A method for predicting stress deformation in a ship section closing process

Abstract

This application discloses a method for predicting stress and deformation during the assembly of ship sections, relating to the field of modular ship construction. The method includes: establishing a finite element model of the ship section to be measured; applying strong constraint tooling to the finite element model of the ship section for straightening; simulating the welding and cooling processes of the ship section with added heat transfer parameters based on a double ellipsoidal welding heat source model to obtain the corresponding temperature field data for the welding and cooling processes; performing thermo-mechanical coupling on the finite element model of the ship section after strong constraint tooling straightening based on the temperature field data of the welding and cooling processes to obtain the deformation and stress field data of the ship section under the superposition of strong constraint tooling straightening and welding heat; removing the strong constraint tooling from the finite element model of the ship section to obtain the predicted results of deformation springback and residual stress field. This application predicts the stress-deformation effect of the strong constraint tooling straightening and welding superposition processes of the ship section.

Description

Technical Field

[0001] This application relates to the field of modular ship construction, and in particular to a method for predicting stress deformation during the assembly of ship sections. Background Technology

[0002] In shipbuilding, the assembly process of ship sections directly affects the overall construction quality of the vessel. In current practices, due to the combined effects of multiple technical factors, the structure of the ship sections is prone to undesigned deformation and residual stress, which significantly impacts the precision of modular assembly and the service life of the vessel. Engineering practice analysis reveals that the causes can be mainly summarized into the following three key aspects:

[0003] First, while the assembly fixture fulfills its functions of positioning, calibration, and geometric shape maintenance, its constraint mechanism has a dual effect. The fixture not only imposes necessary six-degree-of-freedom constraints on the assembly module but also directly leads to the unexpected accumulation of internal stress due to the strong constraint and straightening. Second, dimensional deviations caused by manufacturing tolerance control issues warrant attention. When the actual dimensions of the assembly module exceed the design tolerances of the strong constraint fixture, an interference fit effect will occur at the contact surface, and the resulting compressive stress will significantly alter the structural stress state. Finally, the thermo-mechanical coupling effect of the welding process cannot be ignored. The thermal stress generated during circumferential welding, along with the accompanying welding deformation, combined with the strong constraint stress of the fixture during welding, accumulates a large amount of strain energy. This accumulated strain energy is released during the removal of the fixture after welding, resulting in deformation rebound. These specific stress and deformation cycles may affect weld strength and structural lifespan.

[0004] Based on the problems mentioned above, in order to achieve accurate prediction of deformation control and stress levels during ship construction, and to provide reliable data support for ship assembly quality assessment and life cycle performance prediction, there is an urgent need for a method that can predict the stress-deformation law during the assembly of the main sections. Summary of the Invention

[0005] The purpose of this application is to address at least one of the aforementioned technical deficiencies.

[0006] On the one hand, embodiments of this application provide a method for predicting stress deformation during the assembly of ship sections, the method comprising:

[0007] A finite element model of the ship section to be measured is established. The finite element model of the ship section is a three-dimensional model established based on the actual manufacturing dimensions and tooling structure of the ship section to be measured. The finite element model is obtained by dividing the three-dimensional model into hexahedral meshes. The structure of the finite element model of the ship section includes the ship section and the tooling.

[0008] The finite element model of the ship section is subjected to strong constraint tooling straightening treatment, and the stress and deformation field prediction data of the ship section to be measured after the straightening is obtained based on the finite element model of the ship section after the strong constraint tooling straightening treatment.

[0009] Heat transfer-related parameters were added to the ship sections, and the welding and cooling processes of the ship sections with added heat transfer-related parameters were simulated based on the double ellipsoid welding heat source model to obtain the corresponding temperature field data of the welding and cooling processes.

[0010] The finite element model of the ship section after the strong constraint tooling straightening treatment was thermo-mechanically coupled based on the temperature field data of the welding and cooling process. The resulting finite element model of the ship section after thermo-mechanical coupling treatment was obtained. Based on the finite element model of the ship section after thermo-mechanical coupling treatment, the deformation and stress field data of the ship section under the superposition of the strong constraint tooling straightening and welding heat were obtained.

[0011] The finite element model of the ship section after thermo-coupling treatment is processed by removing the strong constraint tooling to obtain the deformation springback and residual stress field prediction results of the ship section to be measured after the release of the strong constraint load.

[0012] Optionally, the finite element model of the ship section may be subjected to strong constraint tooling correction processing, including:

[0013] A ring-shaped strongly constrained fixture model is established. The ring-shaped strongly constrained fixture model is set as a discrete rigid body. The ring-shaped strongly constrained fixture model is a ring composed of six ring-shaped petal structures. The six ring-shaped petal structures include five fixture indenters that can move radially and a stationary jig.

[0014] Six-degree-of-freedom fixed constraints are applied to the non-welded end faces of the finite element model of the ship section;

[0015] Set the contact properties between the tooling and the ship section;

[0016] Gravity and pressure loads are applied to the finite element model of the ship section.

[0017] Optionally, gravity and pressure loads may be applied to the finite element model of the ship section, including:

[0018] The first contact pair constraint is applied to the contact surface of the jig and the finite element model of the ship section according to the preset contact properties, and gravity is applied to the finite element model of the ship section.

