Finite element analysis method for contact between grillage structure and single structure

Abstract

The invention provides a finite element analysis method for contact of a grillage structure and a single structure, which comprises the following steps of: dividing a contact area of the grillage structure and the single structure into grids, and then stretching each grid of the grillage structure in the contact area into a columnar unit in a direction far away from the grillage structure, in other words, a single structure is dispersed into a plurality of columnar units, the columnar units are spring units or beam units, finally, loads are applied to the ends, away from the grillage structure, of the columnar units, and the structural response of the grillage structure under the action of the loads is obtained. By dispersing the single structure into the spring units or the beam units, the situation that different areas of the grillage structure have different contact rigidities and the single structure can be effectively simulated on the premise of still using statics analysis, the accuracy of local structure simulation is improved, and powerful technical support is provided for actual production and construction.

Description

Technical Field

[0001] The invention relates to the technical field of shipbuilding, and in particular to a finite element analysis method for contact between a plate frame structure and a single structure. Background Art

[0002] Plate frame structure refers to a steel structure composed of plates, vertical and horizontal cross-frames and girders, which is widely used in the field of shipbuilding. With the continuous development of the shipbuilding industry, ship structure design has become increasingly complex, and finite element analysis technology has become one of the indispensable tools to support ship design. In ship structure design, finite element analysis can perform static strength analysis, dynamic analysis, fatigue analysis, thermodynamic analysis and other calculations on the ship structure, among which static strength analysis is the most common. In the static strength analysis of ships, the contact problem between the plate frame structure and the single structure is involved in many links, such as: the contact between the hull outer plate and the dock pier when the ship is docked, the distributed load applied to the plate frame through a single structure, and the contact between the hull outer plate and the dock buffer layer when the ship is berthed.

[0003] At present, the common way to deal with the contact problem between the plate frame structure and the single structure is to simplify the single structure into RBE binding or uniform load. This technical means can meet the calculation requirements of the finite element calculation of large-scale ship structures, but when considering local structures, the simulation results of the contact area are not accurate enough due to its over-simplification of the contact between structures. Another technical means is to use contact calculation and analysis methods to simulate the contact of real structures. This method has accurate results but requires high computing power and is difficult to adapt to the rapid calculation of large-scale structures. Summary of the invention

[0004] In view of the above shortcomings in the prior art, the present invention simulates the contact between the plate frame structure and the single structure by using the spring unit / beam unit commonly used in finite element analysis and an assumed rigid plane. This not only avoids the computing power limitation brought by contact calculation analysis, but also can more accurately simulate the local response of the structural contact area.

[0005] To achieve the above-mentioned and other related purposes, the present invention provides a finite element analysis method applicable to the contact problem between a plate frame structure and a single structure, comprising the following steps:

[0006] S1: Determine the scope of the finite element calculation model according to the location of the plate frame structure, and the finite element calculation model is a hull model including the plate frame structure;

[0007] S2: Divide the finite element calculation model into a coarse grid, and use 3D modeling software to establish a coarse grid model of the finite element calculation model;

[0008] S3: Refine the coarse grid in the contact area between the plate frame structure and the single structure to form a refined grid;

[0009] S4: discretizing the single structure into a plurality of columnar units, stretching each refined grid of the plate-frame structure located in the contact area in a direction away from the plate-frame structure to form a columnar unit, wherein the columnar unit is perpendicular to the plate-shaped plane of the plate-frame structure located in the contact area, and the unit length of the columnar unit is the thickness of the single structure;

[0010] S5: Determine the material parameters of the columnar unit according to the actual material parameters of the single structure;

[0011] S6: Determine the type of contact problem, and divide the finite element calculation of the plate frame structure strength into a load problem and a boundary problem. When a single structure actively applies a known load to the plate frame structure or needs to analyze the effect of the load size on the result, it is a load problem. When the size of the load applied by a single structure to the plate frame structure is unclear, it is a boundary problem. In the boundary problem, the single structure is used as a boundary condition to calculate the structural response of the plate frame structure under other loads.

