Whole-ship finite element batch calculation and post-processing method

Abstract

A kind of whole ship finite element batch calculation and post-processing method, comprising the following steps: S1: according to FPSO working sea area environmental condition and the large number of combined working conditions of assembly load, establish FPSO ship wet surface model;S2: the FPSO ship wet surface model is passed through wave load to ship surface batch generation load file;S3: according to ship data and the latest thickness data of ship, establish FPSO whole ship finite element model, S4: the whole ship finite element model is grouped and named according to ship structure and ship steel material properties;S5: obtain the whole ship stress value and maximum displacement batch file under each group working condition;S6: using ANSYS post1 post-processing module exports the stress value and maximum displacement batch txt file of whole ship area of interest;S7: the stress value and maximum displacement batch data of whole ship area of interest are analyzed and output result, the present application provides strong support for the safety and reliability of FPSO and the establishment of proxy model.

Description

Technical Field

[0001] This invention relates to the field of marine engineering structure design and analysis, specifically to a method for batch calculation and post-processing of finite element data for the entire ship. Background Technology

[0002] FPSOs need to withstand structural damage caused by various alternating loads under harsh sea conditions, as well as corrosion caused by the marine environment and cargo during their service life. From the perspective of structural design and reliability, the working conditions are combined according to the combination values ​​of marine environment and cargo. The wave-induced loads and structural strength that FPSOs may be subjected to throughout their entire life cycle are studied. The finite element method is used to conduct structural strength analysis of FPSOs covering all working conditions. This is of great practical significance for identifying high-stress areas of FPSO hulls and realizing full life cycle structural strength safety monitoring of FPSOs.

[0003] For ultra-large ships, finite element analysis (FEM) of compartment sections is currently the mainstream approach. This involves creating only a portion of the section and applying displacements or constraints at its ends to make it as equivalent as possible to the influence of the rest of the hull on that section. While the compartment FEM method has a small modeling workload and wide application, it primarily examines the hull's ability to withstand longitudinal bending, and the applied loads are generally calculated using empirical formulas, introducing some error. The full-ship FEM method, currently the most accurate calculation method, can precisely simulate all components within the ship, fully considering the influence between internal structural elements. It avoids errors in calculation results caused by load transfer issues at compartment boundaries. Furthermore, the boundary conditions and loads applied by the full-ship FEM method are more accurate, resulting in more detailed calculations that reveal the stress distribution and deformation of the entire ship structure.

[0004] With the increasing size and sophistication of marine engineering structures, digital twin technology is being applied in the field of marine engineering. Establishing a surrogate model capable of approximately predicting the performance of large and complex structural systems and fulfilling some design, optimization, and simulation tasks has become extremely valuable. The surrogate model aims to establish a black-box mapping relationship between the model's input and output parameters to replace detailed simulation. Its foundation lies in a large amount of detailed simulation data of complex structural systems. For FPSOs, this requires full coverage of environmental conditions under their operational conditions, combined with batch finite element analysis of the entire FPSO under different loading conditions, to obtain a large amount of simulation analysis results data. This is fundamental to establishing the surrogate model and even realizing digital twin technology.

[0005] Finite element analysis of an FPSO (Floating Production Ship) involves a large workload and long computation time. Traditional methods for batch calculations under various operating conditions are labor-intensive. Furthermore, when large-scale data is required, relying solely on manual operation using traditional GUI simulation methods inevitably increases the risk of errors, affecting the accuracy of the results. Therefore, establishing a method for batch calculation and post-processing of finite element data for the entire FPSO can help save computational costs, avoid the risk of human error during repeated load application and data extraction, and improve the efficiency and accuracy of finite element analysis. Summary of the Invention

[0006] The technical problem to be solved by this invention is to provide a method for batch calculation and post-processing of finite element analysis of the entire ship, thereby obtaining a large amount of finite element simulation analysis results data of the entire FPSO, determining the high stress area and maximum deformation of the hull, and providing strong support for the safety and reliability of FPSO and the establishment of proxy models.

