An abaqus-based high-efficiency power transmission tower seismic resistance analysis method

Abstract

The application provides a high-efficiency power transmission tower seismic resistance analysis method based on abaqus, first, a 3D model is drawn according to actual design parameters and is imported into abaqus, and basic parameter setting is written to solve the structure input earthquake load, an inp file is obtained by importing a solver, then the earthquake amplitude in the inp file is enlarged and modified, a group of inp files with increasing earthquake intensity are obtained by using a cmd command to automatically import the abaqus solver for calculation, then the odbAccess library in python is used to export the time history curve of the relative displacement of the tower top in the field output variable ODB file with different earthquake intensities, finally, the earthquake intensity and the maximum displacement of the tower top corresponding to the point are plotted, with the increase of the earthquake intensity, the limit of the power transmission tower is gradually approached, and the steep increase curve of the tower top displacement under the intensity is the obvious inflection point, and the earthquake intensity corresponding to the point is used to measure the seismic resistance performance.

Description

Technical Field

[0001] This invention relates to the fields of finite element simulation and dynamic stability analysis, and in particular to a high-efficiency seismic analysis method for transmission towers based on Abaqus. Background Technology

[0002] Power transmission lines are the lifeline of my country's energy supply. These structures, composed of transmission towers and lines of varying grades, form the main arteries for energy transmission, traversing diverse and complex geographical locations. Much of China's land area is prone to earthquakes, and as the importance of transmission lines for power delivery deepens, the economic losses caused by transmission towers under seismic loads become increasingly concerning. The seismic performance of transmission towers, as tall, flexible steel structures, hinges on their dynamic stability under dynamic loads. Studying the structural response of transmission towers under dynamic loads helps to more intuitively represent their seismic performance, and using finite element method (FEM) software to simulate and analyze transmission tower models with similar parameters helps to comprehensively consider both economic efficiency and practicality.

[0003] Transmission towers are the primary equipment in power transmission and are also the most affected by earthquakes; their seismic performance directly impacts the safety of the entire transmission line. While there are many types of transmission towers, they are currently mainly tall, flexible structures composed of different angle steel combinations, broadly categorized as T-shaped towers, drum-shaped towers, cat-head towers, and goblet towers. Considering these towers in parallel, given their similar properties, can significantly improve efficiency and allow for cross-referencing to verify the accuracy of the analysis. Seismic analysis of transmission towers based on Abaqus finite element simulation technology, leveraging its vast and effective element library, nonlinear simulation capabilities, and advantages such as simple setup, high speed, and adaptive meshing, is widely used in various transmission tower simulations. However, the rich field definitions make the model difficult to converge and prone to singular values, raising the barrier to entry for Abaqus. The introduction of too many nonlinear parameters exponentially increases the computational load, and Abaqus's visual interface also makes it difficult to modify model parameters, further increasing the workload.

[0004] Transmission towers are frame-type steel structures, and their damage is often caused by local components entering a nonlinear state and losing their original material strength, which then extends to the entire structure. The characteristics of the target structure make conventional energy dissipation curves and probabilistic vulnerability seismic analyses difficult to apply. Currently, the optimal solution is to perform a nonlinear analysis of the entire transmission tower under seismic loading to obtain its full-process time-history response. This makes comprehensively representing the entire process of the transmission tower from linear response to nonlinear process until collapse extremely complex. Summary of the Invention

[0005] To address the aforementioned problems, this invention provides a high-efficiency seismic analysis method for transmission towers based on Abaqus. This scheme designs a complete process from detailed modeling of specific transmission towers to simulation result output and finally to seismic performance analysis of transmission towers. Starting with the commonalities of existing transmission tower seismic analysis methods, this invention first solves problems such as overly complex details, model non-convergence, and large computational load in the finite element simulation of transmission towers. While ensuring computational accuracy, it greatly improves the efficiency of seismic analysis of transmission lines, facilitating seismic performance analysis for different types of transmission lines. It can accurately characterize the overall seismic performance of the transmission tower structure, facilitating guidance for actual production, improving the understanding of transmission tower structures, and can be widely applied in the field of transmission line construction and design.

