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

Abstract

The application provides a finite element analysis method for contact between a panel structure and a single structure. The method comprises the following steps: dividing a contact area between the panel structure and the single structure into grids; stretching each grid of the panel structure in the contact area into a columnar unit away from the panel structure, that is, discretizing the single structure into a plurality of columnar units; the columnar unit is a spring unit or a beam unit; and finally, applying a load to one end of the columnar unit away from the panel structure to obtain a structural response of the panel structure under the load. By discretizing the single structure into a spring unit or a beam unit, the application can effectively simulate the case that different regions of the panel structure contact different single structures with different stiffnesses under the premise of still using statics analysis, improves the accuracy of local structure simulation, and provides strong technical support for actual production and construction.

Description

TECHNICAL FIELD

[0001] The present application relates to the field of shipbuilding technology, in particular to a finite element analysis method for contact between a grillage structure and a single structure. BACKGROUND

[0002] The grillage structure refers to a steel structure composed of plates, and longitudinal and transverse intersecting bars and stringers, and is widely used in the field of shipbuilding. With the continuous development of the shipbuilding industry, ship structure design is becoming 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 be used to calculate various aspects of ship structure, such as static strength analysis, dynamics analysis, fatigue analysis, and thermodynamics analysis, among which static strength analysis is the most common. In ship static strength analysis, the contact problem between the grillage structure and the single structure is involved in many aspects, such as the contact between the ship hull plate and the dock pier when the ship is docked, the distributed load applied to the grillage through the single structure, and the contact between the ship hull plate and the dock cushion layer when the ship is berthed.

[0003] Currently, the common way to deal with the contact problem between the grillage structure and the single structure is to simplify the single structure as RBE binding or uniform load. This technical means can meet the calculation requirements of 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 the oversimplification of the contact between the structures. Another technical means is to use contact calculation analysis method to simulate the real structure contact situation, which is accurate but requires high computing power and is difficult to adapt to the rapid calculation of large-scale structures. SUMMARY

[0004] In view of the above-mentioned deficiencies in the prior art, the present application simulates the contact between the grillage structure and the single structure by using the commonly used spring element / beam element and a hypothetical rigid plane in finite element analysis. This avoids the computing power limitation brought by the contact calculation analysis, and can accurately simulate the local response of the structure contact area.

[0005] To achieve the above-mentioned purposes and other related purposes, the present application provides a finite element analysis method suitable for the contact problem between the grillage structure and the single structure, comprising the following steps:

[0006] S1: determining the range of the finite element calculation model according to the position of the grillage structure, the finite element calculation model being a ship model including the grillage structure;

[0007] S2: dividing the finite element calculation model into coarse meshes, and establishing a coarse mesh model of the finite element calculation model by using a three-dimensional modeling software;

[0008] S3: refining the coarse meshes of the contact area between the grillage structure and the single structure to form refined meshes;

[0009] S4: Discretize the single structure into a plurality of columnar units, stretch the refined grid of the plate structure at the contact area towards the direction away from the plate structure to form columnar units, the columnar units are perpendicular to the plate plane of the plate structure at the contact area, and the unit length of the columnar units is the thickness of the single structure;

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

[0011] S6: Determine the type of the contact problem, and divide the plate structure strength finite element calculation into a load problem and a boundary problem; when the single structure actively applies a known size of load to the plate structure or the influence of the load size on the result needs to be analyzed, it belongs to the load problem; when the size of the load applied by the single structure to the plate structure is unknown, it belongs to the boundary problem, and the single structure is taken as a boundary condition to calculate the structural response of the plate structure under the action of other loads;

[0012] S7: Plate structure strength calculation;

[0013] In the case of the load problem, a rigid plane is established at the end of the columnar unit away from the plate structure, the elastic modulus of the material of the rigid plane is set to be much larger than the elastic modulus of the plate structure, and a uniform load is applied on the rigid plane according to the actual load size, and the structural strength of the plate structure is calculated;

[0014] In the case of the boundary problem, the boundary condition is set at the end of the columnar unit away from the plate structure or the actual model is established as the prerequisite condition for calculation of other regions.

