIPTION OF THE DRAWINGS

[0039] In order to more clearly illustrate the technical solutions of the embodiments of the present invention, the accompanying drawings required for describing the embodiments will be briefly introduced below. Obviously, the accompanying drawings described below are only some embodiments of the present invention. For ordinary technicians in this field, other accompanying drawings can be obtained based on these accompanying drawings without paying creative work.

[0040] Figure 1 Schematic diagram of welded parts structure: (a) matching connection interface and (b) non-matching connection interface;

[0041] Figure 2 Schematic diagram of simulated welds for different connection elements; (a) rigid connection element (RE) and (b) entity connection element (AE);

[0042] Figure 3 Flow chart of the CSE weld dynamics modeling method;

[0043] Figure 4 Schematic diagram of weld dynamics model constructed for CSE;

[0044] Figure 5 Different types of n-node ISEs; (a) quadrilateral element and (b) triangular element;

[0045] Figure 6 is the shape function of the eight-node quadrilateral element;

[0046] Figure 7 Schematic diagram of the mesh consistency optimization process;

[0047] Figure 8 It is a schematic diagram of the WTWS structure and fixture;

[0048] Fig. 9 Finite element models for different welding modeling methods; (a) RE modeling method and (b) CSE modeling method;

[0049] Fig.10 The vibration contours of different finite element models; (a) RE modeling method and (b) CSE modeling method;

[0050] Fig.11 It is a schematic diagram for comparing the natural frequency and maximum deformation values ​​of different finite element models;

[0051] Fig.12 This is a schematic diagram of the distribution of measurement points for harmonic response analysis;

[0052] Fig.13 It is a schematic diagram for comparing the frequency response curves of different weld dynamic models in the X, Y, and Z directions;

[0053] Fig.14 Schematic diagram of experimental measurement point distribution and experimental setup;

[0054] Fig.15 Comparison of the frequency response curve of the experimental value and the frequency response curve of the predicted value; (a) experimental value, (b) predicted value by CSE modeling method and (c) predicted value by RE modeling method;

[0055] Fig.16 Schematic diagram for comparison between predicted and experimental values ​​of natural frequencies of different weld dynamic models;

[0056] Fig.17 Schematic diagram of the comparison between the predicted and experimental values ​​of acceleration amplitudes of different weld dynamic models. DETAILED DESCRIPTION

[0057] The following will be combined with the drawings in the embodiments of the present invention to clearly and completely describe the technical solutions in the embodiments of the present invention. Obviously, the described embodiments are only part of the embodiments of the present invention, not all of the embodiments. Based on the embodiments of the present invention, all other embodiments obtained by ordinary technicians in this field without creative work are within the scope of protection of the present invention.

[0058] Example 1

[0059] The present embodiment provides a thin-walled shell weld dynamics modeling method based on common shell elements, comprising:

[0060] like Figure 1 As shown, two welded parts with thicknesses h1 and h2 are connected by a weld in the welding area. Figure 1 (a) represents the matching connection interface, Figure 1 (b) represents a non-matching connection interface. For different types of connection interfaces, the mid-surface of the weldment is discretized into GSM using regular quadrilateral shell elements, and the rigid element (RE) or adhesive element (AE) connection element is used at the edge of the GSM near the welding area to construct the weld finite element model, such as Figure 2 As shown. Among them, RE simulates the stress of the weld by transmitting force and moment at the node through beam elements, but it cannot load the material properties of the weld and cannot reflect the actual characteristics of the weld; AE belongs to a three-dimensional solid element, which can simulate the real characteristics of the weld very well, but the workload of model construction and calculation is large. In order to solve the limitations of the above-mentioned connection elements in weld modeling, a CSE weld dynamic modeling method is proposed, which can give material properties and thickness properties and fully reflect the weld connection characteristics; the flow chart of the modeling method is shown in Figure 3 The specific operations are as follows:

[0061] Basic model construction

[0062] Construct CSE in the welding area to replace the connection unit to simulate the weld, as shown in 4(a) and (c). The thickness property of the weld is set through the HyperMesh property card, and the density, Poisson's ratio, elastic modulus and other parameters that reflect the material properties are set through the material card. As can be seen from the figure: compared with the three-dimensional solid unit, the CSE structure is simpler and has fewer nodes, making it easier to create and solve; compared with the one-dimensional unit, the material properties and thickness properties that can be given to the CSE can more realistically reflect the actual characteristics of the weld joint. In addition, the accuracy of the weld simulation is also related to the mesh quality of the CSE.

