Study on Analysis Principle of Spatial System Method for a Hydraulic Steel Gate

Abstract

The target of this paper is to ensure that the spatial system method has scientific and efficient rules to follow in structural analysis of a hydraulic steel gate, and to overcome the problems of randomness and fuzziness in the analysis process. Based on the idea of part and whole, the analysis principle of the spatial system method for a steel gate is systematically studied using the combination of theoretical calculation, finite element analysis, and prototype testing. First, the method is verified, with theoretical calculation used to ensure the authenticity of geometric modeling, the appropriateness of the element type, the rationality of meshing, the accuracy of constraints, and load application when the spatial system method is used to analyze the gate structure (panel, arm, and beam). The specific and practical feasible analysis principles of using the spatial system method to analyze the gate structure are provided. Second, the analysis of the gate structure is carried out using the analysis principle of the spatial system method. Finally, a prototype test is used to verify the analysis results of the spatial system method. Based on the prototype test results, the maximum absolute error of static displacement is 0.58 mm and the maximum relative error of static stress is 9.19%, which verifies the rationality and accuracy of the analysis principle of the spatial system method. The key technical problems restricting the transition of the gate structure analysis from the plane system method to the spatial system method are preliminarily solved. This first exploration is made for the popularization and application of the spatial system method, and lays a technical foundation for improving the quality and efficiency of gate structure design.

1. Introduction

Although the development and utilization of hydropower resources in China has reached 55.6%, it is far below the average development and utilization level of 80% in developed countries. In order to catch up with and surpass developed countries, reduce carbon emissions, and achieve carbon neutralization, it is necessary to vigorously build water conservancy and hydropower projects [1,2]. As the regulating throat of water conservancy and hydropower projects, the gate can play an important role in flood control, silt reduction, power generation and water resources allocation only if it is able to be opened and closed flexibly. The spatial effect of the gate is very strong. Although the plane system method has the advantages of a clear mechanical concept and simple calculation, the overall structure is often too safe and dangerous to fully reflect the real working state of the gate. The plane system method cannot be used to analyze the static stability, dynamic stability, welds, and bolts of the overall structure of the gate, nor can it be used to analyze the low temperature and low cycle fatigue failure of gate in severe cold environments [3]; thus, the plane system method cannot be used to analyze the gate structure to meet the unity of safety and economy. China’s gate design code has been revised seven times in the past 60 years, and adopts the plane system method, which lags behind the national codes [4,5,6,7] of the United States, Europe and other national codes [8,9,10,11,12,13] as well as scientific research progress [14,15,16,17]. In 1977, Lanzhou University used the finite element method to analyze the gate structure for the first time in China [18]; however, the analysis program compiled was not universal. In 1991, Jin Yahe et al. used SAP5 software to analyze the structure of a radial gate, although the analysis process was not described and the analysis results were not compared [19]. In 2012, Xi Xiaoya et al. used ANSYS12.0 software to analyze the safety of radial gate, and did not provide a specific modeling and analysis process either [20]. In 2022, Yao Jiahui and others used ANSYS18.0 software to analyze the deformation of the miter gate, although they did not provide their structural analysis principles [21]. Up to now, the seventh edition of the gate design code [22,23,24,25,26,27,28] has stated the spatial system method; however, it has not clearly provided the specific application standards and relevant principles, which restricts the transition process of gate structural analysis from the plane system method to the spatial system method.

