A finite element solving method for thermal deformation of rotating equipment based on measured temperature information

Abstract

A kind of finite element solving method of thermal deformation of rotating equipment based on measured temperature information, by constructing the finite element model of rotating equipment, with heat source temperature load as input, real-time adjustment rotating equipment component contact surface heat transfer coefficient, with multiple point measured temperature value and simulation value optimization test, the temperature field of the full solid model of rotating equipment is calculated;Finally, the calculated temperature field is applied to the rotating equipment model to solve its thermal deformation;The present application solves the problem that the existing rotating equipment model is calculated complex by applying convective heat transfer boundary, which further leads to low efficiency of rotating equipment thermal deformation calculation, under the premise of ensuring calculation accuracy, effectively utilize industrial field measured temperature data, greatly improve the efficiency of calculating rotating equipment temperature field and thermal deformation.

Description

Technical Field

[0001] This invention belongs to the field of service performance monitoring of rotating equipment, and specifically relates to a finite element method for solving the thermal deformation of rotating equipment based on measured temperature information. Background Technology

[0002] Rotating equipment is a critical component in many industries, including petroleum, chemical, energy, and metallurgy, where safety, reliability, and functional availability are paramount. With the development of modern industrial technology, the increasing performance parameters and the emergence of various complex and variable operating conditions pose greater challenges to the operation and maintenance of rotating equipment. Increased performance parameters amplify the internal temperature gradient, leading to increased thermal stress in solid components. During variable operating conditions, the temperature, pressure, and other key parameters of the fluids within the entire unit constantly change. The non-uniform and constantly changing temperature field within the rotating equipment causes uneven expansion of metal components, potentially leading to dynamic-static rubbing between the rotor and stator components in the flow path. Frequent and rapid start-ups and shutdowns of rotating equipment significantly impact unit lifespan. Furthermore, unstable operating conditions can cause low-cycle fatigue damage to metals, increasing the difficulty of lifespan prediction and reducing the overall lifespan of the rotating equipment. Therefore, in order to accurately monitor the operating status of critical components of rotating equipment, research on the temperature field and thermal deformation during the start-up and shutdown processes is particularly important.

[0003] In terms of research methods, the main methods for studying the temperature field of rotating equipment include theory, experiment, and simulation, each with its own advantages and disadvantages. The current main approach is to combine all three, using theory as the foundation and experimentation or simulation as the primary method, with each method mutually reinforcing the other. For example, traditional thermal analysis of steam turbines is based on the fluid-structure interaction heat transfer conditions inside the cylinder. Given the cylinder structural parameters, thermophysical parameters, initial conditions, and boundary conditions, the solution is obtained through heat conduction differential equations. Solving the temperature field of rotating equipment based on the heat conduction problem is computationally very complex, especially for rotating equipment like steam turbines where complex flow and heat transfer processes exist inside the cylinder, and the heat transfer boundary on the inner wall is difficult to determine. Therefore, it often leads to large errors in temperature field calculations. Moreover, because numerical iteration methods are used, solving complex flow and heat transfer behaviors is very time-consuming, especially for phenomena involving intense two-phase flow heat transfer. The computational units are enormous; solving for physical phenomena that occur in a few seconds can take several hours or even days, which cannot meet the requirements for rapidly calculating the temperature field distribution during the start-up and shutdown processes of rotating equipment.

[0004] In summary, current research methods for studying the transient thermal behavior of complex flow processes prevalent in industry are not yet mature. Rotating equipment such as steam turbines have temperature sensors installed in their cylinders and bearing housings, recording a large amount of temperature data during unit operation. Combining temperature monitoring data with numerical simulation methods to find a high-precision modeling and rapid solution approach is an effective method for studying the transient behavior of complex flow and heat transfer systems. Research in this area is currently very limited and should be vigorously explored. Summary of the Invention

[0005] In order to overcome the shortcomings of the prior art, the present invention aims to provide a finite element method for solving the thermal deformation of rotating equipment based on measured temperature information, which combines numerical simulation with measured temperature data, taking into account both computational efficiency and accuracy.

[0006] To achieve the above objectives, the technical solution adopted by the present invention is as follows:

[0007] A finite element method for solving the thermal deformation of rotating equipment based on measured temperature information includes the following steps:

[0008] Step 1: Build a 3D solid model of the rotating equipment in the modeling software NX, simplify the structure of the rotating equipment appropriately, and export the solid model as a general model format file in NX software.

