Hypermesh secondary development-based damper finite element model automatic modeling method

Abstract

The invention relates to an automatic modeling method for a finite element model of a shock absorber based on Hypermesh secondary development. The automatic modeling method comprises the following steps: inputting a geometric model; automatically extracting the middle surface of the thin-wall part; a thin-wall part 2D mesh and a solid part 3D mesh are automatically divided; batch creation of Rbe1, Rbe2 and Rbe3, batch creation of welding spots and welding seams, batch creation of contact pairs, and batch creation of working condition stress and control cards; and submitting calculation and automatically exporting a simulation report. According to the method, secondary development is carried out by applying TCL and TK languages on the basis of the Hypermesh environment, a solution is provided for solving the difficult problems that modeling of a finite element model of the shock absorber is tedious and the manual operation error rate is high, when finite element modeling is carried out on the shock absorber, tedious manual operation can be greatly reduced by adopting the method, the working efficiency is improved, and the method is suitable for large-scale popularization and application. Meanwhile, the labor cost can be remarkably reduced, the modeling speed is increased, and the research and development period is shortened.

Description

TECHNICAL FIELD

[0001] The present application relates to the technical field of secondary development of finite element software, and particularly relates to a shock absorber finite element model automatic modeling method based on Hypermesh secondary development, which is mainly used for automatic modeling of automobile shock absorbers. BACKGROUND

[0002] The automobile shock absorber (also known as the suspension damper) is one of the core components of the vehicle chassis system, and its performance is directly related to the driving safety, ride comfort and handling stability of the vehicle. In the process of automobile research and development, the dynamic simulation analysis of the shock absorber by using the computer aided engineering (CAE) technology has become a key link for optimizing the performance, shortening the development cycle and reducing the test cost. As one of the most important CAE methods, the precision and efficiency of the finite element analysis (FEA) are highly dependent on the quality of the finite element model established in the pre-processing stage.

[0003] At present, in the finite element pre-processing process in the automobile industry, especially in the field of shock absorbers, the modeling work mainly depends on the general pre-processing software platform, such as Altair HyperMesh, ANSA, MSC Patran, etc. Although these software has powerful functions and mature meshing technology, its operation mode is essentially still based on manual processing with human-computer interaction. The modeling engineer needs to manually perform a series of highly repetitive and tedious operations, including but not limited to: geometry cleaning, mid-surface extraction, beam creation, definition of component connection relationships (such as welding, gluing, bolt connection), material property assignment, meshing and quality checking, application of load and boundary conditions, etc.

[0004] The traditional manual modeling method has the following significant technical bottlenecks and inherent defects: 1. extremely low efficiency and long development cycle: it takes hours or even days for an experienced engineer to complete a complete finite element model of a complex shock absorber assembly (including piston rod, working cylinder, oil storage cylinder, base valve, connecting piece, etc.); 2. poor model quality consistency and reliability difficult to guarantee: the modeling process is highly dependent on the personal experience and skill level of the engineer, and different engineers or even the same engineer at different times may have differences in meshing standards (such as element size, type), connection relationship processing method, boundary condition simplification assumption, etc.; 3. difficulty in professional knowledge solidification and inheritance: an excellent finite element modeling engineer needs to have deep theoretical knowledge of mechanics, rich engineering experience and skilled software operation skills.

[0005] To overcome the aforementioned problems of traditional manual modeling, some industry players have attempted to automate certain operations by recording operation macros using software's built-in scripting functions (such as HyperMesh's Tcl / Tk scripts). However, this simple macro recording method lacks flexibility and fault tolerance, and cannot cope with changes in geometric models or structural forms. Essentially, it is still "recording operations" rather than "intelligent modeling," failing to fundamentally solve the problems of process standardization and knowledge integration.

[0006] Therefore, there is an urgent need in this field for an intelligent system that can deeply integrate expert knowledge and automate the entire process of finite element modeling for vibration dampers. This system should be able to generate high-quality, standardized finite element models that can be directly calculated with a single click based on the input model, thereby completely liberating engineers' productivity, significantly improving the efficiency, consistency, and reliability of simulation analysis, and ultimately accelerating the R&D and innovation process of automotive products. Summary of the Invention

[0007] To address the problems of low efficiency, poor model quality consistency, and high human resource costs in existing finite element modeling techniques for vibration dampers, this invention provides an automated finite element modeling method for vibration dampers based on Hypermesh secondary development. This invention aims to achieve fully automated generation of high-quality finite element models from vibration damper geometric models, fundamentally transforming the traditional manual modeling mode, thereby significantly improving simulation analysis efficiency and ensuring model quality consistency.