[0006] To achieve the above-mentioned technical features, the objective of this invention is as follows: A high-efficiency seismic resistance analysis method for transmission towers based on Abaqus, characterized by comprising the following steps: Step 1: Based on the design drawings and parameter details in the actual engineering transmission line construction, use the visualization interface in 3D drawing software to draw a 3D point-line model of the transmission tower from points and lines. Step 2: Import the 3D point-line model of the transmission tower established in Step 1 into the Abaqus software and run it to obtain the transmission tower component model information. Then, in Abaqus, based on the parameters obtained in Step 1, create material property assignment beam elements and set parameters according to the corresponding angle steel section. Finally, according to the component model in the transmission tower design, select the predetermined line to assign the section. Step 3: Assemble the transmission tower component models from Step 2 into an overall model and create an analysis step. The analysis step is divided into two steps: the first step is a static general type, used to apply gravity loads, and the second step is a dynamic implicit type, used to apply seismic loads. Step 4: Create a load in the analysis step created in step 3. In analysis step 1, the load is set to gravity. Further, in the boundary conditions of the initial analysis step, set the four tower feet as a set and fix them completely. Transfer this boundary from the initial analysis step to analysis step 1 and deactivate this boundary in analysis step 2. In analysis step 2, deactivate the seismic wave input direction of the fixed tower foot set, set the acceleration boundary in the direction of the proposed input seismic wave, and set the amplitude to the input seismic wave waveform. Step 5: Place the model instance components, assign a mesh with beam element type, establish a job analysis in the job module, set the maximum memory and number of parallel processors, and import the inp file to obtain all parameters of the model from the solver. Step 6: Open the calculation results submitted in Step 5. In the ODB field variable history output interface, select the highest point of the transmission tower and the tower foot position. Export the history information of the displacement of the two points with time variables. Further operate the two sets of data by subtracting the tower foot displacement curve from the tower top displacement curve to obtain the tower top relative displacement time history curve, and obtain the maximum value of the tower top relative displacement in the earthquake history. Step 7: Locate the seismic wave parameters in the model's total parameter inp file obtained in step 5. Scale the input seismic wave amplitude proportionally using the intensity reduction method. Modify the scaled-up values ​​to obtain a new inp file. Repeat this process to obtain a series of model inp files with the same parameters whose seismic intensities gradually increase. Step 8: Name the series of .inp files obtained in Step 7 according to the earthquake intensity, and use the Windows command line to write the execution commands in sequence, and import them into the Abaqus software for calculation. Step 9: Obtain the tower apex number and tower foot number operated in Step 6. Locate steps-2 in the Steps repository of the command in the post-processing hierarchy. Obtain historyRegions. Sequentially operate and retrieve the history output ODB files under different input earthquake intensities obtained in Step 8 to obtain the maximum displacement value under different input earthquake conditions. Step 10: Plot a curve with the maximum relative displacement at the top of the tower as the abscissa and the seismic input intensity as the ordinate. Find the inflection point and use the seismic intensity at the inflection point as the seismic performance index of this transmission tower model.

[0007] In step 1, the 3D drawing function of the 3D drawing software is used to draw the three-dimensional model frame of the transmission tower structure with dots and lines, and the size of the three-dimensional model frame is consistent with the design size, and the format is sat, igs, stp or dxf.

[0008] Step 2 specifically includes: Step 2.1: Create material parameters in Abaqus, including at least density, Young's modulus, Poisson's ratio, plastic strain, yield stress, damping Alpha, and Beta. Step 2.2: Design the angle steel section parameters as required to create a beam model, assign the element type as beam element, and assign the material parameters to the created angle steel section. Step 2.3: Adjust the orientation of the angle steel beam model to align it with the design direction.

[0009] Step 3 specifically includes: creating a two-step analysis step by applying gravity load and seismic dynamic load sequentially.

[0010] Step 4 specifically includes: Step 4.1: The seismic dynamic load is applied in step two of the analysis, and the application method is the acceleration boundary application in the boundary conditions; Step 4.2, when applying the acceleration boundary, cancel the complete fixation of the seismic input direction in the boundary where the tower foot was completely fixed in the previous step; Step 4.3: Input the acceleration waveform into the boundary acceleration waveform table in the boundary conditions as an acceleration-time relationship.

[0011] Step 5 specifically includes: meshing the specified beam element mesh.

[0012] Step 6 specifically includes: Step 6.1: Complete the task to obtain the field variable output file, select the tower top and tower foot to generate time history displacement curves, and subtract them to obtain the tower top relative displacement time history curve; Step 6.2: Record the unit numbers of the selected tower top and tower foot.