[0009] Step 2: Preprocessing for temperature field calculation;

[0010] Step 3: Select the temperature near the heat source from each temperature measurement point as the model temperature load input, and use the return oil temperature, etc., as the temperature boundary constraint conditions.

[0011] Step 4: Simplify radiation heat transfer and convection heat transfer, adjust the heat conduction of the contact surfaces between various components, and use the contact surface heat conduction with thermal conductivity related to temperature and pressure to replace the fluid convection heat transfer and radiation heat transfer effects. That is, select a composite contact surface thermal conductivity to replace the radiation heat transfer and convection heat transfer it bears, and perform temperature field calculation of the all-solid model.

[0012] Step 5: Perform preprocessing for thermal deformation calculation;

[0013] Step 6: Submit a thermal deformation calculation request in the finite element mesh calculation model to solve for the thermal deformation of the rotating equipment.

[0014] In step one, when performing geometric modeling of the rotating equipment, based on its structural symmetry, the meridional plane is used as the plane of symmetry, and half of it is taken.

[0015] Step two specifically includes:

[0016] 2.1) Import the general model format file into the finite element analysis software Abaqus. In the material properties module of Abaqus, define the physical property parameters for the rotating equipment parts. The physical property parameters include thermal conductivity, material density, thermal expansion coefficient, Young's modulus, and specific heat capacity.

[0017] 2.2) Mesh the 3D solid model of the rotating device imported in step 2.1);

[0018] 2.3) Establish transient heat transfer analysis steps according to the actual start-up and shutdown processes of the rotating equipment, and establish steady-state heat transfer analysis steps for the cold state before start-up, the full-power state, and the cold state after shutdown.

[0019] The meshing described in step 2.2) involves dividing the interior of the rotating equipment bearing housing into meshes, since there are cooling and lubricating oil pipes inside. Tetrahedral meshes are used in areas with extremely irregular shapes, while hexahedral meshes are used in the remaining areas.

[0020] In step three, the temperature load input is taken as the temperature near the heat source. In addition, since the lubricating and cooling oil carries away a large amount of heat, the return oil temperature is used as the boundary temperature constraint.

[0021] Step four specifically includes:

[0022] 4.1) The initial values ​​of the thermal conductivity of the composite contact surface between each contact pair are initially determined based on the quadratic polynomial function of the local temperature;

[0023] The thermal conductivity λ of the composite contact surface between the i-th contact pair i * (t) is defined as a quadratic polynomial function of local temperature:

[0024] λ i * (t)=A1T 2 +A2T+A3

[0025] In the above formula, t is time, T is local temperature, and the other three parameters A1, A2, and A3 need to be optimized and corrected using multi-point temperature measurements.

[0026] 4.2) Add a temperature field calculation request to the finite element mesh calculation model to solve for the initial temperature field;

[0027] 4.3) In the transient heat transfer model, select the remaining N measurement points that are not used as temperature load inputs as optimized measurement points. During the heat transfer process, select M uniformly distributed time points, and output the temperature of N measurement points at each time point. Let the temperature of the nth measurement point at the tth time point obtained by finite element simulation be... The measured temperature was The temperature difference at the nth measuring point at the tth time point is:

[0028] Define the error function:

[0029]

[0030] The method for identifying the thermal conductivity parameters A1, A2, and A3 of the composite contact surface between each contact pair is to minimize the error function, with the objective function being:

[0031]

[0032] 4.4) Determine if the optimization has converged, i.e., calculate the error between the simulated temperature and the measured temperature at the same location. If the error is less than the preset error threshold, confirm the temperature field and output the temperature field result file; otherwise, generate a new set of parameters based on the error value and return to step 4.2).

[0033] Step five specifically includes:

[0034] 5.1) Based on the established temperature field solution model, modify the temperature solution analysis type in step four to general deformation solution analysis;

[0035] 5.2) Define the contact interaction mode between the contact surfaces of rotating equipment components, including friction properties;

[0036] 5.3) Add displacement boundary conditions, symmetric constraints, add a gravity field, and apply the temperature field calculated in step four to the rotating device model;

[0037] 5.4) Change the mesh type to the deformation stress solution type.

