Simplified finite element structural analysis method based on stiffness equivalence

Abstract

The present invention relates to the field of numerical analysis technology, in particular to a finite element structure simplified analysis method based on stiffness equivalence, which is implemented using finite element software abaqus. The entire simplified analysis process is divided into three stages: establishing an equivalent structure model, calculating an equivalent stiffness matrix, and calculating a target structure, which are calculated sequentially. Through the stiffness attribute, the influence of the equivalent structure on the mechanical calculation of the target structure is considered, and compared with the general simplified method, the force characteristics of the target structure can be simulated more accurately.

Description

Technical Field

[0001] The present invention relates to the technical field of numerical analysis, and particularly to a finite element structural simplified analysis method based on stiffness equivalence. Background Art

[0002] With the rapid development of computer technology, the finite element method has been more and more widely used to solve complex engineering problems, thus avoiding the establishment of cumbersome mechanical and mathematical models, and it is a practical and efficient numerical analysis method. In order to calculate the mechanical properties of engineering structures more accurately, usually the real shape and boundary conditions of the structure are simulated as much as possible during modeling, but this will also consume more computing resources and reduce the computing efficiency. Especially for the engineering design of large structures, usually the local structure is continuously iteratively optimized. For example, when conducting the strength design of the offshore wind power cylindrical foundation structure, after the cylindrical structure below the mud surface is determined, it is necessary to adjust and check the stress of the upper transition section structure many times to ensure that the final structure meets the economic and strength design requirements; in this process, whether to consider the influence of the cylinder-soil interaction on the stress calculation result of the upper structure is very significant. Although considering the cylinder-soil interaction can more truly reflect the mechanical characteristics of the foundation structure and the calculation result is more accurate, it will also greatly increase the calculation workload and take longer. For the problem of needing to consider the influence of the overall structure on the mechanical calculation of the local structure and at the same time avoiding the reduction of the calculation efficiency due to the huge amount of data of the overall structure, finding a finite element simplified analysis method is very important for the mechanical calculation of the structure.

[0003] At present, there have been some finite element equivalent methods based on substructures attempting to simplify complex structures, so as to achieve the purpose of both accurate calculation and improved calculation efficiency. However, this method has certain limitations, that is, it can only perform numerical simulation based on the same finite element software, and it is impossible to comprehensively utilize the advantages of two software to perform simulation calculation on the same structure. For example, the abaqus commercial software can effectively solve the nonlinear problems of geotechnical engineering, while the ansys software has more advantages in solving the linear and coupling problems of the upper structure. If an equivalent method can be found as a medium for the interaction between the two software, it will more specifically solve different professional problems in the same project and ensure the relative accuracy of the calculation results. The stiffness matrix can be used as such a medium. By inputting the stiffness matrix of the equivalent structure at the interface of software interaction, the mechanical characteristics of the target structure can be calculated. However, the current overall stiffness matrix extraction method is mainly for all element stiffness matrices of the equivalent structure. For the stiffness matrix of a large structure, this amount of data is extremely huge, and it is not applicable for both data storage and transfer input. Summary of the Invention

[0004] In order to effectively solve the problems in the above-mentioned background art, the present invention proposes a finite element structure simplified analysis method based on stiffness equivalence.

[0005] The specific technical solution is as follows:

[0006] A finite element structure simplified analysis method based on stiffness equivalence is implemented using the finite element software abaqus. The entire simplified analysis process is divided into three stages: establishing an equivalent structure model, calculating the equivalent stiffness matrix, and calculating the target structure, which are calculated in sequence.

[0007] Preferably, the stage of establishing the equivalent structure model includes the following steps:

[0008] Step 1: Create an equivalent structure model I, and establish the component models included in the equivalent structure in the equivalent structure model I. The equivalent structure is the part of the overall structure that needs to be equivalently replaced by the stiffness matrix. The equivalent structure usually consists of multiple different components;

[0009] Step 2: Set the material properties and assign them to the corresponding components in the equivalent structure;

[0010] Step 3: Assemble all components to form an assembly;

[0011] Step 4: Set the calculation analysis step; establish a substructure generation analysis step, select the linear perturbation substructure generation option, select the entire equivalent structure model when setting the calculation recovery matrix area, and name the substructure identifier as Z(X), where X is generally an integer greater than or equal to 1;

[0012] Step 5: Establish interactions; set the contact conditions and constraint conditions according to the connection relationships between different components in the equivalent structure;

[0013] Step 6: Set the loads and boundary conditions; no loads are applied in the calculation of the equivalent structure model I, and only the boundary constraint conditions are set: based on the substructure analysis step, select the cross-section part of the equivalent structure that intersects with the following target structure, retain its nodal degrees of freedom, and the remaining boundary constraints are set the same as the boundary constraints inherent in the equivalent structure in the overall structure; the target structure is the part remaining after removing the equivalent structure from the overall structure, and the target structure will be used for the target calculation of the structure;

[0014] Step 7: Perform the finite element mesh division;

[0015] Step 8: Submit the job for calculation to obtain the calculation result _Z(X).sim file.