[0015] Optionally, in step S1, when the plate 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 hull assembly, large assembly and section; when the plate structure is located in a complete structure, a part of the complete structure is selected as the finite element calculation model according to a preset rule, and the complete structure includes a total section of the hull and a whole ship.

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

[0017] In the length direction of the hull, the contact area between the plate structure and the single structure is taken as the benchmark, and the plate structure is extended at least two distances of the strong frame along the longitudinal direction of the hull bow and stern;

[0018] In the width direction of the hull, if the contact area is located on one side of the hull, the half width of the hull is taken, and if the contact area crosses the centerplane, the full width of the hull is taken;

[0019] In the height direction of the hull, the complete height is taken.

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

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

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

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

[0024] In the formula, E is the elastic modulus of the single structure, A is the area covered by the single spring unit, and L is the length of the spring unit.

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

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

[0027] As described above, the present application provides a finite element analysis method for the contact between a panel structure and a single structure, which comprises the following steps: first, dividing the contact area between the panel structure and the single structure into a grid; then, stretching out columnar units from each grid of the panel structure in the contact area in a direction away from the panel structure, that is, discretizing the single structure into a plurality of columnar units, the columnar units being spring units or beam units; finally, applying a load to one end of the columnar units away from the panel structure to obtain the structural response of the panel structure under the load. By discretizing the single structure into spring units or beam units, the present application can effectively simulate the case that different regions of the panel structure contact different single structures with different stiffnesses under the premise of still using static analysis, thereby improving the accuracy of the simulation of the local structure and providing strong technical support for actual production and construction. BRIEF DESCRIPTION OF DRAWINGS

[0028] Fig. 1 It is a structural arrangement schematic diagram of the embodiment one of the present application.

[0029] Fig. 2 It is a structural contact simplified diagram of the embodiment one of the present application.

[0030] Fig. 3 It is a model load boundary diagram of the embodiment one of the present application.

[0031] ELEMENT NUMBER EXPLANATION

[0032] 1-ship outer plate; 2-support frame; 3-support frame end face; 4-floating ball; 5-dock shore; 6-beam unit; 7-rigid plane; 8-hydrostatic force; 9-boundary fixed constraint. Detailed Implementation

[0033] The following specific examples illustrate the implementation of the present invention. Those skilled in the art can easily understand other advantages and effects of the present invention from the content disclosed in this specification. The present invention can also be implemented or applied through other different specific embodiments, and various details in this specification can also be modified or changed 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 schematic representations of the basic concept of the present invention. Therefore, the illustrations only show the components related to the present invention and are not drawn according to the actual number, shape and size of the components in the actual implementation. In the actual implementation, the form, quantity and proportion of each component can be arbitrarily changed, and the layout of the components may also be more complex.

[0035] To address the shortcomings of the existing technologies, this invention uses spring / beam elements, commonly used in finite element analysis, and an assumed rigid plane to simulate the contact between a plate frame structure and a single structure. This avoids the computational limitations of contact analysis while accurately simulating the local response of the structural contact area.

[0036] This invention provides a finite element analysis method applicable to contact problems between plate-frame structures and single structures, 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 a local structure, the local structure includes: hull assembly, large assembly, segment, etc., and 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 within a complete structure, the complete structure includes: hull sections, the entire ship, etc. The finite element calculation model takes a local model of the complete structure according to the following rules:

[0040] Along the length of the hull, based on the contact area between the plate frame structure and the single structure, at least two strong frames extend longitudinally from the bow and stern.

[0041] In the hull width direction, if the contact area is only located 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 should be taken.

[0042] The height of the hull is taken as the complete height.

[0043] S2: Apply a coarse mesh to the finite element calculation model.

[0044] A coarse mesh model of the finite element calculation model is established by using a three-dimensional modeling software. The coarse mesh size is taken as an interval between longitudinal bones.

[0045] S3: contact area frame structure mesh refinement

[0046] The coarse mesh of the contact area frame structure is refined according to the actual size of the structure and the calculation checking requirements, and the refined mesh is formed. As a preferred embodiment, the size of the refined mesh can be 50*50mm.

[0047] S4: single structure is discretized into columnar units, including spring units or beam units.