[0063] In actual processing, the weld gap is often smaller than the plate size. If the GSM unit size is too large, a regular low-quality rectangular shell mesh will be formed in the welding area of ​​the matching connection interface; a low-quality distorted shell mesh will be formed in the welding area of ​​the non-matching connection interface, thus affecting the accuracy of modeling. Figure 4 Therefore, it is necessary to further refine the GSM to ensure the mesh quality of CSE, but directly refining the mesh will cause a significant increase in the workload of modeling and calculation. Therefore, it is necessary to further simplify the mesh while ensuring modeling efficiency to avoid low-quality meshes and a large workload.

[0064] Grid common node processing

[0065] In order to solve the large computational workload caused by the refinement of GSM, the mesh common node processing method is used to simplify the CSE modeling process. By merging the corresponding GSM nodes of different welded parts at the edge of the welding area, CSE and GSM are merged into one mesh. The merged result is shown in the figure below. Figure 4 (b) and (d). When the plate and weld have the same material properties and thickness properties, this simplified method can avoid the low-quality rectangular shell mesh formed in the matching connection interface, and there is no need to refine the GSM, which reduces the workload of model construction while ensuring the mesh quality. However, the quality of the distorted shell mesh in the welding area of ​​the non-matching connection interface is difficult to improve because the GSM of the non-matching connection interface does not meet the mesh consistency requirements.

[0066] Therefore, for non-matching connection interfaces, both the construction of CSE and the mesh common node processing method require GSM to meet the mesh consistency requirements, otherwise distorted shell meshes will be generated in the welding area due to the unequal number of meshes or nodes, or even the shell mesh cannot be formed. Figure 4 (c) and (d). The Jacobian value of the distorted shell mesh is small, resulting in low unit quality, which is easy to produce non-singular matrices during finite element calculations, leading to solution failure, thus affecting the accuracy of weld simulation. In addition, the use of ordinary four-node shell elements to discretize non-matching connection interfaces can easily lead to poor mesh consistency of GSM. Therefore, special shell elements are also needed to process the nodes at the edge of the welding area to ensure that the GSM at the edge has an equal number of nodes, thereby meeting the consistency requirements of the mesh.

[0067] Mesh consistency optimization

[0068] In order to solve the mesh common node problem of non-matching connection interface, ISE is introduced to achieve mesh consistency requirements. ISE is a polygonal variable node shell element with arbitrary number of nodes, which can improve the transition mesh quality of non-matching connection interface. There are two main forms, one is quadrilateral multi-node shell element, such as Figure 5(a) shows a triangular multi-node shell element. Figure 5 (b) The triangular element can be obtained by merging the 2- and 3-node quadrilateral elements.

[0069] ISE mainly achieves the purpose of improving mesh quality by giving a consistent shape function at the interface of mismatched meshes to connect different independently designed meshes. Its shape function can be constructed by moving least squares (MLS) approximation, transfinite two-variable Lagrangian interpolation and generalized centroid coordinate method. It can be represented by a piecewise bilinear function.

[0070]

[0071] Where d = 2 / (n-3) means that the node spacing is equal. When n = 4, the shape function of ISE becomes a standard quadrilateral bilinear shape function. The shape function of the eight-node quadrilateral master unit is as follows: Figure 6 As shown:

[0072] Therefore, ISE is used to replace some GSM on both sides of the welding area. By adjusting the nodes of ISE, the number of nodes of the mesh on both sides of the welding area is equal. The processed mesh is as follows: Figure 7 As shown in the figure, compared with the ordinary four-node GSM, ISE can meet the mesh consistency requirements by adjusting the number of nodes for both matching connection interfaces of different mesh sizes and non-matching connection interfaces of the same mesh size, thereby building high-quality CSE in the welding area without further mesh refinement. Therefore, the modeling workload can be reduced during the mesh consistency optimization process while ensuring the accuracy of the weld simulation.

[0073] Example 2

[0074] In order to verify the feasibility of the method, different weld modeling methods were applied to a certain enterprise product WTWS for dynamic simulation analysis. Figure 8 As shown, a special fixture is set up according to the actual processing situation to position and clamp it. First, RE and CSE are used to simulate the weld, the finite element model of WTWS is constructed, the boundary conditions are set as constraint states, the modal analysis and harmonic response analysis of the shell are performed, the dynamic response parameters of the shell structure are obtained, and finally compared with the experimental values.

