A Virtual Test Loading Analysis Method for Airfoil Structures Based on Digital Simulation

Abstract

This invention belongs to the field of aircraft design technology and discloses a virtual test loading analysis method for wing structures based on digital simulation. First, detailed finite element modeling is performed according to the wing structure's digital model, including the actual dimensions and properties of the wing structure. Then, based on the characteristics of the connectors, the properties of the connectors are calculated and assigned values ​​using the simplification principle of bush elements. The center coordinates of the loading point are determined according to the location of the adhesive tape or tension / compression block in the test load distribution scheme. After loading, simulation analysis is performed. Loading is carried out according to the initial load direction, and the load is discretized to a single loading point. The coordinates of the center node of the loading point and the actuator connection point after deformation are recorded for each single loading point. The direction of the loading vector is then obtained. Loading is performed on all loading points of the simulation model, and linear / nonlinear static, buckling, and post-buckling calculations are conducted. Based on the calculation results, stress and strain are analyzed to identify test risk locations, and strain gauges are then attached. This invention can guide the design of loading schemes in wing structure tests, improve calculation accuracy, identify test risks, avoid test piece loss, and reduce test costs.

Description

Technical Field

[0001] This invention belongs to the field of aircraft design technology and relates to virtual simulation analysis of the static / fatigue test state strength of aircraft wing structures. Specifically, it relates to a virtual test loading analysis method for wing structures based on digital simulation. Background Technology

[0002] Traditional aircraft static / fatigue testing relies on finite element models with natural meshes to obtain internal force results. This is then combined with engineering algorithms to perform calculations, identify test risks, and derive theoretical strain values ​​for the load-bearing structure. Engineering algorithms are reliable for simple structures with a single load and reasonable simplification. However, their drawback lies in the significant model simplification, which fails to represent local conditions. For example, in engineering testing, the application of test loads using adhesive tape is common. This loading method itself has practical limitations, leading to discrepancies in test measurements within the load-affected zone. These discrepancies can easily be misjudged as unreasonable model simplification during model validation. Furthermore, inaccurate identification of areas with complex load transmission or those affected by loading during test risk identification can result in substantial test risks.

[0003] In addition, the load-bearing capacity of the location where adhesive tape is applied is generally calculated using engineering algorithms. The calculation results are conservative and the conservative amount is large. When the load intensity on the wing surface is large, the load distributed by the adhesive tape is likely to exceed the allowable load limit of the structure at the bonding point, making the loading scheme unusable and making experimental loading difficult, so other loading methods must be used.

[0004] Digital simulation-based analysis methods can effectively address such problems. However, most digital simulations focus on macroscopic behavior, neglecting changes in local structures. This can significantly impact the results in certain situations, such as the loading point failing before the structural body, leading to substantial resource waste. Therefore, there is an urgent need for a reasonable and less biased virtual simulation method for analyzing loading conditions, enabling strength analysis and experimental design. Summary of the Invention

[0005] To address the aforementioned issues, this invention provides a virtual test loading analysis method for wing structures based on digital simulation. This method focuses on boundary constraints, guides the design of loading schemes in wing structure tests, improves computational accuracy, identifies test risks, and reduces test costs.

[0006] The technical solution of the present invention is as follows:

[0007] A virtual test loading analysis method for airfoil structures based on digital simulation includes the following steps:

[0008] S1: Perform detailed finite element modeling based on the wing structure digital model, including the actual dimensions and properties of the wing structure;

[0009] S2: Based on the characteristics of the connector, calculate the properties of the connector using the simplification principle of the bush unit and assign values;

[0010] S3: Determine the center coordinates of the loading point based on the location of the tape or tension block in the test load distribution scheme;

[0011] S4: If the test uses adhesive tape for loading, then create an MPC unit with the same size as the adhesive tape; if the test uses tension / compression block for loading, then create a double-layer unit with the same size as the tension / compression block for loading.

[0012] S5: After loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction. The load is discretized to a single loading point. Then, the coordinates of the center node of the loading point and the actuator connection point are recorded after deformation.

