Part turning method based on software CAM milling module and application

Abstract

The invention relates to a part turning method based on a software CAM milling module and application, and belongs to the technical field of turning programming. The part turning method comprises the steps that S1, a software CAD function is started, and a curve model of a part is established; s2, starting a software CAM function, selecting a plane milling mode, setting in the plane milling mode, and generating a tool path code; s3, post-processing the tool path code to generate a numerical control program; and S4, the numerical control program is modified, a part is clamped on a machine tool, turning is started according to the modified numerical control program, and the part is an unconventional curved surface part. According to the turning programming method, whether a modeling module or a machining module is adopted, parameter setting is simple, errors are not prone to occurring, programming work of the unconventional curved surface can be efficiently completed, and the accuracy of a program is guaranteed.

Description

Technical Field

[0001] The invention relates to the technical field of turning programming, and in particular to a turning parts method and application based on a software CAM milling module. Background Art

[0002] The head is an indispensable and important component in pressure vessel equipment. It is the end cover of the pressure vessel, which is used to seal the end of the container to isolate the internal and external media. It plays an important sealing and pressure-bearing role. The quality of the head is directly related to the long-term safe and reliable operation of the pressure vessel.

[0003] A convex head is a type of head, which refers to a head with convex inner and outer surfaces. The inner and outer surfaces of this type of head are usually processed by turning. However, the inner or outer surfaces of some convex heads are unconventional surfaces that cannot be solved by standard formulas and need to be processed by manual parameter programming or software turning module programming. However, manual parameter programming requires the derivation of parameter formulas, which requires the programmer to have a good foundation in mathematical logic, and the derivation time is long, the process is prone to errors, and even some unconventional surfaces cannot establish parameter formulas; and when programming the software turning module, there are many tool parameters and process parameters that need to be set, which leads to a long production cycle.

[0004] Therefore, there is an urgent need for a turning programming method to more efficiently and accurately complete the turning of unconventional curved head parts. Summary of the invention

[0005] In view of the above analysis, the present invention aims to provide a method and application of turning parts based on the software CAM milling module to complete the turning of unconventional curved head parts.

[0006] In one aspect, the present invention provides a method for turning a part based on a software CAM milling module, comprising the following steps:

[0007] S1: Enable the CAD function of the software to establish the curve model of the part;

[0008] S2: Enable the software CAM function, select the plane milling mode, perform settings in the plane milling mode, and generate tool path codes;

[0009] S3: post-processing the tool path code to generate a numerical control program;

[0010] S4: modifying the numerical control program, clamping the part on the machine tool, and starting turning processing according to the modified numerical control program;

[0011] The part described is an irregular curved surface part.

[0012] Furthermore, in step S1, a part curve model is established, and the modeling coordinate system and the processing coordinate system are kept consistent.

[0013] Furthermore, in step S2, any milling cutter is created, the curve to be processed is selected, and the bottom surface, tool axis and cutting mode are specified.

[0014] Further, in step S2, the tool path code is composed of coordinate points on the curve, and the accuracy of the fitting is adjusted by changing the allowance tolerance in the cutting parameters.

[0015] Furthermore, during rough machining, the excess tolerance is 0.06-0.1 mm, and during fine machining, the excess tolerance is 0.01-0.05 mm.

[0016] Furthermore, in step S4, the tool starting position is determined at the program header, and a tool compensation instruction and a tool compensation cancellation instruction are added at the end of the program.

[0017] Furthermore, the G18 instruction and the Y coordinate value at the program header are removed, and the X coordinate value and the Z coordinate value are increased; the Y coordinate value at the end of the program is removed, and the X coordinate value and the Z coordinate value are increased.

[0018] Furthermore, a tool radius left compensation instruction G41 or a tool radius right compensation instruction G42 is added to the program header, and the tool number T and the compensation number D are added; and a tool radius compensation cancel instruction G40 is added to the end of the program.

[0019] On the other hand, the present invention provides an application of the method for turning parts based on the software CAM milling module as described in the present invention in the processing of parts with unconventional curved surfaces.

[0020] Furthermore, the unconventional curved surface parts include head-type parts.