[0075] Finite Element Modeling

[0076] After extracting the mid-surface of WTWS, it is discretized into a regular quadrilateral shell mesh, which is connected by different weld simulation methods. The mesh size is 5 mm. Since the materials of the weld and the plate are both aluminum alloy with a thickness of 1 mm, the CSE is processed by mesh common nodes to reduce the modeling workload of CSE. The mesh division results and related model properties are shown in Fig. 9 As shown. Fig. 9 (a) is the finite element model using RE modeling method; Fig. 9 (b) is the finite element model using the CSE modeling method.

[0077] Modal Analysis

[0078] Modal analysis was performed on WTWS to obtain the structural natural frequency and corresponding modal vibration shape. The upper torus of WTWS was mainly milled at low speed, with the main speed concentrated in the range of 300rpm to 600rpm. The excitation frequency was low, so the analysis focused on the low-order frequency range of the structure, that is, the response modes and vibration shapes of the first 10 orders. Based on ANSYS WORKBENCH, modal parameter identification and vibration shape prediction analysis were performed on the finite element models established by different methods, and the corresponding vibration shapes were obtained. Fig.10 The first 10 natural frequencies and maximum deformations are shown in Table 1. Fig.11 shown.

[0079] From the modal vibration cloud diagram, it can be seen that the same structure can obtain significantly different vibration cloud diagrams using two different weld modeling methods. Comparison of the 3rd, 4th, and 5th order vibration modes shows that the vibration position distribution of the shell obtained by the two modeling methods is significantly different, and the maximum deformation position is also inconsistent; comparison of the remaining vibration modes shows that the maximum deformation position of the shell obtained by the two modeling methods is roughly the same, but there are significant differences in the deformation area range and deformation degree; in general, different modeling methods have significant differences in the prediction of structural vibration modes, which have a greater impact on the maximum deformation position results in the low-frequency range, and have a greater impact on the deformation area range and deformation degree of vibration modes in other ranges.

[0080] In addition, it can be seen from Table 1 that there are also significant differences in the natural frequency values ​​and maximum deformations predicted by the two methods. Compared with the first 10 natural frequencies, the average absolute deviation of the same-order frequency is 4.47Hz, and the absolute deviations of the 3rd, 5th, and 7th orders are all greater than 7Hz, with a maximum value of 9.34Hz; compared with the first 10 maximum deformations, the average absolute deviation of the same-order maximum deformation is 15.15mm, and the absolute deviations of the 6th order are all greater than 11mm, with a maximum value of 39.49mm. This shows that different modeling methods do have a great impact on the prediction results. Therefore, using appropriate methods to establish an accurate dynamic model is the key to obtaining accurate prediction results and improving the accuracy of structural performance analysis.

[0081] Table 1 Comparison of predicted values ​​of natural frequency and maximum deformation of different weld finite element models

[0082]

[0083] Harmonic response analysis

[0084] Based on modal analysis, harmonic response analysis is performed on the WTWS structure to study the dynamic response of the structure to external excitation. According to the modal analysis results, four maximum deformation points are set as measurement points to obtain good dynamic response, such as Fig.12 As shown. An experimental scheme of multi-point excitation and single-point vibration pickup is adopted. One of the measuring points is selected as the pickup point and the other points are selected as the excitation points in turn, and the excitation force is set to 2N for transient excitation. According to the set load application method and the boundary conditions of the fixture setting, a harmonic response analysis is performed based on ANSYS WORKBENCH to obtain the frequency response function of the measuring point to the excitation response in the three directions of X, Y, and Z. After completion, the pickup point is updated and the above process is repeated to obtain the origin excitation frequency response curve of measuring point 4 in three directions, as shown below. Fig.13 shown.

[0085] It can be seen from the frequency response curve that both different weld modeling methods can obtain good frequency response function curves. In the range of 0-450Hz, the curve peaks correspond well to the natural frequency values. Compared with the Z-direction frequency response results, the average value of the peaks corresponding to the first 10 natural frequencies of the RE modeling method is 1.72mm, and the maximum value is 8.75mm. The average value of the peaks corresponding to the first 10 natural frequencies of the CSE modeling method is 2.06mm, and the maximum value is 16.63mm. Compared with the frequency response curves in the X and Y directions, the average values ​​of the first 10 peaks of the RE modeling method are 0.0084mm and 0.014mm, respectively, and the average values ​​of the first 10 peaks of the CSE modeling method are 0.009mm and 0.012mm, respectively. This shows that the response degree of the structure to the excitation in the X and Y directions is significantly smaller than that in the Z direction, which is consistent with the clamping force of the structural fixture. In addition, the CSE modeling method has fewer peaks in the frequency response function curve within 500Hz than the RE modeling method.