[0007] The technical solution adopted by this invention to solve its technical problem is: a finite element evaluation method for the entire FPSO based on ANSYS, comprising the following steps:

[0008] S1: Construct a large number of combined working conditions of FPSO working sea area environmental conditions and loading, covering all working conditions under FPSO operation; establish FPSO hull wet surface model, transfer wave load to hull surface, and generate load files in batches.

[0009] S3: Based on the hull design data and the latest hull thickness measurement report, establish a full finite element model of the FPSO and perform mesh generation;

[0010] S4: Group and name the finite element elements of the entire ship according to the hull structure and the properties of the marine steel; S5: Apply loads and boundary conditions to the FPSO finite element model described in S3, perform batch static analysis on all mesh elements, and obtain the stress level and maximum deformation of the entire ship under each working condition.

[0011] S6: Using the ANSYS post1 general post-processing module, the stress values ​​and maximum displacements of the region of interest are exported in batches to txt files for analysis.

[0012] According to the above scheme, in step S1, the independent variable of the combined working condition includes: significant wave height H. s Spectral peak period T p 1. Loading status of the liquid cargo tank.

[0013] According to the above scheme, the method for establishing the wetted surface model of the hull in step S2 is as follows:

[0014] Write the coordinates of the key points on the wetted surface of the hull half-side in a text editor, generate a command stream in .dat format, save it in the storage path, and use the / INPUT command to call the command stream file to create the key points on the wetted surface of the hull.

[0015] In the ANSYS GUI interface, select Spline Thru KP, select key points to generate spline curves for each station of the hull and the bow and stern.

[0016] Use the ASKIN command to connect the above spline curves to generate the wetted surface on the half-hull side of the FPSO.

[0017] Use the ARSYM command to generate the double side wet surface model, and use the AL command to generate the bottom outer plate plane;

[0018] The grid is adjusted based on the minimum wave period of the FPSO working area. Different subsequent solution requirements have different requirements for grid quality. The judgment principle is that the grid size is not less than 1 / 7 of the wavelength corresponding to the minimum wave period.

[0019] According to the above scheme, in step S2, the wave load is calculated using the post-processing program AQWA Wave, and the AQWA calculation results are exported as an aqld file.

[0020] According to the above scheme, in step S3, the thickness measurement method of the latest hull thickness measurement report should include underwater visual inspection and ultrasonic thickness measurement. The underwater visual inspection range includes the bilge keel, side plates, and bottom plate; the ultrasonic thickness measurement range should include the underwater side plates and the outer plate of the bottom plate, measuring at least three ribs according to the hull length distribution.

[0021] According to the above scheme, the specific steps for creating the "FPSO full-ship finite element model" in step S3 are as follows:

[0022] Establish a full-ship geometric model of the FPSO, including all major longitudinal and transverse components, including the inner shell and outer plate structure, double bottom ribs and longitudinal girder system, transverse strong frame and vertical girder, horizontal girder, transverse bulkhead and longitudinal bulkhead.

[0023] Create a plate thickness library. The thickness of the underwater side plates and bottom plates of the hull is corrected according to the thickness measurement report. The thickness of the remaining plates is determined according to the hull design data. Assign values ​​to the plate units of the FPSO, set the mesh size to the spacing of the longitudinal reinforcing members, and mesh the plates into shell units.

[0024] Create a skeleton section library, assign values ​​to the skeleton reinforcement members of the FPSO, set the mesh size to the spacing of the longitudinal reinforcement members, and mesh the skeleton into beam elements and rod elements.

[0025] According to the above scheme, in step S4, the hull structure of one of the finite element unit grouping methods for the whole ship includes: cargo oil tank inner wall, cargo oil tank inner bottom plate, bottom outer plate, side outer plate, bilge outer plate, longitudinal bulkhead, transverse bulkhead, transverse strong frame, bottom longitudinal girder, functional platform, main deck, etc.

[0026] According to the above scheme, in step S4, the properties of the marine steel in the second group of the finite element elements of the whole ship are determined according to the allowable stress σ of the steel. 1, ,σ2,…,σ n It is divided into n levels.