[0021] Compared with the prior art, the present invention can achieve at least one of the following beneficial effects:

[0022] 1. The present invention provides a turning processing programming method based on the plane milling mode in CAD and CAM software. First, a curve model is created, and then the parameters in the plane milling mode are set to generate the tool path code. Then, a NC program is generated after post-processing. Finally, the program header and program tail of the NC program are modified and directly used for turning processing. The programming method provided by the present invention has a simple and fast modeling process, which saves time in model establishment;

[0023] 2. The plane milling mode parameter setting in the present invention only requires creating any milling cutter, selecting the curve to be processed, specifying the bottom surface, cutter axis and cutting mode, and no other parameter settings are required to generate the tool path code of the part curve contour. The parameter setting is simple and time-saving;

[0024] 3. In traditional applications, lathe processing programming should be completed in the turning module of the software CAM function. In the present invention, program codes available for lathe processing are generated in the plane milling mode, and the turning module is replaced by the milling module, which successfully applies the milling module to lathe processing. The turning processing programming method of the present invention, whether it is a modeling module or a processing module, has simple parameter settings and is not prone to errors. It can not only efficiently complete the programming work of unconventional surfaces, but also ensure the accuracy of the program.

[0025] In the present invention, the above-mentioned technical solutions can also be combined with each other to achieve more preferred combination solutions. Other features and advantages of the present invention will be described in the subsequent description, and some advantages can become obvious from the description, or can be understood by practicing the present invention. The purpose and other advantages of the present invention can be realized and obtained through the contents particularly pointed out in the description and the drawings. BRIEF DESCRIPTION OF THE DRAWINGS

[0026] The drawings are only for the purpose of illustrating particular embodiments and are not to be considered limiting of the present invention. Like reference symbols denote like components throughout the drawings.

[0027] Figure 1 It is a schematic flow chart of a method for turning parts based on a software CAM milling module in the present invention;

[0028] Figure 2 It is a schematic diagram of modeling of the unconventional curve in the present invention;

[0029] Figure 3 It is the plane milling parameter setting interface;

[0030] Figure 4 It is the interface for setting component boundary parameters;

[0031] Figure 5 is the generated tool path diagram;

[0032] Figure 6 It is the interface for adjusting the allowance tolerance;

[0033] Figure 7 It is a comparison chart before and after the program is modified;

[0034] Figure 8 This is the parameter interface of the turning processing module in Example 2. DETAILED DESCRIPTION

[0035] The preferred embodiments of the present invention are described in detail below in conjunction with the accompanying drawings, wherein the accompanying drawings constitute a part of this application and are used together with the embodiments of the present invention to illustrate the principles of the present invention, but are not used to limit the scope of the present invention.

[0036] When turning standard curved surface parts, it is necessary to use standard formulas to solve. Parts that cannot be solved using standard formulas are called unconventional curved surface parts, such as head parts.

[0037] At present, the turning processing of unconventional curved surface parts is mainly handled by manual parameter programming or turning module programming. However, when manual parameter programming is used, formula derivation is required, which takes a long time and is prone to errors, which can easily lead to the scrapping of parts during the processing; when the turning module programming in CAM is used, more parameters need to be set, resulting in a long programming time and extending the processing production cycle.

[0038] Therefore, the present invention provides a method for turning parts based on a software CAM milling module, comprising the following steps:

[0039] S1: Enable the CAD function of the software to establish the curve model of the part;

[0040] S2: Enable the software CAM function, select the plane milling mode, perform settings in the plane milling mode, and generate tool path codes;

[0041] S3: post-processing the tool path code to generate a numerical control program;

[0042] S4: modifying the numerical control program, clamping the part on the machine tool, and starting turning processing according to the modified numerical control program;

[0043] The part described is an irregular curved surface part.

[0044] Compared with the prior art, the present invention generates program codes that can be used for lathe processing in the plane milling mode, replaces the turning module with the milling module, and successfully applies the milling module to lathe processing. First, create a curve model of the part, then set the parameters in the plane milling mode, generate the tool path code, and then generate the NC program after post-processing, and finally modify the program header and program footer of the NC program and directly use it for turning processing.

[0045] The turning machining programming method of the present invention has simple parameter settings for both the modeling module and the machining module, is not prone to errors, and can not only efficiently complete the programming of unconventional surfaces, but also ensure the accuracy of the program.

[0046] Specifically, in step S1, a part curve model is established, and the modeling coordinate system and the processing coordinate system are kept consistent.

[0047] Start the CAD software, enter the modeling module of the software, select the sketch command, specify the plane where the sketch is located, and enter the drawing environment. Draw the curve according to the drawing size and requirements, constrain the position of the curve in the modeling coordinate system, and ensure that the curve is fully constrained, neither under-constrained nor over-constrained. The modeling coordinate system is consistent with the subsequent processing coordinate system to avoid re-establishing or adjusting the coordinate system in the processing module later, saving time.

