Finite element analysis method for tubular seat shell model based on Ansys workbench

Abstract

The invention discloses a tubular seat shell model finite element analysis method based on Ansys workbench, and relates to the technical field of water turbines, and the method comprises the following steps: 1, extracting the middle surfaces of all steel plates, and converting a solid model into a shell model; 2, expanding and trimming the shell; thirdly, the shell is divided; step 4, dividing grids, and simultaneously realizing grid connection; 5, parameterizing the thickness of the steel plate; according to the method, the tubular seat solid model is converted into the shell model, shell model processing is simple and rapid, shell connection does not need to be achieved, grid connection is achieved while grid division is conducted, tedious and time-consuming pretreatment of the solid model is avoided, the number of grids of the shell model is small, and the method is easy to implement. And the thickness of the steel plate can be parameterized, a calculation result can be obtained by changing the thickness parameter, the steps of changing the model, dividing grids and the like do not need to be repeated, and the finite element analysis efficiency of the tubular seat is improved.

Description

Technical Field

[0001] The present invention relates to the technical field of hydraulic turbines, and specifically to a finite element analysis method for a tubular seat shell model based on Ansys workbench. Background Technique

[0002] The tubular seat is an important support structure of a bulb tubular hydro-generating unit. The self-weight, hydraulic load and mechanical load of the unit are all transmitted to the concrete through the tubular seat. Therefore, it is a very necessary work to conduct a finite element analysis on the tubular seat.

[0003] Most of the existing finite element analyses of tubular seats based on Ansys workbench adopt solid models. Since the structure of the tubular seat is complex and is welded by hundreds of steel plates with different shapes and thicknesses, there are often a large number of geometric incoherences at the joints of the steel plates in the solid model. It is necessary to check one by one and perform geometric processing on the incoherences to achieve solid connection. Improper processing is likely to lead to failure of mesh generation, which is very cumbersome and time-consuming. Moreover, the number of solid meshes generated is relatively large, and it requires higher computer hardware. Further, in the design, the tubular seat is often strengthened or optimized for weight reduction by changing the thickness of the steel plate. Changing the thickness of the steel plate requires changing the solid model and re-meshing for analysis, resulting in a large amount of repetitive work. Summary of the Invention

[0004] The purpose of the present invention is to provide a finite element analysis method for a tubular seat shell model based on Ansys workbench. The shell model is simple and fast to process, realizes mesh connection while meshing, has a small number of meshes, and can parameterize the thickness of the steel plate, improving the efficiency of finite element analysis of the tubular seat, so as to solve the problems raised in the above background technique.

[0005] To achieve the above purpose, the present invention provides the following technical solution: A finite element analysis method for a tubular seat shell model based on Ansys workbench, including the following steps:

[0006] Step 1: Convert the solid model into a shell model. Create a Mechanical modal project in Ansys workbench, import the tubular seat solid model in the Geometry module, extract the mid-planes of all steel plates, and convert the solid model into a shell model;

[0007] Step 2: Expand and trim the shell. Set a maximum trimming distance, and batch trim the shell within the range of the maximum distance to remove redundant edges, and expand the shell to remove shell gaps;

[0008] Step 3: Divide the shell. Divide the shell according to the requirements of finite element analysis to obtain the constraint surface and the load application surface as boundary conditions, and then close the Geometry module;

[0009] Step 4: Mesh generation. Open the Model module, and use the Mesh function to generate a mesh with the mesh size, connection size, and connection tolerance as the constraints, and at the same time achieve mesh connection.

[0010] Step 5: Parametrize the thickness of the steel plate. In the Geometry of the Model module, select the target steel plate, mark the thickness as a parameter, and achieve the parametrization of the thickness of the target steel plate.

[0011] Step 6: Finite element analysis. Create a finite element analysis module in Ansys workbench, apply loads and constraints, and perform finite element analysis. If it is necessary to change the thickness of the target steel plate, simply change the thickness parameter in the Parameters module to obtain the calculation results, without repeating steps such as changing the model and generating the mesh.

[0012] Preferably, in Step 1, the mid-plane extraction of the steel plate includes box-selecting the entire or part of the solid model, setting the maximum thickness Dmax and the minimum thickness Dmin according to the steel plate thickness within the box-selection range, and extracting the mid-planes of all steel plates within the box-selection range at one time.

