Pipe bending strength simulation analysis method based on interference assembly

Abstract

The application relates to a pipe bending strength simulation analysis method based on interference assembly, which comprises the following steps: S1, establishing a finite element model of a pipe to be processed; S2, giving material properties and section attributes, and establishing a displacement constraint application point; S3, setting all contact relations except an overlapping area between an elastic block and an outer pipe, applying a pressure load on the upper surface of the elastic block, making the overlapping area between the elastic block and the outer pipe less than a preset overlapping area threshold, applying a fixed constraint at one end of the outer pipe, and applying a displacement constraint at the displacement constraint application point; S4, setting the contact relation between the elastic block and the outer pipe, performing pre-compression calculation, and eliminating the pressure load on the elastic block; and S5, controlling the displacement constraint at one end of an inner pipe, and obtaining the pipe bending strength. The application can avoid finite element calculation non-convergence in the simulation calculation process of the pipe bending strength of the elastic block large deformation interference assembly, and improves the calculation convergence and calculation efficiency of the pipe bending strength simulation analysis.

Description

TECHNICAL FIELD

[0001] The present application relates to the technical field of pipeline bending strength simulation analysis, and particularly relates to a pipeline bending strength simulation analysis method based on interference assembly. BACKGROUND

[0002] In order to achieve better fixing effect in pipeline assembly, elastic blocks (such as rubber blocks) are often installed in the form of interference assembly, and the elastic blocks in interference assembly often have large deformation. In finite element analysis, the meshes of the two parts before interference assembly are a small amount of superimposed together, and automatic pre-tightening can be realized during calculation. After automatic pre-tightening, the superimposed meshes are separated. However, when the interference amount is large, the amount of superimposed meshes is large, and automatic pre-tightening is difficult to realize, resulting in that the finite element calculation does not converge, and therefore the pipeline bending strength based on interference assembly cannot be accurately and quickly analyzed through finite element calculation. Therefore, how to solve the problem of finite element calculation not converging in the simulation calculation process of the pipeline bending strength of the elastic block with large deformation in interference assembly, and accurately and quickly analyze the pipeline bending strength of the elastic block with large deformation in interference assembly become technical problems to be solved. SUMMARY

[0003] The present application aims to provide a pipeline bending strength simulation analysis method based on interference assembly, which can solve the technical problem of calculation not converging of the elastic block with large deformation in interference assembly when the pipeline is bent, thereby improving the calculation convergence and calculation efficiency of the pipeline bending strength simulation analysis of the elastic block with large deformation in interference assembly.

[0004] According to the first aspect of the present application, a pipeline bending strength simulation analysis method based on interference assembly is provided, comprising:

[0005] Step S1, establishing a to-be-processed pipeline finite element model according to a pipeline structure, the pipeline structure comprising an outer pipe, an inner pipe, a steel hoop and an elastic block located between the connection position of the inner pipe and the outer pipe, and the deformation amount of the elastic block being greater than a preset deformation threshold when the pipeline structure is subjected to interference assembly;

[0006] Step S2, giving the to-be-processed pipeline finite element model material properties and cross-section properties, and establishing a displacement constraint application point at one end of the inner pipe;

[0007] Step S3, in a preset first analysis step, setting all contact relationships except the overlapping area between the elastic block and the outer pipe, applying a pressure load on the upper surface of the elastic block, the pressure direction pointing to the inner side of the rubber, so that the overlapping area between the elastic block and the outer pipe is less than a preset overlapping area threshold, applying a fixed constraint at one end of the outer pipe, applying a displacement constraint at the displacement constraint application point, and the displacement amount of the six degrees of freedom is 0;

[0008] Step S4, in the preset second analysis step, the contact relationship between the elastic block and the outer tube is set, the pre-compression calculation is carried out based on the current overlapping area between the elastic block and the outer tube, and then the pressure load applied to the upper surface of the elastic block is eliminated;

[0009] Step S5, in the preset third analysis step, the displacement constraint applied to one end of the inner tube is controlled, the one end of the inner tube is bent to a target displacement along a direction perpendicular to the axial direction of the inner tube, and the bending strength of the pipeline structure is obtained.