[0038] Compared with existing technologies and methods, the present invention has the following advantages:

[0039] This invention can effectively utilize on-site measured temperature data to accurately and quickly calculate the temperature field of rotating equipment structural components and the thermal deformation under the action of the temperature field, balancing calculation efficiency and accuracy, thereby accurately monitoring the operating status of key components of rotating equipment. Attached Figure Description

[0040] Figure 1 This is a flowchart of the present invention.

[0041] Figure 2 This is a schematic diagram of the model structure of the high-pressure and intermediate-pressure steam turbine, bearing housing, etc., in the embodiment.

[0042] Figure 3 This is a schematic diagram of the turbine temperature monitoring points in an example.

[0043] Figure 4The following are simulation results of the temperature field in the example: (a) Temperature field when the turbine speed is increased to 500 rpm; (b) Temperature field when the turbine speed is increased to 1500 rpm; (c) Temperature field when the turbine power is increased to 400 MW; (d) Temperature field when the turbine is operating at full power; (e) Temperature field when the turbine power is reduced to 400 MW; (f) Temperature field when the turbine power is reduced to 50 MW; (g) Temperature field when the turbine speed is reduced to 500 rpm. Detailed Implementation

[0044] To make the objectives, technical solutions, and advantages of this invention clearer, the invention will now be described in detail with reference to the accompanying drawings and embodiments. Figure 2 Taking the high-pressure and intermediate-pressure cylinder and bearing housings on both sides of the steam turbine as an example, the main sources of heat in the steam turbine are the heat transferred by the steam in the cylinder, the heat generated by the friction between the bearing and the rotor, and the cooling lubricating oil / jacking oil dissipates some of the heat to maintain the bearing within an acceptable temperature range.

[0045] To calculate the thermal deformation during the start-up and shutdown of the steam turbine, refer to Figure 1 A finite element method for solving the thermal deformation of rotating equipment based on measured temperature information includes the following steps:

[0046] Step 1: Taking the high-pressure and intermediate-pressure cylinders of the steam turbine and the bearing housings on the cylinder side as the research object, solid models of the high-pressure and intermediate-pressure cylinders, bearing housing #1 (high-pressure side), bearing housing #2 (intermediate-pressure side), shaft, and cylinder clamping device are created in the 3D modeling software NX. Figure 3 As shown, a 3D solid model of the steam turbine is constructed. The cylinder structure is appropriately simplified (ignoring minor components such as pipe fittings, split bolts, nuts, and diaphragms). Based on the symmetry of the cylinder, bearing housing structure and support method, half of it is taken with the meridional plane as the symmetry plane. The solid model is exported in NX software as a general model format file, such as the STEP format.

[0047] Step two, preprocessing for temperature field calculation, specifically includes:

[0048] 2.1) Import the general model format file into the finite element analysis software Abaqus. In the material properties module of Abaqus, define the physical property parameters for components such as the high-pressure and intermediate-pressure cylinders, bearing housings, shafts, and cylinder clamping devices of the steam turbine. The cylinders and bearing housings are assumed to be isotropic materials. The physical property parameters include thermal conductivity, material density, thermal expansion coefficient, Young's modulus, specific heat capacity, etc. (as shown in Table 1).

[0049] Table 1 Material Properties

[0050]

[0051] 2.2) Mesh the 3D solid model of the steam turbine imported in step 2.1); Since there are cooling and lubricating oil pipes inside the bearing housing, mesh the inside separately. Use tetrahedral meshes in areas with extremely irregular shapes. The quality of tetrahedral meshes is not as high as that of hexahedral meshes, but the number of tetrahedral meshes is small, so they have little impact on the temperature field of the entire model. Set the heat transfer element type to C3D10R mesh element format.

[0052] 2.3) Establish transient heat transfer analysis steps according to the actual turbine start-up and shutdown processes, including temperature analysis of cold state, upward turning gear, speed increase, power increase, full power, power decrease, speed decrease, downward turning gear, and cold state. Among them, the cold state and full power conditions are steady state temperature analysis, and the rest are transient temperature analysis.

[0053] Step 3: Select the temperature of the measuring point near the heat source as the temperature load input, and the return oil temperature as the temperature boundary constraint condition; in this embodiment, the measuring point temperature of the cylinder wall of the high pressure part of the high-pressure cylinder, the measuring point temperature of the cylinder wall of the medium pressure part of the high-pressure cylinder, and the temperature of the bearing bush of 1 / 2# are used as the temperature load input, and the return oil temperature data of the bearing seat of 1 / 2# are used as the temperature boundary constraint condition.

