A Simulation and Mechanical State Characterization Method for an Engine Rotor Bolt Group

Abstract

The present invention discloses a method for simulating an engine rotor bolt group and characterizing the mechanical state, which includes the following steps: Step S1, establish an engine rotor model, which includes a thin-layer unit surface, and extract the information input file of the structural finite element model; Step S2, extract the information input file, and use the method of Python to read image information to number the bolt holes; Step S3, use the functions of Python to call the Abaqus load and analysis step modules, and according to the bolt hole numbers in S1, apply pre-tightening force to the bolts according to the bolt numbers, and import the Python file into Abaqus for analysis; Step S4, output the stress change values and connection stiffness change values of each unit of the cylinder and frustum around the screw rod with the bolt as the axis obtained from the Abaqus mechanical analysis in S3. The present invention improves the analysis efficiency of the bolt connection structure and improves the simulation accuracy at the same time.

Description

Technical Field

[0001] The present invention relates to the fields of computer technology and finite element simulation technology, and particularly relates to a method for simulating a bolt group and characterizing a mechanical state. Background Art

[0002] The connection of bolt groups is widely used in engines. Due to elastic interaction, the tightening sequence of bolt groups has a great influence on the final pre-tightening force and connection stiffness of the bolt groups. Therefore, in order to determine the optimal tightening process of bolts, it is necessary to use finite element simulation software to simulate and analyze the pre-tightening force of bolt group connections.

[0003] With the development of computer technology, the use of Python to process and analyze data has been widely applied, and the secondary development of Abaqus using Python can greatly simplify the modeling and analysis steps.

[0004] Traditional methods require a lot of time in setting up the preprocessing and subsequent analysis steps in the modeling and simulation of engine rotor bolts. When traditional methods analyze the influence of the tightening sequence on the pre-tightening force and connection stiffness, they mostly process the data of the entire rotor, while the bolts only play a greater role in some areas of the connected parts. In addition, traditional methods do not consider the influence of bolt pre-tightening force on the contact stiffness of the joint surface during calculation, resulting in a certain difference between the simulation results and the actual situation. Therefore, when using traditional methods for modeling and simulation, there are problems such as low efficiency and long time consumption, and the effects are not satisfactory. Summary of the Invention

[0005] The purpose of the present invention is to solve the deficiencies of the prior art, and provide a method for simulating an engine rotor and characterizing its mechanical state in combination with Python. This method can perform batch modeling and simulation analysis on some structures of the engine rotor model, obtain the stress change values and connection stiffness change values of the cylinders and frustum bodies around the screw with the bolt as the axis. The invention calculates the contact stiffness value between the contact surfaces by using the thin layer element method, and gives the value range of the angle between the side of the frustum body and the axis, thus solving the problems of low efficiency and inaccurate calculation results of traditional methods.

[0006] To solve the above technical problems, the present invention adopts the following technical solutions: A method for simulating an engine rotor bolt group and characterizing its mechanical state, characterized by including the following steps:

[0007] Step S1: Establish a finite element model of the engine rotor, which includes a thin layer element surface, and the thin layer element surface is respectively arranged between the flange and the rotor contact surface. The area around the screw with the bolt as the axis is divided into frustum body units on the upper and lower sides and a cylinder unit in the middle; extract the information input file of the structural finite element model;

[0008] Step S2: Read the information input file and number the bolt holes by using the method of reading image information in Python.

[0009] Step S3: Use Python to call the functions of the Abaqus load and analysis step modules. According to the bolt hole numbers obtained in S1, apply the pre-tightening force to the bolts in sequence according to the bolt numbers, and import the Python file into Abaqus for batch analysis.

[0010] Step S4: Output the stress change values and connection stiffness change values of each unit around the screw rod with the bolt as the axis obtained from the Abaqus mechanical analysis in S3.

[0011] Further, in the said step S1: The engine rotor model includes a flange, a rotor, and bolt nuts, where the bolt nuts are bolt nuts after simplifying the threads.

[0012] Further, the upper surface of the frustum element is the contact surface between the bolt head and the flange. The calculation formula for the included angle θ between the frustum side and the screw rod is:

[0013]

[0014] K is the thickness ratio of the two rotors, K ≤ 1; C is the difference between the bolt hole and the nominal diameter of the bolt; H is the total thickness of the bolt connection; D is the diameter of the nut support surface; the height of the cylinder element is the distance between the lower surfaces of the two frustum elements.