[0019] A smooth radial displacement load is set for the tooling pressure head, and a second contact pair constraint is set according to the preset contact properties. Uniform pressure is applied to the welding end face included in the finite element model of the ship section.

[0020] Optionally, the contact properties include setting the friction coefficient for tangential behavior and setting the directional behavior to hard contact between surfaces. In the first contact pair constraint, the principal surface is the upper arc-shaped surface of the jig, and the secondary surface is the outer surface of the ship section. In the second contact pair constraint, the principal surface is the inner annular surface of all tooling indenters except the jig, and the secondary surface is the outer surface of the ship section.

[0021] Optionally, the ship section is set with a grid size according to the requirements of welding and interference contact, and is divided into a regular hexahedral grid using the neutral axis algorithm. The tooling head and jig are equipped with rounded corners.

[0022] Optionally, based on a double-ellipsoidal welding heat source model, the welding and cooling processes of the ship section with added heat transfer parameters are simulated to obtain the corresponding temperature field data for the welding and cooling processes, including:

[0023] Based on the preset actual welding process parameters, the parameters of the double ellipsoidal welding heat source model are adjusted to obtain the adjusted double ellipsoidal welding heat source model.

[0024] Based on the weld path of the ship section and the adjusted double ellipsoidal welding heat source model, a moving heat source DFLUX welding subroutine is generated, and heat transfer analysis parameters are added.

[0025] Based on the DFLUX welding subroutine with a mobile heat source and heat transfer analysis parameters, the welding and cooling processes of ship sections are simulated to obtain the corresponding temperature field data for the welding and cooling processes.

[0026] Optionally, the parameters required to generate the DFLUX welding subroutine for the moving heat source include welding path, welding current, welding voltage, conversion efficiency, welding speed, length of the first half-axis of the welding direction, length of the second half-axis of the welding direction, length of the second half-axis of the weld width direction, length of the second half-axis of the weld depth direction, and energy ratio of the front and rear ellipsoids. The heat transfer analysis parameters include thermal analysis step duration, predefined temperature field, surface heat exchange condition film coefficient, surface radiation emissivity, and mesh element type.

[0027] Optionally, the finite element model of the ship section after the strong constraint tooling straightening treatment is thermo-coupled based on the temperature field data of the welding and cooling processes, including:

[0028] The finite element model of the ship section after the strong constraint tooling straightening treatment is assigned thermo-coupling material parameters;

[0029] Temperature field data of welding and cooling processes are added to the finite element model of the ship section after the strong constraint tooling straightening treatment in the predefined temperature field, and stress data and deformation field data obtained after the strong constraint tooling straightening treatment are added to the initial conditions of the predefined stress field.

[0030] Optional, thermo-coupled material parameters include Young's modulus, coefficient of thermal expansion, yield stress, specific heat, and Poisson's ratio as a function of temperature.

[0031] Optionally, the process of removing the strongly constrained tooling from the finite element model of the ship section after thermo-coupling treatment includes:

[0032] The tooling pressure head in the finite element model of the ship section after thermal coupling is subjected to smooth displacement and repositioning, and the applied pressure is removed.

[0033] The beneficial effects of the technical solutions provided in this application include at least the following:

[0034] In this application, a mesh model of the ship section to be measured can be established, and the mesh model is subjected to strong constraint tooling straightening treatment. This yields stress and deformation field data for the ship section after straightening. Then, based on a double-ellipsoidal welding heat source model, the welding and cooling processes of the ship section with added heat transfer parameters are simulated, obtaining corresponding temperature field data for the welding and cooling processes. Finally, thermo-mechanical coupling is performed based on the temperature field data of the welding and cooling processes, and the strong constraint tooling is removed to simulate the springback process after its removal. Ultimately, the predicted deformation springback and residual stress field of the ship section after the release of the strong constraint load are obtained. Therefore, this application comprehensively considers the stress-deformation response of non-ideal ship sections with manufacturing deviations or gravity deformation under the superposition of strong constraint tooling straightening and welding thermal stress, as well as the stress release and deformation springback process after the removal of the strong constraint tooling. This provides data support for determining whether the deformation and stress levels of the ship meet design standards, and for predicting the assembly accuracy and service life of subsequent hull section docking.

[0035] Furthermore, in this application, after fixing the ship section mesh model with a jig and performing smooth displacement processing at a set distance on the ship section mesh model after loading, a first contact pair and a second contact pair can be set according to preset contact attributes. That is, "hard contact" and interference settings are added to the contact surfaces of the tooling and the section in ABAQUS. This can avoid the interference problem that exists in the ship section during the straightening process due to manufacturing errors, thereby ensuring that the ship section will not penetrate the tooling surface during the simulation. Attached Figure Description

[0036] To more clearly illustrate the technical solutions in the embodiments of this application, the accompanying drawings used in the description of the embodiments will be briefly introduced below. Obviously, the accompanying drawings described below are only some embodiments of this application. For those skilled in the art, other drawings can be obtained based on these drawings without creative effort.