[0027] According to the above scheme, in step S5, the load includes: deck static load, wave load, cargo tank load, and gravity.

[0028] According to the above scheme, in step S5, the static load on the deck is calculated using the following formula:

[0029] P = P stat ·A+P deck-L ·L+m un ·g

[0030] Among them, P stat P is the uniformly distributed pressure on the supporting structure. deck-L For a linearly distributed uniform pressure on the supporting structure, m un The mass of equipment that acts on the supporting structure.

[0031] According to the above scheme, in step S5, the wave load is applied in the following manner:

[0032] A pressure value of 1 is applied to the unit below the waterline and marked accordingly;

[0033] Import the aqld result file from step S2 into ANSYS and apply normal loads to all marked elements.

[0034] According to the above scheme, in step S5, the load on the liquid cargo tank is applied in the following manner:

[0035] Create a liquid cargo tank pressure loading program that obtains the command stream file in the storage path based on the input liquid cargo tank level, thereby realizing automated pressure loading of the liquid cargo tank.

[0036] According to the above scheme, in step S5, the boundary conditions are applied at one point at the bow and two points at the stern.

[0037] According to the above scheme, in step S5, the batch calculation is implemented by using a Python secondary development ANSYS command stream batch generation program.

[0038] According to the above scheme, the stress value is derived in step S6 as follows:

[0039] Record the node numbers of high stress and large deformation locations based on the finite element analysis results, and enter them into the command stream in a text editor;

[0040] The *DIM function in ANSYS is used to generate an array to store the stress and deformation values ​​calculated under different working conditions;

[0041] Use the *set command to export the stress and deformation values ​​stored in the array as a txt file.

[0042] According to the above scheme, in step S6, the allowable stress value based on different material properties is calculated using the following formula:

[0043] [σ]=R eH / S

[0044] Among them, R eH Let S be the minimum yield stress of the material, and S be the safety factor.

[0045] Beneficial effects

[0046] The beneficial effects of the technical solution provided by this invention include at least the following:

[0047] Compared with existing technologies, this invention proposes a batch calculation method for finite element analysis based on ANSYS. By using Python to write load application command streams for a large number of working conditions, and realizing automatic batch calculation of a large number of working conditions, the manual cost of calculating a large number of working conditions is greatly reduced. At the same time, it avoids the risk of human error in the process of repeatedly applying loads, thereby improving the efficiency and accuracy of finite element analysis.

[0048] Compared with existing technologies, this invention proposes a batch extraction method for finite element calculation results based on ANSYS. While performing batch calculations for a large number of working conditions, the data results of each group of working conditions are recorded, which greatly saves the cost of data collection and avoids the risk of human error in the process of extracting the results, thereby improving the efficiency and accuracy of finite element analysis. Attached Figure Description

[0049] The present invention will be further described below with reference to the accompanying drawings and embodiments. In the accompanying drawings:

[0050] Figure 1 This is a schematic diagram of the process structure of the FPSO whole ship finite element batch calculation and post-processing method based on ANSYS of the present invention.

[0051] Figure 2 This is a schematic diagram of the wetted surface model of the FPSO hull in an embodiment of the present invention;

[0052] Figure 3 This is a schematic diagram of wave load file loading in an embodiment of the present invention;

[0053] Figure 4 This is a schematic diagram of the finite element model of the entire FPSO in an embodiment of the present invention;

[0054] Figure 5 This is a schematic diagram showing the application positions of boundary conditions at the bow and stern of an FPSO in an embodiment of the present invention.

[0055] Figure 6 This is a schematic diagram of the calculation results of a certain working condition of the finite element model of the entire FPSO in an embodiment of the present invention;

[0056] Figure 7 This is a schematic diagram of an array in ANSYS used to store calculation results in an embodiment of the present invention. Detailed Implementation

[0057] To provide a clearer understanding of the technical features, objectives, and effects of the present invention, specific embodiments of the invention will now be described in detail with reference to the accompanying drawings. It should be understood that the specific embodiments described herein use data from a certain project and are merely for explaining the invention, and are not intended to limit the invention.