The spatial system method (SSM) has a perfect theoretical basis in structural analysis, and there is an urgent need for it in practice, which is easily recognized and accepted subjectively. At present, the SSM is used to analyze gate structure, and almost all such analyses are directly transformed from geometric models to the finite element model. When the final analysis results are provided, the structure geometric modeling of the gate, element type selection, mesh generation-specific processes, and corresponding principles such as restraint and load application [29] are precisely the processes that determine the final analysis results. Only by clarifying the above process through clear quantitative and operable normative principles can we ensure the authenticity of the geometric model of the gate structure, the correctness of the finite element model, the appropriateness of the boundary conditions, and the rationality of the analysis results. With the progress of science and technology, the continuous maturity and improvement of finite element theory and calculation software, and the promulgation and implementation of the general rules for finite element analysis of mechanical product structures [30], the time is ripe to systematically study the analysis principles of gate SSM. The formulation of quantitative and practical analysis principles will solve the key technical problems that restrict the transition of gate structural analysis from the plane system method to the SSM, enrich and improve the gate specifications that have been adopted for 60 years and continue to be designed based on the plane system method after seven revisions, promote the development and progress of the overall design level of gates at home and abroad, achieve the goal of overall analysis of gate structures, support the whole process CAE (Computer Aided Engineering) design of gate structures, improve the quality and efficiency of gate design, explore new gate structures, verify the safety of gate structures in service, and repeat and determine the process and causes of gate accidents [31]. Therefore, it is necessary and urgent to study the analysis principle of the gate SSM (mainly the finite element method), and it has good prospects for application.

2. Gate Structure Composition and Research Method

The commonly used gate types in water conservancy and hydropower projects mainly include plane gates (Figure 1a) and radial gates (Figure 1b). The main difference between the two shape structures is that the radial gate panel has a certain curvature and arm structure, meaning that a plane gate can be regarded as a special case in which the curvature of the radial gate panel structure is zero. A radial gate is mainly composed of a panel, arm, support hinge, and other structures, which can be regarded as composed of plate (panel structure), beam (main beam structure, secondary beam structure, top beam structure, bottom beam structure, side beam structure), and column (arm structure) through welding or bolt connection. In order to ensure the universality of the analysis principle, the analysis principle of radial gate structure SSM is studied here.

Only when the spatial system analysis principles of each component of the gate structure are clearly quantified and feasible is it possible to ensure the rationality and accuracy of the overall structure analysis principles. The idea of division and entirety is utilized, and the reasonable SSM analysis principles of panel structure, beam structure, and arm structure are respectively explored. The method verified through the theoretical analytical solution is used to ensure the authenticity of geometric modeling, the appropriateness of element types, the rationality of grid division, and the accuracy of constraints and loads when the SSM is used to analyze the divisional structure. On the other hand, the analysis results of the overall structure are verified by comparison with the prototype test to ensure the rationality and accuracy of the gate structure analysis by the finite element method.

3. Analysis Principle of SSM for Gate Structure

In view of the many advantages of SSM, scholars and designers have used various types of finite element software to analyze different gate structures. However, different personnel have different professional knowledge, software operation ability, and understanding of the actual project, resulting in greater randomness and fuzziness in the process of geometric modeling, element type selection, mesh generation, constraints, and load application, even for the same project, Different people often obtain different results using the same software and which cannot be repeated, arousing the doubts of scholars and designers. If the accuracy and efficiency of SSM cannot be guaranteed, the analysis loses its significance. The basic process of using SSM (especially the finite element method) to analyze the gate structure includes the specific steps of establishing a geometric model (where the workload accounts for 30–40% of the whole process), meshing (40–50%), applying loads and constraints (4%), solving the model (2%), and processing the results (4%); these steps are closely linked. Only when the gate geometric model is established reasonably and perfectly can high-quality grid division be carried out smoothly. Only high-quality meshes can lead to high-precision analysis results. The finite element analysis of a gate is a systematic project. Only by grasping the overall situation can the advantages of high precision and high efficiency of the finite element method be brought into play.

3.1. Authenticity of Geometric Modeling

Geometric modeling is the basis of finite element analysis. Only by ensuring the authenticity of the geometric model can we ensure the accuracy of the analysis results. There are two commonly used gate geometric modeling methods at this stage: (1) directly using 3D modeling software, such as PowerChina Kunming survey and Design Institute using Autodesk Inventor software [32], Anhui Water Resources and Hydropower Survey and Design Institute using Bentley software [33], the Design Institute of the Standing Committee and the Design Institute of the Yellow River Commission using CATIA software [34,35], and the Water Resources and Hydropower Engineering Bureau using SolidWorks software [36]; (2) for the geometric modeling module in the finite element software, we can take the large general finite element software ANSYS as an example. The geometric modeling methods include GUI (graphical user interface) and APDL (ANSYS parametric design language). The GUI operation method is simple and easy to learn, although the modification of complex models is cumbersome and the workload of repeated operations is large. Due to the complexity of the gate structure, three-dimensional modeling software is directly used to establish the gate geometric model. At present, the mesh generation function of the software cannot directly mesh the gate geometric model, and often returns a low-quality finite element model; such analysis results can hardly be used for design. (3) The geometric model established by 3D software is directly imported into the finite element software to generate the finite element model. Unfortunately, the finite element model is often distorted due to the loss of detailed structural information during mesh generation.