[0013] S6: Connect the coordinates of the center node of the loading point and the actuator connection point after deformation to obtain the direction of the loading vector;

[0014] S7: Load all loading points of the simulation model, constrain them according to the experimental constraints, carry out simulation analysis combining geometric nonlinearity and material nonlinearity, and perform linear / nonlinear static, buckling and post-buckling calculations;

[0015] S8: Based on the calculation results of the detailed finite element model, analyze the stress and strain, and identify the locations of experimental risks;

[0016] S9: Attach strain gauges at locations identified as test risk points in the analysis;

[0017] S10: Test verification. If any abnormal situation occurs during the test, stop the test in time, perform local reinforcement, and repeat S7 to S9 to restart the test.

[0018] Furthermore, in S1, based on the wing structure digital model, the spars, panels and ribs are modeled in detail using two-dimensional shell elements. The model includes the actual thickness and actual offset properties of the structure.

[0019] Furthermore, in S2, based on the characteristics of the fasteners: if the meshes of two fasteners are adjacent within a continuous interval and the fasteners are subjected to shear loads, then point-to-point connections using CBUSH elements are used; if the number of meshes between fasteners exceeds 3, the connection form of MPC+CBUSH+MPC should be used as much as possible for fastener simulation.

[0020] Furthermore, in S3, the coordinates of the geometric center of the tape or tension block obtained from the test load distribution scheme are the coordinates of the center of the loading point.

[0021] Furthermore, in S4, if the test involves adhesive tape loading, an MPC unit with the same size coverage area as the adhesive tape is established, and loading is implemented based on the stiffness of the structural connection area; if the test involves tension / compression block loading, a double-layer solid unit with the same size coverage area as the tension / compression block is established. If a rubber pad structure exists, an additional layer of units is added near the structural side to simulate the stiffness characteristics of the rubber pad structure at the connection surface, and MPC units are used on the top surface of the solid unit to simulate loading.

[0022] Furthermore, in S5, after loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction, and the load is discretized to a single loading point. For a single loading point, loading is first performed in the direction perpendicular to the chord plane, and the force following option in nonlinear calculation is turned on to obtain the coordinates of the center node of the loading point after deformation. Then, the coordinates of the actuator connection point are obtained according to the position of the gantry loading actuator in the experiment.

[0023] Furthermore, in S6, the coordinates of the two points, the center node of the loading point after deformation and the actuator connection point, are connected to obtain the direction of the real loading vector. The loading vector direction is obtained for each discretized loading point.

[0024] Furthermore, in S7, load is applied to each discrete loading point in the simulation model and constrained according to experimental constraints. After debugging the model, NASTRAN or Abaqus software is used to conduct simulation analysis combining geometric nonlinearity and material nonlinearity. Linear / nonlinear static, buckling, and post-buckling calculations are performed as needed.

[0025] Furthermore, in S8, based on the calculation results of the detailed finite element model, stress, strain, and connector loads are extracted for the entire airfoil structure; the strength of the entire structural component, as well as the strength of the adhesive tape or tension / compression block connection area, are analyzed to identify the minimum margin, discover test risks, and clarify the risk occurrence area.

[0026] The beneficial effects of this invention are as follows:

[0027] 1. This invention can guide the design of loading schemes and improve the calculation accuracy of wing structure strength tests for large amphibious aircraft and other wing structures with high load concentration or where the pressure center deviates from the wing box section structure. It can also identify test risks, avoid test piece loss, and reduce test costs.

[0028] 2. This invention provides a modeling method and loading process for airfoil structure strength testing. The usage is clear and straightforward, and it can be used to guide virtual simulation analysis of airfoil structure strength testing and obtain relatively accurate results. Attached Figure Description

[0029] To more clearly illustrate the technical solutions of the embodiments of this invention, the drawings used in the embodiments will be briefly introduced below. It should be understood that the following drawings only show some embodiments of this invention and should not be regarded as a limitation of the scope. For those skilled in the art, other related drawings can be obtained from these drawings without creative effort.

[0030] Figure 1 This is a schematic diagram of the test specimen structure and loading arrangement according to an embodiment of the present invention;

[0031] In the diagram, 5 and 7 are the size markings for the applied adhesive tape;

[0032] Figure 2 This is a schematic diagram of the loading results from the finite element simulation of the wing structure in the embodiment. Detailed Implementation

[0033] This section describes embodiments of the present invention, used to explain and illustrate the technical solutions of the present invention. Unless otherwise specified, the embodiments and features described herein can be combined with each other.