[0012] S7: Calculation of plate frame structure strength;

[0013] In the case of a load problem, a rigid plane is established at one end of the columnar unit away from the plate frame structure. The elastic modulus of the rigid plane material is set to be much larger than the elastic modulus of the plate frame structure. Then, a uniformly distributed load is applied to the rigid plane according to the actual load size to calculate the structural strength of the plate frame structure.

[0014] In the case of boundary problems, boundary conditions are set or actual models are established at the end of the column element away from the plate frame structure as a prerequisite for calculations in other areas.

[0015] Optionally, in step S1, when the plate frame structure is located in a local structure, the finite element calculation model takes the complete model of the local structure, and the local structure includes the mid-assembly, large assembly, and sections of the hull; when the plate frame structure is located in a complete structure, partial blocks of the complete structure are selected as the finite element calculation model according to preset rules, and the complete structure includes the hull section and the entire ship.

[0016] Optionally, when the panel frame structure is in a complete structure, the preset rule for selecting the finite element calculation model is:

[0017] In the length direction of the hull, based on the contact area between the plate frame structure and the single structure, the distance extending from the bow and stern is at least two strong frames in the longitudinal direction of the hull;

[0018] In the width direction of the hull, if the contact area is only on one side of the hull, half the hull width is taken; if the contact area spans the mid-longitudinal section, the full hull width is taken;

[0019] In the hull height direction, take the full height.

[0020] Optionally, in step S2, the coarse grid size is one longitudinal bone spacing.

[0021] Optionally, in step S3, the size of the refined grid is 50*50 mm.

[0022] Optionally, the columnar unit includes a spring unit or a beam unit.

[0023] Optionally, when a spring unit is used, the stiffness coefficient k of the spring unit is determined by the following formula: k = EA / L;

[0024] Where: E is the elastic modulus of a single structure; A is the area covered by a single spring unit; L is the length of the spring unit;

[0025] When beam elements are used, the cross section of the beam element is set to a rectangle with the same size as the refined mesh, and the material parameters are consistent with the actual material parameters of the single structure.

[0026] Optionally, the plate frame structure is a support frame installed in the side area of ​​the ship, and the single structure is a floating ball located between the support frame and the dock.

[0027] As described above, the present invention provides a finite element analysis method for the contact between a plate frame structure and a single structure. The finite element analysis method first divides the contact area between the plate frame structure and the single structure into grids, and then stretches each grid of the plate frame structure located in the contact area in a direction away from the plate frame structure to form a columnar unit, that is, the single structure is discretized into a plurality of columnar units, the columnar unit is a spring unit or a beam unit, and finally a load is applied to one end of the columnar unit away from the plate frame structure to obtain the structural response of the plate frame structure under the load. By discretizing the single structure into spring units or beam units, the present invention can effectively simulate the situation where different regions of the plate frame structure have different contact stiffness with a single structure while still using static analysis, thereby improving the accuracy of local structure simulation and providing strong technical support for actual production and construction. BRIEF DESCRIPTION OF THE DRAWINGS

[0028] Figure 1 It is a schematic diagram of the structural arrangement of the first embodiment of the present invention.

[0029] Figure 2 This is a simplified diagram of the structural contacts of the first embodiment of the present invention.

[0030] Figure 3 This is a model load boundary diagram of the first embodiment of the present invention.

[0031] Component number description

[0032] 1-hull outer plate; 2-support frame; 3-support frame end face; 4-buoy; 5-dock; 6-beam unit; 7-rigid plane; 8-horizontal average force; 9-boundary fixed constraint. DETAILED DESCRIPTION

[0033] The following describes the embodiments of the present invention through specific examples, and those skilled in the art can easily understand other advantages and effects of the present invention from the contents disclosed in this specification. The present invention can also be implemented or applied through other different specific embodiments, and the details in this specification can also be modified or changed in various ways based on different viewpoints and applications without departing from the spirit of the present invention.