[0058] like Figure 1-7 As shown, the present invention provides a method for batch calculation and post-processing of FPSO full-ship finite element data based on ANSYS, comprising the following steps:

[0059] S1: Construct a large number of combined working conditions of FPSO working sea area environmental conditions and loading, covering all working conditions under FPSO operation status;

[0060] Step S1 specifically involves: determining the effective wave height H based on the wave scattering map of the FPSO operating area. s Spectral peak period T p The permutations and combinations were used to randomly sample the load conditions of the FPSO using the Latin hypercube sampling method. Ten load conditions were selected for each combination of effective wave height and spectral peak period, covering all possible load conditions encountered during the FPSO's working years.

[0061] S2: Establish a wetted surface model of the FPSO hull, transfer wave loads to the hull surface, and generate load files in batches;

[0062] Step S2 is as follows: Enter the coordinates of the key points on the wetted surface of the hull (half-hull side) in a text editor to generate a command stream in .dat format, save it to the storage path, and use the / INPUT command to call the command stream file to create the key points on the wetted surface of the hull. In the ANSYS GUI interface, select Spline Thru KP, select the key points to generate spline curves for each station on the hull and for the bow and stern, use the ASKIN command to connect the spline curves to generate the wetted surface of the FPSO (partial hull side), use the ARSYM command to generate the wetted surface model of both sides, use the AL command to generate the plane of the outer plating of the hull bottom, and adjust the mesh according to the minimum spectral peak period of the FPSO working area, ensuring the mesh size is not less than 1 / 7 of the wavelength corresponding to the minimum spectral peak period. Use the post-processing program AQWA Wave to export the wave load results calculated by AQWA as an aqld file, automatically generating file numbers corresponding one-to-one with the S1 working condition.

[0063] S3: Based on the hull design data and the latest hull thickness measurement report, establish a full finite element model of the FPSO and perform mesh generation;

[0064] Step S3 specifically involves: conducting underwater visual inspection and ultrasonic thickness measurement of the FPSO hull. The underwater visual inspection range includes the bilge keel, side plates, and bottom plate. The ultrasonic thickness measurement range includes the underwater side plates and the outer bottom plate portion of the hull. Measurements are taken at least at three rib locations based on the hull's length distribution, generating a complete thickness measurement report. A complete geometric model of the FPSO is established, including all major longitudinal and transverse components. These components include the inner shell and outer plate structures, double-layer bottom ribs and longitudinal girder system, transverse strong frames and vertical trusses, horizontal trusses, transverse bulkheads, and longitudinal bulkheads. A plate thickness library is created. The thicknesses of the underwater side plates and the outer bottom plate are corrected based on the thickness measurement report, while the thicknesses of the remaining plates are determined based on the hull design data. Values ​​are assigned to all plate elements of the FPSO, with the mesh size set to the longitudinal reinforcement member spacing. The plate elements are then meshed into shell elements. A skeleton section library is created, and values ​​are assigned to all skeleton reinforcement members of the FPSO, with the mesh size set to the longitudinal reinforcement member spacing. The skeleton elements are then meshed into beam and rod elements.

[0065] S4: Group and name the finite element elements of the entire ship according to the hull structure and the properties of the marine steel;

[0066] Step S4 specifically involves using the CM command in ANSYS to generate the hull structure components, including the cargo oil tank inner walls, cargo oil tank inner bottom plates, bottom outer plates, side outer plates, bilge outer plates, longitudinal bulkheads, transverse bulkheads, transverse strong frames, bottom longitudinal girder, functional platforms, and main deck. The CM command in ANSYS is used to calculate the yield stress as 235 N / mm². 2 Grade A steel with a yield stress of 315 N / mm 2 Grade A high-strength steel with a yield stress of 355 N / mm²2 The three grades of high-strength steel produced by D grade are components.