[0016] Preferably, the calculation of the equivalent stiffness matrix includes the following steps:

[0017] Step 1: Create a substructure model II. Import the calculation result _Z(X).sim file of the equivalent structure model I to form the components of the substructure model II. This component contains all the properties of the equivalent structure model I, including material properties, interactions, loads, boundary conditions, and mesh division. Then assemble the components to form an assembly;

[0018] Step 2: Set the calculation analysis step to static general and the time to 1 second;

[0019] Step 3: Establish an interaction and create a reference point RP 1 , which is generally located at the center of the intersection section of the equivalent structure and the target structure, and couple it with the nodes in the substructure model II that retain degrees of freedom, denoted as the coupling point RP 1 ;

[0020] Step 4: Submit the job for calculation, create a job and write it into an.inp file. Add the keyword for generating the global stiffness matrix to this.inp file, resubmit the modified.inp file for calculation, obtain the calculation result.mtx file, and organize to obtain the stiffness matrix of the coupling point RP 1 , and this matrix is the equivalent stiffness matrix.

[0021] Preferably, the calculation of the target structure includes the following steps:

[0022] Step 1: Create a target structure model III. The modeling methods for the components, material properties, and assembly of the target structure in the target structure model III are the same as those for the equivalent structure in the equivalent structure model I;

[0023] Step 2: Set the calculation analysis step and set the corresponding calculation analysis step according to the calculation objective;

[0024] Step 3: Establish an interaction and create a reference point RP 2 , in principle, this point and the point RP 1 are points at the same position in the overall structure. Select the cross-section part of the target structure that intersects with the above equivalent structure, and couple it with the point RP 2 , denoted as the coupling point RP 2 . Establish a connector at the coupling point RP 2 , and input the equivalent stiffness matrix in the connection property settings, then assign the connection property to the connector; then set the remaining contact conditions and constraint conditions according to the connection relationships between different components in the target structure;

[0025] Step 4: Set the loads and boundary conditions. Set the corresponding load conditions according to the calculation objective, and set the equivalent boundary constraints for the connector according to the boundary constraints inherent to the target structure in the overall structure;

[0026] Step 5: Perform the finite element mesh division;

[0027] Step 6: Submit the job for calculation.

[0028] Compared with the prior art, the beneficial effects of the present invention are as follows: 1. Through the stiffness attribute, the influence of the equivalent structure on the mechanical calculation of the target structure is considered. Compared with the general simplification method, the stress characteristics of the target structure can be simulated more accurately.

[0029] 2. Through structural simplification, the problems of low calculation efficiency, long calculation time, and even inability to calculate caused by the huge amount of calculation data of the overall structure are avoided, and the calculation efficiency of the finite element method is greatly improved on the premise of meeting the calculation accuracy requirements.

[0030] 3. Through the form of the stiffness matrix, it can be input at the interaction interface of different software, so that the advantages of different software can be integrated to perform simulation calculations on the same structure, and different professional problems in the same project can be solved more pertinently, effectively expanding the application scope of the finite element method.

[0031] 4. Through the equivalent stiffness matrix, the problem of insufficient data storage space caused by the original stiffness matrix extraction method can be avoided, and the storage space is effectively saved on the premise of meeting the calculation accuracy requirements, which is convenient, feasible and easy to calculate. Description of the Drawings

[0032] Figure 1 It is a schematic diagram of the overall structure (offshore wind turbine structure);

[0033] Figure 2 It is a schematic diagram of the equivalent structure (lower barrel-soil structure);

[0034] Figure 3 It is a schematic diagram of the sub-structure;

[0035] Figure 4 It is a schematic diagram of the target structure (upper tower barrel jacket structure);

[0036] Figure 5 It is a flowchart of the implementation of the present invention. Detailed Embodiment

[0037] For ease of description, spatial relative terms such as "above", "over", "on the upper surface", "upper" etc. can be used here to describe the spatial positional relationship of a device or feature shown in the figure with other devices or features. It should be understood that spatial relative terms are intended to include different orientations in use or operation in addition to the orientation described in the figure for the device. For example, if the device in the attached drawing is inverted, a device described as "above" or "over" other devices or structures will then be positioned "below" or "under" other devices or structures. Thus, the exemplary term "above" can include both the orientations of "above" and "below". The device can also be positioned or rotated in other different ways by 90 degrees or in other orientations, and corresponding interpretations will be made for the spatial relative descriptions used here.