[0034] It should be noted that the illustrations provided in this embodiment are only used to illustrate the basic concept of the present invention in a schematic manner, and therefore the illustrations only show components related to the present invention rather than being drawn according to the number, shape and size of components in actual implementation. In actual implementation, the type, quantity and proportion of each component may be changed arbitrarily, and the component layout may also be more complicated.

[0035] In view of the above shortcomings in the prior art, the present invention simulates the contact between the plate frame structure and the single structure by using the spring unit / beam unit commonly used in finite element analysis and an assumed rigid plane. This not only avoids the computing power limitation brought by contact calculation analysis, but also can more accurately simulate the local response of the structural contact area.

[0036] The present invention provides a finite element analysis method applicable to the contact problem between a plate frame structure and a single structure, comprising the following steps:

[0037] S1: Determine the scope of the finite element calculation model

[0038] When the object to be calculated (plate frame structure) is located in the local structure, the local structure includes: mid-hull assembly, large assembly, section, etc., the finite element calculation model takes the complete model of the local structure;

[0039] When the object to be calculated (plate frame structure) is located in a complete structure, the complete structure includes: hull section, whole ship, etc., the finite element calculation model takes the local model of the complete structure according to the following rules:

[0040] In the length direction of the hull, based on the contact area between the plate frame structure and the single structure, the bow and stern extend at least the distance of two strong frames along the longitudinal direction of the hull.

[0041] In the width direction of the hull, if the contact area is only on one side of the hull, half the hull width can be taken. If the contact area spans the mid-longitudinal section, the full hull width can be taken.

[0042] In the hull height direction, take the full height.

[0043] S2: Divide the finite element calculation model into a coarse grid

[0044] The coarse mesh model of the finite element calculation model is established using 3D modeling software. The coarse mesh size is set to a longitudinal bone spacing.

[0045] S3: Mesh refinement of the plate-frame structure in the contact area

[0046] According to the actual size of the structure and the calculation verification requirements, the coarse grid of the plate frame structure in the contact area is refined to form a fine grid. As a preferred embodiment, the size of the fine grid can be 50*50mm.

[0047] S4: The single structure is discretized into cylindrical elements, including spring elements or beam elements.

[0048] Each refined grid of the plate-frame structure in the contact area is stretched in a direction away from the plate-frame structure to form a columnar unit (the columnar unit is a spring unit or a one-dimensional beam unit). The columnar unit is perpendicular to the plate plane of the plate-frame structure in the contact area, and the unit length of the columnar unit is the thickness of the single structure.

[0049] The selection of spring element and one-dimensional beam element has no obvious effect on the results, and both can be used as equivalent replacement solutions.

[0050] S5: Parameter determination of columnar elements

[0051] When a spring unit is used, the stiffness coefficient k of the spring unit is determined by the following formula:

[0052] k=EA / L

[0053] Where: E——Elastic modulus of a single structure

[0054] A——Area covered by a single spring unit

[0055] L - length of the spring unit

[0056] When beam elements are used, the cross section of the beam element is set to a rectangle that is basically the same as the fine grid size, and the material parameters are consistent with those of the actual structure.

[0057] S6: Determine the type of contact problem

[0058] According to the difference in positioning of single structure in structural contact problem, the finite element calculation of hull plate structure strength can be divided into load problem and boundary problem.

[0059] When a single structure actively applies a known load to the plate frame structure or needs to analyze the effect of the load on the result, it is a load problem, such as placing a heavy object on the deck. The load problem is to regard the effect of the single structure on the hull as a load and calculate the structural response of the hull structure under the action of the single structure.

[0060] When the magnitude of the load applied by a single structure to the plate frame structure is unclear, it is a boundary problem, such as the hull docking analysis. The boundary problem is to regard the single structure as the boundary as a known prerequisite before the load calculation, and calculate the structural response of the hull structure under the action of other loads.

