Finite element simulation method for analyzing debonding progressive damage of T-shaped joint of composite material
Through the finite element simulation method, combined with the Mises strength criterion and Hashin failure criterion, the damage process of composite T-type joints is simulated, and the problem of complexity of the overall structural damage analysis of composite materials is solved, and the progressive damage of T-type bonding joints is achieved The accurate analysis improves the scientific nature of structural health monitoring and the safety of the aircraft.
Patent Information
- Application Number
- CN202410988928.9
- Authority / Receiving Office
- CN · China
- Patent Type
- Applications(China)
- Current Assignee / Owner
- Filing Date
- 2024-07-23
- Publication Date
- 2024-11-12
AI Technical Summary
The overall structural damage analysis of composite materials is complex, especially in aircraft applications. It is difficult to accurately predict the progressive damage process of T-type adhesive joints, which affects structural health monitoring and safety.
Using finite element simulation method, the VUMAT subroutine was written to simulate the damage process of composite T-type joints in ABAQUS software through the Mises strength criterion and strain-based three-dimensional Hashin failure criterion, so as to realize gradual damage analysis, and define the damage of the glue layer in combination with energy method. Evolution to ensure the accuracy of the calculation results.
It improves the accuracy of damage analysis of composite T-type joint structures, provides calculation results that are closer to reality, enhances the scientificity and early warning capabilities of structural health monitoring, reduces maintenance costs, and improves the safety of the aircraft.
Smart Images

Figure CN118940575A_ABST
Abstract
Description
Technical Field
[0001] The invention belongs to the field of finite element simulation of composite materials, and in particular relates to a finite element simulation method for debonding progressive damage analysis of a T-shaped adhesive joint of a composite material. Background Art
[0002] Advanced Composite Materials (ACM) refers to composite materials made of high-performance reinforcing phases such as carbon fiber, fabric, and whisker. With its outstanding advantages such as high specific strength, high specific modulus, low density, strong designability, excellent fatigue resistance, strong corrosion resistance, and easy large-area integral molding, it has shown its strong vitality as soon as it came out. It has incomparable superior performance over traditional steel, aluminum alloy and other materials, and has been widely used in aircraft. As the dominant material in the 21st century, the amount of composite materials used has become an important indicator of the advancement of aircraft and even the advancement of the aerospace field.
[0003] The application of composite materials makes it easy to realize the integral forming of aircraft structures, which is also one of the unique advantages and characteristics of composite materials. Composite integral structure refers to an integral part designed and manufactured by designing and manufacturing several composite components using technologies such as co-curing, co-bonding, secondary bonding, and preform liquid molding process methods. The integral structure reduces the number of structural parts, improves the efficiency and reliability of the structure, and reduces the manufacturing cost. However, due to the heterogeneity and anisotropy of composite materials, there are many interface areas and defects, and environmental changes in applications. The damage forms of composite materials are multiple, the failure modes are diverse, the damage evolution laws and failure processes span the micro and macro scales, and the damage analysis and strength prediction are very complex. With the development of composite integral structures and their extensive application in aircraft, a series of problems to be studied have also emerged, and composite integral structure damage monitoring is one of them.
[0004] Research on health monitoring technology for overall structures of composite materials can provide necessary, reasonable and scientific theoretical support for the application of health monitoring technology in overall structures of composite materials. It can also provide a simple and effective health monitoring method for overall structure quality assurance, product acceptance, working status evaluation and failure warning, achieve early warning of structural damage and load prediction, reduce or avoid catastrophic accidents, and play a very important role in improving the safety, intelligence and flexibility of aircraft and reducing maintenance costs. Summary of the invention
[0005] According to the technical problems raised above, the present invention provides a finite element simulation method for debonding progressive damage analysis of composite T-shaped adhesive joints, so as to be closer to the actual process and ensure more accurate calculation results.