[0015] Further, the normal load of the bolt within the range of the frustum and cylinder elements accounts for 98.7% - 99.2% of the bolt pre-tightening force.

[0016] Further, in the said step S1, the diameter of the thin layer element is the same as the diameter of the end face of the divided cylinder element, the diameter of the cylinder is equal to the diameter of the lower bottom surface of the frustum, the height of the frustum is 1 / 2 of the rotor thickness, and the thickness of the thin layer element is 1 / 30 - 1 / 100 of its diameter.

[0017] Further, the contact stiffness and stress change values are introduced into the prediction function Compose to comprehensively analyze the influence of the flange-rotor contact surface on the tightening sequence. The formula is as follows:

[0018] Compose = Change j + 100(κ upj + κ downj + κ mediumj + κ linkj ), j = 1, 2, 3...n

[0019] Where, Change j represents the stress change amount of the frustum-cylinder element around the j-th bolt after all bolts are tightened, κupj represents the stiffness value of the flange bolt within the range of the j-th bolt near the bolt head frustum after all bolts are tightened; κ downj represents the stiffness value of the flange bolt within the range of the j-th bolt near the nut frustum after all bolts are tightened; k mediumj represents the stiffness value of the flange bolt within the range of the j-th bolt cylinder after all bolts are tightened; k linkj represents the total contact stiffness between the flange and the rotor mating surface or between rotors; all quantities in this formula are dimensionless quantities.

[0020] Furthermore,

[0021] where i represents the serial number of the grid within the bolt cylinder and frustum range, j represents the serial number of the bolt tightening sequence, n represents the total number of bolts to be tightened, σ in represents the stress value of the i-th grid after the n-th bolt is tightened, σ ij represents the stress value of the i-th grid after the j-th bolt is tightened, m j represents the total number of grids contained within the frustum and cylinder of the j-th tightened bolt; note that the stress unit in the calculation process of this formula is MPa.

[0022] Furthermore,

[0023] k linkj represents the contact stiffness of the q-th contact surface after the j-th bolt is tightened, and Q represents the total number of contact surfaces between bolt connectors (excluding bolts).

[0024] Furthermore, for any two adjacent bolts, the distance between the geometric centers of the two bolts is less than 50 cm.

[0025] Compared with the prior art, the beneficial effects of the present invention are as follows:

[0026] ① The present invention utilizes the secondary development function of python for Abaqus to batch analyze the bolt tightening process in one operation. Compared with the traditional sequential analysis method, the operation steps are greatly simplified.

[0027] ② Through the function of python to retrieve data in Abaqus, the stress change values and connection stiffness change values of the cylinder and frustum around the screw rod with the bolt as the axis are obtained, and the value range of the angle between the side of the frustum and the axis is given. By narrowing the data processing range, the calculation efficiency is greatly improved.

[0028] ③By using Python, the contact surface between the flange rotors is changed to a thin layer element surface, and the contact stiffness value between the contact surfaces is creatively introduced into the connection stiffness, improving the accuracy of the calculation results, thus solving the problems of low efficiency and inaccurate calculation results in the traditional method.

[0029] ④This invention combines the stress change value and the stiffness change value. Compared with the traditional method that only considers stress or stiffness, it is more comprehensive and the results obtained are more reliable. Description of the Drawings

[0030] Figure 1 Schematic diagram of the traditional method

[0031] Figure 2 Schematic diagram of the method of the present invention

[0032] Figure 3 For the division range of the frustum, cylinder with the bolt as the axis, and the thin layer element on the contact surface. Where ① represents the frustum, ② represents the thin layer element, ③ represents the cylinder, ④ represents the rotor, and ⑤ represents the flange

[0033] Figure 4 Schematic diagram of the steps for batch analysis of the Python file imported into Abaqus and then data processing using Python. Detailed Implementation Manner

[0034] Next, the technical solutions in the embodiments of the present invention will be clearly and completely described in conjunction with the accompanying drawings in the embodiments of the present invention. Obviously, the described embodiments are only a part of the embodiments of the present invention, rather than all of the embodiments. Based on the embodiments of the present invention, all other embodiments obtained by those of ordinary skill in the art without creative efforts shall fall within the protection scope of the present invention.

