Rubber bushing parametric modeling and rapid plotting system based on CATIA

Abstract

A rubber bushing parameterization modeling and rapid plotting system based on CATIA comprises the following steps that firstly, all template files of a rubber bushing are established based on CATIA modeling software, and all the template files are stored in a resource folder; 2, establishing a CATScript script file through VBA secondary development, starting a CATIA application through the script file, and modifying an assembly template file, a component template file and an engineering drawing template file in a current folder according to a parameter list template file in the current folder where the script file is located; thirdly, an AutoDrawing application is developed based on VB for a user to input lining parameters and a lining storage path, template files and script files in the resource folder are copied to the input storage path, and parameters of the parameter list template files in the storage path are modified according to the lining parameters; and 4, running the script file copied in the step 3, starting CATIA, automatically generating a model and a drawing of the rubber bushing, and reducing the working difficulty of engineering personnel.

Description

TECHNICAL FIELD

[0001] The application relates to a modeling and drawing system of a rubber bushing, in particular to a CATIA-based parameterized modeling and rapid drawing system of a rubber bushing. BACKGROUND

[0002] As a core flexible connecting piece of an automobile suspension system, a power assembly suspension and a chassis transmission, the rubber bushing has developed from a single shock absorption and buffering function to an intelligent element with multi-physical field coupling. While bearing alternating loads and attenuating high-frequency vibrations, the rubber bushing also needs to accurately control the stiffness matching between subsystems, and the dynamic characteristics directly affect the NVH performance (noise, vibration and harshness) and handling stability index of the whole vehicle. According to statistics, the use amount of rubber bushings of a single medium and high-end passenger vehicle has exceeded 40, which involves 18 key positions such as engine suspension, control arm bushing and stabilizer link.

[0003] With the acceleration of the automobile industry towards electrification and intelligentization, the product development cycle of the rubber bushing is compressed to 1 / 3 of the traditional cycle, which puts higher requirements on the product development efficiency of the bushing manufacturer. In the traditional forward development process, the CAD modeling and engineering drawing of a single bushing in the early stage accounts for about 35% of the overall development cycle, and in order to make the product meet the specified performance and meet the durability requirements and industrialization specifications, several iterations are still needed on the basis of the initial model. The cumbersome steps of product modeling and drawing engineering drawings have become a major obstacle to improving the development efficiency of the rubber bushing.

[0004] In order to improve the modeling efficiency, the current industry generally adopts parameterized modeling technology, which can realize the rapid generation of basic configurations under certain conditions. By developing the existing software functions, a software or method that can realize product parameterized design and auxiliary engineering drawing marking is developed, which is also a hot spot in the field of mechanical manufacturing industry.

[0005] For example, the patent application with the publication number CN 114462111 A and the publication date of May 10, 2022 discloses a CATIA-based tire engineering drawing automatic marking method, device, medium and program. The method creates a tire contour, pattern and sidewall parameterized template through a CATIA software design platform, and exports a CATDrawing engineering drawing drawing. Then, the engineering drawing automatic marking is realized by creating an engineering drawing template file and CAA secondary development, and the elements of the engineering drawing drawing are automatically divided into layers according to the color of the model elements. This method can improve the marking efficiency of the engineering drawing drawing, and can standardize the marking of the same pattern series drawing. However, this method of reading and re-marking the size marking at different positions through CAA has certain limitations, such as low universality, complicated development adaptation process and high software environment requirements. SUMMARY

[0006] The present application aims at the problem of low efficiency of current rubber bushing design tool, and provides a CATIA-based rubber bushing parameterized modeling and rapid drawing system, which realizes automatic generation of a whole process from a three-dimensional model to an engineering drawing by constructing a multi-level parameter driving architecture through CATIA VBA secondary development technology.