[0048] The refined mesh of the frame structure in the contact area is stretched out of the columnar unit (the columnar unit is the spring unit or the one-dimensional beam unit) away from the frame structure, the columnar unit is perpendicular to the plate plane of the 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 units and one-dimensional beam units has no obvious influence on the result, and they can be used as equivalent alternative solutions.

[0050] S5: parameter determination of columnar unit

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

[0052] k=EA / L

[0053] In the formula: E——elastic modulus of single structure

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

[0055] L——length of spring unit

[0056] When the beam unit is used, the beam unit section is set to be a rectangle with a size basically same as the fine mesh size, and the material parameters are consistent with the material parameters of the actual structure.

[0057] S6: determine the type of contact problem

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

[0059] When the single structure actively applies a known size of load to the frame structure or the influence of the load size on the result needs to be analyzed, it belongs to the load problem, such as placing a heavy object on the deck; the load problem regards the action of the single structure on the ship body as a load, and calculates the structural response of the ship body structure under the action of the single structure;

[0060] When the magnitude of the load applied by a single structure to a plate frame structure is unknown, it falls under the category of boundary problems, such as ship docking analysis. Boundary problems refer to treating the single structure as a boundary, using it as a known prerequisite before load calculation, and calculating the structural response of the hull structure under other loads.

[0061] S7: Contact Issue Handling

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

[0063] In the case of boundary problems, set boundary conditions or build an actual model at the end of the column element that is away from the plate structure, depending on the actual situation. If the end of the column element that is away from the plate structure is the ground or a structure that is not related to the calculation, then setting boundary conditions is sufficient. If the other end is a structure that is related to the calculation, then an actual model should be built.

[0064] The above process will be described in detail below through examples.

[0065] Example 1

[0066] like Figs. 1 to 3 As shown, a support frame 2 is installed on the side of the ship. A buoy 4 with a diameter of approximately 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, while the buoy 4 is a single structure. The contact between the two conforms to the application scenario of this invention, thereby allowing the finite element analysis method to calculate the maximum thrust that the support frame can withstand. The specific process includes:

[0067] The longitudinal length of the support frame 2 connecting to the hull is 15 ribs. Along the longitudinal direction of the hull, at least two strong frames extend from the bow and stern, resulting in a final model with a longitudinal length of 31 ribs. The width of the ship is half the ship's width, and the height is the full height of the hull.

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

[0069] The grid on the end face of the support frame and the area where the support frame connects to the hull is refined, with a grid size of approximately 50*50mm.

[0070] like Fig. 2As shown, the floating ball 4 is discretized into beam elements 6. In actual contact, the floating ball 4 is extruded and deformed, and the contact area with the end surface of the support frame is a circular area with a diameter of about 1 m. Taking the contact area with a diameter of 1 m, each refined grid in the contact area is stretched into a beam element 6 with a length of 2 m away from the support frame, so as to simulate the actual floating ball with the beam element 6. The cross section of a single beam element 6 is a rectangle with a size of 50*50 mm, and the material parameters are consistent with those of the actual floating ball.

[0071] As shown, the embodiment needs to analyze how large the thrust force that the support frame 2 can bear is, which belongs to the load problem, so the action of the floating ball 4 on the support frame 2 is regarded as load application, a rigid plane 7 is established at the other end of the beam element 6, and a uniformly distributed force is applied horizontally to the left, and the value of the applied uniformly distributed force is gradually increased, so as to obtain the maximum value of the support frame. Fig. 3

[0072] The finite element calculation adopts a half-ship model, and a boundary fixed constraint 9 is applied at the ship section.

[0073] The significant effect of the embodiment is that the interaction between the floating ball and the support frame is reasonably simplified, and by adjusting the size of the horizontal uniformly distributed load, the maximum value of the dock shore reaction force can be quickly calculated under the premise of ensuring the safety of the structure, thereby providing a reference basis for the on-site construction.