[0013] Preferably, the maximum trimming distance in Step 2 is half of the maximum thickness Dmax.

[0014] Preferably, the mesh type generated in Step 4 is shell mesh elements, and the connection tolerance is determined by the maximum gap existing between the shells, and the connection tolerance is not greater than the connection size.

[0015] Preferably, the connection tolerance in Step 4 is set using the Mesh-batch connection function to perform batch mesh generation on multiple geometric components or the entire assembly, and ensure that the meshes between adjacent components can be correctly connected and matched with each other.

[0016] Preferably, the Geometry module in Step 1 is opened using Space claim software, and the mid-plane with the steel plate thickness parameter is extracted using the Prepare-middle face function, and it can be viewed and changed in the mid-plane properties.

[0017] Preferably, in Step 3, the shell is split using the combination of the sketch and split functions in Space claim. By combining functions such as Sketch and Split, SpaceClaim users can efficiently complete various geometric operation tasks from preliminary design concepts to complex model modifications.

[0018] Preferably, when dividing the mesh using the Mesh function in Step 4, opening Batchconnection in the detail options can better connect, control, and improve the shell model.

[0019] Preferably, the connection tolerance is less than or equal to half of the maximum thickness Dmax.

[0020] In summary, the beneficial effects of the present invention are as follows:

[0021] By converting the solid model of the pipe seat into a shell model, the shell model is simple and fast to process, without the need to implement shell connection. Mesh connection is achieved while dividing the mesh, avoiding the cumbersome and time-consuming preprocessing of the solid model. The shell model has a small number of meshes, and the steel plate thickness can be parameterized. By changing the thickness parameter, the calculation result can be obtained without repeating steps such as changing the model and dividing the mesh, improving the efficiency of the finite element analysis of the pipe seat. BRIEF DESCRIPTION OF THE DRAWINGS

[0022] In order to more clearly illustrate the technical solutions in the embodiments of the invention or the prior art, the following will briefly introduce the drawings required for use in the description of the embodiments or the prior art. Obviously, the drawings in the following description are only some embodiments of the invention. For those of ordinary skill in the art, other drawings can be obtained based on these drawings without creative efforts.

[0023] Figure 1 It is a schematic diagram of the process framework structure of a finite element analysis method for a pipe seat shell model based on Ansys workbench of the present invention;

[0024] Figure 2 It is a solid model diagram of the pipe seat in the embodiment of a finite element analysis method for a pipe seat shell model based on Ansys workbench of the present invention;

[0025] Figure 3 It is a shell model diagram of the pipe seat in the embodiment of a finite element analysis method for a pipe seat shell model based on Ansys workbench of the present invention;

[0026] Figure 4 It is a mesh diagram of the pipe seat shell model in the embodiment of a finite element analysis method for a pipe seat shell model based on Ansys workbench of the present invention. DETAILED DESCRIPTION OF THE EMBODIMENTS

[0027] All features disclosed in this specification, or all steps in any method or process disclosed, except for mutually exclusive features and / or steps, can be combined in any manner.

[0028] Any feature disclosed in this specification (including any additional claims, abstract, and drawings), unless specifically recited, may be replaced by other equivalent or similar-purpose alternative features. That is, unless specifically recited, each feature is only an example of a series of equivalent or similar features.

[0029] In the present invention, unless otherwise clearly specified and defined, terms such as "install", "connect", "join", "fix", etc. shall be understood in a broad sense. For example, it may be a fixed connection, a detachable connection, or integrated; it may be a mechanical connection, a direct connection, or an indirect connection through an intermediate medium. It may be the communication inside at least two elements or the interaction relationship between at least two elements, unless otherwise clearly defined. For those of ordinary skill in the art, the specific meanings of the above terms in the present invention can be understood according to specific circumstances.