[0037] Figure 1 A flowchart illustrating a method for predicting stress and deformation during the assembly of ship sections, provided as an embodiment of this application;

[0038] Figure 2 Schematic diagrams showing the relevant dimensions of the finite element model of the ship section provided in the embodiments of this application;

[0039] Figure 3 This is a schematic diagram of the mesh division method provided in the embodiments of this application;

[0040] Figure 4 A schematic diagram of material parameters provided for embodiments of this application;

[0041] Figure 5 This is a schematic diagram of a double ellipsoidal heat source model provided in an embodiment of this application;

[0042] Figure 6 The welding temperature field distribution cloud map provided for the embodiments of this application;

[0043] Figure 7 Residual stress cloud diagram of a ship section provided for embodiments of this application;

[0044] Figure 8 Deformation cloud diagram of tooling release after welding completion, provided in an embodiment of this application;

[0045] Figure 9 A schematic diagram of the stress field of the main section placed on the jig in an embodiment of this application;

[0046] Figure 10 A schematic diagram of the deformation field of the main section placed on the jig in an embodiment of this application;

[0047] Figure 11 This is a flowchart illustrating another method for predicting stress and deformation during the assembly of ship sections, provided in an embodiment of this application. Detailed Implementation

[0048] The embodiments of this application are described in detail below. Examples of these embodiments are shown in the accompanying drawings, wherein the same or similar reference numerals denote the same or similar elements or elements having the same or similar functions throughout. The embodiments described below with reference to the accompanying drawings are exemplary and are only used to explain this application, and should not be construed as limiting the invention.

[0049] Those skilled in the art will understand that, unless specifically stated otherwise, the singular forms “a,” “an,” “the,” and “the” used herein may also include the plural forms. It should be further understood that the term “comprising” as used in this application means the presence of the stated features, integers, steps, operations, elements, and / or components, but does not exclude the presence or addition of one or more other features, integers, steps, operations, elements, components, and / or groups thereof. It should be understood that when we say an element is “connected” or “coupled” to another element, it can be directly connected or coupled to the other element, or there may be intermediate elements. Furthermore, “connected” or “coupled” as used herein can include wireless connections or wireless coupling. The term “and / or” as used herein includes all or any units and all combinations of one or more associated listed items.

[0050] To make the objectives, technical solutions, and advantages of this application clearer, the embodiments of this application will be described in further detail below with reference to the accompanying drawings.

[0051] The technical solution of this application and how the technical solution of this application solves the above-mentioned technical problems are described in detail below with specific embodiments. These specific embodiments can be combined with each other, and the same or similar concepts or processes may not be described again in some embodiments. The embodiments of this application will now be described with reference to the accompanying drawings.

[0052] Specifically, such as Figure 1 As shown, the method may include:

[0053] Step S101: Establish the finite element model of the ship section to be measured. The finite element model of the ship section is a three-dimensional model established based on the actual manufacturing dimensions and tooling structure of the ship section to be measured. The finite element model is obtained by dividing the three-dimensional model into hexahedral meshes. The structure of the finite element model of the ship section includes the ship section and the tooling.

[0054] Optionally, in practical applications, a corresponding finite element model of the ship section can be determined based on the manufacturing dimensions and tooling structure of the ship section to be measured. This finite element model of the ship section is obtained by performing hexahedral mesh generation.

[0055] The structure of the finite element model of the ship section includes the ship section and the tooling. The ship section is represented by an elliptical cylinder, which represents the actual ship section being measured. The tooling is a ring-shaped strongly constrained tooling.

[0056] In an optional embodiment of this application, the ship section is set with a grid size according to the requirements of welding and interference contact, and is divided into a regular hexahedral grid using a neutral axis algorithm. The tooling head and jig are provided with rounded corners.

[0057] Optionally, the established finite element model of the ship section includes an elliptical cylinder and an annular strongly constrained fixture representing the actual ship section to be measured. The elliptical cylinder is divided into a regular hexahedral mesh according to the requirements of welding and interference contact and using the neutral axis algorithm. The fixture is a ring composed of six annular petal structures. The six annular petal structures include five fixture indenters that can move radially and a stationary jig. The edges of the fixture indenters and jig are set to rounded corners.

[0058] Optionally, the element type of the elliptical cylinder can be set to C3D8R. Assuming the material of the ship section finite element model is SUS304 steel, the tooling is set as a discrete rigid body and does not need to be assigned material properties. For example, the material parameters of the ship section can all be set to... Figure 4 The value that can be taken in the range.

[0059] For example, an elliptical cylinder with a major semi-axis length of 200.2 mm, a minor semi-axis length of 199.98 mm, a thickness of 6 mm, and a length of 500 mm can be created to represent the ship section. When meshing the elliptical cylinder, it can be divided at 50 mm and 100 mm from the edge of the weld end (end face A). The unit length transitions from 5 mm to 1 mm from the plane 100 mm from end face A to the plane 50 mm from end face A (i.e., the weld plane). The unit transitions from end face A to the plane 50 mm (i.e., the weld plane) also transitions from 5 mm to 1 mm. At the same time, it is necessary to ensure that there is a dense area with a width of 10 mm centered on the weld, consisting of units with a side length of 1 mm. In addition, four seeds are scattered along the thickness direction of the elliptical cylinder. Scattering seeds is a common method in ABAQUS mesh generation. Specifically, the size of the mesh is determined by controlling the interval or number of seeds (initial nodes). The remaining annular edges are seeded at intervals of about 2mm, and the neutral axis algorithm is used to divide it into a regular hexahedral mesh. The total number of elements in the hexahedral mesh is 331,584.