[0067] S5: Apply loads and boundary conditions to the FPSO full-ship finite element model described in S3, perform batch static analysis on all mesh elements, and obtain the stress level and maximum deformation of the whole ship under each working condition;

[0068] Step S5 specifically involves: Using a Python-based secondary development program to generate batch ANSYS command streams, multiple sets of command stream files are generated. In each set of command stream files, a pressure value of 1 is applied to the elements below the waterline of the FPSO full-ship finite element model for marking. The aqld result file from step S2 is imported into ANSYS, and normal loads are applied to all marked elements. Using the cargo tank pressure loading program, command stream files are automatically generated in the storage path based on the input array-style loading information, automatically loading cargo tank loads. Gravity is applied to the FPSO full-ship finite element model. Y- and Z-direction displacement constraints are applied to the bow finite element nodes, X- and Z-direction displacement constraints are applied to the finite element nodes at the junction of the stern and port side plate, and Y- and Z-direction displacement constraints are applied to the finite element nodes at the junction of the stern and starboard side plate. An ANSYS MAC macro program is written using Python to perform batch analysis of all design conditions of the FPSO full-ship finite element model. The deck static load mentioned in step S5 is calculated using the following formula:

[0069] P = P stat ·A+P deck-L ·L+m un ·g

[0070] Among them, P stat P is the uniformly distributed pressure on the supporting structure. deck-L For a linearly distributed uniform pressure on the supporting structure, m un The mass of equipment that acts on the supporting structure.

[0071] S6: Using the ANSYS post1 general post-processing module, the stress values ​​and maximum displacements of the region of interest are exported in batches to txt files for analysis.

[0072] Step S6 specifically involves: recording the node numbers of high-stress and large-deformation locations based on the finite element analysis results; writing the post-processing command stream in a text editor; using the *DIM function in ANSYS to generate n m-dimensional arrays corresponding to the high-stress locations, where n is the number of high-stress locations and m is the number of working cases; writing and storing the stress and deformation values ​​calculated for all working cases; and using the *set command to export the stress and deformation values ​​stored in the arrays, saving them as txt files in the storage path. The allowable stress values ​​for different material properties are calculated using the following formula:

[0073] [σ]=R eH / S

[0074] Among them, R eH Let S be the minimum yield stress of the material, and S be the safety factor.

Claims

1. A method for batch calculation and post-processing of finite element analysis for an entire ship, characterized in that, Includes the following steps: S1: Establish a wet surface model of the FPSO hull based on the environmental conditions of the FPSO working sea area and a large number of combined working conditions of the loading. S2: The wetted surface model of the FPSO hull generates load files in batches by transferring wave loads to the hull surface; S3: Establish a full-ship finite element model of the FPSO based on hull data and the latest hull thickness measurements, where: Establish a full-ship geometric model of the FPSO, including all major longitudinal and transverse components, including the inner shell and outer plate structure, double bottom ribs and longitudinal girder system, transverse strong frame and vertical girder, horizontal girder, transverse bulkhead and longitudinal bulkhead. Underwater visual inspection and ultrasonic thickness measurement were conducted to obtain the latest thickness measurement report for the hull. Create a plate thickness library. The thickness of the underwater side plates and bottom plates of the hull is corrected according to the thickness measurement report. The thickness of the remaining plates is determined according to the hull design data. Assign values ​​to the plate units of the FPSO, set the mesh size to the spacing of the longitudinal reinforcing members, and mesh the plates into shell units. Create a skeleton section library, assign values ​​to the skeleton reinforcement members of the FPSO, set the mesh size to the longitudinal reinforcement member spacing, and mesh the skeleton into beam elements and rod elements; S4: The full-ship finite element model is grouped and named according to the hull structure and the properties of marine steel; S5: Apply loads, boundary conditions, and perform batch static analysis on the FPSO full ship finite element model to obtain batch files of full ship stress values ​​and maximum displacement under each working condition; S6: Based on the batch files of stress values ​​and maximum displacements of the entire ship under each working condition, use the ANSYS post1 post-processing module to output batch txt files of stress values ​​and maximum displacements of the areas of interest of the entire ship. S7: Analyze and output the results of batch data on stress values ​​and maximum displacements in the areas of interest across the entire ship.