After a great deal of engineering practice [37], the geometric modeling and meshing of the gate structure directly using the APDL method can make up for the shortcomings of the GUI modeling method, overcome the loss of detailed structural information in the process of model transformation of 3D modeling software and the problem of repeated meshes in professional meshing software (such as HyperMesh), and adapt to the working mode of “Design—Analysis—Modify Design—Redesign— Modify Reanalysis” of the gate. Furthermore, it can improve the efficiency of geometric modeling and the quality of mesh generation.

3.2. Appropriateness of Finite Element Type

Whether the element type is appropriate or not directly determines the accuracy and efficiency of finite element analysis. The selection of the element type is based on the basic principle of ensuring that the selected element can completely and accurately simulate the mechanical properties of the actual structure under load. Only when fully familiar with the analysis problems and element types can the appropriate element type be selected in order to simulate the actual structure of the project. The gate is a spatial thin-walled structure. When the finite element method is used for analysis, the finite element model of the gate structure can generally adopt the following types (

Table 1. Type of finite element for gate analysis.

Modeling Method	Gate structure Composition	Element Type	Advantage	Disadvantage
I	Panel structure	Shell element	Easy to build geometric model	Model is too simplified, the calculation accuracy is low, and the connection between different element types is complex.
	Beam structure	Beam element
	Arm structure	Beam element
II	Panel structure, beam structure and arm structure	Beam element	Realistic gate geometry	Workload of geometric modeling and mesh generation is large, which cannot truly reflect the mechanical response of the gate.
III	Panel structure, beam structure and arm structure	Shell element	Truly presents the geometric structure of the gate and truly reflects the mechanical response of the gate.	Workload of geometric modeling is relatively large

). In view of the complexity of the gate structure and a large amount of engineering practice [37], the full spatial thin-walled structure (mode III) can flexibly simulate the real structure of the gate.

3.3. Rationality of Finite Element Mesh Generation

When the geometric model and element type of the gate structure are determined, the number of element grids becomes a key factor affecting the accuracy and efficiency of the analysis. When the number of element grids is small, increasing the number of element grids can significantly improve the accuracy of analysis and make the numerical solution converge to the exact solution; however, the workload increases somewhat. When the number of element grids is increased to a certain extent, the accuracy of analysis is not significantly improved, the workload increases greatly, and the accuracy of analysis can even be reduced due to the accumulation of calculation errors [38].

In gate structure analysis, how to divide the mesh to ensure the high accuracy of the calculation results without greatly increasing the workload is a difficult problem for engineering designers. Although there are many kinds of automatic mesh generation software, due to the connection between different software the mesh of automatic mesh generation software often cannot meet the requirements of computational accuracy. In order to obtain a high-quality mesh, it is often necessary to perform this step manually. General principles to be followed for mesh generation include the following. (1) the mesh generation should have a global idea and reasonably plan the mesh relationship between adjacent structures. (2) The geometric outline of the structure should be retained for mesh generation in order to truly reflect the geometric characteristics of the structure. (3) The parts with large changes in structure, curvature, and load or connections of different materials should be refined. (4) The size of adjacent elements should be smoothly transited, and there should be corresponding element transitions between dense grids to avoid large difference in mass and stiffness of adjacent elements. (5) The number of element grids should be consistent with the type of analysis results. In static displacement analysis, the number of element grids can be less, while in static stress analysis, the number of element grids should be a little more. When analyzing dynamic characteristics and dynamic response, the number of element grids should be more [39]. Higher order modes require more mesh elements than lower order modes. (6) When the structure is symmetrical, the number of grids should be as symmetrical as possible. (7) The order of meshing affects the number of nodes and elements formed [40]. Although various kinds of finite element analysis software include the function of bandwidth and wavefront optimization, these should be meshed according to the order of structural force transmission. (8) Mapping grid division should be adopted as far as possible. Due to free mesh division, abnormal element shapes may occur, such as too large or too small internal angles of the element, and long and thin element shapes. A poor quality mesh causes large local structural errors, which may have a significant impact on the overall analysis results. Therefore, the overall mesh quality of the structure should be guaranteed to the greatest extent.