[0060] In addition, the ship section mesh model also includes a fixture, which is a circle with an inner diameter of 400mm composed of six annular petal-shaped fixture heads. The edges of the fixture heads are rounded to prevent cutting and deformation during the extrusion process and to avoid convergence issues in contact calculations. It is important to note that the element side length is larger than that of the elliptical cylinder during mesh generation. The mesh size of the fixture head contact surface (i.e., the inner surface of the fixture head's annular ring) is approximately 6.23mm. The fixture head comprises a total of 1476 elements, and the entire model is designed using a discrete rigid body configuration to save computational resources. During assembly, except for the gravity-oriented fixture head (i.e., the jig), all others are offset radially outward by 0.2mm to fit precisely against the outer surface of the elliptical cylinder. The resulting dimensions of the ship section mesh model are as follows: Figure 2 As shown, the corresponding mesh division method is as follows: Figure 3 As shown, where Figure 2 and Figure 3 All dimensions are in mm.

[0061] Step S102: Perform strong constraint tooling straightening treatment on the finite element model of the ship section, and obtain the stress and deformation field prediction data of the ship section to be measured after the straightening is completed based on the finite element model of the ship section after the strong constraint tooling straightening treatment.

[0062] In practical applications, the assembly fixtures for ship sections play a role in maintaining and straightening the shape, which adds additional constraints and introduces internal stress. In order to predict the impact of the introduced internal stress, the finite element model of the ship section is subjected to strong constraint fixture straightening treatment. Then, based on the finite element model of the ship section after strong constraint fixture straightening treatment, the stress and deformation field data of the ship section to be measured after straightening are obtained.

[0063] In an optional embodiment of this application, the finite element model of the ship section is subjected to strong constraint tooling straightening treatment, including:

[0064] A ring-shaped strongly constrained fixture model is established. The ring-shaped strongly constrained fixture model is set as a discrete rigid body. The ring-shaped strongly constrained fixture model is a ring composed of six ring-shaped petal structures. The six ring-shaped petal structures include five fixture indenters that can move radially and a stationary jig.

[0065] Six-degree-of-freedom fixed constraints are applied to the non-welded end faces of the finite element model of the ship section;

[0066] Set the contact properties between the tooling and the ship section;

[0067] Gravity and pressure loads are applied to the finite element model of the ship section.

[0068] Optionally, a ring composed of six annular petal-shaped tooling heads and a jig can be used as an annular strongly constrained tooling model. In practical applications, since the stiffness and hardness of the tooling are much higher than those of the ship section, the deformation can be ignored. Therefore, the annular strongly constrained tooling model can be set as a discrete rigid body, that is, the tooling head and jig are considered as rigid bodies.

[0069] Furthermore, the non-welded end faces of the finite element model of the ship section can be fixed. Specifically, a six-degree-of-freedom fixed constraint can be applied to the non-welded end faces. Then, the contact properties between the tooling and the ship section can be set on the finite element model of the ship section, and gravity and pressure treatment can be applied to complete the strong constraint tooling correction treatment of the finite element model of the ship section.

[0070] In optional embodiments of this application, applying gravity and pressure loads to the finite element model of the ship section includes:

[0071] The first contact pair constraint is applied to the contact surface of the jig and the finite element model of the ship section according to the preset contact properties, and gravity is applied to the finite element model of the ship section.

[0072] A smooth radial displacement load is set for the tooling pressure head, and a second contact pair constraint is set according to the preset contact properties. Uniform pressure is applied to the welding end face included in the finite element model of the ship section.

[0073] Optionally, when simulating the established finite element model of the ship section, the tooling can be mounted on a jig and completely fixed at one end. Then, a first contact pair constraint is applied to the contact surface of the jig and the finite element model of the ship section according to the preset contact properties, thereby applying gravity to the finite element model of the ship section. Under the action of gravity, the outer surface of the ship section can be pre-positioned to fit the arc concave surface of the jig. The ship section will have slight deformation under the action of gravity or manufacturing factors (such as plate rolling and rounding deviation, which cause the cross section of the annular section to appear as an elliptical ring). A second contact pair constraint is set according to the preset contact properties. Then, a smooth displacement load can be set for the tooling head. Specifically, the tooling head can be radially closed to squeeze the ship section, thereby forcing the outer surface of the ship section to fit the tooling surface. Then, uniform pressure is applied to the welding end face included in the finite element model of the ship section to simulate the extrusion force of the docking end face.

[0074] Optionally, in actual ABAQUS operation, the specific steps are as follows: 1. Add initial constraints: the jig is fixed, and the non-welded end face of the hull section is fully constrained (i.e., all translational and rotational motions of this end face are restricted); 2. In analysis step one, apply gravity to the hull section; 3. In analysis step two, the pressure head applies smooth radial displacement to straighten the hull section; 4. In analysis step three, apply uniform pressure to the other end face to simulate the compression between the joined hull sections. At this point, due to manufacturing errors, the hull section will have interference during the straightening process. Based on this, in ABAQUS, a "hard contact" and interference setting can be added to the contact surface between the tooling and the hull section to ensure that the hull section does not penetrate the tooling surface during the simulation.