[0086] Example 3

[0087] Experimental verification

[0088] The dynamic response of the structure under the excitation of the hammer is obtained through the modal experiment of the hammer method to obtain the accurate modal parameters of the structure, and the dynamic performance of the structure is analyzed and optimized. First, the excitation signal is filtered and denoised with the help of the data acquisition system to eliminate noise interference. Then, the important parameters such as the natural frequency, damping ratio and stiffness of the structure are extracted through the spectrum analysis and modal identification algorithm of the data processing module. Finally, the experimental results are used to guide the modification of the theoretical model to make the finite element model more perfect and reasonable.

[0089] Experimental setup

[0090] According to the structural characteristics of WTWS, a thin-walled welded shell dynamics test and analysis experimental platform was built to carry out shell dynamics performance analysis experiments. The experiment used NI (National Instruments) DAQ data acquisition system and NISignal Express data processing software to build the platform; the experimental object was a thin-walled shell formed by full welding of stainless steel plates, and multi-point excitation and single-point picking were used for data acquisition. The PCB force hammer was used as the excitation signal input, and the ICP acceleration sensor acquisition end was used as the output. After obtaining the response signal, the experimental data was post-processed and analyzed based on the Signal Express software.

[0091] Experimental Procedure

[0092] A preliminary experiment is conducted before the formal experiment. The force hammer excites the same point on the structure multiple times along the Z direction to obtain multiple frequency response curves. If the frequency range corresponding to the attenuation of the exciting force frequency response curve by 30dB is much larger than the core frequency range of 0-450Hz, the excitation signal is effective; if the frequency response curves overlap, the structure is linear. In the formal experiment, each measuring point is excited three times and the average value is taken to shield the influence of noise on the measurement signal; the size and direction of the force hammer excitation are kept consistent to ensure that the coherence function value is close to 1. The experimental site is as follows Fig.14 The specific steps are as follows:

[0093] (1) According to the Signal Express software operation process, set the sensor and hammer sensitivity, sampling frequency, window function, filter function and other related parameters based on the IEPE module.

[0094] (2) Excite a fixed measuring point along the Z direction, move the accelerometer clockwise in the same plane, and fix it at the measuring point with instant adhesive or a magnetic base until the sensor traverses all measuring points.

[0095] (3) After the excitation is completed, save the collected frequency response function data. Then change the position of the hammer excitation in turn to ensure that all measurement points are covered, and repeat step 2 to paste the sensor.

[0096] (4) Repeat steps 2 and 3 until data collection at all measuring points is completed, save and record the data.

[0097] Results Analysis

[0098] The frequency response curves of WTWS in the X, Y, and Z directions were obtained through the hammer method modal experiment, as shown in Fig.15 The predicted and experimental values ​​of the natural frequencies are shown in Table 2. Fig.16As shown; the absolute deviation comparison of each order acceleration amplitude is shown in Table 3. Fig.17 shown.

[0099] Table 2 Comparison of predicted and experimental values ​​of natural frequencies of different weld dynamic models

[0100]

[0101] Table 3 Mean, standard deviation and coefficient of dispersion of the absolute deviation between the predicted values ​​and experimental values ​​of the acceleration amplitude of different weld dynamic models

[0102]

[0103] Depend on Fig.15 It can be seen that compared with the dynamic response in the X and Y directions, the response of the shell in the Z direction is significantly greater, which is consistent with the above-mentioned harmonic response finite element analysis results; further, the experimental values ​​are compared with the theoretical prediction values ​​obtained by RE and CSE modeling methods. As shown in Table 2: the natural frequency prediction values ​​using the CSE modeling method are closer to the experimental values, the average relative error of the same order frequency is 2.51%, and the relative errors of the last 8 orders are all less than 3.75%; the average relative error of the same order frequency using the RE modeling method is 4.1%, and the maximum relative error is 11.31%. The natural frequency value comparison is Fig.16 As shown in Table 3, compared with the first 10 acceleration amplitudes, the standard deviations of the absolute deviations between the predicted values ​​and the experimental values ​​in the X, Y, and Z directions of the RE modeling method are 75.84, 80.38, and 70.88, respectively; the standard deviations of the absolute deviations between the predicted values ​​and the experimental values ​​in the X, Y, and Z directions of the CSE modeling method are 7.60, 13.32, and 29.96, respectively; compared with the RE modeling method, the dispersion coefficient of the absolute deviation between the predicted values ​​and the experimental values ​​of the CSE modeling method is smaller, and the dispersion of the acceleration amplitudes in the X, Y, and Z directions is reduced by 36.42%, 12.33%, and 25.69%, respectively. Fig.17 shown.