[0048] Specifically, in step S2, any milling cutter is created, a curve to be processed is selected, and a bottom surface, a cutter axis and a cutting mode are specified.

[0049] Create any milling cutter without any requirement on the milling cutter specifications.

[0050] Create a process, select 2D milling as the process type, select plane milling as the process subtype, select the created milling cutter as the tool, select the coordinate system as the geometry, and enter the plane milling parameter setting environment.

[0051] In this setting environment, specify the part boundary, select the curve to be processed, set the boundary type to "Open", set the tool side to the left or right according to the processing direction, and set the tool position to "Center". After setting "Center", the center point of the milling cutter always falls on the curve to be processed.

[0052] To specify the bottom surface, there is no need to create a separate plane. You can select the coordinate plane where the curve is located.

[0053] The tool axis selects the coordinate axis that is perpendicular to the plane where the curve lies.

[0054] Select "Contour" as the cutting mode.

[0055] After completing the above settings, a tool path that coincides with the curve to be processed is generated. You can check whether the tool path is correct in the tool path visualization.

[0056] Specifically, in step S2, the tool path code is composed of coordinate points on the curve, and the accuracy of the fitting is adjusted by changing the allowance tolerance in the cutting parameters.

[0057] Specifically, during rough machining, the excess tolerance is 0.06-0.1 mm, and during fine machining, the excess tolerance is 0.01-0.05 mm.

[0058] Check the tool path code in the tool path list. The tool path code is composed of coordinate points on the curve. The curve is fitted by multiple coordinate points. Change the allowance tolerance in the cutting parameters to adjust the accuracy of the fitting. The smaller the allowance tolerance value, the higher the accuracy. Through the above parameter settings, a reasonable tool path code for the curve to be processed is generated.

[0059] Specifically, in step S3, the tool path code generated in the software only contains the values ​​of each coordinate point of the curve and cannot be recognized by the numerical control system of the machine tool.

[0060] Post-process the created tool path code. The software is equipped with a complete and comprehensive post-processing file. Select the matching CNC system file in the post-processor. Set the location where the file is saved, the unit of the value in the file (metric or inch or custom), and output the CNC program that the machine tool can recognize.

[0061] Specifically, in step S4, the tool starting position is determined at the program header, and a tool compensation instruction and a tool compensation cancellation instruction are added at the end of the program.

[0062] Specifically, remove the G18 command and Y coordinate value at the program header, and increase the X coordinate value and Z coordinate value; remove the Y coordinate value at the end of the program, and increase the X coordinate value and Z coordinate value.

[0063] Specifically, add a tool radius left compensation instruction G41 or a tool radius right compensation instruction G42 at the program header, add the tool number T and the compensation number D; and add a tool radius compensation cancellation instruction G40 at the end of the program.

[0064] The G18 instruction represents the cutting of the tool in the XZ plane in the coordinate system. Since the lathe cutting is always only involved in the X-axis coordinates and the Z-axis coordinates, that is, it is always cutting in the XZ plane, there is no need to specify it with the G18 instruction, and there is no Y-axis coordinate involved, so remove the G18 instruction and the Y coordinate value in the program header, and add the X coordinate value and the Z coordinate value. The X coordinate value and the Z coordinate value here are the points where the tool starts to move. This point is set near the point where the tool actually cuts into the workpiece, and ensures that the tool can smoothly cut into the workpiece.

[0065] Similarly, remove the Y coordinate value at the end of the program, and add the X and Z coordinate values. The coordinate values ​​here are the values ​​after the tool exits the workpiece after cutting, and are set near the point where the workpiece is cut out. Since the blade has a fillet radius, in order to prevent overcutting or undercutting during cutting, the fillet radius of the blade must be taken into account during cutting, so the tool radius left compensation command G41 or tool radius right compensation command G42 must be added to the program header, and the tool number T and compensation number D must be added; add the tool radius compensation cancellation command G40 at the end of the program.

[0066] The invention discloses an application of a turning processing method for parts based on a software CAM milling module in the processing of unconventional curved surface parts, wherein the unconventional curved surface parts include end cap parts. The diameter of a standard ellipsoid is 15 mm to 3500 mm, and the wall thickness is 1 to 100 mm.

[0067] In order to more clearly describe the present invention, it is further illustrated by the following examples and comparative examples.

[0068] Example 1

[0069] The present invention provides a method for turning parts based on a software CAM milling module, the process is as follows Figure 1 As shown:

[0070] Follow step 1 to enable the software CAD function and create a curve model of the part;

[0071] Follow step 2 to enable the software CAM function;

[0072] Follow step 3 and select plane milling mode;

[0073] Follow step 4 to set the parameters;

[0074] Follow step 5 to generate tool paths;

[0075] According to step 6, post-processing, generate NC program;

[0076] According to step 7, modify the NC program, clamp the head parts on the machine tool, and directly perform turning processing according to the modified NC program.