[0054] Step four: Due to the numerous planes involved in radiative and convective heat transfer, which are highly nonlinear, the calculation is time-consuming. Therefore, radiative and convective heat transfer is simplified, and the heat conduction at the contact surfaces between components is adjusted. The thermal conductivity of the contact surfaces, which is related to temperature and pressure, is used to replace the fluid's convective and radiative heat transfer effects. Specifically, a composite contact surface thermal conductivity is selected to represent the radiative and convective heat transfer, and the temperature field calculation for the all-solid model is performed. This includes:

[0055] 4.1) Based on the quadratic polynomial function of local temperature, the initial values ​​of the thermal conductivity of the composite contact surface between each contact pair are initially determined. The contact pairs include the cat claw and bearing housing support surface contact pair; the cylinder clamping device and cylinder split surface contact pair; the cylinder clamping device and bearing housing support surface contact pair; and the bearing bush and rotor contact pair.

[0056] The thermal conductivity λ of the composite contact surface between the i-th contact pair i * (t) is defined as a quadratic polynomial function of local temperature:

[0057] λ * (t)=A1T 2 +A2T+A3

[0058] In the above formula, t is time and T is local temperature. The initial values ​​of the three parameters A1, A2, and A3 are 0.01, 0.1, and 10, respectively. The three parameters A1, A2, and A3 need to be optimized and corrected by actual temperature measurement.

[0059] 4.2) Submit a temperature field calculation request in the finite element mesh calculation model to solve for the initial temperature field;

[0060] 4.3) In the transient heat transfer model, four measuring points are selected as optimized measuring points. During the heat transfer process, 20 uniformly distributed time points are selected, and the temperatures of the four measuring points are output at each time point. Let the temperature of the nth measuring point at the tth time point obtained by finite element simulation be... The measured temperature was The temperature difference at the nth measuring point at the tth time point is: The error function is:

[0061]

[0062] The method for identifying the thermal conductivity parameters A1, A2, and A3 of the composite contact surface between each contact pair is to minimize the error function, with the objective function being:

[0063]

[0064] 4.4) Determine whether the optimization has converged, that is, calculate the error between the simulated temperature and the measured temperature value at each measuring point. In this embodiment, the error threshold is set to 20. If the error is less than the preset error threshold, the temperature field is confirmed and the temperature field result file is output. Otherwise, a new set of parameters is generated based on the error value, and the process returns to step 4.2).

[0065] Step 5: Perform preprocessing for solving the thermal deformation problem, specifically including:

[0066] 5.1) Based on the established temperature field solution model, modify the temperature solution analysis type in step four to general deformation solution analysis;

[0067] 5.2) Define the contact interaction modes between the contact surfaces of turbine components, including friction properties, etc.;

[0068] 5.3) Add displacement boundary conditions at the cylinder dead point, add symmetric constraints to the axial meridional plane, define the gravity field, and apply the temperature field calculated in step four to the turbine model.

[0069] 5.4) Change the mesh type to the deformation stress solution type;

[0070] Step 6: Submit a hot deformation calculation request in the finite element mesh calculation model to solve for the hot deformation of the steam turbine.

[0071] like Figure 4As shown in Table 2, the method of this invention can efficiently and accurately calculate the temperature field of the entire steam turbine using the turbine's monitored temperature data. The simulated output temperature is close to the measured temperature, with a maximum deviation of only 3.8℃. The maximum root mean square error for all operating conditions is 2.8℃, and the maximum average absolute error is 2.7℃, demonstrating promising application prospects.

[0072] Table 2. Simulated and measured temperature values ​​and their relative errors (°C) at monitoring points during start-up and shutdown processes.

[0073]

[0074]

[0075] The beneficial effects of the embodiments of the present invention are as follows: The present invention utilizes a large amount of temperature monitoring data of the steam turbine to quickly and effectively determine the distribution of the three-dimensional temperature field of the steam turbine, and can meet the requirements for solving the thermal deformation of the steam turbine, while taking into account both computational efficiency and accuracy.