[0075] Step S103: Add heat transfer related parameters to the ship section, and simulate the welding and cooling process of the ship section with added heat transfer related parameters based on the double ellipsoid welding heat source model to obtain the corresponding temperature field data of the welding and cooling process.

[0076] Optionally, the heat transfer parameters required for simulating the welding and cooling process of the ship section can be preset, and then the preset heat transfer parameters can be added to the ship section. These heat transfer parameters may include the parameters required by the DFLUX welding subroutine for the moving heat source used in the simulation, as well as the heat transfer analysis parameters.

[0077] In optional embodiments of this application, the parameters required to generate the DFLUX welding subroutine for the moving heat source include welding path, welding current, welding voltage, conversion efficiency, welding speed, length of the first half-axis of the welding direction, length of the second half-axis of the welding direction, length of the second half-axis of the weld width direction, length of the second half-axis of the weld depth direction, and energy ratio of the front and rear ellipsoids. The heat transfer analysis parameters include cooling analysis step duration, predefined temperature field, surface heat exchange condition film coefficient, surface radiation emissivity, and mesh element type.

[0078] Optionally, the values ​​of each parameter in the required parameters for generating the mobile heat source subroutine and the heat transfer analysis parameters can be adjusted according to actual needs, and this application embodiment does not limit this.

[0079] In an optional embodiment of this application, the welding and cooling process of a ship section with added heat transfer parameters is simulated based on a double ellipsoidal welding heat source model to obtain the corresponding temperature field data of the welding and cooling process, including:

[0080] Based on the preset actual welding process parameters, the parameters of the double ellipsoidal welding heat source model are adjusted to obtain the adjusted double ellipsoidal welding heat source model.

[0081] Based on the weld path of the ship section and the adjusted double ellipsoidal welding heat source model, a moving heat source DFLUX welding subroutine is generated, and heat transfer analysis parameters are added.

[0082] Based on the DFLUX welding subroutine with a mobile heat source and heat transfer analysis parameters, the welding and cooling processes of ship sections are simulated to obtain the corresponding temperature field data for the welding and cooling processes.

[0083] Optionally, since the welding process parameters are set differently for different welding requirements, welding process parameters can be preset according to the actual welding requirements. Then, the parameters of the double ellipsoidal welding heat source model can be adjusted according to the preset welding process parameters to obtain the adjusted double ellipsoidal welding heat source model.

[0084] In an optional embodiment of this application, the heat flux density expression of the double ellipsoidal heat source is:

[0085]

[0086] in, As a heat source energy, For the total welding heat flux density, and The heat source is the energy distribution coefficient of the first and second halves, and , , and These are the shape parameters.

[0087] In practical applications, when using a double ellipsoidal heat source, the welding heat source temperature can reach thousands of degrees Celsius. Various heat dissipation factors cannot be ignored. Specifically, there are three heat transfer modes: heat conduction, heat convection, and radiation. In practical applications, the heat source parameters, moving speed, and cooling step parameters can be determined by the actual welding and post-weld heat treatment processes.

[0088] Heat conduction can be expressed as:

[0089]

[0090] In the formula, Represents heat flux density, Indicates thermal conductivity, For temperature, The normal direction, This is the temperature gradient (i.e., the rate of change of temperature along the normal direction of the boundary surface).

[0091] The expression for convective heat transfer is:

[0092]

[0093] In the formula, Represents heat flux density, Indicates the convective heat transfer coefficient. and These represent the surface temperature of a solid and the temperature of a liquid or gas, respectively.

[0094] The expression for thermal radiation is:

[0095]

[0096] In the formula, Represents heat flux density, For emission rate, Boltzmann's constant, and These represent the solid surface temperature and the ambient temperature, respectively.

[0097] Furthermore, a DFLUX welding subroutine with a moving heat source can be generated based on the weld path of the ship section. Then, the heat transfer analysis parameters to be added can be obtained. Finally, based on the generated DFLUX welding subroutine with the moving heat source and the added heat transfer analysis parameters, the welding and cooling process of the ship section can be simulated to obtain the corresponding temperature field data of the welding and cooling process.

[0098] For example, a welding-specific plugin can be used to generate a welding moving heat source subroutine, DFLUX, which sets the welding path to a parallel plane 50mm from end face A and intersects with the outer surface of the elliptical cylinder (e.g., Figure 2As shown in the diagram, the welding current is set to 140A, the welding voltage to 9V, the conversion efficiency to 0.9, the welding speed to 5mm / s, and the welding heat source is set to a double ellipsoidal heat source model (as shown in the diagram). Figure 5 As shown in the figure, the length of the first half-axis a in the welding direction is set to 5mm, the length of the second half-axis a2 in the welding direction is set to 10mm, the length of the second half-axis b in the weld width direction is set to 4mm, the length of the second half-axis c in the weld depth direction is set to 3mm, and the energy ratio of the front and rear ellipsoids is set to 0.5. Then, the welding time is automatically calculated to be 251.33s based on the welding moving heat source DFLUX subroutine plugin.