[0077] Reference Figure 2 In step 1, enter the modeling module of the software, select the sketch command, specify the plane where the sketch is located, and select the XOZ plane as the sketch plane because only the X-axis and Z-axis are involved in turning. Then enter the drawing environment. Draw the standard elliptical curve first according to the drawing size and requirements, and then draw the unconventional curve with the offset distance W. The modeling coordinate system is consistent with the subsequent processing coordinate system.

[0078] The origin of the coordinate system is set at the center of the ellipse, and a turning program is generated in which the inner surface is a standard ellipse curve with a major semi-axis a=90mm and a minor semi-axis b=57mm, and the outer surface is a non-standard curve with a constant wall thickness W=20mm.

[0079] In step 4, enter the plane milling mode of the software CAM module, create any milling cutter, select the XOZ plane for the bottom surface, and the Z axis for the tool axis;

[0080] Reference Figure 3 , specify the part boundary, specify the bottom surface, select the tool axis, and select the cutting mode.

[0081] To specify the bottom surface, you do not need to create a separate plane, you can select the coordinate plane where the curve is located;

[0082] The tool axis selects the coordinate axis that is perpendicular to the plane where the curve is located;

[0083] Select "Contour" for cutting mode;

[0084] Reference Figure 4, specify the part boundary, select the curve to be processed, set the boundary type to "open", set the tool side to the left according to the processing direction, and set the tool position to "center". After setting "center", the center point of the milling cutter always falls on the curve to be processed;

[0085] Reference Figure 5 After completing the above settings, a tool path that coincides with the curve to be processed is generated. You can check whether the tool path is correct in the tool path visualization. In step 5, generate code: View the tool path code in the tool path list. The tool path code consists of coordinate points on the curve.

[0086] Reference Figure 6 The curve is fitted by multiple coordinate points. The accuracy of fitting is adjusted by changing the allowance tolerance in the cutting parameters. The inner tolerance is set to 0.03mm and the outer tolerance is set to 0.03mm. Through the above parameter settings, a reasonable tool path code for the curve to be processed is generated.

[0087] Reference Figure 7 , set the tool starting point at the program header, add tool compensation instructions and cancel tool compensation instructions at the end of the program, remove the G18 instruction and Y coordinate value at the program header, and increase the X coordinate value and Z coordinate value. Remove the Y coordinate value at the end of the program, and increase the X coordinate value and Z coordinate value.

[0088] Add tool radius left compensation command G41 or tool radius right compensation command G42 at the program header, add tool number T and compensation number D; add tool radius compensation cancel command G40 at the end of the program to form a complete CNC program for lathe processing, and directly carry out subsequent turning processing.

[0089] Specifically, according to the part size, the starting coordinate value of the tool entering the part is (110, 0). The first line of the program sets the starting point at (130, -10), which is near the entry point but not in contact with the part. In the second line of the program, the tool moves to the X=110 position, which is the same as the X coordinate value of the entry point. At the same time, the tool compensation command G41, tool number T1, and compensation number D1 are added. The tool cuts from bottom to top. From the positive direction of the coordinate axis, the tool is located on the left side of the part, so the left compensation command G41 is used. T1 represents the digital code of this tool in the machine tool. The blade itself has a fillet radius. The ideal cutting state of the tool is the zero fillet state of the blade. In order for the tool to correctly cut the part, the fillet radius of the blade itself needs to be considered during programming, so the tool compensation command G41 or G42 should be used, and the blade fillet radius value should be written into the compensation number D1 in the machine tool. In the third line of the program, the tool moves to the Z=0 position, which is the position where the tool enters the part, and formal cutting begins.

[0090] After cutting is completed, set Z=90 at the end of the program to make the tool exit the part, and use the G40 command to cancel the blade corner radius compensation, retract the tool to the X=130 position, and keep the tool away from the part to ensure safe cutting. A complete cutting process is completed.

[0091] Place the head parts on the lathe with the opening facing downward and the center of the ellipse located on the rotation center of the lathe. Clamp it, select the appropriate turning tool and process the parts from bottom to top using the modified program.

[0092] Example 2

[0093] This embodiment provides a method for turning parts based on a software CAM milling module, which is applied to efficient programming of turning of conventional surfaces solved by standard formulas. Figure 1 Steps 1-7 shown generate a usable NC program for a lathe.