[0006] The technical solution adopted by the present invention is as follows:
[0007] The finite element simulation method for debonding progressive damage analysis of composite material T-joints of the present invention is as follows:
[0008] Step S1: Select the Mises strength criterion as the damage criterion of the filler in the composite T-joint, and simulate the failure of the filler in the composite T-joint by writing the subroutine VUMAT_MAT1;
[0009] Step S2: Select the strain-based three-dimensional Hashin failure criterion as the damage criterion for the L-type laminate and the strip-type laminate in the composite T-joint, and simulate the failure of the L-type laminate and the strip-type laminate in the composite T-joint by writing the subroutine VUMAT_MAT2;
[0010] Step S3: The finite element software ABAQUS is used to establish a progressive damage analysis model for debonding of composite T-joints, so as to realize the debonding analysis of composite T-joints subjected to displacement loads.
[0011] Further, step S1 comprises:
[0012] Step S11: Open the Visual Studio compiler and input the ABAQUS solver interface code;
[0013] Step S12: Add an IF statement and write a VUMAT subroutine that calls subroutines VUMAT_MAT1 and VUMAT_MAT2;
[0014] Step S13: Write a subroutine VUMAT_MAT1, set variables and dimensions, and write material properties according to the user material (USER MATERIAL) set in ABAQUS; input the code of Mises failure criterion and stiffness matrix; write stress calculation, and then determine whether the filler fails. If failure occurs, perform stiffness degradation processing;
[0015] Furthermore, the VUMAT subroutine that calls subroutine VUMAT_MAT1 and subroutine VUMAT_MAT2 is as follows:
[0016] IF(CMNAME.EQ.'MATERIAL-1')THEN
[0017] CALL VUMAT_MAT1
[0018] ELSEIF(CMNAME.EQ.'MATERIAL-2')THEN
[0019] CALL VUMAT_MAT2
[0020] END IF;
[0021] Further, step S2 is specifically as follows: after the subroutine VUMAT_MAT1, a subroutine VUMAT_MAT2 is written, a user-defined material is input, a strain-based three-dimensional Hashin failure criterion, and a code of a stiffness matrix are input, and whether the L-type laminate and the strip-type laminate are damaged is determined by the strain-based three-dimensional Hashin failure criterion, and if damage occurs, the elastic modulus and / or shear modulus is multiplied by a reduction factor to perform stiffness degradation processing;
[0022] Among them, the strain-based three-dimensional Hashin failure criterion includes the following failures:
[0023] 1) Fiber stretching:
[0024]
[0025] 2) Fiber compression:
[0026]
[0027] 3) Matrix stretching:
[0028]
[0029] 4) Matrix compression:
[0030]
[0031] 5) In-plane shear:
[0032]
[0033] 6) Out-of-plane shear:
[0034]
[0035] Among them, 1, 2, and 3 represent the fiber direction (X), the in-plane vertical direction (Y), and the out-of-plane vertical direction (Z), respectively, and XYZ constitutes a three-axis rectangular coordinate system. 11T and ε 11C is the tensile and compressive failure strain in the fiber direction, ε 22T and ε 22C are the tensile and compressive failure strains in the matrix direction, ε ijf (i,j=1,2,3,i≠j) is the shear failure strain.
[0036] Further, step S3 includes:
[0037] Step S31: Establishing a composite material T-joint model through ABAQUS;
[0038] Step S32: dividing the composite material T-joint model into regions by using the splitting function in the mesh module;
[0039] Step S33: Meshing the composite T-joint model: Meshing two L-joints and one laminate, and selecting the C3D8R reduced integration unit; segmentation processing is performed at the filler, and the C3D4 tetrahedron unit is selected to solve the invalid mesh caused by extreme stress concentration during the calculation process; the glue layer is specified by editing the mesh function, and the glue layer selects the Cohesive unit, which is connected to other units in a shared node manner, and the theoretical thickness is set to 0, so as to achieve the coordination of force transmission and displacement between the units;
[0040] Step S34: assigning material parameters in the property module and defining the damage evolution of the adhesive layer by the energy method;
[0041] Step S35: after setting the analysis step, set the load and boundary conditions, apply a tensile displacement load to the glued ends of the two L-shaped laminates, and apply a completely fixed constraint to the back of the strip-shaped laminate;
[0042] Step S36: Select the VUMAT subroutine in the JOB module, submit the job, and call the VUMAT subroutine to solve the problem.