[0061] S7: Contact problem handling

[0062] In the case of load problems, a rigid plane is established at one end of the columnar unit away from the plate frame structure. The elastic modulus of the rigid plane material is set to be much larger than the elastic modulus of the plate frame structure (hull structure). In simulation calculations, the elastic modulus of the rigid plane is at least 100 times or 1000 times that of the plate frame structure material. Then, a uniform load is applied to the rigid plane according to the actual load size.

[0063] In the case of boundary problems, boundary conditions are set or an actual model is established at the end of the columnar unit away from the frame structure according to actual conditions. If the end of the columnar unit away from the frame structure is the ground or a structure unrelated to the calculation, it is sufficient to set the boundary conditions. If the other end is a structure related to the calculation, an actual model should be established.

[0064] The above process is specifically introduced below through embodiments.

[0065] Embodiment 1

[0066] like Figures 1 to 3 As shown, a support frame 2 is installed on the side area of ​​the ship, and a buoy 4 with a diameter of about 2m is placed between the support frame 2 and the dock 5 as a buffer. The end face of the support frame 2 is a plate frame structure, and the buoy 4 is a single structure. The contact between the two meets the application scenario of the present invention, so the finite element analysis method is used to calculate how much thrust the support frame can withstand. The specific process includes:

[0067] The longitudinal length of the connection area between the support frame 2 and the hull is 15 ribs. Along the longitudinal direction of the hull, at least two strong frames extend from the bow and stern respectively. The longitudinal length of the final model is 31 ribs; the width direction is half the ship; the height direction is the full height of the hull.

[0068] The coarse mesh model was established using CATIA and FASTTRACK finite element modeling software.

[0069] The mesh of the support frame end face and the connection area between the support frame and the hull is refined, and the refined mesh size is about 50*50mm.

[0070] like Figure 2As shown, the float 4 is discretized into beam elements 6. In actual contact, the float 4 is squeezed and deformed, and the contact area with the end face of the support frame is a circle with a diameter of about 1m. Take the contact area with a diameter of 1m, and stretch each refined grid in the contact area in the direction away from the support frame to form a beam element 6 with a length of 2m, so as to simulate the actual float with the beam element 6. The cross-section of a single beam element 6 is a rectangle of 50*50mm, and the material parameters are consistent with the material parameters of the actual float.

[0071] like Figure 3 As shown, this embodiment needs to analyze how much thrust the support frame 2 can withstand, which is a load problem. Therefore, the effect of the float 4 on the support frame 2 is regarded as load application. A rigid plane 7 is established at the other end of the beam unit 6, and a horizontal uniform force is applied to the left. The value of the applied uniform force is gradually increased, thereby obtaining the bearing limit of the support frame.

[0072] The finite element calculation adopts a half-ship model and applies boundary fixed constraints at the midship section9.

[0073] The significant effects of this embodiment are: the interaction between the buoy and the support frame is reasonably simplified, and by adjusting the size of the horizontally distributed load, the maximum value of the dock reaction force can be quickly calculated while ensuring the safety of the structure, providing a reference basis for on-site construction.

[0074] In summary, the present invention provides a finite element analysis method for the contact between a plate frame structure and a single structure. The finite element analysis method first divides the contact area between the plate frame structure and the single structure into grids, and then stretches each grid of the plate frame structure located in the contact area in a direction away from the plate frame structure to form a columnar unit, that is, the single structure is discretized into a plurality of columnar units, the columnar unit is a spring unit or a beam unit, and finally a load is applied to one end of the columnar unit away from the plate frame structure to obtain the structural response of the plate frame structure under the load. By discretizing the single structure into spring units or beam units, the present invention can effectively simulate the situation where different areas of the plate frame structure have different contact stiffness with a single structure while still using static analysis, thereby improving the accuracy of local structure simulation and providing strong technical support for actual production and construction.