[0035] Next, the present invention will be further described in conjunction with the drawings and embodiments. As Figure 1 Schematic diagram of the steps of the traditional method, Figure 2 Schematic diagram of the method in the present invention, a method for simulating the bolt group of an engine rotor and characterizing the mechanical state.

[0036] Step 1: Modeling of the thin layer element. Calculate the diameter of the thin layer element according to the action range of the bolt. The thickness of the thin layer element is 1 / 30 - 1 / 100 of its diameter. Here, 1 / 50 is taken. The elastic modulus and shear modulus of the thin layer element are obtained through theoretical calculation, and a model of the thin layer element is established.

[0037] Step 2: Establish parts such as the rotor, flange, and bolt in Abaqus, and assemble them together with the thin layer element. The assembly is as Figure 3As shown, it is a multi-layer structure. Set the material parameters, perform contact settings and mesh generation. Extract the information input file, and the file information includes: the dimension information of the engine rotor model parts, material parameters, contact conditions, mesh information, and analysis steps. Open this file with python.

[0038] Step 3: According to the calculation formula of the angle θ,

[0039]

[0040] where, K = h1 / h2 = 25 / 25 = 1 ≤ 1; C = d2 - d1 = 1; H = h2 + h3 + h4 + 2*h5; D = 3.7;

[0041] Calculate to obtain that the inclination angle of the frustum side is 19°. Set the ranges of the cylinders and frustum bodies to be divided in the program. Use the function of python image analysis to number the bolts.

[0042] The cylinder and the frustum are the areas delimited on the rotor. The frustum area is the range included by rotating the trapezoid formed with the longest part of the bolt head as the upper side by 180° around the screw rod. The cylinder area is the range formed by rotating the bottom diameter of the frustum by 180° around the screw rod.

[0043] Step 4: As Figure 4 shown, input the sequence of bolts that need to be loaded with pre-tightening force, the stress values of the bolts, and the loading surface in the program. When using python to set the loading load, directly program and set different tightening sequences. Convert the written python program into an inp file.

[0044] Step 5: Import the inp file into abaqus, use Abaqus to perform post-processing analysis on the engine rotor, output the stiffness values and stress values of the bolts in the divided cylinders and frustum bodies, and the output files are rpy and MTX files. Under different tightening sequences, the rpy file and the MTX file are output respectively.

[0045] Save the rpy file and the MTX file output at each step, and use the data processing function of python to input the data into python for analysis.

[0046] Step 6: Use python to output the calculated values of the prediction function. By comparing the magnitudes of the predicted values under different tightening sequences, obtain the optimal tightening sequence. The larger the predicted value, the worse the tightening sequence. The smaller the value, it proves that after the bolts are tightened, the interaction between the bolts is smaller, and the tightening sequence is better.

[0047] Experimental conditions required for the invention: one small server, a Python program, Abaqus software, model drawings, bolt tightening sequence, bolt stress values, etc.

[0048] According to another implementation manner of the present invention, when a gasket is installed between the bolt and the rotor, the gasket and the nut are regarded as the same part. The area of the upper surface of the frustum is the area within the diameter region of the gasket.

[0049] When the gasket is rectangular, a circular region is constructed with the shortest side of the rectangle as the diameter, and the gasket and the nut within the circular region are regarded as a whole. The area of the upper surface of the frustum is the area within the diameter region of the gasket.

[0050] After installing the gasket, the two end faces of the cylinder are no longer the same, and at this time, the cylinder becomes a frustum region.

[0051] According to another implementation manner of the present invention, when the thickness of the rotor and the flange is thin enough (less than 3 mm), the frustum part can be converted into a cylinder part to improve the calculation accuracy.

[0052] As described above, only the specific implementation manners of the present invention are provided, but the protection scope of the present invention is not limited thereto. Any changes or substitutions that can be easily thought of by those skilled in the art within the technical scope disclosed by the present invention should be covered by the protection scope of the present invention.

[0053] The technical means disclosed in the solution of the present invention are not limited to the technical means disclosed in the above implementation manners, but also include technical solutions composed of any combination of the above technical features. It should be noted that for those of ordinary skill in the art, without departing from the principle of the present invention, several improvements and refinements can be made, and these improvements and refinements are also regarded as the protection scope of the present invention.