[0010] Compared with the prior art, the application has obvious advantages and beneficial effects. By the above technical scheme, the pipeline bending strength simulation analysis method based on interference assembly provided by the application can achieve considerable technical progress and practicality, and has wide industrial utilization value, and at least has the following advantages:

[0011] The application adopts the mode of applying compression load and elastic block contact relationship in multiple analysis steps to solve the problem of non-convergence of finite element calculation of large deformation interference assembly of rubber blocks in pipeline simulation, thereby improving the calculation convergence and calculation efficiency of the pipeline bending strength simulation analysis of large deformation interference assembly of elastic blocks.

[0012] The above description is only a summary of the technical scheme of the application, in order to more clearly understand the technical means of the application, the content of the specification can be implemented, and in order to make the above and other purposes, characteristics and advantages of the application more obvious and easy to understand, the following preferred embodiments are described in detail, and the accompanying drawings are described as follows. BRIEF DESCRIPTION OF DRAWINGS

[0013] Figure 1 The pipeline bending strength simulation analysis method based on interference assembly provided by the embodiment of the application is shown in the flowchart.

[0014] Figure 2 The pipeline structure schematic diagram provided by the embodiment of the application is shown in the flowchart.

[0015] Figure 3 The pipeline structure cross-section schematic diagram provided by the embodiment of the application is shown in the flowchart.

[0016] Figure 4 The elastic block and the outer tube overlapping area schematic diagram provided by the embodiment of the application is shown in the flowchart.

[0017] Figure 5 The elastic block upper surface pressure load application schematic diagram provided by the embodiment of the application is shown in the flowchart.

[0018] Figure 6 The load and boundary condition parameter setting schematic diagram in the first analysis step provided by the embodiment of the application is shown in the flowchart.

[0019] Figure 7A second analysis step pressure load elimination parameter setting schematic diagram provided for the embodiment of the present application is shown in the figure;

[0020] Figure 8 A maximum analysis step parameter setting schematic diagram provided for the second analysis step of the embodiment of the present application is shown in the figure;

[0021] Figure 9 A quality scaling multiple parameter setting schematic diagram provided for the second analysis step of the embodiment of the present application is shown in the figure;

[0022] Figure 10 A displacement constraint concentrated force load elimination parameter setting schematic diagram provided for the third analysis step of the embodiment of the present application is shown in the figure. DETAILED DESCRIPTION

[0023] In order to further illustrate the technical means and effects adopted by the present application to achieve the predetermined inventive purpose, the specific implementation and effects of the pipe bending resistance strength simulation analysis method based on interference assembly according to the present application are described in detail as follows in combination with the accompanying drawings and preferred embodiments.

[0024] The embodiment of the present application provides a pipe bending resistance strength simulation analysis method based on interference assembly, as shown in the figure, which comprises the following steps. Figure 1

[0025] Step S1, a pipe finite element model to be processed is established according to a pipe structure, the pipe structure comprising an outer pipe, an inner pipe, and a steel hoop and an elastic block located between the connection positions of the inner pipe and the outer pipe, as shown in the figures. Figure 2 Figure 3 When the pipe structure is subjected to interference assembly, the deformation amount of the elastic block is greater than a preset deformation threshold value.

[0026] When the deformation amount of the elastic block is greater than the preset deformation threshold value, it belongs to large deformation interference assembly, and direct use of existing finite element calculation will cause non-convergence. The preset deformation threshold value refers to the deformation threshold value that allows the calculation to converge. As an example, the preset deformation threshold value can be set to 5%. As an embodiment, the pipe structure can be a self-anchored pipe, and the elastic block can be a rubber block.

[0027] As an embodiment, the step S1 comprises the following steps.

[0028] Step S11, a pipe digital model is established, the elastic block is in an undeformed assembly state, and the elastic block and the outer pipe have an overlapping area.