[0104] However, in certain specific frequency bands, such as 300Hz to 420Hz, the experimental value has slightly more peaks and valleys than the predicted value. The main reason is that the structural simplification of WTWS before finite element simulation analysis weakens the influence of welds on the nonlinear characteristics of the structure, which causes a certain deviation between the finite element model and the actual structural characteristics, resulting in more peaks and valleys in the experimental value than the predicted value in a certain frequency band. The overall trend of the predicted frequency response curve of the shell obtained by the CSE modeling method is consistent with the experimental frequency response curve obtained by the modal experiment. The experimental values ​​at the peaks and troughs have a small deviation from the predicted values, and the corresponding natural frequency values ​​are in good agreement, which proves the feasibility of using CSE to simulate welds for shell finite element model construction and performance analysis; at the same time, compared with RE and other traditional modeling methods, the dynamic characteristics of the shell finite element model established by CSE are more consistent with the actual structural characteristics response, which proves the good accuracy and good prediction effect of the CSE modeling method.

[0105] In summary, the present invention proposes a thin-walled shell weld dynamic modeling method based on ordinary shell elements, which can realize the assignment of weld material and thickness properties, and more realistically reflect the structural characteristics of the weld and the shell while reducing the modeling workload. Among them, the use of mesh common node processing can simplify the CSE modeling process and avoid the appearance of low-quality meshes at the connection interface where the weldment and the weld have the same material and thickness properties; ISE is used to optimize the mesh consistency of non-matching connection interfaces to ensure the mesh quality of CSE. In addition, the above-mentioned mesh optimization processing can also avoid the large modeling and calculation workload caused by mesh refinement. Then, the dynamic characteristics simulation analysis and experiments of the thin-walled welded shell are carried out based on different weld modeling methods. The results show that compared with RE and other modeling methods, the predicted value of the structural natural frequency obtained by the CSE modeling method proposed in this invention is closer to the experimental value, the average value of the relative error of the first 10 orders is 2.51%, and the relative error of the last 8 orders is less than 3.75%; the overall change trend of the frequency response curve is more consistent, the peak value corresponding to the natural frequency is better matched, and the discrete degree between the acceleration amplitude in the X, Y, and Z directions and the experimental value is reduced by 36.42%, 12.33%, and 25.69%, respectively. This shows the feasibility of this method in the modeling and analysis of thin-walled welded shells; at the same time, this method can further improve the accuracy of the construction of thin-walled welded shell models, lay a theoretical and experimental foundation for the next step of accurate analysis and precise prediction of structural performance, and can be extended to the finite element modeling and analysis of similar large thin-walled welded parts, with good promotion and engineering application value.

[0106] The preferred embodiments of the present invention disclosed above are only used to help illustrate the present invention. The preferred embodiments do not describe all the details in detail, nor do they limit the invention to the specific implementation methods described. Obviously, many modifications and changes can be made according to the content of this specification. This specification selects and specifically describes these embodiments in order to better explain the principles and practical applications of the present invention, so that those skilled in the art can understand and use the present invention well. The present invention is limited only by the claims and their full scope and equivalents.

Claims

1. A thin-walled shell weld dynamics modeling method based on ordinary shell elements, characterized in that: The following steps are involved: S1: Global shell mesh discretization of weldment mid-surface, ordinary shell elements replace rigid link elements to simulate welds; S2: The mesh common node processing method is used to simplify the modeling process of ordinary shell elements; S3: Construct interface shell elements to replace part of the global shell mesh on both sides of the welding area to achieve the mesh consistency requirement of the non-matching connection interface; S4: applying the common shell element weld modeling method of steps S1-S3 above to the welded thin-walled shell for dynamic simulation analysis; S5: Verify and adjust the simulation results obtained in S4.

2. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 1, characterized in that: The step S1 specifically includes: performing three-dimensional modeling on the thin-walled shell, extracting the mid-surfaces of the welded parts, and discretizing these mid-surfaces using quadrilateral shell elements to form a global shell mesh; Use the HyperMesh property card to set the weld thickness property and the material card to set the weld material properties, including but not limited to density, Poisson's ratio, and elastic modulus; finally, assign the above cards to ordinary shell elements to simulate the real characteristics of the weld.

3. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 1, characterized in that: The step S2 specifically includes: The mesh of the matching connection interface at the edge of the welding area meets the consistency requirements and can be directly processed with common nodes; however, the non-matching connection interface requires the global shell mesh to be optimized before ordinary shell element modeling and common node processing can be performed; The non-matching connection interface will cause the global shell mesh to fail to meet the mesh consistency requirements due to the inconsistency between the mesh size and the weldment size; thus, when constructing ordinary shell elements and mesh common node processing, distorted shell meshes will be generated in the welding area due to the unequal number of meshes or nodes, or even the shell mesh cannot be formed; Special shell elements are introduced to process the mesh at the edge of the weld area to ensure that the global shell mesh at the edge has an equal number of nodes to meet the mesh consistency requirement; Only when the global shell meshes on both sides of the welding area meet the mesh consistency requirements, use the replace command of HyperMesh to merge the mesh nodes corresponding to the ordinary shell elements and the global shell mesh; so that the ordinary shell elements and the global shell mesh are merged into one mesh to simplify the modeling process of the ordinary shell elements.

4. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 1, characterized in that: The step S3 specifically includes: The interface shell element is a polygonal variable-node shell element with an arbitrary number of nodes. It improves the mesh quality by giving a consistent shape function at the interface of mismatched meshes to connect different independently designed meshes. Its shape function can be represented by a piecewise bilinear function: Where d = 2 / (n-3) means that the node spacing is equal. When n = 4, the shape function of the interface shell element becomes a standard quadrilateral bilinear shape function. Interface shell elements are used to replace part of the global shell mesh on both sides of the non-matching connection interface welding area. On the basis of not refining the mesh, the nodes of the interface shell elements are adjusted so that the meshes on both sides of the welding area have equal number of nodes to meet the mesh consistency requirements; thereby avoiding the problems existing in the construction of ordinary shell elements and the processing of mesh common nodes of non-matching interfaces.

5. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 1, characterized in that: The step S4 specifically includes: The RE modeling method and the ordinary shell unit modeling method are used to construct the finite element model of the welded thin-walled shell for dynamic simulation analysis; the natural frequency and modal vibration shape of the structure are obtained through modal analysis; and the frequency response function curve of the structure is obtained through harmonic response analysis.

6. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 5, characterized in that: The modal analysis specifically includes: performing modal analysis on the welded thin-walled shell to obtain the structural natural frequency and the corresponding modal vibration shape; performing low-speed milling on the upper annular surface of the welded thin-walled shell to analyze the response modes and vibration shapes of the first 10 orders; performing modal parameter identification and vibration shape prediction analysis on the finite element models established by different methods based on ANSYS WORKBENCH; The harmonic response analysis specifically includes: based on modal analysis, performing harmonic response analysis on the welded thin-walled shell structure to study the dynamic response of the structure to external excitation; according to the modal analysis results, setting four maximum deformation points as measuring points to obtain a good dynamic response, and adopting a multi-point excitation and single-point vibration pickup experimental scheme; selecting one of the measuring points as a pickup point and the remaining points as excitation points in turn, and setting the excitation force to a transient excitation of 2N; according to the set load application method and the boundary conditions of the fixture, performing harmonic response analysis based on ANSYS WORKBENCH, and obtaining the frequency response function of the measuring point to the excitation response in the three directions of X, Y, and Z; after completion, updating the pickup point, repeating the above process, and obtaining the origin excitation frequency response curve of the measuring point in the three directions.

7. The thin-walled shell weld dynamics modeling method based on ordinary shell elements according to claim 1, characterized in that: The step S5 specifically includes: The dynamic response of the structure under the hammer excitation is obtained through the modal experiment of the hammer method to obtain the accurate modal parameters of the structure, and the dynamic performance of the structure is analyzed and optimized; the excitation signal is filtered and denoised with the help of the data acquisition system to eliminate noise interference; the natural frequency, damping ratio and stiffness parameters of the structure are extracted through the spectral analysis and modal identification algorithm of the data processing module; finally, the experimental results are used to guide the modification of the theoretical model.

8. Application of the method according to any one of claims 1 to 7 in dynamic simulation analysis of thin-walled shells.

Images