[0013] Step 7 specifically includes: finding the earthquake intensity parameters in the inp file and scaling them up proportionally to obtain a set of model files with increasing earthquake intensity.

[0014] Step 8 specifically includes: using the Windows cmd command to automatically import the inp files into the solver, and solving the problem to obtain a set of field variable output files.

[0015] Step 9 specifically includes: Step 9.1: Use the odbAccess library in Python to open the Abaqus field variable output file; Step 9.2: Use the command to find the hierarchical relationship and obtain the displacement time history data of the tower top and tower legs for the fixed unit number; Step 10 specifically includes; Step 10.1: Plot the earthquake intensity and its corresponding relative displacement curves. Step 10.2: The sudden change in the maximum value of the relative displacement of the top of the transmission tower as the earthquake intensity increases is regarded as the transmission tower itself being damaged and losing its load-bearing capacity. Step 10.3: Use the seismic intensity at the location of the inflection point in the image as an indicator to measure the seismic performance of the transmission tower.

[0016] The present invention has the following beneficial effects: 1. This invention provides a high-efficiency seismic analysis method for transmission towers based on Abaqus. This scheme designs a complete process from detailed modeling of specific transmission towers to simulation result output and finally to seismic performance analysis of transmission towers. Starting from the commonalities of existing seismic analysis of transmission towers, this scheme first solves the problems of excessively cumbersome details, model non-convergence, and large amount of calculation in the finite element simulation of transmission towers. While ensuring the accuracy of calculation, it greatly improves the efficiency of seismic analysis of transmission lines, and facilitates seismic performance analysis of different types of transmission lines.

[0017] 2. This invention can accurately characterize the overall seismic performance of the transmission tower structure, which is convenient for guiding actual production, improving the understanding of the transmission tower structure, and can be widely applied in the field of transmission line construction and design. Attached Figure Description

[0018] The present invention will be further described below with reference to the accompanying drawings and embodiments.

[0019] Figure 1 This is a flowchart illustrating a high-efficiency seismic resistance analysis method for transmission towers based on Abaqus, provided as an example of the present invention.

[0020] Figure 2 To adjust the interactive interface for assigning cross-sectional direction attributes to transmission towers.

[0021] Figure 3 A transmission tower model completed for simulation software.

[0022] Figure 4 Displacement curve of the tower top relative to the tower feet.

[0023] Figure 5 A graph showing the relationship between the maximum relative displacement at the top of the tower and the input earthquake intensity is attached, along with the curve of the relative displacement at the top of the tower when determining the seismic strength. Detailed Implementation

[0024] The embodiments of the present invention will be further described below with reference to the accompanying drawings.

[0025] Example 1: See Figure 1 , Step 1: Based on the design drawings and parameter details in the actual engineering transmission line construction, use the visualization interface in 3D drawing software to draw a 3D point-line model of the transmission tower from points and lines. In this process, the 3D drawing function in the 3D drawing software is used to draw the three-dimensional model framework of the transmission tower structure with dots and lines, and the size of the three-dimensional model framework is ensured to be consistent with the design size, and the format is sat, igs, stp or dxf.

[0026] Step 2: Import the 3D point-line model of the transmission tower established in Step 1 into the Abaqus software and run it to obtain the transmission tower component model information. Further, in Abaqus, create material properties based on the parameters obtained in Step 1, create angle steel sections, select beam models to simulate the properties of angle steel, and set parameters according to the corresponding angle steel sections. Further, after creating the angle steel interface, follow the angle steel specification interface of the actual line design, select the predetermined line according to the component model in the transmission tower design, assign the section, and finally adjust the assigned angle steel direction to make it consistent with the actual design. In Abaqus, material parameters are created that include at least density, Young's modulus, Poisson's ratio, plastic strain, yield stress, damping alpha, and beta.