[0076] Finally, it should be noted that the above embodiments are only used to illustrate the technical solutions of the present invention, and not to limit them. Although the present invention has been described in detail with reference to the foregoing embodiments, those skilled in the art should understand that modifications can still be made to the technical solutions described in the foregoing embodiments or equivalent substitutions can be made to some of the technical features. Such modifications or equivalent substitutions do not cause the essence of the corresponding technical solutions to deviate from the spirit and scope of the technical solutions of the embodiments of the present invention.

Claims

1. A finite element method for solving the thermal deformation of rotating equipment based on measured temperature information, characterized in that, Includes the following steps: Step 1: Build a 3D solid model of the rotating equipment in the modeling software NX, simplify the structure of the rotating equipment, and export the solid model as a general model format file in NX software. Step 2: Preprocessing for temperature field calculation; Step 3: Select the temperature near the heat source from each temperature measurement point as the model temperature load input, and use the return oil temperature as the temperature boundary constraint condition. Step 4: Simplify radiation heat transfer and convection heat transfer, adjust the heat conduction of the contact surfaces between various components, and use the contact surface heat conduction with thermal conductivity related to temperature and pressure to replace the fluid convection heat transfer and radiation heat transfer effects. That is, select a composite contact surface thermal conductivity to replace the radiation heat transfer and convection heat transfer it bears, and perform temperature field calculation of the all-solid model. Step four specifically includes: 4.1) Initial values ​​of thermal conductivity of the composite contact surface between each contact pair are determined based on the quadratic polynomial function of local temperature; No. i Thermal conductivity of the composite contact surface between the contact pairs Defined as a quadratic polynomial function of local temperature: In the above formula For time, T For local temperature, the other three parameters A 1. A 2. A 3. Optimization and correction are needed using multiple temperature measurements; 4.2) Add a temperature field calculation request to the finite element mesh calculation model to solve for the initial temperature field; 4.3) Select the remaining parameters in the transient heat transfer model. N Selecting measurement points that were not previously used as temperature load inputs as optimization measurement points during the heat transfer process. M A uniformly distributed number of time points, outputting at each time point. N The temperature at the nth measuring point, let the nth... n The measuring point at the ... t The temperature obtained by finite element simulation at each time point is: The measured temperature was Then the first n The measuring point at the ... t The temperature difference at each point in time is ; Define the error function: Thermal conductivity of the composite contact surface between each contact pair A 1. A 2. A The three-parameter identification method involves minimizing the error function, with the objective function being: 4.4) Determine if the optimization has converged, i.e., calculate the error between the simulated temperature and the measured temperature at the same location. If the error is less than the preset error threshold, confirm the temperature field and output the temperature field result file; otherwise, generate a new set of parameters based on the error value and return to step 4.1). Step 5: Perform preprocessing for thermal deformation calculation; Step 6: Submit a thermal deformation calculation request in the finite element mesh calculation model to solve for the thermal deformation of the rotating equipment.

2. The method according to claim 1, characterized in that, In step one, when performing geometric modeling of the rotating equipment, based on its structural symmetry, the meridional plane is used as the plane of symmetry, and half of it is taken.

3. The method according to claim 1, characterized in that, Step two specifically includes: 2.1) Import the general model format file into the finite element analysis software Abaqus. In the material properties module of Abaqus, define the physical property parameters for the rotating equipment parts. The physical property parameters include thermal conductivity, material density, thermal expansion coefficient, Young's modulus, and specific heat capacity. 2.2) Mesh the 3D solid model of the rotating device imported in step 2.1); 2.3) Establish transient heat transfer analysis steps according to the actual start-up and shutdown processes of the rotating equipment, and establish steady-state heat transfer analysis steps for the cold state before start-up, the full-power state, and the cold state after shutdown.

4. The method according to claim 3, characterized in that, The meshing described in step 2.2) involves dividing the interior of the rotating equipment bearing housing into meshes, since there are cooling and lubricating oil pipes inside. Tetrahedral meshes are used in areas with extremely irregular shapes, while hexahedral meshes are used in the remaining areas.

5. The method according to claim 1, characterized in that, Step five specifically includes: 5.1) Based on the established temperature field solution model, modify the temperature solution analysis type in step four to general deformation solution analysis; 5.2) Define the contact interaction mode between the contact surfaces of rotating equipment components, including friction properties; 5.3) Add displacement boundary conditions, symmetric constraints, add a gravity field, and apply the temperature field calculated in step four to the rotating device model; 5.4) Change the mesh type to the deformation stress solution type.

Images