[0074] In summary, the present application provides a finite element analysis method for the contact between a plate frame structure and a single structure, which first divides the contact area between the plate frame structure and the single structure into grids, then stretches each grid of the plate frame structure in the contact area away from the plate frame structure into a columnar element, that is, discretizes the single structure into a plurality of columnar elements, the columnar elements are spring elements or beam elements, and finally applies a load at one end of the columnar element away from the plate frame structure to obtain the structural response of the plate frame structure under the action of the load. By discretizing the single structure into spring elements or beam elements, the present application can effectively simulate the case that different regions of the plate frame structure contact different single structures with different contact stiffnesses under the premise of still using statics analysis, thereby improving the accuracy of local structure simulation and providing strong technical support for actual production and construction.

[0075] The above embodiments only exemplarily illustrate the principles and effects of the present application, but are not used to limit the present application. Any person skilled in the art can modify or change the above embodiments without departing from the spirit and scope of the present application. Therefore, all equivalent modifications or changes completed by those skilled in the art without departing from the spirit and technical thought disclosed by the present application should be covered by the claims of the present application.​

Claims

1. A finite element analysis method for a grillage structure and a single structure contact problem, characterized by, The method comprises the following steps: S1: determining the range of a finite element calculation model according to the location of the grillage structure, the finite element calculation model being a hull model including the grillage structure; S2: dividing the finite element calculation model into coarse meshes, and establishing a coarse mesh model of the finite element calculation model by using a three-dimensional modeling software; S3: refining the coarse meshes of the contact area between the grillage structure and the single structure to form refined meshes; S4: discretizing the single structure into a plurality of columnar units, and stretching each refined mesh of the grillage structure in the contact area in a direction away from the grillage structure to form a columnar unit, the columnar unit being perpendicular to the plate plane of the grillage structure in the contact area, and the unit length of the columnar unit being the thickness of the single structure; S5: determining the material parameters of the columnar unit according to the actual material parameters of the single structure; S6: determining the type of the contact problem, and dividing the grillage structure strength finite element calculation into a load problem and a boundary problem; the load problem refers to a case where the single structure actively applies a load with a known size to the grillage structure or the influence of the load size on the result needs to be analyzed; and the boundary problem refers to a case where the size of the load applied by the single structure to the grillage structure is unknown, in which case the single structure is taken as a boundary condition to calculate the structural response of the grillage structure under the action of other loads; S7: grillage structure strength calculation; in the case of the load problem, a rigid plane is established at the end of the columnar unit away from the grillage structure, the elastic modulus of the material of the rigid plane is set to be much greater than the elastic modulus of the grillage structure, and a uniform load is applied on the rigid plane according to the actual load size to calculate the structural strength of the grillage structure; in the case of the boundary problem, a boundary condition is set at the end of the columnar unit away from the grillage structure or an actual model is established as a prerequisite condition for calculation of other areas.

2. The finite element analysis method of claim 1, wherein: In step S1, when the grillage 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 a sub-assembly, a large sub-assembly, and a section; and when the grillage structure is located in a complete structure, a part of the complete structure is selected as the finite element calculation model according to a preset rule, and the complete structure includes a total section of a hull and a whole ship.

3. The finite element analysis method of claim 2, wherein: When the grillage structure is located in a complete structure, the preset rule for selecting the finite element calculation model is as follows: in the hull length direction, the contact area between the grillage structure and the single structure is taken as a benchmark, and at least two strong frames are extended in the hull longitudinal direction bow and stern; in the hull width direction, if the contact area is located on one side of the hull, the half width of the hull is taken, and if the contact area crosses the centerplane, the full width of the hull is taken; in the hull height direction, the complete height is taken.

4. The finite element analysis method of claim 1, wherein: In step S2, the size of the coarse mesh is one longitudinal spacing.

5. The finite element analysis method of claim 1, wherein: In step S3, the size of the refined mesh is 50*50 mm.

6. The finite element analysis method of claim 1, wherein: The columnar unit includes a spring unit or a beam unit.

7. The finite element analysis method of claim 6, wherein: When the spring unit is adopted, the stiffness coefficient k of the spring unit is determined according to the following formula: k=EA / L; in the formula, E is the elastic modulus of the single structure, A is the area covered by a single spring unit, and L is the length of the spring unit; when the beam unit is adopted, the cross section of the beam unit is set to be 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 of claim 1, wherein: The panel structure is a support frame installed in the side area of the ship, and the single structure is a floating ball between the support frame and the dock shore.

Images