[0094] In step 1, in the modeling module of the software, draw a standard elliptical curve according to the drawing size and requirements. The modeling coordinate system is consistent with the subsequent processing coordinate system.

[0095] The remaining steps are consistent with Example 1, and a complete NC program for lathe processing is generated and applied to actual processing.

[0096] Comparative Example 1

[0097] The difference between Comparative Example 1 and Example 1 is that in Comparative Example 1, a manual parameter programming method is used in programming of unconventional surfaces, and it is necessary to derive available parameter equations. Figure 2 As shown, the formula for the outer curve of equal wall thickness is derived from the standard elliptic curve formula.

[0098] Standard ellipse parametric equation:

[0099] Equation of the outer curve of equal wall thickness:

[0100] Comparative Example 2

[0101] The difference between Comparative Example 2 and Example 1 is that in step 3 of Comparative Example 2, a turning processing module is selected in the software CAM, and after reasonable parameters are set, a program code that can be used for a lathe is generated, but the parameter setting is complicated.

[0102] like Figure 8 As shown, in the turning processing module, the tool needs to set the accurate blade shape and size, tool bar style and size, and tool position; the process parameters need to set the cutting strategy, tool path parameters, and feed and retract parameters.

[0103] Detection

[0104] Through Example 1 and Example 2, the method of the present invention can be applied not only to the turning of unconventional surfaces, but also to the turning of conventional surfaces, and has a wide applicability, does not require cumbersome settings and calculations, has a low error rate, and the entire process takes an average of about 0.25 hours. Comparative Example 1 requires a professional to perform the calculation, has a high error rate, and takes a long time, and takes an average of about 1.5 hours to complete the calculation. Comparative Example 2 takes 0.5 hours. The present invention improves efficiency by more than 80% over Comparative Example 1 and 50% over Comparative Example 2. The time used in the present invention refers to the time used from the beginning to the time when the part is processed by the machine tool.

[0105] The above description is only a preferred specific implementation manner of the present invention, but the protection scope of the present invention is not limited thereto. Any changes or substitutions that can be easily conceived by any technician familiar with the technical field within the technical scope disclosed by the present invention should be covered within the protection scope of the present invention.

Claims

1. A method for turning parts based on a software CAM milling module, characterized in that: The following steps are involved: S1: Enable the CAD function of the software to establish the curve model of the part; S2: Enable the software CAM function, select the plane milling mode, perform settings in the plane milling mode, and generate tool path codes; S3: post-processing the tool path code to generate a numerical control program; S4: modifying the numerical control program, clamping the part on the machine tool, and starting turning processing according to the modified numerical control program; The part described is an irregular curved surface part.

2. The method for turning parts based on the software CAM milling module according to claim 1, characterized in that: In step S1, a part curve model is established, and the modeling coordinate system and the processing coordinate system are kept consistent.

3. The method for turning parts based on the software CAM milling module according to claim 1, characterized in that: In step S2, create any milling cutter, select the curve to be processed, and specify the bottom surface, tool axis and cutting mode.

4. The method for turning parts based on the software CAM milling module according to claim 1, characterized in that: In step S2, the tool path code is composed of coordinate points on the curve, and the accuracy of the fitting is adjusted by changing the allowance tolerance in the cutting parameters.

5. The method for turning parts based on the software CAM milling module according to claim 4 is characterized in that: During rough machining, the excess tolerance is 0.06-0.1 mm, and during fine machining, the excess tolerance is 0.01-0.05 mm.

6. The method for turning parts based on software CAM milling module according to claim 1, characterized in that: In step S4, the tool starting position is determined at the program header, and a tool compensation instruction and a tool compensation cancellation instruction are added at the end of the program.

7. The method for turning parts based on software CAM milling module according to claim 6, characterized in that: Remove the G18 command and Y coordinate value at the program header, and increase the X and Z coordinate values; remove the Y coordinate value at the end of the program, and increase the X and Z coordinate values.

8. The method for turning parts based on software CAM milling module according to claim 6, characterized in that: Add tool radius left compensation command G41 or tool radius right compensation command G42 at the program header, and add tool number T and compensation number D; add tool radius compensation cancel command G40 at the end of the program.

9. Application of the turning method for parts based on the software CAM milling module as claimed in any one of claims 1 to 8 in the processing of parts with unconventional curved surfaces.

10. The application of the turning method for parts based on the software CAM milling module according to claim 9 in the processing of parts with unconventional curved surfaces, characterized in that: The unconventional curved surface parts include head-type parts.

Images