[0007] The technical means adopted by the present application to solve the above problem is a CATIA-based rubber bushing parameterized modeling and rapid drawing system, which comprises the following steps: first, based on the CATIA modeling software, establishing a rubber bushing assembly template file, a separate part template file, an engineering drawing template file and a parameter list template file, and saving the above template files to a resource folder; second, establishing a CATScript script file through VBA secondary development and saving it to the resource folder in the first step, starting the CATIA application through the script file, and modifying the assembly template file, the separate part template file and the engineering drawing template file in the current folder according to the parameter list template file in the current folder; third, developing an AutoDrawing application based on VB and saving it to the resource folder in the first step, inputting the bushing parameters and the bushing saving path by the user, copying each template file and script file in the resource folder to the input saving path, and modifying the parameters of the parameter list template file in the saving path according to the bushing parameters; fourth, running the script file copied to the saving path in the third step, starting CATIA, and automatically generating the separate part model, the assembly model and the engineering drawing of the rubber bushing.

[0008] Further, in the first step, the parameter list template file is stored as a txt file.

[0009] Further, in the second step, the specific operation comprises: One: starting the CATIA application through CreateObject("CATIA.Application"); Two: opening the parameter list template file in the current folder in read-only mode through Set file = fso.OpenTextFile("path", 1); Three: after assigning each parameter value in the parameter list template file in the current folder to each separate part, updating the separate part template file; Four: measuring the volume of each part and calculating the mass of each part according to the material type; Five: updating the assembly template file according to the updated separate part template file; Six: updating the engineering drawing template file according to the updated assembly template file.

[0010] Further, in the second step, the operation of modifying the names of the assembly template file, the part template file and the drawing template file in the resource folder to the names of the assembly template file, the part template file and the drawing template file saved in the first step is further included. After the template files are modified to the original names, CATIA will automatically establish the links between the part template file and the assembly template file and between the assembly template file and the drawing template file.

[0011] Specifically, the names of the part template file, the assembly template file and the drawing template file in the resource folder are modified by fso.MoveFile A’, A, where A’ is the resource folder path + the current part template file name, or the resource folder path + the current assembly template file name, or the resource folder path + the current drawing template file name, and A is the resource folder path + the part template file name in the first step, or the resource folder path + the assembly template file name in the first step, or the resource folder path + the drawing template file name in the first step.

[0012] Further, in the second step, the operation of re-establishing the links between the part template file and the assembly template file and between the assembly template file and the drawing template file in the current folder is further included.

[0013] Further, in the second step, the specific operation further includes: Two seven: modifying the names of the assembly template file, the part template file and the drawing template file in the current folder; (after the modification to the new names, CATIA will automatically disconnect the links between the new bushing part, the assembly and the drawing) Specifically, the names of the part template file, the assembly template file and the drawing template file in the resource folder are modified by fso.MoveFile B, B’, where B is the current folder path + the current part template file name, or the current folder path + the current assembly template file name, or the current folder path + the current drawing template file name, and B’ is the current folder path + the modified part template file name, or the current folder path + the modified assembly template file name, or the current folder path + the modified drawing template file name.

[0014] Two eight: re-establishing the links between the assembly template file, the part template file and the drawing template file after the name modification.

[0015] Specifically, the modified assembly template file and the sub-part template file in the current folder are opened in sequence by documents1.Open("path + name"), wherein the "path" is the path of the current folder, and the "name" is the name of the assembly template file or the name of the sub-part template file. The assembly set is obtained by Set product1 = productDocument1.Product; Set products1 = product1.Products. All links of the sub-parts in the assembly template file are modified in sequence by Set product2 = products1.Item("Part1.1"); Set product3 = partDocument1.GetItem("Part1"); Set product2 = products1.ReplaceProduct(product2, product3, False).

[0016] Further, in the third step, the operation of checking the input bushing parameters is further included.

[0017] Further, in the third step, after the template files and the script files in the resource folder are copied to the input saving path, the operation of modifying the names of the assembly template file, the sub-part template file and the engineering drawing template file in the resource folder is further included. After the names of the assembly template file, the sub-part template file and the engineering drawing template file in the resource folder are modified, the assembly template file, the sub-part template file and the engineering drawing template file in the saving path are automatically linked.