2. The method for batch calculation and post-processing of finite element analysis of an entire ship according to claim 1, characterized in that, In step S1, the method for establishing the wetted surface model of the hull is as follows: The independent variables for obtaining the combined working conditions include: effective wave height H s , spectral peak period T p , and liquid cargo tank loading conditions, and the working condition files are automatically generated by arranging and combining through a program; Write the coordinates of the key points on the wetted surface of the hull half-side in a text editor, generate a command stream in .dat format, save it in the storage path, and use the / INPUT command to call the command stream file to create the key points on the wetted surface of the hull. In the ANSYS GUI interface, select Spline Thru KP and manually select key points to generate spline curves for each station of the hull and the bow and stern. Use the ASKIN command to connect the above spline curves to generate the wetted surface on the half-hull side of the FPSO. Use the ARSYM command to generate the double side wet surface model, and use the AL command to generate the bottom outer plate plane; The grid is adjusted based on the minimum wave period of the FPSO working area. Different subsequent solution requirements have different requirements for grid quality. The judgment principle is that the grid size is not less than 1 / 7 of the wavelength corresponding to the minimum wave period.

3. The method for batch calculation and post-processing of finite element analysis of an entire ship according to claim 1, characterized in that, In step S4, one of the grouping methods for the whole ship finite element model includes the hull structure: cargo oil tank inner wall, cargo oil tank inner bottom plate, bottom outer plate, side outer plate, bilge outer plate, longitudinal bulkhead, transverse bulkhead, transverse strong frame, bottom longitudinal girder, functional platform, and main deck; the second grouping method for the whole ship finite element units includes the marine steel properties according to the allowable stress σ1, σ2, ..., σ n It is divided into n levels.

4. The method for batch calculation and post-processing of finite element analysis for an entire ship according to claim 1, characterized in that, Step S5, which involves obtaining batch files of the ship's stress values ​​and maximum displacements for each set of operating conditions, includes: A pressure value of 1 is applied to the elements below the waterline of the FPSO full-ship finite element model and marked. Import the batch generated load file results from step S2 into ANSYS and apply normal loads to all marked elements. Create a liquid cargo tank pressure loading program, obtain the command stream file in the storage path based on the input liquid cargo tank level, and realize the automatic pressure loading of the liquid cargo tank; Write deck static load, wave load, and cargo tank load into a Python program and generate batch command stream files in TXT format.

5. The method for batch calculation and post-processing of finite element analysis for an entire ship according to claim 4, characterized in that, In step S5, the loads include: deck static load, wave load, cargo tank load, and gravity; wherein: The static load on the deck is calculated using the following formula: P=P stat ·A+P deck-L ·L+m un ·g Among them, P stat P is the uniformly distributed pressure on the supporting structure. deck-L For a linearly distributed uniform pressure on the supporting structure, m un The mass of equipment that acts concentratedly on the supporting structure; The wave load is applied in the following manner: A pressure value of 1 is applied to the unit below the waterline and marked accordingly; Import the aqld result file from step S2 into ANSYS, and apply normal loads to all marked elements; the cargo tank loads are applied as follows: Create a liquid cargo tank pressure loading program that obtains the command stream file in the storage path based on the input liquid cargo tank level, thereby realizing automated pressure loading of the liquid cargo tank.

6. The method for batch calculation and post-processing of finite element analysis for an entire ship according to claim 1, characterized in that, In step S6, the step of outputting batch txt files of stress values ​​and maximum displacements of the entire ship's area of ​​interest: Record the node numbers of high stress and large deformation locations based on the finite element analysis results in AYSYS, and enter them into the command stream in a text editor; Use the *DIM function in AYSYS to generate an array to store the stress and deformation values ​​calculated under different working conditions; Use the *set command to export the stress and deformation values ​​stored in the array as a txt file.

Images