[0029] ​​The pipe digital model can be established by using CAD modeling software such as Solidworks or UG. As an example, the pipe digital model has the same size as the pipe structure. The pipe digital model includes pipe chamfers, round corners and other features. At this time, the elastic block is in an undeformed assembly, and thus the elastic block has an overlapping area with the outer pipe, as shown in Figure 4

[0030] Step S12: outputting the pipe digital model as a first target file that can be recognized by a preset meshing software, and importing the first target file into the meshing software to perform surface meshing and volume meshing;

[0031] If the CAD software is used to establish the pipe digital model, the first target file can be an x_t file. The meshing software can be Hypermesh.

[0032] As an example, before the meshing and volume meshing in step S12, the step S12 further includes:

[0033] Step S121: first suppressing the redundant lines generated due to modeling on the pipe digital model, and combining the narrow surfaces and scattered surfaces into a smooth surface.

[0034] Step S121 can reduce the number of low-quality meshes caused by dense lines.

[0035] Step S13: performing finite element meshing on the pipe digital model by using tetrahedral meshes, deleting the surface meshes, and only retaining the volume meshes to generate the finite element model of the pipe to be processed.

[0036] Performing finite element meshing on the pipe digital model by using tetrahedral meshes can reduce the difficulty of meshing and improve the quality of the meshes. By establishing a pipe digital model that is completely consistent with the actual pipe structure and optimizing the surface curve, a high-quality finite element model of the pipe to be processed is established.

[0037] Step S2: assigning material properties and cross-sectional properties to the finite element model of the pipe to be processed, and establishing a displacement constraint application point at one end of the inner pipe;

[0038] The one end of the inner pipe refers to the end of the inner pipe structure exposed to the outside in the pipe structure, i.e., the left end of the pipe in Figure 2

[0039] As an example, the step S2 includes:

[0040] ​​Step S21, output the to-be-processed pipeline finite element model as a second target file recognizable by a preset engineering structure simulation software, and import the second target file into the engineering structure simulation software;

[0041] The preset engineering structure simulation software can be Abaqus, and the second target file can be an inp file.

[0042] Step S22, establish material properties and cross-section properties of the outer pipe, the inner pipe, the steel hoop and the elastic block, and assign the material properties and the cross-section properties to the to-be-processed pipeline finite element model;

[0043] For example, the outer pipe material property is cast iron, the steel hoop material is carbon steel, and the elastic block material is rubber.

[0044] Step S23, establish a displacement constraint application point at one end of the inner pipe along the pipeline axis direction.

[0045] Step S3, in a preset first analysis step, set all contact relationships except an overlapping area between the elastic block and the outer pipe, apply a pressure load on the upper surface of the elastic block, as shown in Figure 5 The pressure direction points to the inner side of the rubber, so that the overlapping area between the elastic block and the outer pipe is less than a preset overlapping area threshold, that is, less than an overlapping area threshold allowing calculation convergence, a fixed constraint is applied at one end of the outer pipe, and a displacement constraint is applied at the displacement constraint application point, and the displacement amount of 6 degrees of freedom is 0.

[0046] Specifically, a dynamic explicit method can be used to establish the first analysis step (Step 1), the second analysis step (Step 2) and the third analysis step (Step 3) respectively. The dynamic display can increase the convergence of calculation, and the quality scaling function can be used to speed up the calculation efficiency.

[0047] The all contact relationships except the overlapping area between the elastic block and the outer pipe include a contact relationship between the elastic block and the steel hoop, a contact relationship between the elastic block and the inner pipe, a contact relationship between adjacent two elastic blocks, a contact relationship between the steel hoop and the inner pipe, and a contact relationship between the steel hoop and the outer pipe.

[0048] As an embodiment, in the step S3, a smooth step is used to control the pressure load applied on the upper surface of the elastic block, so that the pressure is smoothly increased from 0 to a preset pressure value within a preset time, so that the pressure is smoothly increased from 0 to the set value within 1 second, and the calculation convergence is increased.