[0099] Furthermore, the welding analysis step duration was set to 251.33 s, and the cooling analysis step duration in the heat transfer analysis parameters was set to 2000 s. All mechanical and displacement loads (including displacement boundary condition constraints and gravity loads) were deleted. The initial temperature in the predefined field was defined as 25℃, and the surface heat exchange condition film coefficient was set to 0.015 mW / (mm²·℃), with an ambient temperature of 25℃. The surface radiation emissivity was set to 0.7, with an ambient temperature of 25℃. Simultaneously, the pre-generated mesh was kept unchanged, and the mesh element type was modified to an eight-node linear heat conduction element DC3D8. Finally, the temperature field data for the welding and cooling processes were obtained by submitting the calculation based on the generated DFLUX subroutine using transient heat conduction. The temperature field distribution during the welding process of the ship section is shown below. Figure 6 As shown, the maximum temperature is 1489℃ at the welding heat source, which is slightly higher than the set material melting point temperature. The temperature of the rest of the part is 25℃, which is consistent with the set ambient temperature. There are no abnormal conditions such as negative temperatures, indicating that the mesh element size is reasonable and the heat conduction simulation results are correct.

[0100] Step S104: Based on the temperature field data of the welding and cooling process, perform thermo-mechanical coupling on the finite element model of the ship section after the strong constraint tooling straightening treatment to obtain the finite element model of the ship section after thermo-mechanical coupling treatment, and obtain the deformation and stress field data of the ship section under the superposition of the strong constraint tooling straightening and welding heat based on the finite element model of the ship section after thermo-mechanical coupling treatment.

[0101] Optionally, after obtaining the temperature field data of the welding and cooling processes, the finite element model of the ship section after the strong constraint tooling straightening treatment can be thermo-coupled to obtain a thermo-coupled finite element model of the ship section. This thermo-coupled finite element model can be obtained under the influence of welding heat. Furthermore, based on the thermo-coupled finite element model of the ship section, the deformation and stress field data of the ship section under the superimposed effects of strong constraint tooling straightening and welding heat can be obtained.

[0102] In an optional embodiment of this application, thermo-mechanical coupling is performed on the finite element model of the ship section after the strong constraint tooling straightening treatment based on the temperature field data of the welding and cooling processes, including:

[0103] The finite element model of the ship section after the strong constraint tooling straightening treatment is assigned thermo-coupling material parameters;

[0104] Temperature field data of welding and cooling processes are added to the finite element model of the ship section after the strong constraint tooling straightening treatment in the predefined temperature field, and stress data and deformation field data obtained after the strong constraint tooling straightening treatment are added to the initial conditions of the predefined stress field.

[0105] Optionally, when performing thermo-mechanical coupling on the finite element model of the ship section after the strong constraint tooling has been straightened, thermo-mechanical coupling material parameters can be assigned to the finite element model of the ship section after the strong constraint tooling has been straightened. The coupling material parameters include Young's modulus, coefficient of thermal expansion, yield stress, specific heat and Poisson's ratio that vary with temperature.

[0106] Furthermore, welding temperature field data can be added to the predefined field of the finite element model of the ship section after the strong constraint tooling straightening treatment to calculate welding stress, and cooling temperature field data can be added to the predefined field to simulate the cooling contraction process. Finally, stress data and deformation field data obtained after the strong constraint tooling straightening treatment can be added to the initial conditions of the predefined stress field.

[0107] Step S105: Remove the strong constraint tooling from the finite element model of the ship section after the thermo-coupling treatment to obtain the deformation springback and residual stress field prediction results of the ship section to be measured after the release of the strong constraint load.

[0108] Optionally, the strong constraint fixtures can be removed from the finite element model of the ship section after the thermo-coupling process, that is, the strong constraint fixtures can be released to simulate the springback deformation of the section, and then the deformation springback and residual stress field prediction results of the ship section to be measured after the strong constraint load is released can be obtained.

[0109] In optional embodiments of this application, the process of removing the strong constraint tooling from the finite element model of the ship section after thermal coupling treatment includes:

[0110] The tooling pressure head in the finite element model of the ship section after thermal coupling is subjected to smooth displacement and repositioning, and the applied pressure is removed.

[0111] Optionally, when performing strong constraint tooling processing on the finite element model of the ship section, the tooling head is subjected to smooth radial displacement processing and pressure application processing. Then, when removing the strong constraint tooling, the tooling head can be subjected to smooth displacement return processing and pressure removal processing.

[0112] For example, in practical applications, based on the temperature field data of the welding and cooling processes obtained above, a predefined temperature field can be set. Assuming the elliptical cylinder in the finite element model of the ship section is a tooling removed after cooling for 2000 seconds, the displacement load of the fixture can be set to expand radially outward by 0.2 mm to simulate the springback process after the removal of the strongly constrained tooling. The final residual stress of the ship section... Figure 7 As shown, the maximum residual stress is located at the highest point of the weld in the main section. This is due to the effect of gravity during the welding process. Figure 7 The right end of the middle weld forms a cantilever beam-like structure. At the highest point, a large tensile stress is required to counteract the weight of the structure. At the same time, the stress is superimposed on the residual stress of the welding, making this area the point of maximum stress. Figure 8 This indicates that the area with the greatest deformation is located at the lowest point of the welded end. Because both the weld start and end points are located below the main section, even after 2000 seconds of cooling, there is still a slightly higher residual temperature than elsewhere, resulting in the largest thermal deformation value. The stress field of the ship section placed on the jig before welding (e.g., ...) Figure 9 ) and deformation fields (such as Figure 10 (As shown).