[0027] Step 3: Assemble the transmission tower component models from Step 2 into an overall model and create an analysis step. The analysis step is divided into two steps: the first step is a static general type, used to apply gravity loads, and the second step is a dynamic implicit type, used to apply seismic loads. Step 4: Create loads in the analysis step created in step 3. In analysis step 1, set the load to gravity, apply it to the entire model, and set the direction to be perpendicular to the model and downwards. Then, transfer the load to the next analysis step. In the boundary conditions of the initial analysis step, set the four tower legs as a set and fix them completely. Transfer this boundary from the initial analysis step to analysis step 1 and deactivate this boundary in analysis step 2. In analysis step 2, release the fixation of the seismic wave input direction, set the acceleration boundary in the direction of the proposed input seismic wave, and set the amplitude to the input seismic wave waveform. Step 5: Place the model instance components, select the entire model, set the step interval to 1m, assign the element type to the beam mesh, in the job module, establish job analysis, set the maximum memory and the number of parallel processors, and obtain the model's total parameter inp file; Step 6: Open the calculation results submitted in Step 5 to obtain the entire response process of the transmission tower for seismic wave time history analysis. In the ODB field variable history output interface, select the highest point and the tower foot position of the transmission tower, export the history information of the displacement of the two points with time variables, and plot the time history displacement curve with them. Further operate the two sets of data by subtracting the tower foot displacement curve from the tower top displacement curve to obtain the tower top relative displacement time history curve, and obtain the maximum value of the tower top relative displacement in the seismic history. Step 7: Locate the seismic wave parameters in the model's total parameter inp file obtained in step 5. Scale the input seismic wave proportionally using the intensity reduction method. Modify the scaled-up model to obtain a new inp file. Repeat this process to obtain a series of model inp files with the same parameters whose seismic intensities gradually increase. Step 8: Name the series of .inp files obtained in Step 7 according to the earthquake intensity, and use the Windows command line to write the execution command in sequence. Import them one by one into the Abaqus software for calculation. Set the maximum time interval so that the next file will not be submitted if it is exceeded. The previous calculation will be automatically submitted after it is completed, and a series of result files will be obtained. Step 9: Obtain the tower apex number and tower foot number operated in Step 6. Locate steps-2 in the Steps repository of the command in the post-processing hierarchy. Obtain historyRegions and retrieve myField = fieldOutput["U"] (which is the displacement) of fieldOutputs with respect to the node number. Sequentially retrieve the history output ODB files under different input earthquake intensities obtained in Step 8 to obtain the maximum displacement value under different input earthquake conditions. Step 10: Plot a curve with the maximum displacement value on the x-axis and the seismic input intensity on the y-axis. Find the inflection point and use the seismic intensity at the inflection point as a measure of the seismic performance of this transmission tower model.

[0028] Example 2: This example provides a high-efficiency seismic resistance analysis method for transmission towers based on Abaqus. Figure 1-5 As a reference explanation for this example, its specific implementation process includes the following specific steps: Step 1: Collect the design drawings of the transmission tower. Use large-scale 3D modeling software such as CAD, SolidWorks, Rhino, etc. to draw the three-dimensional model framework of the transmission tower structure with points and lines using the 3D drawing function. Ensure that the dimensions are consistent. The 3D sketch export format should be a file with the sat, igs, stp, or dxf extension. When importing the model, select the acceptable error equal to the minimum precision. Step 2: Import the model created in Step 1 into Abaqus to generate the transmission tower model components. Create material parameters in Abaqus. The basic parameters are for three types of angle steel: Q235, Q345, and Q420. Parameter types should at least include density, Young's modulus, Poisson's ratio, plastic strain, yield stress, damping Alpha, and Beta. Find the relevant constitutive parameters from experiments on the angle steel components. The execution code for its inp representation file is as follows: *Material, name=Q235 *Damping, alpha=0.103855, beta=0.000962737 *Density 7.8e-09, *Elastic 206000, 0.3 *Plastic 235., 0. 423.3, 0.147434 Further, create a beam model according to the required angle steel section parameters, and assign material parameters to the created section. In the interactive interface, select the corresponding parameter material area and assign section attributes to the component line model, setting them sequentially according to the design parameters. Next, assign the beam model direction, check "Render Profile," and in the visualization interface, select the angle steel to be adjusted and assign the beam model direction, such as... Figure 2 As shown, taking reference directions 1, 2, and 3 as examples, select the rotation axis and adjust the vertical sequence to adjust the orientation of the angle steel beam model to match the design.

[0029] Step 3: Select all the transmission tower models set in Step 2 and create an analysis step. To ensure convergence, apply the load in segments. Divide the analysis step into two steps and gradually apply gravity and seismic loads. In the first analysis step, select static analysis in general analysis, set the specified attenuation factor to 0.0002, and the time span to 1 second. After the model stabilizes and converges under gravity, proceed to the second analysis step. In the second step, set dynamic implicit analysis. To ensure model convergence, set the initial increment step to a small value of 0.01 and set a sufficiently large maximum increment step so that the software can gradually converge in a small-scale linear process with multiple spans. The time span of the second step needs to exceed 20% of the earthquake duration so that the model still has enough time to sway and release kinetic energy after the earthquake input. This setting can fully reflect the entire process of the model's response and energy consumption under earthquake action.