[0030] The following is a detailed description of the present invention in conjunction with Figures 1-4 A method for finite element analysis of a tubular seat shell model based on Ansys workbench provided by the present invention will be described in detail. The method for finite element analysis of a tubular seat shell model based on Ansys workbench includes the following steps:

[0031] The first step: Convert the solid model into a shell model

[0032] Create a Mechanical modal project in Ansys workbench and import the solid model of the tubular seat in the Geometry module. Here, a tubular seat with a steel plate thickness range of 20 - 110 mm is taken as an example;

[0033] Open the Geometry module with Space claim software, select the Prepare - middle face function, perform specific processing on the middle face of the model to meet the subsequent simulation analysis requirements. In the details option, select Use range, input the maximum thickness Maximum thickness = 110 mm, the minimum thickness Minimum thickness = 20 mm, which can be viewed and changed in the middle face characteristics. Select the entire solid model and extract the middle faces of all steel plates to convert the solid model into a shell model;

[0034] The second step: Expand and trim the shell

[0035] In the Space claim, use the Prepare - extend function to preprocess and repair the imported model. Since data exchange between different systems may cause model incompatibilities or errors, such as broken surfaces, unclosed solids, redundant geometries, etc., by using the Prepare tool, users can automatically detect and fix these problems, making the model reach an ideal state for subsequent analysis or further editing. In the detail options, select Extend to curve and Trim surface, and enter the maximum distance Maximum distance = 55mm. Batch - trim the shell within the Maximum distance range to remove redundant edges and extend the shell to remove shell gaps;

[0036] Step 3: Divide the shell;

[0037] In the Space claim, according to the finite - element analysis requirements, use the sketch and split functions to divide the shell. By combining functions such as Sketch and Split, various geometric operation tasks from preliminary design concepts to complex model modifications can be efficiently completed, obtaining constraint surfaces and load - application surfaces, and then close the Geometry module;

[0038] Step 4: Mesh generation and simultaneous mesh connection;

[0039] Open the Model module and use the Mesh function to generate a mesh. First, set the global mesh parameters to let the software automatically generate the mesh. Subsequently, for specific regions in the model, such as stress - concentration regions, fluid - flow boundary layers, etc., local refinement parameters can be manually set to generate a finer mesh. Through built - in quality metrics and optimization algorithms, ensure that the generated mesh meets the requirements of analysis accuracy. After generating the mesh, it can be inspected, and problems can be repaired in a timely manner to ensure the accuracy of subsequent simulation analysis;

[0040] Open the Batch connection function in the detail options to better connect, control, and improve the shell model. Then enter the global mesh parameters: Element size = 100mm, Connection size = 60mm, Connection tolerance = 55m, and generate a shell - mesh element while achieving mesh connection, with a total of 46,000 meshes;

[0041] For comparison, under the condition of the same mesh size Element size = 100mm, the number of meshes of the solid model is 586,000, which is 12.7 times that of the shell model;

[0042] It should be noted that in order to perform batch meshing on multiple geometric components or the entire assembly and ensure that the meshes between adjacent components can be correctly connected and matched to each other, the Connection tolerance among them is set using the Mesh-batch connection function;

[0043] The Connection tolerance parameter is mainly used to control the matching accuracy of the shared boundaries between different mesh regions. Specifically, when the meshing algorithm attempts to align the mesh nodes of different components, a permitted error range will be considered. If the distance between two surfaces is within this tolerance range, they will be considered to be matched and a good coupling boundary condition will be formed, which is crucial for simulating contact problems or achieving seamless docking between components;

[0044] Setting a reasonable Connection tolerance value can help reduce unnecessary degrees of freedom and ensure the accuracy of the calculation results. If the tolerance value is too large, it may be difficult to match the meshes, increasing the computational cost and possibly failing to generate effective meshes. If the tolerance value is too small, there may be a large gap at the boundaries that should be in close contact physically, thus affecting the accuracy of the analysis results. Therefore, choosing an appropriate connection tolerance is an important step in the finite element modeling process;

[0045] Step 5: Parametrize the thickness of the steel plate

[0046] Refer to the appendix Figure 2 , take the horizontal support plate as the target steel plate. In the Geometry of the Model module, select the target steel plate and mark the thickest part, Thickness, as a parameter to achieve the parametrization of the thickness of the target steel plate;

[0047] Step 6: Finite element analysis

[0048] Create a Modal module in Ansys workbench, constrain the contact surface between the pipe socket and the concrete, perform a modal analysis on the pipe socket, obtain the first-order modal frequency of 44.3 Hz, the calculation takes 13 seconds, and the result file occupies 15 MB. Further, it is necessary to change the thickness of the target steel plate from 110 mm to 120 mm. In the Parameters module, change the parameter of the thickness of the target steel plate to 120 mm, and update the result to obtain the first-order modal frequency of 44.7 Hz.