[0018] Further, in the third step, the specific operation includes: Three one: obtaining the resource folder path; Three two: after the user inputs the bushing parameters and the bushing saving path, it is judged whether the input of the bushing parameters is reasonable; Specifically, all the parameter values input by the user in the text box are obtained in sequence by A = CDbl(NumericUpDown1.Text). The obtained parameter values are comprehensively judged to ensure that the correct bushing model can be generated. If the parameter input is unreasonable, an error prompt is popped up until all the parameter inputs are correct.

[0019] Three three: copying the template files and the script files in the resource folder to the input saving path; Specifically, the file in the resource folder is copied to the save path by File.Copy(Path1, Path2, True), where Path1 is the resource folder path, and Path2 is the user-selected save path.

[0020] Three four: modify the assembly template file, part template file, and engineering drawing template file names in the resource folder. Specifically, the ligand template file, part template file, and engineering drawing template file names in the resource folder are modified by File.Move(filename1, filename2), where filename1 is the original assembly template file name, or part template file name, or engineering drawing template file name, and filename2 is the modified assembly template file name, or part template file name, or engineering drawing template file name.

[0021] Three five: modify the parameters in the parameter list template file in the current folder according to the user inputted bushing parameters. Three six: add the user inputted save path to the script file.

[0022] Specifically, the CATScript in the current folder is changed to txt format by Path.ChangeExtension(A, ".txt") (where A is the CATScript file in the save path, i.e., the script file in the current folder); Read all characters in txt by File.ReadAllLines(A); Iterate through the lines of txt by For i = 0 To fileLines.Length – 1; Find the variable line corresponding to the resource folder by If fileLines(i).StartsWith("currentDirectory = ") Then fileLines(i) = "currentDirectory = " &Path1, and write Path1 (where Path1 is the resource folder path) to this line; Similarly, write this line by If fileLines(i).StartsWith("targetPath = ") Then fileLines(i) = "targetPath = " &Path2 (where Path2 is the user-selected save path); Refresh the modification by updated = True; ChangeExtension(A, ".CATScript") to change txt back to CATScript format.

[0023] The beneficial effects of the present application are: 1. The software system of the present application integrates rubber bushing size information inspection, part and assembly three-dimensional model automatic generation, engineering drawing automatic generation, can simplify the work steps of CAD engineers, is conducive to improving the development efficiency of products. Can greatly reduce the development difficulty, and also simplify the operation steps of users.

[0024] 2. The software of the present application runs by modifying the CATScript file, does not directly connect with CATIA, so it is not only suitable for the case that CATIA is installed locally, but also suitable for the case that CATIA is installed on a cloud server, can avoid the case that CATIA is installed on a cloud server and users cannot run CAA, VBA plug-ins, and broaden the use scene of the software.

[0025] 3. In the future, if it is needed to adapt other kinds of bushings, such as bushings with bumps, bushings with holes, etc., only the model and engineering drawing template need to be modified, and the part of code related to bushing parameter transmission needs to be modified, and finally the GUI needs to be redesigned, which lays a good foundation for realizing automatic modeling and drawing of more complex bushings and even TOP Mount in the future. BRIEF DESCRIPTION OF DRAWINGS

[0026] Figure 1 The figure is a schematic diagram of the part template file in step 1 of the embodiment; Figure 2 The figure is a schematic diagram of the assembly template file in step 1 of the embodiment; Figure 3 The figure is a schematic diagram of the engineering drawing template file in step 1 of the embodiment; Figure 4 The figure is a schematic diagram of the parameter list template file in step 1 of the embodiment; Figure 5 The figure is a schematic diagram of the input interface when the user of the embodiment operates; Figure 6 The figure is a schematic diagram of the files in the current folder during the operation process of the user of the embodiment; Figure 7 The figure is a schematic diagram of the automatically generated model and drawing when the user of the embodiment operates; Figure 8 The figure is a schematic diagram of the system running process of the embodiment; Figure 9 The figure is a schematic diagram of the user operation process of the embodiment. DETAILED DESCRIPTION