[0008] The technical solution of the present invention is as follows:

[0009] This invention presents an automated modeling method for finite element models of shock absorbers based on Hypermesh secondary development. Utilizing the TCL language and Hypermesh's own API, it automates the simulation process by using secondary development plugins to automatically build finite element models of automotive shock absorbers and perform simulation analyses under different operating conditions. Specifically, this includes importing the 3D model of the shock absorber; automatic mid-surface extraction of thin-walled components; automatic mesh generation of 2D meshes for thin-walled components and 3D meshes for solid parts; batch creation of Rbe2 and Rbe3, weld points and weld seams, contact pairs, loads, and load analysis steps; submission of calculations; and automatic export of simulation reports. This method can reduce manual operations that previously took hours or days to minutes, eliminating model discrepancies caused by human factors and achieving automated parametric finite element modeling and simulation result reporting.

[0010] Furthermore, this invention also defines an automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development, specifically including the following steps:

[0011] Step 1: Import the 3D model of the vibration damper;

[0012] Step 2: Perform secondary development of Hypermesh based on TCL / TK language and Hypermesh API to automate the simulation process;

[0013] Step 3: Using secondary development plugins, automatically extract the mid-surface of thin-walled parts, automatically generate 2D meshes for thin-walled parts and 3D meshes for solid parts; batch create Rbe2 and Rbe3, batch create weld points and weld seams, batch create contact pairs, batch create working condition stress, load and load analysis steps, and control cards to complete the finite element model of the vibration damper.

[0014] Step 4: Use the secondary development plugin to submit the calculation and automatically export the simulation report.

[0015] Furthermore, the present invention further specifies the specific process of step 3 as follows:

[0016] 3.1) Mid-surface extraction of thin-walled parts: Mid-surface extraction adopts the offset method. The offset distance is extracted and calculated by TCL / TK language, and then the outer surface is extracted for offset mid-surface extraction.

[0017] 3.2) Mesh generation: In the mesh generation stage, the parts are first grouped according to the identifiers, and then the mesh is automatically generated using the Batchmesh command. The specific process of part grouping is as follows: the part name contains the identifier, for example, the thin-walled part name contains 2d and the solid part name contains 3d. The 2d and 3d parts are grouped according to the identifiers.

[0018] 3.3) Batch creation of Rbe2 and Rbe3: Obtain the master and slave nodes of Rbe2 and Rbe3 through code, and create them in batches;

[0019] 3.4) Batch creation of weld points and weld seams: Extract weld point node information and create weld points in batches using a foreach loop; extract weld seam nodes and automatically create weld seams by the user selecting spatial order based on the x, y, or z axis.

[0020] 3.5) Batch creation of contact pairs: First, obtain the main face node information, then obtain the secondary face nodes through the main face nodes, and create contact pairs in batches according to the contact pair type;

[0021] 3.6) Batch creation of loads and load analysis steps.

[0022] Furthermore, the present invention further specifies the following details for the extraction of the thin-walled part's mid-surface in step 3.1):

[0023] Step 1: Extract the outer surface of the thin-walled part using *midsurface_edit_base_surfaces and *midsurface_extract_10solids;

[0024] Step 2: Use regular expressions to extract the thickness parameter set in componentname. Half of the thickness parameter is the distance to be offset.

[0025] Step 3: Offset the plane using *offset_surfaces_and_modify surfaces. Further, this invention also specifies the batch creation of Rbe2 in step 3.3) as follows:

[0026] Step 1: The main node originates from the center of the hole and is created in batches using *createnode with the coordinates of the center.

[0027] Step 2: Starting from the nodes on the circular hole washer, use a foreach loop to find a certain node on the hole, and denote it as node 'a'. Use hm_holedetectionidentifyhole to get the number of the hole containing node 'a', and denote it as hole 'a'.