[0038] Introduction to example working conditions: It is intended to conduct an analysis of the natural vibration frequency of the entire structure of an offshore wind turbine (see the attached Figure 1 ), calculate using the finite element structural simplified analysis method based on stiffness equivalence of the present invention, and compare the calculation results with those calculated by the traditional finite element method to illustrate the feasibility of the present invention.

[0039] The specific steps are as follows:

[0040] The first stage: Establish an equivalent structure model

[0041] Step 1: See the attached Figure 2 , create a new equivalent structure model I, and establish models of each component included in the equivalent structure in the equivalent structure model I, including: soil body 1, steel cylinder 2, and local jacket 8 (since it is not easy to select unit nodes at the cross-section mutation position, therefore, when modeling, retain the local structure model of the overall jacket 3 to make the calculation results more accurate).

[0042] Step 2: Set the material properties and assign them to the corresponding components in the equivalent structure.

[0043] In Step 1 and Step 2, the model dimensions and material parameters are set as shown in Table 1:

[0044] Table 1 Equivalent structure model dimensions and material parameters

[0045]

[0046] Step 3: Assemble all components to form an assembly.

[0047] Step 4: Set the calculation analysis step. Establish a substructure generation analysis step, select the linear perturbation substructure generation option, select the entire equivalent structure model when setting the calculation recovery matrix area, and name the substructure identifier as Z1.

[0048] Step 5: Establish interaction. The contact type between the soil mass 1 and the steel cylinder 2 is selected as surface-to-surface contact, with finite slip adopted. The normal behavior is set to "hard" contact, and the penalty function for the tangential behavior is taken as 0.35. The bottom edge of the local jacket 8 and the cylinder top cover 6 are subjected to a tied constraint.

[0049] Step 6: Set loads and boundary conditions. No loads are applied in the calculation of the equivalent structural model I, and only boundary constraint conditions are set: Based on the substructure analysis step, select the top edge part of the local jacket 8, and retain its nodal degrees of freedom; set a fixed constraint at the bottom boundary of the soil mass 1, and only vertical displacement is allowed at the side boundary.

[0050] Step 7: Perform finite element mesh division.

[0051] Step 8: Submit the job for calculation to obtain the calculation result _Z1.sim file.

[0052] The second stage: Calculate the equivalent stiffness matrix

[0053] Step 1: Create a new substructure model II as shown in the appendix Figure 3 Import the calculation result _Z1.sim file of the equivalent structural model I into the substructure model II to form the components of the substructure model II. This component contains all the properties of the equivalent structural model I, including material properties, interactions, loads and boundary conditions, and mesh division. Then assemble the components to form an assembly.

[0054] Step 2: Set the calculation analysis step as static general and the time as 1 second.

[0055] Step 3: Establish interaction. Create a reference point RP 1 , which is located at the center of the top section of the local jacket in the substructure, and couple it with the nodes that retain degrees of freedom in the substructure model II, denoted as the coupling point RP 1 .

[0056] Step 4: Submit the job for calculation. Create a job and write it into the.inp file. Add the keyword for generating the global stiffness matrix to this.inp file, resubmit the modified.inp file for calculation, obtain the calculation result.mtx file, and organize to obtain the stiffness matrix of the coupling point RP 1 , and this matrix is the equivalent stiffness matrix.

[0057] The third part: The target structural model III

[0058] Step 1: Refer to the appendix Figure 4Create a new target structure model III. The modeling methods of the components, material properties, and assemblies of the target structure in target structure model III are the same as those of the equivalent structure in equivalent structure model I. Each component model includes: the main jacket 9, the flange transition section 4, and the tower barrel 5. The main dimensions and material parameters of the model are set as shown in Table 2:

[0059] Table 2 Main Dimensions and Material Parameters of the Target Structure Model

[0060]

[0061] Step 2: Set up the calculation analysis step. Establish a frequency calculation analysis step, select the linear perturbation frequency option, and set the number of eigenvalues to 20, that is, calculate the first 20 order modal vibration modes.