Whether the grid division is reasonable, that is, whether the grid division quality is the most intuitive performance, is determined by whether the grid geometry (Figure 2) is regular. A high quality finite element model can be obtained by reasonable mesh generation, allowing high-precision analysis results to be obtained. In order to ensure the accuracy and reliability of the finite element analysis results, it is necessary to verify the mesh independence and to evaluate or eliminate the mesh discretization error in the analysis process. The basic principle is to gradually encrypt the mesh until the calculation results do not change after adding the mesh. At the same time, the most reasonable number of element meshes can be determined by comparison with the theoretical analytical solution.

3.4. Accuracy of Constraints and Loads

Only by ensuring that accurate constraints and loads are applied can the accurate stiffness matrix and equilibrium equation of the overall structure be obtained, allowing accurate analysis results to be obtained. Only through familiarity with the constraint type and element type of the gate structure in the actual project is it possible to ensure that the constraints imposed on the model are consistent with those in project. In practical engineering, when the gate is closed to retain water, the bottom of the panel is equivalent to directly contacting the gate bottom plate under the action of water pressure, and the line displacement of the bottom of the panel is generally directly constrained in the finite element analysis. At the side beam of the gate, the vertical flow direction and the linear displacement along the flow direction are directly constrained in order to simulate the constraint effect of the side pier on the gate. No linear displacement is allowed at the gate hinge. The linear displacement in three directions and the angular displacement in two directions are constrained, and only the angular displacement that can rotate around the hinge is relaxed. When the gate is opened instantaneously, the restraint at the bottom of the panel disappears, while the restraint at the side beam and hinge continues to exists. At this time, the restraint effect of the hoist rod (hydraulic hoist) or steel wire rope (winch hoist) should be considered.

When the water retaining gate is closed, the load borne by the gate is mainly due to the water load and self-weight. The hydrostatic pressure changes linearly along the water depth. The SFGRAD command in the software is used to apply the surface load gradient, and the self-weight is applied by the ACEL command. In case of instantaneous opening, the load is mainly due to the hydrostatic pressure, self-weight, and gate opening force. The hydrostatic pressure and self-weight are applied in the same way, and the gate opening force is directly applied to the lifting structure in the form of a concentrated load.

4. Analysis Principle of Beam Structure

The gate structure is mainly composed of a plate structure, column structure, and beam structure through welding or bolt connection. The relevant research on the finite element analysis principles of gate column structure [38] and plate structure [41] is detailed in the literature, and is not repeated here. The gate beam structure generally adopts the solid web structure, in which I-shaped and box section beams are the most common. According to the research results, when the element type is selected, the number of element grids becomes the key to determining the accuracy and efficiency of the analysis. Due to the structural type of the gate, the stability of the beam structure is generally not specially calculated [42], and only the strength and stiffness of the beam most concerned in the engineering design are analyzed by means of verification with the theoretical calculation to determine the most reasonable number of element grids in the finite element analysis of the gate beam structure.

4.1. Reasonable Finite Element Mesh Number of I-Beam

According to statistics [43], the length of common beams in gate structures is generally between 10.0 m and 20.0 m. The deflection and normal stress of 10.0 m, 12.0 m, 14.0 m, 16.0 m, 18.0 m, and 20.0 m simply supported I-beams under uniformly distributed load (600 kN/m) are compared and analyzed by theoretical calculation and numerical analysis methods, respectively. The section size, mid-span deflection and error, and mid-span normal stress and error of the I-beams are shown in

Table 2. Section dimensions and theoretical results for I-beams.