[0034] In the description of this invention, it should be understood that the terms "center," "longitudinal," "lateral," "upper," "lower," "front," "rear," "left," "right," "vertical," "horizontal," "top," "bottom," "inner," and "outer," etc., indicating directions or positional relationships, are given in the accompanying drawings and are used only for the convenience of describing the invention and simplifying the description, and do not indicate or imply that the device or device referred to must have a specific orientation, or be constructed and operated in a specific orientation, and therefore should not be construed as a limitation of the invention. Furthermore, the terms "first," "second," etc., are used for descriptive purposes only and should not be construed as indicating or implying relative importance or implying the number of indicated technical features. Thus, features defined with "first," "second," etc., may explicitly or implicitly include more than one of those features. In the description of this invention, unless otherwise stated, "a plurality of" means two or more.

[0035] In the description of this invention, it should be noted that, unless otherwise explicitly specified and limited, the terms "installation," "connection," and "linking" should be interpreted broadly. For example, they can refer to a fixed connection, a detachable connection, or an integrated connection; they can refer to a mechanical connection or a point connection; they can refer to a direct connection or a connection through an intermediate medium; and they can refer to the internal communication between two components. Those skilled in the art can understand the specific meaning of the above terms in this invention based on the specific circumstances.

[0036] Example 1:

[0037] A virtual test loading analysis method for airfoil structures based on digital simulation includes the following steps:

[0038] S1: Perform detailed finite element modeling based on the wing structure digital model, including the actual dimensions and properties of the wing structure;

[0039] S2: Based on the characteristics of the connector, calculate the properties of the connector using the simplification principle of the bush unit and assign values;

[0040] S3: Determine the center coordinates of the loading point based on the location of the tape or tension block in the test load distribution scheme;

[0041] S4: If the test uses adhesive tape for loading, then create an MPC unit with the same size as the adhesive tape; if the test uses tension / compression block for loading, then create a double-layer unit with the same size as the tension / compression block for loading.

[0042] S5: After loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction. The load is discretized to a single loading point. Then, the coordinates of the center node of the loading point and the actuator connection point are recorded after deformation.

[0043] S6: Connect the coordinates of the center node of the loading point and the actuator connection point after deformation to obtain the direction of the loading vector;

[0044] S7: Load all loading points of the simulation model, constrain them according to the experimental constraints, carry out simulation analysis combining geometric nonlinearity and material nonlinearity, and perform linear / nonlinear static, buckling and post-buckling calculations;

[0045] S8: Based on the calculation results of the detailed finite element model, analyze the stress and strain, and identify the locations of experimental risks;

[0046] S9: Attach strain gauges at locations identified as test risk points in the analysis;

[0047] S10: Test verification. If any abnormal situation occurs during the test, stop the test in time, perform local reinforcement, and repeat S7 to S9 to restart the test.

[0048] In S1, based on the wing structure digital model, the spars, panels and ribs are modeled in detail using two-dimensional shell elements. The model includes the actual thickness and actual offset properties of the structure.

[0049] In S2, based on the characteristics of the fasteners: if the meshes between two fasteners are adjacent in a continuous interval and the fasteners are subjected to shear loads, then point-to-point connection using CBUSH elements is used; if the number of meshes between fasteners exceeds 3, the connection form of MPC+CBUSH+MPC should be used as much as possible for fastener simulation.

[0050] In S3, the coordinates of the geometric center of the tape or tension block obtained from the test load distribution scheme are the coordinates of the center of the loading point.

[0051] In S4, if the test involves adhesive tape loading, an MPC element with the same size coverage area as the adhesive tape is created, and loading is implemented based on the stiffness of the structural connection area. If the test involves tension / compression block loading, a double-layer solid element with the same size coverage area as the tension / compression block is created. If a rubber pad structure exists, an additional layer of elements is added near the structure to simulate the stiffness characteristics of the rubber pad structure at the connection surface. The loading is simulated using an MPC element on the top surface of the solid element.

[0052] In S5, after loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction, and the load is discretized to a single loading point. For a single loading point, loading is first performed in the direction perpendicular to the chord plane, and the force following option in nonlinear calculation is turned on to obtain the coordinates of the center node of the loading point after deformation. Then, the coordinates of the actuator connection point are obtained according to the position of the gantry loading actuator in the experiment.

[0053] In S6, the coordinates of the two points, the center node of the loading point after deformation and the actuator connection point, are connected to obtain the direction of the real loading vector. The loading vector direction is obtained for each discretized loading point.