[0028] Step 3: Then, obtain the washer number contained in hole a and the node number on the washer by using hm_holedetectiongetwasherelementslist;

[0029] Step 4: Since the node information on the washer obtained in Step 3 contains parentheses, first use split to separate the parentheses and extract the number of the node unit on the washer, which is the required slave node number.

[0030] Step 5: Use *rigidlink to create Rbe2 in batches for the master and slave nodes.

[0031] Furthermore, the present invention further specifies the batch creation of Rbe3 in step 3.3) as follows:

[0032] Step 1: Use *createnode to create master nodes in batches by coordinates, and use *findmarksurs to obtain slave nodes;

[0033] Step 2: Use *createarray$L$arry, *createdoublearray$nodel$darry, and *rbe311$L 1$L$Main_node 1234561 to create Rbe3 in batches.

[0034] Furthermore, the present invention further specifies that in step 3.4), taking sorting by the x-axis direction as an example, the automatic creation of weld seams is as follows:

[0035] Step 1: First, use *findmark to extract the nodes on the weld, and then use hm_getnodeinitialcoords to extract the x-coordinate values ​​of the nodes on the arc.

[0036] Step 2: Set the node number as a variable and assign it to the node x-coordinate value. That is, use the node x-coordinate value as the variable name, and then sort the node x-coordinate values ​​from smallest to largest. Use a foreach loop to iterate through each x-coordinate value variable, replace it with the node number, and then sort.

[0037] Step 3: Use *CE_ConnectorCreateByListAndRealizeWithDetails to automatically create weld connections.

[0038] Furthermore, the present invention further specifies the specific steps of step 3.5) for batch creation as follows:

[0039] Step 1: Use *createmark to obtain the main face nodes, and then use *findmark to obtain the main face mesh cells;

[0040] Step 2: By calling the hm_getclosestnode function, find the nearest node on the subordinate face based on the coordinates of the primary face node, and store these nodes;

[0041] Step 3: Use the *findmark function to locate the mesh containing dependent surfaces based on these nodes;

[0042] Step 4: Depending on the contact type, select TIE or CONTACT to create a contact pair.

[0043] Furthermore, the present invention further specifies the specific process of step 4 as follows:

[0044] 4.1) Automatically import result files and model files;

[0045] 4.2) Automatically extract stress contour maps and displacement contour maps;

[0046] 4.3) Export to create a PPT report.

[0047] By employing the above-described technology, the beneficial effects of the present invention compared to the prior art are as follows:

[0048] This invention employs a defined, automated modeling method for vibration damper finite element models based on Hypermesh secondary development. This method reduces manual operations that previously took hours or days to minutes, enabling "one-click generation" of finite element models. This allows simulation analysis to quickly respond to design changes, significantly accelerating product iteration cycles. It eliminates model discrepancies caused by human factors, ensuring that models built by different projects and engineers adhere to the same high standards, greatly improving the credibility and comparability of simulation results. Furthermore, it frees CAE engineers from tedious and repetitive tasks, allowing them to focus on higher-value simulation result analysis, design optimization, and theoretical research. Attached Figure Description

[0049] Figure 1 This is a schematic diagram of the automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to the present invention;

[0050] Figure 2 This is a system interaction logic diagram of the present invention;

[0051] Figure 3 This is the plugin interface layer of the present invention;

[0052] Figure 4 This diagram illustrates the main functions and implementation methods of preprocessing in a specific embodiment of the present invention.

[0053] Figure 5 This diagram illustrates the main functions and implementation methods of post-processing in a specific embodiment of the present invention.

[0054] Figure 6 This is a diagram illustrating the Hyperview secondary development hierarchy in a specific embodiment of the present invention.

[0055] Figure 7 The image shows a comparison of simulation results between manual and automatic modeling methods under unit force conditions in a specific embodiment of the present invention. The left image represents the manual simulation result, and the right image represents the automatic simulation result. Detailed Implementation

[0056] To make the objectives, advantages, and technical solutions of this invention clearer, the invention will be described in detail below with reference to the accompanying drawings and embodiments. However, it should be understood that the embodiments described below are only for explaining the invention and are not limited to it. The invention will be described in detail below, and through these details, those skilled in the art will fully understand the invention.