[0030] Step 4: Create dynamic loads. The load application is divided into two parts: gravity load and seismic load, which belong to dynamic and static loads respectively. In analysis step 1, the gravity load is set to be borne by the entire model, with the direction perpendicular to the model downwards and the magnitude of 9.8 m / s^2. This load is then transferred to the next analysis step. The seismic dynamic load is different from the load acting on the tower body in conventional actual situations. This load is input from the tower legs and transferred upwards by the model structure. Therefore, the appropriate application method is to add it to the bottom of the tower legs in the boundary settings as acceleration. In the initial boundary settings and analysis step 1, the four tower legs are set to be completely fixed. In analysis step 2, two boundary settings are set: one is to release the fixed load in the direction of the seismic input, while the other directions remain fixed. The second boundary is set as a mechanical-acceleration boundary, with acceleration in the direction of the seismic input. The acceleration amplitude is referenced from the actual seismic acceleration wave. Specific values ​​are found in the Pacific Earthquake Engineering Research. This example uses EL-centro waveforms, and the seismic waveforms are entered in tabular form in the boundary waveforms.

[0031] Step 5: Plant the model instance components. Select the entire model and set the planting interval to 1m. In this example, under the dynamic stability simulation of the transmission tower, the main model is a linear model and is not in a singular node situation. The shear stress and strain of the main components are simple. The main shaft component is connected to multiple auxiliary materials. There are discontinuities at the connection points, and the mesh is automatically divided. The properties of individual unit components are continuous. This dense mesh can ensure the overall response results. Assign a beam mesh as the unit type. In the job module, establish the job analysis, set the maximum memory and the number of parallel processors, obtain the inp file of all model parameters, and after submitting the job, the Abaqus visualization interface will generate a source file that records all model operation parameters. It records all settings operations. The creation of the 3D model and the assignment of component parameters are too large. Using the visualization interface can complete the preliminary work more intuitively and conveniently. When the main model is built, it is necessary to modify the input parameters. Directly modifying the inp file can greatly improve the operation efficiency. When it is necessary to perform multi-array input calculations on complex models, this combination of visualization and secondary development greatly improves the running efficiency.

[0032] Step 6: Using the results calculated in Step 5, obtain the complete response process of the transmission tower under seismic wave time history analysis. Since the addition of accelerated seismic waves to the boundary conditions removes the fixed constraint in the seismic input direction, the overall model continuously advances in the input direction under seismic action. The tower top moves forward continuously in a swaying state. Therefore, the maximum displacement of the tower top reflecting the seismic response should be the relative displacement of the tower top relative to the tower legs. In the ODB field variable history output interface, select the highest point and the tower leg position of the transmission tower, export the displacement history information of these two points over time, and plot the time history displacement curves. Further, subtract the tower leg displacement curve from the tower top displacement curve to obtain the relative displacement time history curve of the tower top, and record the element numbers corresponding to the tower top and tower legs. The results are as follows: Figure 4 The graph shows the relative displacement of the tower top over time, from which the maximum displacement of the tower top under this earthquake intensity can be determined.

[0033] Step 7: Locate the seismic wave parameters in the model's total parameter inp file obtained in Step 5. Scale the input seismic waves proportionally using the intensity reduction method. Modify the scaled-up parameters to obtain a new inp file. Repeating this process yields a series of inp files with the same parameters and progressively increasing seismic intensities. The boundary region settings in the inp file are as follows: ** Name: BC-3 Type: Displacement / Rotation** Boundary Set-BC, 1, 1 Set-BC, 2, 2 Set-BC, 4, 4 Set-BC, 5, 5 Set-BC, 6, 6 ** Name: BC-4 Type: Acceleration / Angular Acceleration *Boundary, amplitude=Amp-1, type=ACCELERATION Set-BC, 3, 3, 100. The acceleration amplitude under the boundary conditions represents the earthquake intensity. By scaling this parameter proportionally, .inp input files of different earthquake intensities can be generated. The code for batch generating .inp input files of different earthquake intensities is as follows: import re f=open(' / c / desktop / inp100.txt','r') alllines = f.readlines() f.close() f=open(' / c / desktop / inp100.txt ','w+') for each line in alllines: a=re.sub('Set-BC, 3, 3, 100.','Set-BC, 3, 3, 101.',eachline) f.writelines(a) f.close() Step 8: Rename the series of .inp files obtained in Step 7 according to the earthquake intensity, and use the Windows command line to write the execution command sequentially into a .txt file. Change the file extension to .bat and run the command to automatically input the data into Abaqus for calculation. The specific command is as follows: call abaqus job=job100 int cpus=8 call abaqus job=job101 int cpus=8 call abaqus job=job102 int cpus=8 … This will generate calculation result files for different earthquake intensities, including field variable ODB files.