[0043] Furthermore, in step S34, the energy method defines the stiffness degradation after the adhesive layer is damaged, specifically:
[0044] Introducing criteria:
[0045]
[0046] The degree of adhesive layer damage is defined as D = 0, indicating that the adhesive layer is not damaged; D = 1, indicating that the adhesive layer is completely damaged. IC , G IIC They represent the critical strain energy release rate per unit length of the adhesive material under type I load and type II load, respectively. I , G II They represent the current strain energy release rate per unit length of the material under type I load and type II load, respectively.
[0047] After the damage occurs, the stiffness of the adhesive layer is expressed as:
[0048] E=(1-D)E 0 , G=(1-D)G 0
[0049] In the formula, E 0 , G 0It represents the elastic modulus and shear modulus when the adhesive layer is not damaged, and E and G represent the elastic modulus and shear modulus after the adhesive layer is damaged.
[0050] Furthermore, in step S36, before calling the VUMAT subroutine, it is limited that the stress calculation of the filler is performed only when the finite element calculation result is converged, otherwise the filler is meshed and the finite element calculation is performed again.
[0051] The present invention has the beneficial effects:
[0052] The present invention provides a finite element simulation method for debonding progressive damage analysis of a composite material T-joint. The composite material T-joint structure consists of two L-shaped laminates, a strip laminate, a filler and an adhesive layer. With respect to the damage criterion of the filler, a Mises strength criterion applicable to plastic materials is selected as a damage criterion. With respect to the damage criterion of the L-shaped laminate and the strip laminate, a strain-based three-dimensional Hashin failure criterion is selected as the damage criterion. With respect to the damage criterion of the adhesive layer, the damage evolution of the adhesive layer is defined by an energy method. Meanwhile, two subroutines VUMAT_MAT are called in a VUMAT subroutine. Finite element simulation software is used to perform numerical simulation analysis on the composite material T-joint structure, so that the simulation method of the present invention is closer to reality and the calculation result is guaranteed to be more accurate. BRIEF DESCRIPTION OF THE DRAWINGS
[0053] Figure 1 The present invention is a flow chart of a finite element simulation method for progressive damage analysis of a composite material T-joint.
[0054] Figure 2 It is a schematic structural diagram of the composite material T-joint in the present invention.
[0055] Figure 3 It is a simulation flow chart of filler failure in the present invention.
[0056] Figure 4 The figure is a flow chart of finite element calculation of failure of composite material layer (L-type laminate or strip-type laminate) of the present invention.
[0057] Figure 5 This is a model diagram of the composite material T-joint in the present invention.
[0058] Figure 6 Schematic diagram of the boundary conditions of the composite T-joint in the present invention. DETAILED DESCRIPTION
[0059] In order to further understand the content of the present invention, further detailed description is made below in conjunction with the accompanying drawings. It should be understood that the embodiments are only used to explain the present invention but not to limit it.
[0060] As attached Figure 2 As shown, the composite material T-joint includes two L-shaped laminates, a strip laminate (a Skin laminate is used in this embodiment), a filler (mainly made of plastic material) and an adhesive layer. A filler area is formed between the strip laminate and the two L-shaped laminates, the filler is placed in the filler area, and the strip laminate and the two L-shaped laminates, the strip laminate and the filler, the filler and the two L-shaped laminates, and the two L-shaped laminates are all bonded by the adhesive layer.