[0027] The application will be further described below with reference to the drawings. The drawings are only used for exemplary description, and the representation is only a schematic diagram, not a physical diagram, and cannot be understood as a limitation on the patent; in order to better illustrate the embodiments of the application, some components in the drawings will be omitted, enlarged or reduced, and do not represent the size of the actual product; it is understandable for those skilled in the art that some well-known structures and their descriptions in the drawings can be omitted. Embodiment one

[0028] A CATIA-based rubber bushing parameterized modeling and rapid drawing system, as shown in Figure 8 , specifically comprises the following steps: Step 1: based on CATIA parameterized modeling, obtain the rubber bushing three-dimensional model template file and engineering drawing template file; Step 1.1: based on CATIA modeling software, establish rubber bushing sub-assembly template files through parameterized modeling method; Step 1.1.1: based on CATIA modeling software, model the rubber bushing sub-assembly through parameterized modeling method, as shown in Figure 1 ; Step 1.1.2: assemble the sub-assembly template file to obtain the rubber bushing assembly, as shown in Figure 2 ; Step 1.2: based on CATIA, make engineering drawings for the assembly template file, as an engineering drawing template file; Step 1.2.1: project the assembly template file in the existing standardized frame, establish necessary projection views, sectional views, partial views, etc., to ensure that the views can reflect all geometric features of the rubber bushing assembly; Step 1.2.2: make necessary dimension marks for each view, and add BOOM table to perfect material information, weight and other technical requirements, as an engineering drawing template file, as shown in Figure 3 ; Step 1.3: all parameters involved in the modeling process of the rubber bushing sub-assembly template file and the material type of the sub-assembly are sorted into a TXT file, and the parameter name and value are separated by a TAB symbol, as a parameter list template file; Step 1.4: as shown in Figure 4 , store the rubber bushing assembly template file, sub-assembly template file, engineering drawing template file and parameter list template file to the resource folder; Step 2: establish a CATScript script file through VBA secondary development and save it in the resource folder; Step 2.1: Start CATIA application by CreateObject("CATIA.Application"); Step 2.2: Read parameter list template file (TXT file) in the associated path in the script file, and assign the parameters involved in the bushing modeling to the variables; (When establishing the script file, the first associated path in the script file is the resource folder) Step 2.2.1: Open the parameter list template file in the current path in read-only mode by Set file = fso.OpenTextFile("path", 1); Step 2.2.2: Traverse all lines of the parameter list template file from top to bottom by Do While Not file.AtEndOfStream--Loop; Step 2.2.3: In the process of traversal, separate the parameter name and value by Tab key by InStr(line, vbTab) > 0, and get the parameter name by Trim(Split(line, vbTab)(0)) and the parameter value and material string by Trim(Split(line, vbTab)(1)); Step 2.2.4: Close the parameter list template file by file.Close; Step 2.3: Modify the part parameters according to the read parameters; Step 2.3.1: Open the part template file in CATIA by CATIA.Documents.Open("path"), where the path is the associated path in the script file; Step 2.3.2: Get the current part Part by Set partDocument1 = catia.ActiveDocument; Set part1 = partDocument1.Part; Step 2.3.3: Identify the parameter name of the current Part by parameters1.Item("parameter name"), and assign the corresponding parameter value obtained from the parameter list template file to the Part by length1.ValuateFromString("parameter value"); Step 2.3.4: After reassigning