[0034] Step 9: Obtain the tower apex number and tower foot number obtained in Step 6. Use the Python library odbAccess to open the Abaqus variable output ODB file. Locate steps-2 in the Steps repository of the command in the post-processing hierarchy. Obtain historyRegions and set myField = fieldOutput["U"] for the fieldOutputs related to the node number, which is to retrieve the displacement. Then, retrieve the history output ODB files obtained in Step 8 under different input earthquake intensities in sequence to obtain the relative displacement curve of the tower top under different earthquake intensities. The specific implementation code is as follows: import odbAccess import numpy as np myOdb = odbAccess.openOdb(r"C:\desktop\Job-100.odb", readOnly=False) myFrames = myOdb.steps["Step-2"].frames n_top="256" n_dwon="14671" time = [] data = [] for i in range(len(myFrames)): tempField1 = [myFrames[i].frameValue,n_top] tempField2 = [myFrames[i].frameValue,n_down] tempField =tempField1-tempField2 for key in ["U","S"]: myValues ​​= myField[key].values tempField.append(np.mean(np.array(temp))) data.append(tempField) data = np.array(data) np.savetxt(r"C:\desktop\Job-100.txt") Step 10: Find the maximum displacement value of the relative displacement curve at the top of the tower obtained in Step 9, and plot the curve with this value as the x-axis and the seismic input intensity as the y-axis, as shown below. Figure 5 As shown, the specific process involves inputting seismic waves, modulating the amplitude of the seismic waves using the intensity reduction method, and then applying them to the target structure. Time history analysis is performed sequentially according to the intensity to obtain the response of the target structure under different intensity levels of earthquakes. As the earthquake intensity increases, the structural response gradually increases until the structure reaches a state of complete instability. Therefore, this can describe the overall elastic and plastic properties of the structure. This curve reflects the changes in the structure's elasticity, energy dissipation characteristics, and other indicators with earthquake intensity. As the earthquake intensity increases until the structure experiences dynamic instability, some structural components completely lose their original strength properties, reaching a plastic state, and this plasticity rapidly extends from localized areas to the entire structure. This phenomenon is reflected in the curve by a clear inflection point, and the intensity measure at which this inflection point occurs can be used to determine the critical value for dynamic instability of the structure. Figure 5 The inflection point in the figure shows the time curve of the relative displacement of the tower top. This indicates that the maximum displacement of the tower body seriously exceeded the limit and collapsed. The seismic intensity at this point is used as an indicator to measure the seismic performance of this transmission tower model.