Number	1	2	3	4	5	6
Section	I-beam
Constraint	Simply supported at both ends
Beam length (m)	10	12	14	16	18	20
Lower flange width (m)	0.80	0.90	1.00	1.20	1.35	1.40
Thickness of lower flange (m)	0.032	0.032	0.032	0.034	0.036	0.036
Upper flange width (m)	0.80	0.90	1.00	1.20	1.35	1.40
Thickness of upper flange (m)	0.032	0.032	0.032	0.034	0.036	0.036
Web height (m)	1.00	1.20	1.40	1.50	1.60	1.80
Web thickness (m)	0.032	0.032	0.032	0.034	0.036	0.036
Midspan deflection (m)	0.027	0.033	0.040	0.048	0.057	0.065
Midspan normal stress (MPa)	264.4	275.1	283.4	276.0	277.1	287.5
Midspan bending moment (kN·m)	7500	10,800	14,700	19,200	24,300	30,000

.

The shell element (shell 181) is used to establish the I-shaped beam model (see Figure 3). First, in order to save space, and second because the analysis results are similar, we take a beam length of 20.0 m as an example according to the conclusions in the literature [41]. The flange width is 1.40 m, the reasonable mesh number is 6, the web height is 1.80 m, the reasonable mesh number is 8, and the beam length of 20.0 m is divided into 40 grids. The finite element analysis results when the element size is 0.5 m are shown in Figure 4.

According to Figure 4, when the shell 181 element is used to simulate the I-section beam, the mid-span deflection is 0.064 m and the mid-span normal stress is 284.0 MPa. Compared with Table 2, the absolute error values of numerical solution and theoretical solution are 0.36% and 1.23%, respectively. The shell 181 element is used to analyze the mid-span deflection and normal stress of 10.0 m, 12.0 m, 14.0 m, 16.0 m, 18.0 m, and 20.0 m simply supported I-beams under uniformly distributed load (600 kN/m). The relationship between the mid-span deflection and normal stress error and the number of element grids is shown in Figure 5. The calculation error in Figure 5 is based on the calculation results of the material mechanics method. The relative error between the numerical analysis results and the theoretical results is compared with the relative error of the mid-span deflection and normal stress of the simply supported I-shaped beam at both ends. The specific values of section size, length, midspan deflection, and normal stress of the I-shaped beam are shown in Table 2.

It can be seen from Figure 5 that when the shell element is used to simulate the beam structure, when the mesh numbers of the flange width and web height meet the requirements of a reasonable mesh number, only the element mesh number in the beam length direction is changed. When the element mesh number is 2, the errors of the mid-span deflection and normal stress reach about 35% and 50% respectively. With the increase in the number of element grids, the analysis error decreases gradually. When the number of element grids is greater than 10, the error of mid-span deflection and normal stress is reduced to about 1%. In order to coordinate the relationship between calculation accuracy and efficiency, a reasonable number of grids of 40 to 60 can be used, meaning that the element size is 0.16 m to 0.5 m.

4.2. Reasonable Finite Element Mesh Number of Box Beam

Similarly, the mid-span deflection and normal stress of 10.0 m, 12.0 m, 14.0 m, 16.0 m, 18.0 m, and 20.0 m simply supported box beams under uniformly distributed loading (600 kN/m) are compared and analyzed by theoretical calculation and numerical analysis. The section size, mid-span deflection and error, mid-span normal stress, and error of the box beams are shown in

Table 3. Sectional dimensions and calculation results of box beams.

Number	1	2	3	4	5	6
Section	Box beam
Constraint	Simply supported at both ends
Beam length (m)	10	12	14	16	18	20
Section width of box beam (m)	1.00	1.15	1.25	1.40	1.55	1.70
Section height of box girder (m)	0.80	0.95	1.05	1.20	1.35	1.50
Wall thickness of upper flange (m)	0.032	0.032	0.036	0.036	0.036	0.036
Wall thickness of lower flange (m)	0.032	0.032	0.036	0.036	0.036	0.036
Wall thickness of front flange (m)	0.032	0.032	0.036	0.036	0.036	0.036
Wall thickness of rear flange (m)	0.032	0.032	0.036	0.036	0.036	0.036
Midspan deflection (m)	0.033	0.041	0.051	0.058	0.066	0.073
Midspan normal stress (MPa)	259.3	266.9	268.4	269.4	270.2	270.9

.