[0057] Example: Figures 1-7As shown, this invention takes a certain brand of vibration damper as an example to describe in detail the automatic modeling method of vibration damper finite element model based on Hypermesh secondary development. First, the vibration damper model is imported into Hypermesh. Then, based on TCL / TK language and Hypermesh's own API, Hypermesh is further developed to form an analysis system that automatically builds the vibration damper finite element model, performs automatic structural analysis, and automatically reports simulation results, thus automating the simulation process. Furthermore, using secondary development plugins, automatic mid-surface extraction of thin-walled parts and automatic generation of 2D meshes for thin-walled parts and 3D meshes for solid parts are achieved. Specifically, in the mesh generation stage, the components are first grouped according to identifiers, and then the mesh is automatically generated using the Batchmesh command. The specific process of component grouping is as follows: the component name contains an identifier, for example, the thin-walled component name contains 2d, and the solid component name contains 3d. The 2d and 3d components are grouped by the identifier; Rbe2 and Rbe3 are created in batches, weld points and weld seams are created in batches, contact pairs are created in batches, and working condition stress, load and load analysis steps, and control cards are created in batches to complete the finite element model of the vibration damper. Finally, the secondary development plugin is used to submit the calculation and automatically export the simulation report.

[0058] The system interaction logic of this invention is as follows: Figure 2 As shown, the system consists of three parts: the interface layer, the interaction layer, and the software layer. In... Figure 3 The plugin interface layer, as shown, accepts modeling data input, such as material parameters, weld connection parameters, Rbe2 and Rbe3 connection parameters, and mesh size parameters. In the interaction layer, subroutines are connected via command methods to process these parameters. The processed parameters are then output to the software kernel, interacting with the kernel's API for automated software operations. The interaction layer is divided into pre-processing and post-processing. Pre-processing includes material and property creation, Rbe2 and Rbe3 connection creation, and contact pair creation. Post-processing includes reading simulation results and automatically exporting simulation results as a PowerPoint report. The Hypermesh software layer then performs modeling calculations. After the calculations are complete, the interaction layer reads the user's required data and displays the results. The interaction layer consists of two parts: preprocessing and postprocessing. Its functionality is based on secondary development of the Tcl language in the Hypermesh 2022 Optistruct environment. The preprocessing mainly involves automatic mesh generation for 2D meshes of thin-walled parts and 3D meshes of solid parts; batch creation of Rbe2 and Rbe3, batch creation of weld points and weld seams, batch creation of contact pairs, and batch creation of loads and load analysis steps; the postprocessing is the function of submitting calculations and automatically exporting simulation reports. The specific development process is as follows (I)-(VI):

[0059] (I) Offset Method Mid-Surface Extraction: Mid-surface extraction is a core and crucial preprocessing operation. Its main function is to create ideal neutral geometric surfaces for shell element meshing of thin-walled solid structures. The manual operation involves selecting the surface of the component whose mid-surface needs to be extracted. The function button is located in the midsurface interface of Geom, and its command stream in the command file is *midsurface_extract_10surfaces. It can be used for secondary development to batch extract mid-surfaces of ordinary parts. However, when dealing with components with complex surfaces, it may cause geometric deformation. Compared with the direct extraction method, the offset method for mid-surface extraction can effectively avoid the geometric damage caused by direct mid-surface extraction of some complex surfaces. The specific steps are as follows: Steps 1-4:

[0060] Step 1: Group components by component name, and categorize thin-walled components into one group;

[0061] Step 2: Extract the outer surface of the thin-walled part using *midsurface_edit_base_surfaces and *midsurface_extract_10solids;

[0062] Step 3: Extract component thickness information using regular expressions and calculate the offset distance, i.e., half the thickness is the distance the outer surface needs to be offset.

[0063] Step 4: Use a foreach loop to batch extract and offset the outer surface, use regular expressions to extract the thickness parameter set in componentname, and half of the thickness parameter is the distance to be offset; at the same time, use *setvalue to batch assign the middle surface attributes and material.