[0049] Since the contact relationship between the elastic block and the outer tube is not set in the first analysis step, the meshes in the overlapping area do not interact with each other in the finite element analysis, and the overlapping area does not participate in the calculation, so although the area of the overlapping area of the elastic block is large, it does not affect the convergence of the calculation. At the same time, under the action of the pressure load, the elastic block is compressed, and the area of the overlapping area between the elastic block and the outer tube is reduced. It can be understood that the overlapping area can be 0, that is, the compressed elastic block does not overlap with the outer tube. In addition, in the first analysis step, a fixed constraint is applied at one end of the outer tube (i.e. the right end of the pipeline in the figure), which constrains all degrees of freedom of the right end of the outer tube, and a displacement constraint is applied at the displacement constraint point on the left side of the inner tube (see Figure 2 ). The displacement of the 6 degrees of freedom is 0. As an example, the load and boundary condition can be set as the parameters shown in Figure 6 .

[0050] Step S4, in a preset second analysis step, set the contact relationship between the elastic block and the outer tube, and perform pre-compression calculation based on the current overlapping area between the elastic block and the outer tube, and then eliminate the pressure load applied to the upper surface of the elastic block;

[0051] In the preset second analysis step, the contact relationship between the elastic block and the outer tube is set (at this time the overlapping area has been reduced under the action of the pressure, and the number of overlapping meshes between the elastic block and the outer tube is reduced). Since the contact relationship between the elastic block and the outer tube is set in the preset second analysis step, the pre-compression calculation of the current overlapping area between the elastic block and the outer tube will be automatically performed in the preset second analysis step. Since the overlapping area has been reduced in the first analysis step, the number of overlapping meshes is small, and the pre-compression calculation can converge. After the pre-compression calculation, the pressure applied to the surface of the rubber is gradually reduced to 0 Pa in this analysis step, so as to eliminate the influence of the pressure. In order to increase the convergence of the calculation, the pressure load is eliminated by using Smooth Step, as shown in Figure 7 . In the second analysis step, the pre-compression calculation, the contact calculation (between the elastic block and the outer tube), and the pressure load elimination calculation must be completed. A large time step leads to non-convergent calculation. Therefore, the analysis step size must be adjusted according to the convergence of the calculation in this analysis step, and the maximum analysis step can be set to 1e-5, as shown in Figure 8 . In addition, the calculation time of this analysis step is relatively long, in order to speed up the calculation efficiency, mass scaling is used, and the mass scaling multiple can be set to 10000, as shown in Figure 9 .

[0052] Step S5, in a preset third analysis step, control the displacement constraint applied to one end of the inner tube, bend one end of the inner tube to a target displacement in a direction perpendicular to the axial direction of the inner tube, and obtain the bending strength of the pipeline structure.

[0053] Wherein, by controlling the displacement constraint applied to one end of the inner tube, the displacement of the inner tube in the Y direction is modified to a set value, so as to realize the left side of the inner tube bending in the Y direction, thereby obtaining the bending strength of the pipe structure. It should be noted that the specific calculation process of calculating the bending strength of the pipe structure by simulation bending is prior art, and will not be described here. In order to increase the calculation convergence, the displacement constraint concentrated force load is also eliminated by Smooth Step, and the specific parameter setting is as follows Figure 10

[0054] It should be noted that some example embodiments are described as processes or methods depicted as flow diagrams. Although each step of the processes is described as occurring sequentially, many of the steps can be performed in parallel, concurrently, or at the same time. In addition, the order of the steps can be re-arranged. The processes can be terminated when their operations are completed, but can also have additional steps not included in the figure. The processes can correspond to methods, functions, procedures, subroutines, subprograms, etc.

[0055] The method described in the embodiments of the present application solves the problem of non-convergence of finite element calculation of large deformation interference assembly of rubber blocks in pipe simulation by adopting the mode of applying compression load and elastic block contact relationship in multiple analysis steps, thereby improving the calculation convergence and calculation efficiency of the bending strength simulation analysis of large deformation interference assembly of elastic blocks.