[0061] As attached Figure 1 As shown in FIG. 1 , the finite element simulation method for debonding progressive damage analysis of composite T-joints has the following steps:
[0062] Step S1: Select the Mises strength criterion applicable to plastic materials as the damage criterion of the filler, and simulate the failure of the filler by writing the subroutine VUMAT_MAT1;
[0063] Step S2: Select the strain-based three-dimensional Hashin failure criterion as the damage criterion for the L-type laminate and the strip-type laminate, and simulate the failure of the L-type laminate and the strip-type laminate by writing the subroutine VUMAT_MAT2;
[0064] Step S3: The finite element software ABAQUS is used to establish a debonding progressive damage analysis model for carbon fiber composite T-shaped adhesive joints to realize the debonding analysis of composite T-shaped adhesive joints subjected to displacement loads.
[0065] Step S1 includes:
[0066] Step S11: Open the Visual Studio compiler and input the ABAQUS solver interface code;
[0067] Step S12: Add an IF statement and write a VUMAT subroutine that calls subroutines VUMAT_MAT1 and VUMAT_MAT2;
[0068] IF(CMNAME.EQ.'MATERIAL-1')THEN
[0069] CALL VUMAT_MAT1
[0070] ELSEIF(CMNAME.EQ.'MATERIAL-2')THEN
[0071] CALL VUMAT_MAT2
[0072] END IF
[0073] Step S13: Write the subroutine VUMAT_MAT1, set the variables and dimensions, write the material properties according to the user material (USER MATERIAL) set in Abaqus, and enter the Mises failure criterion, stiffness matrix and other codes; the simulation flow chart of filler failure is shown in the attached figure. Figure 3 As shown, write the stress calculation, then determine whether the filler fails, and if failure occurs, perform stiffness degradation processing.
[0074] Step S2 includes: writing a subroutine VUMAT_MAT2 after the subroutine VUMAT_MAT1, inputting a user-defined material, a strain-based three-dimensional Hashin failure criterion, a stiffness matrix and other codes, and judging whether damage occurs (fiber tensile damage parameter F) through an IF statement. ft , fiber compression damage parameter F fc , matrix tensile damage parameter F mt , matrix compression damage parameter F mc , in-plane shear damage parameter F ip , out-of-plane shear damage parameter F op If any of them exceeds 1, damage occurs. If damage occurs, the elastic modulus and / or shear modulus is multiplied by the reduction factor to perform stiffness degradation processing, as shown in the attached Figure 4 As shown here, attached Figure 4 When the displacement load is increased, the strain also increases accordingly.
[0075] The strain-based three-dimensional Hashin failure criterion includes the following failures:
[0076] 1). Fiber stretching:
[0077]
[0078] 2). Fiber compression:
[0079]
[0080] 3). Matrix stretching:
[0081]
[0082] 4). Matrix compression:
[0083]
[0084] 5). In-plane shear:
[0085]
[0086] 6). Out-of-plane shear:
[0087]
[0088] Among them, 1, 2, and 3 represent the fiber direction (X), the in-plane perpendicular direction (Y), and the out-of-plane perpendicular direction (Z), respectively. 11T and ε 11C is the tensile and compressive failure strain in the fiber direction, ε 22T and ε 22C are the tensile and compressive failure strains in the matrix direction, ε ijf (i,j=1,2,3,i≠j) is the shear failure strain.
[0089] As attached Figure 4 As shown in Table 1, when the material is damaged, the elastic modulus and shear modulus of the material are reduced macroscopically. The corresponding elastic modulus and shear modulus are reduced, and the reduction coefficients are shown in Table 1.