Claims

1. A high-efficiency seismic resistance analysis method for transmission towers based on Abaqus, characterized in that, Includes the following steps: Step 1: Based on the design drawings and parameter details in the actual engineering transmission line construction, use the visualization interface in 3D drawing software to draw a 3D point-line model of the transmission tower from points and lines. Step 2: Import the 3D point-line model of the transmission tower established in Step 1 into the Abaqus software and run it to obtain the transmission tower component model information. Then, in Abaqus, based on the parameters obtained in Step 1, create material property assignment beam elements and set parameters according to the corresponding angle steel section. Finally, according to the component model in the transmission tower design, select the predetermined line to assign the section. Step 3: Assemble the transmission tower component models from Step 2 into an overall model and create an analysis step. The analysis step is divided into two steps: the first step is a static general type, used to apply gravity loads, and the second step is a dynamic implicit type, used to apply seismic loads. Step 4: Create a load in the analysis step created in step 3. In analysis step 1, the load is set to gravity. Further, in the boundary conditions of the initial analysis step, set the four tower feet as a set and fix them completely. Transfer this boundary from the initial analysis step to analysis step 1 and deactivate this boundary in analysis step 2. In analysis step 2, deactivate the seismic wave input direction of the fixed tower foot set, set the acceleration boundary in the direction of the proposed input seismic wave, and set the amplitude to the input seismic wave waveform. Step 5: Place the model instance parts, assign the element type to the beam mesh, create a job analysis in the job module, set the maximum memory and the number of parallel processors, and import the inp file to obtain all parameters of the model from the solver. Step 6: Open the calculation results submitted in Step 5. In the ODB field variable history output interface, select the highest point of the transmission tower and the tower foot position. Export the history information of the displacement of the two points with time variables. Further operate the two sets of data by subtracting the tower foot displacement curve from the tower top displacement curve to obtain the tower top relative displacement time history curve, and obtain the maximum value of the tower top relative displacement in the earthquake history. Step 7: Locate the seismic wave parameters in the model's total parameter inp file obtained in step 5. Scale the input seismic wave amplitude proportionally using the intensity reduction method. Modify the scaled-up values ​​to obtain a new inp file. Repeat this process to obtain a series of model inp files with the same parameters whose seismic intensities gradually increase. Step 8: Name the series of .inp files obtained in Step 7 according to the earthquake intensity, and use the Windows command line to write the execution commands in sequence, and import them into the Abaqus software for calculation. Step 9: Obtain the tower apex number and tower foot number operated in Step 6. Locate steps-2 in the Steps repository of the command in the post-processing hierarchy. Obtain historyRegions. Sequentially operate and retrieve the history output ODB files under different input earthquake intensities obtained in Step 8 to obtain the maximum displacement value under different input earthquake conditions. Step 10: Plot a curve with the maximum relative displacement at the top of the tower as the abscissa and the seismic input intensity as the ordinate. Find the inflection point and use the seismic intensity at the inflection point as the seismic performance index of this transmission tower model.

2. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, In step 1, the 3D drawing function of the 3D drawing software is used to draw the three-dimensional model frame of the transmission tower structure with dots and lines, and the size of the three-dimensional model frame is consistent with the design size, and the format is sat, igs, stp or dxf.

3. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 2 specifically includes: Step 2.1: Create material parameters in Abaqus, including at least density, Young's modulus, Poisson's ratio, plastic strain, yield stress, damping Alpha, and Beta. Step 2.2: Design the angle steel section parameters as required to create a beam model, assign the element type as beam element, and assign the material parameters to the created angle steel section. Step 2.3: Adjust the orientation of the angle steel beam model to align it with the design direction.

4. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 3 specifically includes: creating a two-step analysis step by applying gravity load and seismic dynamic load sequentially.

5. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 4 specifically includes: Step 4.1: The seismic dynamic load is applied in step two of the analysis, and the application method is the acceleration boundary application in the boundary conditions; Step 4.2, when applying the acceleration boundary, cancel the complete fixation of the seismic input direction in the boundary where the tower foot was completely fixed in the previous step; Step 4.3: Input the acceleration waveform into the boundary acceleration waveform table in the boundary conditions as an acceleration-time relationship.

6. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 5 specifically includes: meshing the specified beam element mesh.

7. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 6 specifically includes: Step 6.1: Complete the task to obtain the field variable output file, select the tower top and tower foot to generate time history displacement curves, and subtract them to obtain the tower top relative displacement time history curve; Step 6.2: Record the unit numbers of the selected tower top and tower foot.

8. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 7 specifically includes: finding the earthquake intensity parameters in the inp file and scaling them up proportionally to obtain a set of model files with increasing earthquake intensity.

9. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 8 specifically includes: using the Windows cmd command to automatically import the inp files into the solver, and solving the problem to obtain a set of field variable output files.

10. The high-efficiency transmission tower seismic resistance analysis method based on Abaqus according to claim 1, characterized in that, Step 9 specifically includes: Step 9.1: Use the odbAccess library in Python to open the Abaqus field variable output file; Step 9.2: Use the command to find the hierarchical relationship and obtain the displacement time history data of the tower top and tower legs with fixed unit numbers; Step 10 specifically includes; Step 10.1: Plot the earthquake intensity and its corresponding relative displacement curves. Step 10.2: The sudden change in the maximum value of the relative displacement of the top of the transmission tower as the earthquake intensity increases is regarded as the transmission tower itself being damaged and losing its load-bearing capacity. Step 10.3: Use the earthquake intensity at the location where the inflection point appears in the image as an indicator to measure the seismic performance of the transmission tower.

Images