Claims

1. A method for simulating an engine rotor bolt group and characterizing its mechanical state, characterized in that Including the following steps: Step S1: Establish a finite element model of the engine rotor. This model contains a thin layer of element surface, which is respectively set between the flange and the rotor contact surface. The area around the screw with the bolt as the axis is divided into frustum elements on the upper and lower sides and a cylinder element in the middle; extract the information input file of the structural finite element model; the upper surface of the frustum element is the contact surface between the bolt head and the flange, and the calculation formula for the included angle θ between the side and the screw is: K is the thickness ratio of the two rotors, K ≤ 1; C is the difference between the bolt hole and the nominal diameter of the bolt; H is the total thickness of the bolt connection; D is the diameter of the nut support surface; the height of the cylinder element is the distance between the lower surfaces of the two frustum elements; Step S2: Read the information input file, and use the method of using Python to read image information to number the bolt holes; Step S3: Use Python to call the functions of the Abaqus load and analysis step modules. According to the bolt hole numbers obtained in S2, apply pre-tightening forces to the bolts in sequence according to the bolt hole numbers, and import the Python file into Abaqus for batch analysis; Step S4: Output the stress change values and connection stiffness change values of each element around the screw with the bolt as the axis obtained from the Abaqus mechanical analysis in S3; Introduce the contact stiffness and stress change values into the prediction function Compose, and comprehensively analyze the influence of the flange-rotor contact surface on the tightening sequence. The formula is as follows: Compose=Change j +100(κ upj +κ downj +κ mediumj +κ linkj ), j = 1, 2, 3...n Among them, Change j represents the stress change of the frustum cylinder unit around the j-th bolt after all bolts are tightened, and κ upj represents the stiffness value of the flange bolt within the frustum range near the bolt head of the j-th bolt after all bolts are tightened; κ downj represents the stiffness value of the flange bolt within the frustum range near the nut of the j-th bolt after all bolts are tightened; κ mediumj represents the stiffness value of the flange bolt within the cylinder range of the j-th bolt after all bolts are tightened; κ linkj represents the total contact stiffness between the flange and the rotor mating surface or between the rotors; all quantities in this formula are dimensionless quantities.

2. The simulation and mechanical state characterization method for an engine rotor bolt group according to claim 1, characterized in that, In the said Step S1: The engine rotor model includes a flange, a rotor, and bolts and nuts, where the bolts and nuts are bolts and nuts after simplifying the threads.

3. A method for simulating an engine rotor bolt group and characterizing its mechanical state according to claim 1, characterized in that, The normal load of the bolt within the range of the frustum and cylinder elements accounts for 98.7%-99.2% of the bolt pre-tightening force, and the height of the frustum is 1 / 2 of the rotor thickness.

4. A method for simulating an engine rotor bolt group and characterizing a mechanical state according to claim 1, wherein In the said Step S1, the diameter of the thin layer element is the same as the diameter of the end face of the divided cylinder element, the cylinder diameter is equal to the diameter of the lower bottom surface of the frustum, the height of the frustum is 1 / 2 of the flange thickness, and the thickness of the thin layer element is 1 / 30 - 1 / 100 of its diameter.

5. A method for simulating the bolt group of an engine rotor and characterizing the mechanical state according to claim 1, characterized in that where, i represents the serial number of the grid within the cylinder and frustum of the bolt, j represents the serial number of the bolt tightening sequence, n represents the total number of bolts to be tightened, and σ in represents the stress value of the i-th grid after the n-th bolt is tightened, and σ ij represents the stress value of the i-th grid after the j-th bolt is tightened, and m j represents the total number of grids contained in the frustum and cylinder of the j-th tightened bolt. The stress unit in the calculation process of this formula is MPa.

6. A method for simulating the bolt group of an engine rotor and characterizing the mechanical state according to claim 1, characterized in that κ linkqj represents the contact stiffness of the q-th contact surface after the j-th bolt is tightened, and Q represents the total number of contact surfaces between bolted connections.

7. A method for simulating an engine rotor bolt group and characterizing its mechanical state according to claim 3, characterized in that For any adjacent bolts, the distance between the geometric centers of the bolts is less than 50 cm.

Images