[0113] In an optional embodiment of this application, the strong constraint fixture is released after welding, resulting in a maximum deformation of 0.02287 mm (e.g., Figure 8 As shown in the figure, in order to verify whether the results are accurate, strain flowers can be applied to the corresponding positions based on the simulation results for further verification.

[0114] Understandably, in practical applications, the temperature changes caused by structural deformation are negligible compared to the high temperatures of welding. The thermal stress of the hull structure can be considered to be mainly generated by welding. Therefore, this application adopts a sequential coupling method to solve the thermal stress. The sequential coupling method requires first solving the temperature field and storing the temperature field data at the nodes of the deformable body. Then, when solving the thermo-coupling stress and strain, the temperature of the deformable body nodes is re-interpolated to restore the temperature field in order to calculate the thermal stress. Since step S102 is independent of temperature, when the computing power is sufficient, step S103 (i.e., solving the temperature field) can be solved independently and synchronously with the stress and deformation data corresponding to the finite element model of the ship section in step S105 (i.e., solving the deformation-stress field of the ship section under the mechanical load of the strongly constrained tooling before welding). After both are solved, the predefined temperature field technology is applied to the new model (i.e., step 104 is executed), and finally the thermo-coupling deformation and stress are solved. This can significantly save computing time and improve efficiency.

[0115] In this embodiment, the effects of the strong constraint tooling straightening and welding superposition process on the stress-deformation of the ship section during the assembly process are comprehensively considered and effectively predicted to ensure that the deformation and stress level of the ship meet the design standards, providing data support for the prediction of the assembly accuracy and service life of the subsequent hull section docking.

[0116] To better understand the methods provided in the embodiments of this application, the steps and flow of the methods provided in this application are described below.

[0117] In practical applications, a finite element model (i.e., a finite element model of the ship section) can be established using hexahedral elements based on the structure of the ship section and tooling. During modeling, the model's dimensional parameters can be modified according to manufacturing dimensional deviations to create a finite element model with these deviations, and the mesh size of the welding area can be refined to obtain the finite element model of the ship section. Since the stiffness and hardness of the tooling are much higher than those of the ship section, their deformation can be ignored; therefore, the jig and tooling pressure head are considered as rigid bodies.

[0118] Furthermore, such as Figure 11 As shown, initial constraints are added: the jig is fixed, and the non-welded end face of the hull section is fully constrained (i.e., all translational and rotational motions of this end face are restricted); Analysis step one: apply gravity to the hull section; Analysis step two: apply smooth radial displacement with the pressure head to straighten the section; Analysis step three: apply uniform pressure to the other end face to simulate the compression between the joined sections; Analysis step four: add a welding temperature field (i.e., welding temperature field data) to the predefined field to simulate welding stress; Analysis step five: add a cooling temperature field (i.e., cooling temperature field data) to the predefined field to simulate the cooling contraction process; Analysis step six: release the strong constraint fixture to simulate the springback deformation of the section. In analysis steps four and five, the temperature change caused by structural deformation is negligible compared to the high welding temperature. The thermal stress of the hull structure can be considered mainly generated by welding. Therefore, the temperature field can be solved first, and the temperature field data can be stored at the nodes of the deformable body (i.e.,...). Figure 11 In the calculation of the welding temperature field, the temperature at the nodes of the deformed body is re-interpolated when solving for the thermo-coupling stress and strain to restore the temperature field and calculate the thermal stress. After the welding temperature field and heat treatment temperature field are completed, the predefined temperature field technique is then applied to the new model containing analysis steps four to six (i.e., Figure 11 (The tooling process is removed during the temperature field calculation), and finally the thermo-mechanical coupling, residual deformation and stress are solved.

[0119] It should be understood that although the steps in the flowcharts of the accompanying figures are shown sequentially as indicated by the arrows, these steps are not necessarily executed in the order indicated by the arrows. Unless explicitly stated herein, there is no strict order restriction on the execution of these steps, and they can be executed in other orders. Moreover, at least some steps in the flowcharts of the accompanying figures may include multiple sub-steps or multiple stages. These sub-steps or stages are not necessarily completed at the same time, but can be executed at different times, and their execution order is not necessarily sequential, but can be performed alternately or in turn with other steps or at least some of the sub-steps or stages of other steps.

[0120] The above description is only a partial embodiment of the present invention. It should be noted that for those skilled in the art, several improvements and modifications can be made without departing from the principle of the present invention, and these improvements and modifications should also be considered within the scope of protection of the present invention.