The box beam model is established using the shell element (shell 181) (see Figure 6). Similarly, taking the beam length of 20.0 m as an example, according to the conclusion of the literature [41] the flange width is 1.40 m, the reasonable grid number is 6, the web height is 1.80 m, the reasonable grid number is 8, the beam length is 20.0 m, and the mesh number is 40. The finite element analysis results when the element size is 0.5 m are shown in Figure 7.

According to Figure 7, when the shell 181 element is used to simulate the box section beam, the mid-span deflection is 0.072 m and the mid-span normal stress is 269.0 MPa. Compared with Table 3, the absolute error values of the numerical solution and theoretical solution are 1.37% and 0.69%, respectively. The shell 181 element is used to analyze the mid span deflection and normal stress of 10.0 m, 12.0 m, 14.0 m, 16.0 m, 18.0 m, and 20.0 m simply supported box beams under uniformly distributed loading (600 kN/m). The relationship between the mid-span deflection and normal stress error and the number of element grids is shown in Figure 8.

It can be seen from Figure 8 that when the shell element is used to simulate the beam structure and the mesh number of flange width and web height meet the requirements of reasonable mesh number, only the element mesh number in the beam length direction is changed. When the element mesh number is 2, the errors of the mid-span deflection and normal stress reach about 35% and 42%, respectively. With the increase in the number of element grids, the analysis error decreases gradually. When the number of element grids is greater than 10, the error of the mid-span deflection and normal stress is reduced to about 2%. In order to coordinate the relationship between calculation accuracy and efficiency, a reasonable number of grids of 40 to 60 can be used, meaning that the element size is 0.16 m to 0.5 m.

5. Verification of Prototype Test

Taking the radial gate of a water control project as an example, the floor elevation is 209.0 m and the prototype test water level is 266.0 m. The space finite element method and prototype test are used to analyze it. According to the design drawing of the radial gate, the geometric model and finite element model established by APDL are shown in Figure 9. The radial gate structure has a width and height of 8.0 m and 9.0 m, respectively, a radius of 18.0 m, and a working head of 41.0 m. The gate structure material is 16Mn steel, the elastic modulus is 2.06 × 10¹¹ Pa, the material density is 7850 kg/m³, and the Poisson’s ratio is 0.3. According to the research results of the analysis principles of gate SSM [29,38,41], a shell element (shell 181) is selected for simulation and a mapped mesh is adopted. The structure of the radial gate is analyzed using ANSYS 18.1 software. The gate is closed for water retaining, the bottom of the panel is equivalent to directly contacting with the gate bottom plate under the action of water pressure, and the line displacement of the bottom of the panel is generally directly constrained in the finite element analysis. At the side beam of the gate, the vertical flow direction and the linear displacement along the flow direction are directly constrained to simulate the constraint effect of the side pier on the gate. No linear displacement is allowed at the gate hinge. The linear displacement in three directions and the angular displacement in two directions are constrained, and only the angular displacement that can rotate around the hinge is relaxed. The load borne by the gate mainly comes from the water load and self-weight. The hydrostatic pressure changes linearly along with the water depth. The SFGRAD command in the software is used to apply the surface load gradient, and the self-weight is applied by ACEL command. The number of elements and nodes are 46,558 and 46,826, respectively. The strength and stiffness analysis results of the gate structure are shown in Figure 10.

In order to verify the analysis results of the SSM, a prototype test is used to measure the displacement and stress of each component of the radial gate structure during the water retaining state. The layout of the gate measuring points should follow the principle of using the minimum measuring points to reflect the true structural state as much as possible [44]. The prototype test of the radial gate was conducted from 20 to 29 April 2021. The characteristics of the measuring instrument for radial gate stress and displacement are shown in

Table 4. Parameters of radial gate structure stress and displacement measuring equipment.

Texture of material	Q235B
Yield strength (MPa)	235
Resistance of strain gauge	120 Ω
Uncertainty of instrument (με)	<5% ± 3
Elastic modulus (GPa)	206
Model of strain gauge	WFLA-6-11
Treatment method of gate surface	Grinding and polishing
Instrument resolution (με)	1
Poisson’s ratio	0.28
Installation method of strain gauge	Paste
Instrument model	DH5908L
Frequency of data acquisition (Hz)	200

.