all parameters of this part, update the part by part1.Update; Step 2.4: Calculate the weight of the part according to the read material type; Step 2.4.1: Get the part geometry by part1.CreateReferenceFromObject(part1.MainBody); Step 2.4.2: Obtain the measurement tool using partDocument1.GetWorkbench("SPAWorkbench"); Step 2.4.3: Measure the volume of the part geometry using GetMeasurable(); Step 2.4.4: Calculate the mass of the part using the formula Mass = Volume * Density; Step 2.5: Save this part using partDocument1.Save; Step 2.6: Return to Step 2.3 until all component parameters of the bushing have been modified and the quality has been measured before proceeding to the next step; Step 2.7: Update the parts in the assembly template file; Step 2.7.1: Open the assembly file at the specified path using documents1.Open("path"). Since the names of the sub-parts have not changed, CATIA will automatically update the assembly file, where the path is the path associated with the script file. Step 2.7.2: After obtaining the current assembly through CATIA.ActiveDocument, save the assembly file through productDocument1.Save; Step 2.8: Update the dimensions and BOM of the engineering drawing template file; Step 2.8.1: Open the drawing template file at the specified path using documents1.Open("path"), where the path is the path associated with the script file; Step 2.8.2: Obtain the currently active drawing using the code Set DrawingDoc = CATIA.ActiveDocument; SetDrawingSheets = DrawingDoc.Sheets; Set DrawingSheet =DrawingSheets.ActiveSheet; Step 2.8.3: Since the name of the assembly has not changed, the link between the drawing and the assembly does not need to be changed. All dimensions in the drawing can be updated directly through DrawingSheet.Update; Step 2.8.4: Obtain the currently active view using drawingDoc.Sheets.Item(1).Views.ActiveView; Step 2.8.5: Fill the material name and the weight of the subpart calculated in step 2.4.4 into the BOM by drawingView.Texts.Add ("text", x, y) (x, y represent the coordinates of the text box); Step 2.8.6: Save the drawing template file by DrawingDoc.Save; Step 2.9: Reestablish the link between the subpart template and the assembly template, and the link between the assembly template and the drawing template; Step 2.9.1: Close the opened subpart, assembly and drawing in CATIA by Document.Close; Step 2.9.2: Modify the names of the subpart template file, assembly template file and drawing template file in the resource folder in step 1.4 by fso.MoveFile A', A, where A' is the resource folder path + the current file name, and A is the resource folder path + the file name saved in step 1 (after modifying the template file to the original name, CATIA will automatically establish the link between the subpart template and the assembly template, and the link between the assembly template and the drawing template); Step 2.10: Reestablish the link between the new bushing part and the assembly; Step 2.10.1: Modify the names of the new bushing part template file, assembly template file and drawing template file by fso.MoveFile B, B', where B is the folder path associated with the script file + the current file name, and B' is the folder path associated with the script file + the modified file name (after modifying to the new name, CATIA will automatically disconnect the link between the new bushing part, assembly and drawing); Step 2.10.2: Open the modified names of the new bushing part and assembly by documentsl.Open ("path + name") in turn; Step 2.10.3: Get the assembly collection by Set productl = productDocumentl.Product; Set productsl = productl.Products; Step 2.10.4: Modify the link of all sub-parts in assembly one by one by Set product2 = products1.Item("Part1.1"); Set product3 = partDocument1.GetItem("Part1"); Set product2 = products1.ReplaceProduct(product2, product3, False); Step 2.10.5: Get the current active assembly by Set productDocument1 = CATIA.ActiveDocument, and save the assembly by productDocument1.Save.