[0056] The above is only the preferred embodiment of the present application, and is not intended to limit the present application in any form. Although the present application has been disclosed as above with the preferred embodiment, it is not intended to limit the present application. Any skilled person in the art can make some changes or modifications to the above disclosed technical content without departing from the scope of the technical solution of the present application, and any simple modification, equivalent change and modification of the above embodiments according to the technical essence of the present application are still within the scope of the technical solution of the present application.​

Claims

1. A method for simulating the bending strength of a pipe based on interference assembly, characterized in that, The method comprises the following steps: Step S1, establishing a finite element model of a pipe to be processed according to a pipe structure, the pipe structure comprising an outer pipe, an inner pipe, and a steel band and an elastic block between the connection positions of the inner pipe and the outer pipe, the deformation amount of the elastic block being greater than a preset deformation threshold value when the pipe structure is assembled with interference, the preset deformation threshold value referring to a deformation threshold value allowing calculation convergence; Step S2, giving the finite element model of the pipe to be processed material properties and cross-section attributes, and establishing a displacement constraint application point at one end of the inner pipe, the one end of the inner pipe referring to the end of the pipe structure where the inner pipe structure is exposed to the outside; Step S3, in a preset first analysis step, setting all contact relationships except the overlapping area between the elastic block and the outer pipe, applying a pressure load on the upper surface of the elastic block, the pressure direction pointing to the inner side of the rubber, so that the overlapping area between the elastic block and the outer pipe is less than a preset overlapping area threshold value, applying a fixed constraint at one end of the outer pipe, and applying a displacement constraint at the displacement constraint application point, the displacement amount of the six degrees of freedom being 0; Step S4, in a preset second analysis step, setting the contact relationship between the elastic block and the outer pipe, pre-compressing based on the current overlapping area between the elastic block and the outer pipe, and then eliminating the pressure load applied to the upper surface of the elastic block; Step S5, in a preset third analysis step, controlling the displacement constraint applied at the one end of the inner pipe, bending the one end of the inner pipe to a target displacement along a direction perpendicular to the axial direction of the inner pipe, and obtaining the bending strength of the pipe structure.

2. The method according to claim 1, wherein in the step S3, the all contact relationships except the overlapping area between the elastic block and the outer pipe comprise: the contact relationship between the elastic block and the steel band, the contact relationship between the elastic block and the inner pipe, the contact relationship between adjacent two elastic blocks, the contact relationship between the steel band and the inner pipe, and the contact relationship between the steel band and the outer pipe.

3. The method according to claim 1, wherein in the step S3, the pressure load applied to the upper surface of the elastic block is controlled in a smooth step manner, so that the pressure increases smoothly from 0 to a preset pressure value within a preset time.

4. The method according to claim 1, wherein in the step S4, the pressure load applied to the upper surface of the elastic block is controlled in a smooth step manner, so that the pressure decreases from the preset pressure value to 0 within a preset time.

5. The method according to claim 1, wherein the step S1 comprises the following steps: Step S11, establishing a pipe digital model, the elastic block being in an undeformed assembly state, and the elastic block and the outer pipe having an overlapping area; Step S12, outputting the pipe digital model to a first target file recognizable by a preset meshing software, and importing the first target file into the meshing software for surface meshing and volume meshing; Step S13, performing finite element division on the pipe digital model by using a tetrahedral mesh, deleting the surface mesh, and only keeping the volume mesh, to generate the finite element model of the pipe to be processed.

6. The method according to claim 5, wherein before the step S12 of performing meshing and volume meshing, the method further comprises the following steps: ​ ​ ​ ​ ​ Step S121, firstly, the redundant lines generated by modeling on the pipeline digital model are suppressed, and the long and narrow surface and the scattered surface are combined into a smooth surface.

7. The method of claim 1, wherein, The step S2 comprises: Step S21, outputting the to-be-processed pipeline finite element model into a second target file which can be recognized by a preset engineering structure simulation software, and importing the second target file into the engineering structure simulation software; Step S22, establishing material properties and cross-section properties of the outer pipe, the inner pipe, the steel hoop and the elastic block, and assigning the to-be-processed pipeline finite element model; Step S23, establishing a displacement constraint application point at one end of the inner pipe along the pipeline axis direction.

8. The method of claim 1, wherein, The preset deformation threshold is 5%.

Images