[0090] Table 1 Reduction scheme when the modulus of the material is reduced
[0091]
[0092]
[0093] Step S3 includes:
[0094] Step S31: Establish the target model through ABAQUS, as shown in the attached Figure 5 As shown;
[0095] Step S32: Divide the model into regions using the splitting function in the mesh module;
[0096] Step S33: Mesh the model: mesh two L-shaped plates and one laminate, and select the C3D8R reduced integration unit; perform segmentation at the filler, and define the tetrahedron unit with the material property of C3D4 to solve the invalid mesh caused by extreme stress concentration during the calculation process; specify the glue layer through the mesh editing function, select the Cohesive unit for the glue layer, connect it with other units in the form of shared nodes, and set the theoretical thickness to 0, so as to achieve the coordination of force transmission and displacement between units;
[0097] Step S34: assigning material parameters in the property module and defining the damage evolution of the adhesive layer by the energy method;
[0098] The energy method is used to define the stiffness degradation of the adhesive layer after damage, and the criterion is introduced:
[0099]
[0100] To define the degree of adhesive layer damage, when D = 0, it means that the adhesive layer in this area is not damaged; when D = 1, it means that the adhesive layer in this area is completely damaged and debonding cracks occur. IC , G IIC They represent the critical strain energy release rate per unit length of the material under type I (opening type) load and type II (sliding type) load, respectively. I , G II They represent the current strain energy release rate per unit length of the material under type I (opening type) load and type II (sliding type) load, respectively.
[0101] After the damage occurs, the stiffness of the adhesive layer can be expressed as:
[0102] E=(1-D)E 0 , G=(1-D)G 0
[0103] In the formula, E 0 , G 0 It represents the elastic modulus and shear modulus when the adhesive layer is not damaged, and E and G represent the elastic modulus and shear modulus after the adhesive layer is damaged.
[0104] Step S35: Set the analysis step ( Figure 3 and Figure 4 The setting of displacement load is added in the figure (this is done here), and then the load and boundary conditions are set. A tensile displacement load is applied to the ends of the two L-shaped laminates bonded by the adhesive layer, and a completely fixed constraint is applied to the back of the strip laminate. Figure 6 shown.
[0105] Step S36: Select the VUMAT subroutine in the JOB module, submit the job, and call the VUMAT subroutine to solve. In order to deal with the problem that the C3D4 tetrahedral unit causes the finite element calculation to not converge, before calling the VUMAT subroutine, it is limited that the stress calculation of the filler is only performed when the finite element calculation result is converged, otherwise the filler mesh is encrypted and the finite element calculation is performed again.
Claims
1. Finite element simulation method for debonding progressive damage analysis of composite T-joints, characterized by: The method is as follows: Step S1: Select the Mises strength criterion as the damage criterion of the filler in the composite T-joint, and simulate the failure of the filler in the composite T-joint by writing the subroutine VUMAT_MAT1; Step S2: Select the strain-based three-dimensional Hashin failure criterion as the damage criterion for the L-type laminate and the strip-type laminate in the composite T-joint, and simulate the failure of the L-type laminate and the strip-type laminate in the composite T-joint by writing the subroutine VUMAT_MAT2; Step S3: The finite element software ABAQUS is used to establish a progressive damage analysis model for debonding of composite T-joints, so as to realize the debonding analysis of composite T-joints subjected to displacement loads.
2. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to claim 1 is characterized by: Step S1 includes: Step S11: Open the Visual Studio compiler and input the ABAQUS solver interface code; Step S12: Add an IF statement and write a VUMAT subroutine that calls subroutines VUMAT_MAT1 and VUMAT_MAT2; Step S13: Write the subroutine VUMAT_MAT1, set the variables and dimensions, and write the material properties according to the user material set in ABAQUS; input the code of Mises failure criterion and stiffness matrix; write the stress calculation, and then determine whether the filler fails. If failure occurs, perform stiffness degradation processing.
3. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to claim 2 is characterized by: The VUMAT subroutine that calls subroutine VUMAT_MAT1 and subroutine VUMAT_MAT2 is as follows: IF(CMNAME.EQ.'MATERIAL-1')THEN CALL VUMAT_MAT1 ELSEIF(CMNAME.EQ.'MATERIAL-2')THEN CALL VUMAT_MAT2 END IF.
4. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to claim 1 is characterized by: Step S2 is as follows: after the subroutine VUMAT_MAT1, a subroutine VUMAT_MAT2 is written, user-defined materials are input, a strain-based three-dimensional Hashin failure criterion, and a code of a stiffness matrix are input, and whether damage occurs to the L-type laminate and the strip-type laminate is determined by the strain-based three-dimensional Hashin failure criterion. If damage occurs, the elastic modulus and / or shear modulus are multiplied by a reduction factor to perform stiffness degradation processing; Among them, the strain-based three-dimensional Hashin failure criterion includes the following failures: 1) Fiber stretching: 2) Fiber compression: 3) Matrix stretching: 4) Matrix compression: 5) In-plane shear: 6) Out-of-plane shear: Among them, 1, 2, and 3 represent the fiber direction, the in-plane vertical direction, and the out-of-plane vertical direction, respectively. The three directions constitute a three-axis rectangular coordinate system; ε 11T and ε 11C is the tensile and compressive failure strain in the fiber direction, ε 22T and ε 22C are the tensile and compressive failure strains in the matrix direction, ε ijf (i,j=1,2,3,i≠j) is the shear failure strain.
5. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to any one of claims 1 to 4, characterized in that: Step S3 includes: Step S31: Establishing a composite material T-joint model through ABAQUS; Step S32: dividing the composite material T-joint model into regions by using the splitting function in the mesh module; Step S33: Meshing the composite T-joint model: meshing two L-joints and one laminate, and selecting the C3D8R reduced integration unit; performing segmentation processing at the filler, and selecting the C3D4 tetrahedron unit; specifying the glue layer through the edit mesh function, selecting the Cohesive unit for the glue layer, connecting it with other units in a shared node manner, and setting the theoretical thickness to 0; Step S34: assigning material parameters in the property module and defining the damage evolution of the adhesive layer by the energy method; Step S35: after setting the analysis step, set the load and boundary conditions, apply a tensile displacement load to the glued ends of the two L-shaped laminates, and apply a completely fixed constraint to the back of the strip-shaped laminate; Step S36: Select the VUMAT subroutine in the JOB module, submit the job, and call the VUMAT subroutine to solve the problem.
6. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to claim 5 is characterized by: In step S34, the energy method defines the stiffness degradation after the adhesive layer is damaged, specifically: Introducing criteria: To define the degree of adhesive layer damage, D = 0 means that the adhesive layer is not damaged; D = 1 indicates that the adhesive layer is completely damaged, G IC , G IIC They represent the critical strain energy release rate per unit length of the adhesive material under type I load and type II load, respectively. I , G II They represent the current strain energy release rate per unit length of the material under type I load and type II load respectively; After the damage occurs, the stiffness of the adhesive layer is expressed as: E=(1-D)E0,G=(1-D)G0 Where, E0 and G0 represent the elastic modulus and shear modulus when the adhesive layer is not damaged, and E and G represent the elastic modulus and shear modulus after the adhesive layer is damaged.
7. The finite element simulation method for debonding progressive damage analysis of composite T-joints according to claim 5 is characterized by: In step S36, before calling the VUMAT subroutine, it is limited that the stress calculation of the filler is performed only when the finite element calculation result is converged, otherwise the filler is meshed and the finite element calculation is performed again.
Citation Information
Patent Citations
Low-velocity impact composite material multilayer thick plate progressive failure prediction finite element method
CN106777769A
Progressive damage model-based full-SiC composite material multi-nail connection structure failure analysis method
CN107832560A
Numerical simulation method for Ti / CFRP laminated plate structure under impact load
CN110705142A
Finite element simulation method for progressive damage analysis of composite material bolted connection
CN117828936A
Dynamic Progressive Failure Analysis Method For Composite Multi-Scale Model
US20220284150A1