[0029] Step 3: Develop AutoDrawing application based on VB, save the resource folder in the same path, realize the collection of new bushing parameters, the update of parameter list template file and the modification of key code in CATScript script file; Step 3.1: Get the path of resource folder. Get the link of AutoDrawing application by Directory.GetCurrentDirectory, the resource folder is stored in the same location as the application, so the path of the resource folder is "Directory.GetCurrentDirectory" + "ReferenceData"; Step 3.2: Add click event in <Check Parameters> button to check the new bushing size parameters input by user; Step 3.2.1: User inputs the size and material of all parts, and clicks the check button; Step 3.2.2: Get all parameter values input by user in text box one by one by A = CDbl(NumericUpDown1.Text); Step 3.2.3: Make all-round judgment on the obtained parameter values to ensure that the correct bushing model can be generated. For example, the inner diameter of the bushing outer tube is E, the outer diameter of the bushing outer tube is D, and the judgment statement under the condition of the working condition is If E>D Then MessageBox.Show("Reduce the inner diameter E of the outer tube, make it less than the outer diameter D of the outer tube"), if the inner diameter of the outer tube is greater than the outer diameter of the outer tube, which is obviously incorrect, then a window is popped up to prompt the user to reduce the inner diameter E of the outer tube, and the user re-enters; Step 3.2.4: User clicks <Check Parameters> button again, returns to step 3.2.2, until the window pops up in step 3.2.3 to prompt that the parameter input is correct; Step 3.3: In <select path>Add a single-click event to the button to obtain the save path; Step 3.3.1: Call the storage path selection dialog box through Dim folderDialog As New FolderBrowserDialog(); Step 3.3.2: Through the conditional statement If folderDialog.ShowDialog() = DialogResult.OK; Then txtFolderPath.Text = folderDialog.SelectedPath; End If, the save path is displayed in the upper text box when the user selects the path and determines; Step 3.4: Add a single-click event to the button to update the parameter list and modify the CATScript script file, so that the CATScript script file can automatically generate new rubber bushing sub-parts, assemblies and engineering drawings; Step 3.4.1: Copy the template file to the save path by File.Copy(Path1, Path2, True), where Path1 is the resource folder path obtained in step 3.1, and Path2 is the save path selected by the user in step 3.3; The path of the copied part is the part path opened by CATIA in step 2.3.1, that is, the associated path in the script file; Step 3.4.2: Rename the assembly template file, sub-part template file and engineering drawing template file in the resource folder by File.Move(filename1, filename2); At this time, the sub-parts, assemblies and engineering drawings copied to the save path in step 3.4.1 will be automatically linked; Step 3.4.3: Modify the parameter list template file in the save path, so that its parameter value is modified to the parameter input by the user, and the part material type is modified to the material selected by the user: read each line of the parameter list file by File.ReadAllLines(A).ToList (A is the parameter list template file path, that is, the save path + Parameter.txt); Through For i = 0 To lines.Count – 1, each line is traversed; Through Dim fields = lines(i).Split(vbTab), each line is divided by the Tab symbol; In the traversal process, through the condition If fields(0) = parameterNames(j) Then fields(1) = newValues(j); j = j + 1, the parameter name or part name is judged, and the parameter value corresponding to the parameter name and the material corresponding to the part are modified to the input value in step 3.2.1; Through lines(i) = String.Join(vbTab, fields) will re-splice the modified line into a string; until all the parameter values of the parameter list file are modified; the modified parameter list template file is the parameter list template file read in step 2.2.1; step 3.4.4: add the resource folder path obtained in step 3.1 and the save path selected by the user in step 3.3 to the CATScript script file. Change the CATScript copied in step 3.4.1 to a txt file format through Path.ChangeExtension(A, ".txt") (A is the path of the CATScript file in the save path); read all characters of the txt file through File.ReadAllLines(A); perform line-by-line traversal of the txt file characters through For i = 0 To fileLines.Length – 1; find the variable line corresponding to the resource folder through If fileLines(i).StartsWith("currentDirectory =") Then fileLines(i) = "currentDirectory = " &Path1 and write Path1 (the resource folder path obtained in step 3.1) to this line; similarly, write this line through If fileLines(i).StartsWith("targetPath = ") Then fileLines(i) = "targetPath = " &Path2 (Path2 is the save path selected by the user in step 3.3); refresh the modification through updated = True; change the txt back to the CATScript format through Path.ChangeExtension(A, ".CATScript"); step 4: run the CATScript script file in the save path input in step 3 to start CATIA and automatically generate the sub-assembly model, assembly model and engineering drawing of the rubber bushing.