[0054] In S7, load each discrete loading point in the simulation model and constrain it according to the experimental constraints. After debugging the model, use NASTRAN or Abaqus software to carry out simulation analysis combining geometric nonlinearity and material nonlinearity, and perform linear / nonlinear static, buckling and post-buckling calculations as needed.

[0055] In S8, based on the calculation results of the detailed finite element model, stress, strain and connector loads are extracted for the entire airfoil structure; the strength of the entire structural component and the strength of the adhesive tape or tension / compression block connection area are analyzed to identify the minimum margin, discover test risks, and clarify the risk occurrence area.

[0056] Example 2:

[0057] The structure of the wing box segment in this invention includes a front beam, a rear beam, an upper wall panel, a lower wall panel, and wing ribs.

[0058] In this embodiment, the virtual test loading calculation method for wing structure based on digital simulation mainly includes the following steps:

[0059] Step 1: Based on the wing structure model, perform detailed finite element modeling of the wing spars, panels, and ribs using two-dimensional shell elements. The modeling should include the actual thickness, offset, and other properties of the structure, and quadrilateral elements should be used as much as possible to ensure the quality of the element mesh.

[0060] Step 2: Select appropriate fastener elements for simulation based on the characteristics of the fasteners. For example, if two fasteners have adjacent meshes (number < 2) within a continuous interval, and the fasteners are subjected to shear loads, then CBUSH elements can be used for point-to-point connection instead of adding MPC connections. If the number of meshes between fasteners exceeds 3, it is more accurate to use an MPC+CBUSH+MPC connection method for fastener simulation.

[0061] The "CBUSH" and "MPC" elements are special composite connection elements used in the digital simulation software MSC.NASTRAN to simulate the behavior of fasteners in structural components. By assigning element properties, the flexibility, damping, and constraint conditions of fasteners can be simulated to accurately simulate real connection behavior and stress distribution. In practice, the tensile stiffness of the fastener is calculated using beam theory, and the shear stiffness is calculated using the Huss formula. For stiffness characteristics with a small impact on the analysis, simplified values ​​can be assigned; for example, torsional stiffness can be assigned a value of 100 N / mm² / rad, and bending stiffness can be assigned a value of 10⁹ N / mm² / rad. 2 / rad, etc.;

[0062] Step 3: Based on the geometric center coordinates of the tape or tension block obtained from the test load distribution scheme, the center coordinates of the loading point are determined.

[0063] Step 4: In typical digital simulations, loads are applied directly at the center of the loading point, resulting in significant deviations in the surrounding stress distribution. This invention provides the following loading method: If the load is applied using adhesive tape, an MPC element with the same size coverage area as the adhesive tape is created, and loading is applied based on the stiffness of the structural connection area. If the load is applied using tension / compression blocks, a double-layer solid element (such as the CHEXA8 element in NASTRAN software) with the same size coverage area as the tension / compression block is created. If structures such as rubber pads exist, an additional layer of elements should be added near the structural side to simulate the stiffness characteristics of the connection surface, rubber pads, etc. MPC elements are used on the top surface of the solid element to simulate the loading.

[0064] Step 5: After loading is completed, conduct simulation analysis. Typically, the load is applied according to the initial load direction, and the load is discretized to a single loading point. For a single loading point, the load is first applied in a direction perpendicular to the chord plane, and the force following option in the nonlinear calculation is enabled to obtain the coordinates of the center node of the loading point after deformation. Then, the coordinates of the actuator connection point are obtained based on the position of the actuator of the gantry installed in the experiment.

[0065] Step 6: Connect the coordinates of the two points obtained in the previous steps to obtain the direction of the actual loading vector. The loading vector direction is obtained for each discretized loading point.

[0066] Step 7: Load each discrete loading point in the simulation model and constrain it according to the experimental constraints. After debugging the model, use NASTRAN or Abaqus software to carry out simulation analysis combining geometric nonlinearity and material nonlinearity. Perform linear / nonlinear static, buckling and post-buckling calculations as needed.

[0067] Step 8: Based on the calculation results of the detailed finite element model, extract the stress, strain, and connector loads for the entire airfoil structure. Analyze the strength of the entire structural component, as well as the strength of the tape / pressure block connection area, to identify the minimum margin, discover experimental risks, and clarify the risk occurrence areas;

[0068] Step 9: Attach strain gauges to the locations identified as risk points in the test, monitor the strain state during the test, and promptly detect any abnormalities.