The displacement measurement technology for the radial gate prototype test is difficult. Due to the limitations of site conditions and measurement accuracy, traditional measurement methods such as theodolite and total station are not easy to operate and locate. This measurement adopts a three-dimensional photogrammetry system. Three-dimensional photogrammetry is a displacement measurement technology with high precision and accurate positioning, and the uncertainty of photogrammetric instruments is less than 5%. The static displacement measurement and analysis results of the radial gate are shown in

Table 5. Comparison between displacements results of SSM and prototype test.

Number	Position	Analysis Method	Flow Direction (mm)	Vertical Direction (mm)	Lateral (mm)	Illustration
1	Middle main beam	SSM	1.88	0.314	0.082	Figure 11
		Prototype test	1.30	0.80	0
2	Main longitudinal beam	SSM	1.56	0.16	0.35	Figure 12
		Prototype test	1.50	0.60	−0.4
3	Secondary longitudinal beam	SSM	1.88	0.31	0.35	Figure 13
		Prototype test	1.60	1.10	0
4	Panel	SSM	2.47	0.74	0.048	Figure 14
		Prototype test	1.80	0.70	−0.10
5	Arm	SSM	1.38	0.63	1.03	Figure 15
		Prototype test	1.00	0.90	0.70

, and the finite element analysis results are shown in Figure 11, Figure 12, Figure 13, Figure 14 and Figure 15.

A wireless dynamic strain tester (DH5908l) was used for the radial gate stress test, with a resolution of 1 με, where zero drift is 3 με/h. The sensitivity coefficient is 2.0, the material of the strain gauge is Q235B, the elastic modulus is 2.06 × 10¹¹ MPa, the Poisson’s ratio is 0.28, and the resistance is 120 Ω connected by a 1/4 bridge. Due to space limitation, only the measured stress and finite element analysis results for the radial gate are provided; see

Table 6. Stress results.

Number	Position	Stress	Results of Prototype Tests (MPa)	Results of SSM (MPa)
1	Web structure of longitudinal beam	Vertical direction	4.68	4.53
2	Flange structure of longitudinal beam	Vertical direction	−19.35	−20.60
3	Connecting flange of lower arm and main beam	Arm direction	−53.55	−54.70
4	Web structure of lower main beam	Horizontal direction	−6.43	−7.20
5	Panel structure	Horizontal direction	38.10	34.60
6	Arm structure	Arm direction	−65.60	−59.10

.

As the finite element method is an approximate calculation method, it can only be improved from the key steps that determine its accuracy and efficiency to ensure that the analysis results are as close to the real solution as possible. On the other hand, there are inevitably measurement errors and truncation errors in the process of various test instruments, data acquisition, and data analysis during prototype testing. It can be seen from Table 5 that the analysis results of the gate structure according to the analysis principles are close to the prototype test results; based on the prototype test results, the maximum absolute error of displacement is 0.58 mm and the maximum relative error of stress is 9.19%, which strongly verifies the rationality, correctness, and practicality of the analysis principles of the gate SSM.

6. Conclusions

Based on the idea of part and whole, the analysis principle of SSM for gate structure is studied using the method of combining theoretical calculation, finite element analysis, and prototype testing. The specific and practical analysis principles in the process of geometric modeling, element type selection, mesh generation, constraints. and load application of SSM for a gate structure are presented. Our main conclusions are as follows:

(1) On the basis of the finite element analysis principle of the gate arm structure and the panel structure, the finite element analysis principle of a gate beam structure is studied and the appropriate element type and reasonable element mesh number for the SSM analysis of the gate beam structure are determined.

(2) The rationality and accuracy of the analysis principle of the gate SSM are verified by the prototype test.

(3) The key technical problems that restrict the transition of gate structure analysis from the plane system method to the SSM are preliminarily solved. The principles ensuring the authenticity of gate geometric modeling, the appropriateness of the choice of element type, the rationality of mesh generation, and the accuracy of constraints and load application are provided, laying a foundation for improving the quality and efficiency of future gate design.