[0064] (II) Batch Creation of Rbe2: In HyperMesh, Rbe2 (Rigidbody element 2) is a rigid element whose core function is to create rigid connections or constraints in the model. It forces these nodes to move like a rigid connection by defining a master node and one or more slave nodes, and can be used to simulate bolted connections between the outer and inner supports of a vibration damper. Creating an Rbe2 requires first defining a master node, then defining multiple slave nodes. The master node is generally the center of the circular hole, and the slave nodes are generally nodes on the washer around the circular opening. The specific steps are shown in steps 1-5 below:

[0065] Step 1: The main node originates from the center of the hole and is created in batches using *createnode with the coordinates of the center.

[0066] Step 2: Starting from the nodes on the circular hole washer, use a foreach loop to find a certain node on the hole, and denote it as node 'a'. Use hm_holedetectionidentifyhole to get the number of the hole containing node 'a', and denote it as hole 'a'.

[0067] Step 3: Then, obtain the washer number contained in hole a and the node number on the washer by using hm_holedetectiongetwasherelementslist;

[0068] Step 4: Since the node information on the washer obtained in Step 3 contains parentheses, first use split to separate the parentheses and extract the number of the node unit on the washer, which is the required slave node number.

[0069] Step 5: Use *rigidlink to create Rbe2 in batches for both master and slave nodes;

[0070] (III) Batch Creation of Rbe3: Rbe3 is a flexible multi-point constrained element. Its core function is to distribute loads or motions from a master node to a group of slave nodes in a weighted average manner (following the least squares principle), or conversely, to couple the motions of a group of slave nodes to a master node, while minimizing the increase in local stiffness of the model. It is mainly used to simulate concentrated forces or moments. The specific steps are shown in steps 1-2 below:

[0071] Step 1: Use *createnode to create master nodes in batches by coordinates, and use *findmarksurs to obtain slave nodes;

[0072] Step 2: Use *createarray$L$arry, *createdoublearray$nodel$darry, and *rbe311$L 1$L$Main_node 1234561 to create Rbe3 in batches; the following conditions must be met: $L is the number of slave nodes; $arry is a list whose loop count equals the number of slave nodes and repeats from 1 to 3; $darry is a list whose loop count equals the number of slave nodes and repeats from 1; $Main_node is the master node number. Using a for loop and lappend, with the number of slave nodes as the loop limit, create $L lists that repeat from 1 to 3. The creation of $darry is similar.

[0073] (IV) Automatic Weld Creation: Welds and weld points are key technologies for simulating the connections of thin-walled structures (such as automobile bodies, aircraft skins, sheet metal parts, etc.). Their role is to accurately and efficiently simulate the mechanical behavior of real welded connections in the finite element model, ensuring effective load transfer between components while balancing computational accuracy and efficiency. Weld point creation in secondary development uses a foreach loop for batch creation; weld creation is more complex than weld point creation. In secondary development, weld nodes need to be arranged in spatial order. For example, nodes on an arc must be selected in a clockwise or counterclockwise spatial order; otherwise, the created weld will have mesh deformation. However, there is currently no API for clockwise sorting; sorting by the x-axis, y-axis, or z-axis is the only option. Taking sorting by the x-axis as an example, the specific steps are shown in steps 1-3 below:

[0074] Step 1: First, use *findmark to extract the nodes on the weld, and then use hm_getnodeinitialcoords to extract the x-coordinate values ​​of the nodes on the arc and store them as a list;

[0075] Step 2: Assign the node number as a variable to the node x-coordinate value, that is, use the node x-coordinate value as the variable name, and then sort the node x-coordinate values ​​from smallest to largest. By iterating through each x-coordinate value variable with a foreach loop and replacing it with the node number, the nodes are sorted to obtain a list of node numbers sorted from smallest to largest along the x-axis.