[0049] In contrast, a modal analysis was performed on the pipe seat using a solid model, obtaining a first-order modal frequency of 45.2 Hz. The calculation took as long as 19 minutes, and the result file occupied a capacity of 187 MB. Further, if the thickness of the target steel plate needs to be changed from 110 mm to 120 mm, the target steel plate must first be thickened in 3D software, then the mesh needs to be re-divided and the modal analysis is carried out again, obtaining a first-order modal frequency of 45.5 Hz.

[0050] In summary, compared with the finite element analysis method of the pipe seat solid model, the model of the present invention is simple and fast to process, has fewer meshes, parameterizes the steel plate thickness, greatly improves the finite element analysis efficiency of the pipe seat. The shell model is simple and fast to process, does not require the realization of shell connection, realizes mesh connection while dividing the mesh, avoids the cumbersome and time-consuming pre-processing of the solid model, and the calculation results can be obtained by changing the thickness parameters, without repeating steps such as changing the model and dividing the mesh, improving the finite element analysis efficiency of the pipe seat.

[0051] As described above, it is only the specific implementation manner of the invention, but the protection scope of the invention is not limited thereto. Any change or replacement that can be thought of without creative work should be covered within the protection scope of the invention. Therefore, the protection scope of the invention should be subject to the protection scope defined by the claims.

Claims

1. A finite element analysis method for the tubular seat shell model based on Ansys workbench, characterized in that: It includes the following steps: Step 1: Convert the solid model into a shell model. Create a Mechanical modal project in Ansys workbench. Import the solid model of the pipe seat in the Geometry module. Extract the middle surfaces of all steel plates to convert the solid model into a shell model. Step 2: Expand and trim the shell. Set a maximum trimming distance. Batch trim the shell within the maximum distance range to remove the redundant edges and expand the shell to remove the shell gaps. Step 3: Divide the shell. Divide the shell according to the requirements of finite element analysis to obtain the constraint surface and the load application surface as boundary conditions, and then close the Geometry module. Step 4: Mesh generation. Open the Model module and use the Mesh function to generate meshes with the mesh size, connection size, and connection tolerance as the limits, and at the same time achieve mesh connection. Step 5: Parametrize the thickness of the steel plate. In the Geometry of the Model module, select the target steel plate and mark the thickness as a parameter to achieve the parametrization of the thickness of the target steel plate. Step 6: Finite element analysis. Create a finite element analysis module in Ansys workbench, apply loads and constraints, and perform finite element analysis.

2. The finite element analysis method of the tubular seat shell model based on Ansys workbench according to claim 1, characterized in that: The extraction of the middle surfaces of the steel plates in Step 1 includes selecting the whole or part of the solid model by box selection, setting the maximum thickness Dmax and the minimum thickness Dmin according to the thickness of the steel plates within the box selection range, and extracting the middle surfaces of all the steel plates within the box selection range at one time.

3. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 2, characterized in that: The maximum trimming distance in Step 2 is half of the maximum thickness Dmax.

4. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 1, characterized in that: The mesh type generated in Step 4 is shell mesh elements, and the connection tolerance is determined by the maximum gap existing between the shells, and the connection tolerance is not greater than the connection size.

5. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 4, characterized in that: The connection tolerance in Step 4 is set using the Mesh-batch connection function.

6. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 1, characterized in that: The Geometry module in Step 1 is opened using Space claim software, and the middle surfaces with the thickness parameters of the steel plates are extracted using the Prepare-middle face function.

7. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 1, characterized in that: In Step 3, the shell is divided using the combination of the sketch and split functions in Space claim.

8. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 1, characterized in that: In Step 4, when generating meshes using the Mesh function, open Batchconnection in the details options.

9. A finite element analysis method for a tubular seat shell model based on Ansys workbench according to claim 2, characterized in that: The connection tolerance is less than or equal to half of the maximum thickness Dmax.

Images