[0069] Step 10: Test verification. If any abnormal situation occurs during the test, such as the strain significantly exceeding the calculated value and showing an amplifying trend, stop the test in time, strengthen the local area, and repeat steps 7 to 9 to restart the test. This can effectively avoid the loss of the test specimen.

[0070] The above description is merely a specific embodiment of the present invention, but the scope of protection of the present invention is not limited thereto. Any variations or substitutions that can be easily conceived by those skilled in the art within the technical scope disclosed in the present invention should be included within the scope of protection of the present invention. Therefore, the scope of protection of the present invention should be determined by the scope of the claims.

Claims

1. A virtual test loading analysis method for wing structure based on digital simulation, characterized in that, Includes the following steps: S1: Perform detailed finite element modeling based on the wing structure digital model, including the actual dimensions and properties of the wing structure; S2: Based on the characteristics of the connector, calculate the properties of the connector using the simplification principle of the bush unit and assign values; S3: Determine the center coordinates of the loading point based on the location of the tape or tension block in the test load distribution scheme; S4: If the test uses adhesive tape for loading, then create an MPC unit with the same size as the adhesive tape; if the test uses tension / compression block for loading, then create a double-layer unit with the same size as the tension / compression block for loading. S5: After loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction. The load is discretized to a single loading point. Then, the coordinates of the center node of the loading point and the actuator connection point are recorded after deformation. S6: Connect the coordinates of the center node of the loading point and the actuator connection point after deformation to obtain the direction of the loading vector; S7: Load all loading points of the simulation model, constrain them according to the experimental constraints, carry out simulation analysis combining geometric nonlinearity and material nonlinearity, and perform linear / nonlinear static, buckling and post-buckling calculations; S8: Based on the calculation results of the detailed finite element model, analyze the stress and strain, and identify the locations of experimental risks; S9: Attach strain gauges at locations identified as test risk points in the analysis; S10: Test verification. If any abnormal situation occurs during the test, stop the test in time, perform local reinforcement, and repeat S7 to S9 to restart the test.

2. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S1, according to the wing structure digital model, the wing spars, panels and rib structures are modeled in detail using two-dimensional shell elements. The model includes the actual thickness and actual offset properties of the structure.

3. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S2, based on the characteristics of the fasteners: if the meshes of two fasteners are adjacent within a continuous interval and the fasteners are subjected to shear loads, then point-to-point connection using CBUSH elements is used; if the number of meshes between fasteners exceeds 3, the connection form of MPC+CBUSH+MPC should be used as much as possible for fastener simulation.

4. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S3, the geometric center coordinates of the adhesive tape or tension block obtained from the experimental load distribution scheme are the center coordinates of the loading point.

5. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S4, if the test involves loading with adhesive tape, an MPC unit with the same size coverage area as the adhesive tape is established, and loading is implemented based on the stiffness of the structural connection area. If the load is applied by a tension / compression block, a double-layer solid element with the same size coverage area as the tension / compression block is established. If a rubber pad structure exists, an additional layer of elements is added near the structure to simulate the stiffness characteristics of the rubber pad structure at the connection surface. MPC elements are used on the top surface of the solid element to simulate the loading.

6. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S5, after loading is completed, simulation analysis is carried out. Loading is performed according to the initial load direction, and the load is discretized to a single loading point. For a single loading point, loading is first performed in the direction perpendicular to the chord plane, and the force following option in nonlinear calculation is turned on to obtain the coordinates of the center node of the loading point after deformation. Then, the coordinates of the actuator connection point are obtained according to the position of the gantry loading actuator in the test installation.

7. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S6, the coordinates of the two points, the center node of the deformed loading point and the actuator connection point, are connected to obtain the direction of the real loading vector. The loading vector direction is obtained for each discretized loading point.

8. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S7, each discrete loading point in the simulation model is loaded and constrained according to the experimental constraints. After debugging the model, NASTRAN or Abaqus software is used to carry out simulation analysis combining geometric nonlinearity and material nonlinearity. Linear / nonlinear static, buckling and post-buckling calculations are performed as needed.

9. The virtual test loading analysis method for wing structure based on digital simulation according to claim 1, characterized in that, In S8, based on the calculation results of the detailed finite element model, stress, strain, and connector loads are extracted from the entire airfoil structure; the strength of the entire structural component and the strength of the adhesive tape or tension / compression block connection area are analyzed, thereby identifying the minimum margin, discovering test risks, and clarifying the risk occurrence area.

Images