[0075] The above embodiments are merely illustrative of the principles and effects of the present invention, and are not intended to limit the present invention. Anyone familiar with the art may modify or alter the above embodiments without departing from the spirit and scope of the present invention. Therefore, all equivalent modifications or alterations made by a person of ordinary skill in the art without departing from the spirit and technical concept disclosed by the present invention shall still be covered by the claims of the present invention.

Claims

1. A finite element analysis method suitable for the contact problem between a plate frame structure and a single structure, characterized in that: The steps include: S1: According to the location of the plate frame structure, the scope of the finite element calculation model is determined, and the finite element calculation model is a hull model including the plate frame structure; S2: Divide the finite element calculation model into a coarse grid, and use 3D modeling software to establish a coarse grid model of the finite element calculation model; S3: Refine the coarse grid in the contact area between the plate frame structure and the single structure to form a refined grid; S4: discretizing the single structure into a plurality of columnar units, stretching each refined grid of the plate-frame structure located in the contact area in a direction away from the plate-frame structure to form a columnar unit, wherein the columnar unit is perpendicular to the plate-shaped plane of the plate-frame structure located in the contact area, and the unit length of the columnar unit is the thickness of the single structure; S5: Determine the material parameters of the columnar unit according to the actual material parameters of the single structure; S6: Determine the type of contact problem and divide the finite element calculation of the plate frame structure strength into a load problem and a boundary problem; When a single structure actively applies a known load to a plate-frame structure or needs to analyze the effect of the load on the result, it is a load problem. When the load applied by a single structure to a plate-frame structure is unclear, it is a boundary problem. In the boundary problem, the single structure is used as a boundary condition to calculate the structural response of the plate-frame structure under other loads. S7: Calculation of plate frame structure strength; In the case of a load problem, a rigid plane is established at one end of the columnar unit away from the plate frame structure. The elastic modulus of the rigid plane material is set to be much larger than the elastic modulus of the plate frame structure. Then, a uniformly distributed load is applied to the rigid plane according to the actual load size to calculate the structural strength of the plate frame structure. In the case of boundary problems, boundary conditions are set or actual models are established at the end of the column element away from the plate frame structure as a prerequisite for calculations in other areas.

2. The finite element analysis method according to claim 1, characterized in that: In step S1, when the plate frame structure is located in a local structure, the finite element calculation model takes the complete model of the local structure, and the local structure includes the mid-assembly, large assembly, and sections of the hull; when the plate frame structure is located in a complete structure, partial blocks of the complete structure are selected as the finite element calculation model according to preset rules, and the complete structure includes the hull section and the entire ship.

3. The finite element analysis method according to claim 2, characterized in that: When the plate frame structure is in the complete structure, the default rule for selecting the finite element calculation model is: In the length direction of the hull, based on the contact area between the plate frame structure and the single structure, the distance extending from the bow and stern is at least two strong frames in the longitudinal direction of the hull; In the width direction of the hull, if the contact area is only on one side of the hull, half the hull width is taken; if the contact area spans the mid-longitudinal section, the full hull width is taken; In the hull height direction, take the full height.

4. The finite element analysis method according to claim 1, characterized in that: In step S2, the coarse grid size is one longitudinal bone spacing.

5. The finite element analysis method according to claim 1, characterized in that: In step S3, the size of the refined grid is 50*50 mm.

6. The finite element analysis method according to claim 1, characterized in that: The columnar unit includes a spring unit or a beam unit.

7. The finite element analysis method according to claim 6, characterized in that: When a spring unit is used, the stiffness coefficient k of the spring unit is determined by the following formula: k = EA / L; Where: E is the elastic modulus of a single structure; A is the area covered by a single spring unit; L is the length of the spring unit; When beam elements are used, the cross section of the beam element is set to a rectangle with the same size as the refined mesh, and the material parameters are consistent with the actual material parameters of the single structure.

8. The finite element analysis method according to claim 1, characterized in that: The plate frame structure is a support frame installed in the side area of ​​the ship, and the single structure is a floating ball located between the support frame and the dock.

Images