Claims

1. A method for predicting stress and deformation during the assembly of ship sections, characterized in that, include: A finite element model of the ship section to be measured is established. The finite element model of the ship section is a three-dimensional model established based on the actual manufacturing dimensions and tooling structure of the ship section to be measured. The finite element model is obtained by dividing the three-dimensional model into hexahedral meshes. The structure of the finite element model of the ship section includes the ship section and the tooling. The finite element model of the ship section is subjected to strong constraint tooling straightening treatment, and the stress and deformation field prediction data of the ship section to be measured after the straightening is obtained based on the finite element model of the ship section after the strong constraint tooling straightening treatment. Heat transfer-related parameters are added to the ship section, and the welding and cooling process of the ship section with added heat transfer-related parameters is simulated based on the double ellipsoid welding heat source model to obtain the corresponding temperature field data of the welding and cooling process. The finite element model of the ship section after the strong constraint tooling straightening treatment is thermo-mechanically coupled based on the temperature field data of the welding and cooling process to obtain the finite element model of the ship section after thermo-mechanical coupling treatment. Based on the finite element model of the ship section after thermo-mechanical coupling treatment, the deformation and stress field data of the ship section under the superposition of strong constraint tooling straightening and welding heat are obtained. The finite element model of the ship section after the thermo-coupling treatment is subjected to the removal of the strong constraint tooling to obtain the deformation springback and residual stress field prediction results of the ship section to be measured after the release of the strong constraint load.

2. The method according to claim 1, characterized in that, The process of performing strong constraint tooling correction on the finite element model of the ship section includes: A ring-shaped strongly constrained tooling model is established. The ring-shaped strongly constrained tooling model is set as a discrete rigid body. The ring-shaped strongly constrained tooling model is a ring composed of six ring-shaped petal structures. The six ring-shaped petal structures include five tooling indenters that can move radially and a stationary jig. Six-degree-of-freedom fixed constraints are applied to the non-welded end faces of the finite element model of the ship section; Set the contact properties between the tooling and the ship section; Gravity and pressure loads are applied to the finite element model of the ship section.

3. The method according to claim 2, characterized in that, The gravity and pressure loads applied to the finite element model of the ship section include: A first contact pair constraint is applied to the contact surface of the jig and the finite element model of the ship section according to a preset contact property, and gravity is applied to the finite element model of the ship section. A smooth radial displacement load is set on the tooling pressure head, and a second contact pair constraint is set according to the preset contact properties. Uniform pressure is applied to the welding end face included in the finite element model of the ship section.

4. The method according to claim 3, characterized in that, The contact properties include setting the friction coefficient for tangential behavior and setting the directional behavior to hard contact between surfaces. In the first contact pair constraint, the principal surface is the upper arc-shaped surface of the jig, and the secondary surface is the outer surface of the ship section. In the second contact pair constraint, the principal surface is the inner annular surface of all tooling indenters except the jig, and the secondary surface is the outer surface of the ship section.

5. The method according to claim 2, characterized in that, The ship section is set with a grid size according to the requirements of welding and interference contact, and is divided into a regular hexahedral grid using the neutral axis algorithm. The tooling head and the jig are provided with rounded corners.

6. The method according to claim 1, characterized in that, The welding and cooling process of the ship section with added heat transfer parameters is simulated based on the double ellipsoidal welding heat source model to obtain the corresponding temperature field data of the welding and cooling process, including: Based on the preset actual welding process parameters, the parameters of the double ellipsoidal welding heat source model are adjusted to obtain the adjusted double ellipsoidal welding heat source model. Based on the weld path of the ship section and the adjusted double ellipsoidal welding heat source model, a moving heat source DFLUX welding subroutine is generated, and heat transfer analysis parameters are added. Based on the DFLUX welding subroutine of the mobile heat source and the heat transfer analysis parameters, the welding and cooling process of the ship section is simulated to obtain the corresponding temperature field data of the welding and cooling process.

7. The method according to claim 6, characterized in that, The parameters required to generate the DFLUX welding subroutine for the moving heat source include welding path, welding current, welding voltage, conversion efficiency, welding speed, length of the first half-axis of the welding direction, length of the second half-axis of the welding direction, length of the second half-axis of the weld width direction, length of the second half-axis of the weld depth direction, and energy ratio of the front and rear ellipsoids. The heat transfer analysis parameters include thermal analysis step duration, predefined temperature field, surface heat exchange condition film coefficient, surface radiation emissivity, and mesh element type.

8. The method according to claim 1, characterized in that, The process of thermo-coupling the finite element model of the ship section after the strong constraint tooling straightening treatment based on the temperature field data of the welding and cooling processes includes: The finite element model of the ship section after the strong constraint tooling straightening treatment is assigned thermo-coupling material parameters; The temperature field data of the welding and cooling process is added to the finite element model of the ship section after the strong constraint tooling straightening treatment in the predefined temperature field, and the stress data and deformation field data obtained after the strong constraint tooling straightening treatment are added to the initial conditions of the predefined stress field.

9. The method according to claim 8, characterized in that, The thermo-coupled material parameters include Young's modulus, coefficient of thermal expansion, yield stress, specific heat, and Poisson's ratio, which vary with temperature.

10. The method according to claim 1, characterized in that, The process of removing the strongly constrained tooling from the finite element model of the ship section after the thermal coupling treatment includes: The tooling pressure head in the finite element model of the ship section after the thermo-coupling treatment is subjected to smooth displacement and repositioning processing, and the applied pressure is removed.

Images