[0076] Step 3: Use *CE_ConnectorCreateByListAndRealizeWithDetails to automatically create weld connections in batches from the sorted list of node numbers;

[0077] (V) Batch Creation of Contact Pairs: Contact pairs are a core tool in finite element analysis for simulating complex interactions between components. Their function is to define the boundary conditions for the mechanical behavior of two or more components when they may come into contact, separate, slide, or rub under load. The process of creating contact pairs is as follows: Figure 4 As shown. The master face is usually an easily selectable face mesh, while manually selecting subordinate faces, which are difficult to select, is time-consuming. To solve this problem, this invention proposes a method for obtaining subordinate face meshes from the master face mesh, the specific steps of which are shown in steps 1-4 below:

[0078] Step 1: Use *createmark to obtain the main face node, and use *findmark to obtain the mesh cells around the main face node;

[0079] Step 2: By calling the hm_getclosestnode function, find the nearest node on the subordinate surface based on the coordinates of the primary surface node, and store it as a list of subordinate nodes;

[0080] Step 3: Use the *findmark function to locate the mesh containing dependent faces based on these node lists;

[0081] Step 4: Based on the actual contact situation, select TIE for connection under fully bonded conditions; select CONTACT for connection under conditions of relative friction to create contact pairs; Steps (I) to (V) above are the main functions and implementation methods of preprocessing, which can basically complete the construction of the finite element model of the vibration damper. The flowchart is as follows: Figure 4 As shown.

[0082] Taking a specific working condition as an example, the force conditions of each part of the vibration damper are shown in Table 1. Forces and moments in the x, y, and z directions can be created using `loadcreateonentity_curve nodes`. Multiple different forces and moments can be automatically created simply by modifying the parameters. Because this working condition analysis is under inertial release conditions, control cards for inertial release also need to be created. An automatic constraint command can be created using `*attributeupdatestring cards`, and then analysis steps can be created and the calculation submitted using `loadstepscreate`.

[0083] Table 1. Stress conditions of the vibration damper under certain working conditions.

[0084]

[0085] (vi) Automatic Export of Simulation Reports: In the post-processing stage, we developed an automated workflow based on the Tk / Tcl scripting language. This workflow automatically imports the model and simulation results, extracts stress and displacement contour maps, and automatically generates the analysis report, which is then exported as a PPT report. The flowchart is shown below. Figure 5 As shown. Hyperview's secondary development is based on the Hyperview interface framework, dividing Hyperview into various layers, such as... Figure 6 As shown, we need to obtain the handle to the higher level through code and API in order to perform the operations we need under that handle. Specifically:

[0086] 4.1) Taking GetSessionHandle as an example, this command can obtain the handle of the current session, such as... Figure 6 As shown, client privileges can be obtained layer by layer in the same way;

[0087] 4.2) At the client level, result files and model files can be automatically imported using the AddModel and SetResult commands;

[0088] 4.3) Similarly, under the ContourCtrl handle, the contour plot type can be set using SetDataType, and under the Measure handle, the maximum value position can be displayed using SetVisibility, thus enabling automatic extraction of stress contour plots and displacement contour plots;

[0089] 4.4) Under the PPTPublish handle, the simulation report is automatically exported by specifying the PPT template of the simulation report through templatepath.

[0090] Through process automation, the efficiency of simulation modeling and simulation reporting has been greatly improved. As shown in Table 2, the simulation time has been reduced from 60 minutes to 10 minutes, and... Figure 7 The simulation results of manual and automatic modeling in the x-direction under unit force conditions show that the maximum stress areas of the two are basically the same, and the maximum stress values ​​are on the same order of magnitude, which also ensures the accuracy of this secondary development.

[0091] Table 2. Comparison of manual and automatic modeling and simulation times

[0092]

Claims

1. An automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development, characterized in that... The method uses a secondary development plugin to automatically build a finite element model of an automotive shock absorber and perform simulation analysis of the shock absorber under different working conditions. Specifically, it includes importing the 3D model of the shock absorber, automatically extracting the mid-surface of thin-walled parts, automatically generating 2D meshes for thin-walled parts and 3D meshes for solid parts, batch creating Rbe2 and Rbe3, batch creating weld points and weld seams, batch creating contact pairs, and batch creating loads and load analysis steps. Submit the calculation and automatically export the simulation report.

2. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 1, characterized in that... Includes the following steps: Step 1: Import the 3D model of the vibration damper; Step 2: Perform secondary development of Hypermesh based on TCL / TK language and Hypermesh API to automate the simulation process; Step 3: Using secondary development plugins, automatically extract the mid-surface of thin-walled parts, automatically generate 2D meshes for thin-walled parts and 3D meshes for solid parts; batch create Rbe2 and Rbe3, batch create weld points and weld seams, batch create contact pairs, batch create working condition stress, load and load analysis steps, and control cards to complete the finite element model of the vibration damper. Step 4: Use the secondary development plugin to submit the calculation and automatically export the simulation report.

3. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 1, characterized in that... The specific process of step 3 is as follows: 3.1) Mid-surface extraction of thin-walled parts: Mid-surface extraction adopts the offset method. The offset distance is extracted and calculated by TCL / TK language, and then the outer surface is extracted for offset mid-surface extraction. 3.2) Mesh generation: In the mesh generation stage, the components are first grouped according to the identifiers, and then the mesh is automatically generated using the Batchmesh command; 3.3) Batch creation of Rbe2 and Rbe3: Obtain the master and slave nodes of Rbe2 and Rbe3 through code, and create them in batches; 3.4) Batch creation of weld points and weld seams: Extract weld point node information and create weld points in batches using a foreach loop; extract weld seam nodes and automatically create weld seams by the user selecting spatial order based on the x, y, or z axis. 3.5) Batch creation of contact pairs: First, obtain the main face node information, then obtain the secondary face nodes through the main face nodes, and create contact pairs in batches according to the contact pair type; 3.6) Batch creation of loads and load analysis steps.

4. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... The specific steps for extracting the mid-surface of the thin-walled part in step 3.1) are as follows: Step 1: Extract the outer surface of the thin-walled part using *midsurface_edit_base_surfaces and *midsurface_extract_10solids; Step 2: Use regular expressions to extract the thickness parameter set in componentname. Half of the thickness parameter is the distance to be offset. Step 3: Offset the plane using *offset_surfaces_and_modify surfaces.

5. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... The specific steps for batch creation of Rbe2 in step 3.3) are as follows: Step 1: The main node originates from the center of the hole and is created in batches using *createnode with the coordinates of the center. Step 2: Starting from the nodes on the circular hole washer, use a foreach loop to find a certain node on the hole, and denote it as node 'a'. Use hm_holedetectionidentifyhole to get the number of the hole containing node 'a', and denote it as hole 'a'. Step 3: Then, obtain the washer number contained in hole a and the node number on the washer by using hm_holedetectiongetwasherelementslist; Step 4: Since the node information on the washer obtained in Step 3 contains parentheses, first use split to separate the parentheses and extract the number of the node unit on the washer, which is the required slave node number. Step 5: Use *rigidlink to create Rbe2 in batches for the master and slave nodes.

6. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... Step 3.3) involves batch creation of Rbe3 as follows: Step 1: Use *createnode to create master nodes in batches by coordinates, and use *findmarksurs to obtain slave nodes; Step 2: Use *createarray$L$arry, *createdoublearray$nodel$darry, and *rbe311$L 1$L$Main_node 1234561 to create Rbe3 in batches.

7. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... In step 3.4), taking sorting by the x-axis as an example, the automatic creation of weld seams is as follows: Step 1: First, use *findmark to extract the nodes on the weld, and then use hm_getnodeinitialcoords to extract the x-coordinate values ​​of the nodes on the arc. Step 2: Set the node number as a variable and assign it to the node x-coordinate value. That is, use the node x-coordinate value as the variable name, and then sort the node x-coordinate values ​​from smallest to largest. Use a foreach loop to iterate through each x-coordinate value variable, replace it with the node number, and then sort. Step 3: Use *CE_ConnectorCreateByListAndRealizeWithDetails to automatically create weld connections.

8. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... Step 3.5) The specific steps for batch creation are as follows: Step 1: Use *createmark to obtain the main face nodes, and then use *findmark to obtain the main face mesh cells; Step 2: By calling the hm_getclosestnode function, find the nearest node on the subordinate face based on the coordinates of the primary face node, and store these nodes; Step 3: Use the *findmark function to locate the mesh containing dependent surfaces based on these nodes; Step 4: Depending on the contact type, select TIE or CONTACT to create a contact pair.

9. The automatic modeling method for finite element models of vibration dampers based on Hypermesh secondary development according to claim 3, characterized in that... The specific process of step 4 is as follows: 4.1) Automatically import result files and model files; 4.2) Automatically extract stress contour maps and displacement contour maps; 4.3) Export to create a PPT report.

Images