[0062] Step 3: Establish interactions. Create a reference point RP 2 , and couple it with the bottom edge of the main jacket 9, denoted as the coupling point RP 2 . Establish a connector at the coupling point RP 2 , and input the equivalent stiffness matrix in the connection property settings, then assign the connection properties to the connector; calculate the position of the mass point (equivalent the blade and the nacelle as mass points), and couple the mass point with the center of the upper surface of the flange of the tower barrel 5, and assign mass and moment of inertia to the mass point through special-inertia; the connections between other components in the target structure all adopt bonded constraints.

[0063] Step 4: Set the loads and boundary conditions. Set a fixed constraint at the bottom boundary of the connector.

[0064] Step 5: Perform the finite element mesh division.

[0065] Step 6: Submit the job for calculation.

[0066] Calculate according to the finite element structure simplified analysis method based on stiffness equivalence of the present invention. The calculation process is shown in the appendix Figure 5 , and compare the calculation results with those calculated by the traditional finite element method. The comparison results are shown in Table 3. It can be seen that the simplified analysis method of the present invention is in good agreement with the calculation results of the traditional finite element method, indicating that the finite element structure simplified analysis method based on stiffness equivalence of the present invention is feasible.

[0067] Table 3 Comparative Analysis of the Calculation Results of Natural Vibration Frequencies

[0068]

[0069] The above are only the preferred embodiments of the present invention. It should be noted that for those of ordinary skill in the art, without departing from the principle of the present invention, several improvements and modifications can be made, and these improvements and modifications should also be regarded as the protection scope of the present invention.

Claims

1. A simplified finite element structural analysis method based on stiffness equivalence, characterized in that: The finite element software abaqus was used for implementation. The entire simplified analysis process was divided into three stages: establishing an equivalent structural model, calculating the equivalent stiffness matrix, and calculating the target structure, which were calculated in sequence; The establishment of an equivalent structural model includes the following steps: Step 1-1: Create a new equivalent structure model I, and establish models of each component included in the equivalent structure in the equivalent structure model I. The equivalent structure is the part of the overall structure that needs to be equivalently replaced by the stiffness matrix; Step 1-2: Set material properties and assign them to corresponding parts; Step 1-3: Assemble all parts to form an assembly; Step 1-4: Set the calculation analysis step and establish the substructure generation analysis step; Steps 1-5: Establish interactions, set contact conditions and constraints; Step 1-6: Set loads and boundary conditions; no loads are applied in the calculation of the equivalent structure model I, and only boundary constraints are set: based on the substructure analysis step, select the cross-sectional area in the equivalent structure that intersects with the following target structure, retain its node degrees of freedom, and the remaining boundary constraints are set the same as the boundary constraints of the equivalent structure in the overall structure; the target structure is the part of the overall structure that remains after removing the equivalent structure, and the target structure will be used for the target calculation of the structure; Step 1-7: Divide the finite element mesh; Step 1-8: Submit the job for calculation and obtain the calculation result file; Calculating the equivalent stiffness matrix includes the following steps: Step 2-1: Create a new substructure model II, and import the calculation result file of the equivalent structure model I into the substructure model II to form the components of the substructure model II; Step 2-2: Set the calculation analysis step to static general; Step 2-3: Establish interaction and create a reference point RP1, located at the center of the intersection section between the equivalent structure and the target structure, and couple it with the node with the reserved degrees of freedom in the substructure model II, recorded as coupling point RP1; Step 2-4: Submit the job for calculation, add the keyword to generate the overall stiffness matrix, and obtain the stiffness matrix of the coupling point RP1, which is the equivalent stiffness matrix; Computing the target structure includes the following steps: Step 3-1: Create a new target structure model III. The modeling method of the components, material properties and assembly of the target structure in the target structure model III is the same as the modeling method of the equivalent structure in the equivalent structure model I; Step 3-2: Set the calculation analysis step; Step 3-3: Establish interaction and create reference point RP2, which is at the same position as point RP1 in the overall structure. Select the cross-sectional area in the target structure that intersects with the above equivalent structure, couple it with point RP2, record it as coupling point RP2, establish a connector at coupling point RP2, and enter the equivalent stiffness matrix in the connection property settings; Step 3-4: Set loads and boundary conditions; Step 3-5: Divide the finite element mesh; Step 3-6: Submit the job for calculation.

Images