[0030] As shown in FIG. 9, the specific operation steps of the user are as follows: step 1): double-click to run the AutoDrawing application; step 2): as shown in FIG. 5, input the size parameters and materials of the rubber bushing part; step 3): click the button, if the prompt shows that the size is correct, proceed to step 4, if the prompt shows that the size is incorrect, modify the corresponding parameter value in step 2) according to the error information; step 4): click.< / select> button, and select the output path in the pop-up dialog box; Step 5): Click <generate>button, the output path will appear as shown in Figure 6 the following file; Step 6: Run the CATScript script file generated in the output path, at this time CATIA starts, as shown in Figure 7 the rubber bushing part model, assembly model and engineering drawing with dimension and BOOM list are automatically generated.

[0031] The above examples are only for illustrating the present application, and are not limited to the present application. Those skilled in the art can make various changes or modifications without departing from the spirit and scope of the present application. Therefore, all equivalent technical solutions should belong to the protection scope of the present application, and the protection scope of the present application should be defined by the claims.< / generate>

Claims

1. A CATIA-based rubber bushing parameterized modeling and rapid drawing system, characterized in that: The method comprises the following steps: first, based on CATIA modeling software, establishing rubber bushing assembly template file, sub-assembly template file, engineering drawing template file, parameter list template file, and saving the above template files to the resource folder; second, establishing CATScript script file through VBA secondary development and saving to the resource folder in the first step, starting CATIA application through the script file, modifying the assembly template file, sub-assembly template file and engineering drawing template file in the current folder according to the parameter list template file in the current folder; third, developing AutoDrawing application based on VB and saving to the resource folder in the first step, inputting bushing parameters and bushing saving path for the user, copying each template file and script file in the resource folder to the input saving path, and modifying the parameters of the parameter list template file in the saving path according to the bushing parameters; fourth, running the script file copied to the saving path in the third step, starting CATIA, and automatically generating the sub-assembly model, assembly model and engineering drawing of the rubber bushing.

2. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 1, wherein: In the first step, the parameter list template file is stored as a txt file.

3. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 1, wherein: In the second step, the specific operation comprises: Two one: starting CATIA application through CreateObject("CATIA.Application"); Two two: opening the parameter list template file in the current folder in read-only mode through Set file = fso.OpenTextFile("path", 1); Two three: after assigning each parameter value in the parameter list template file in the current folder to each sub-assembly, updating the sub-assembly template file; Two four: measuring the volume of each part and calculating the mass of each part according to the material type; Two five: updating the assembly template file according to the updated sub-assembly template file; Two six: updating the engineering drawing template file according to the updated assembly template file.

4. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 1, wherein: In the second step, it also includes the operation of modifying the names of the assembly template file, sub-assembly template file and engineering drawing template file in the resource folder to the names of the assembly template file, sub-assembly template file and engineering drawing template file saved in the first step.

5. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 4, wherein: The names of the sub-assembly template file, assembly template file and engineering drawing template file in the resource folder are modified through fso.MoveFile A', A, wherein A' is the resource folder path + the current sub-assembly template file name, or the resource folder path + the current assembly template file name, or the resource folder path + the current engineering drawing template file name, and A is the resource folder path + the sub-assembly template file name in the first step, or the resource folder path + the assembly template file name in the first step, or the resource folder path + the engineering drawing template file name in the first step.

6. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 4, wherein: In the second step, it also includes the operation of re-establishing the link between the sub-assembly template file and the assembly template file in the current folder, and the link between the assembly template file and the engineering drawing template file.

7. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 6, wherein: In the second step, the specific operation further comprises: 27: Modify the names of the assembly template file, sub-part template file and engineering drawing template file in the current folder; 28: Reestablish the link between the modified assembly template file, sub-part template file and engineering drawing template file.

8. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 1, wherein: In the third step, the input bushing parameters are also checked.

9. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 8, wherein: In the third step, after copying the template files and script files in the resource folder to the input save path, the names of the assembly template file, sub-part template file and engineering drawing template file in the resource folder are modified. After the names of the assembly template file, sub-part template file and engineering drawing template file in the resource folder are modified, the assembly template file, sub-part template file and engineering drawing template file in the save path are automatically linked.

10. The CATIA-based rubber bushing parameterized modeling and quick drawing system of claim 9, wherein: In the third step, the specific operations include: 31: Obtain the resource folder path; 32: After the user inputs the bushing parameters and the bushing save path, determine whether the input of the bushing parameters is reasonable; 33: Copy the template files and script files in the resource folder to the input save path; 34: Modify the names of the assembly template file, sub-part template file and engineering drawing template file in the resource folder; 35: Modify the parameters in the parameter list template file in the current folder according to the input bushing parameters; 36: Add the input save path to the script file.

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