Processing program correction device

Abstract

The present invention provides a machining program correction device that can correct a machining program with a specified tool path even without the shape data of the target workpiece, without requiring the operator to have high knowledge or spend a lot of time. The machining program correction device (10) includes: a machining program parsing unit (12) that parses the machining program (22) and extracts a group of instruction points; an estimated machining surface generation unit (14) that generates an estimated machining surface based on the group of instruction points; a tool path correction unit (16) that corrects the tool path by moving, adding or deleting instruction points based on the distance to the estimated machining surface; and a machining program output unit (18) that converts the tool path corrected by the tool path correction unit (16) into a machining program and outputs it.

Description

Technical Field

[0001] This disclosure relates to an apparatus for modifying a processing procedure. Background Technology

[0002] To shorten cycle time, improve machining accuracy, or enhance surface quality, machining programs with specified toolpaths are sometimes modified. The re-creation or modification of the machining program is typically performed using CAM, dialog programming devices, or text editors, referencing the shape data of the target workpiece. Regarding the modification of machining programs accompanying toolpath modifications, Patent Document 1 discloses a technique for generating curved paths between command points and modifying the toolpaths considering their allowable range. Furthermore, Patent Document 2 discloses a polygon generation system capable of being used when estimating the shape of the workpiece based on the machining program.

[0003] Existing technical documents

[0004] Patent documents

[0005] Patent Document 1: International Publication WO2020 / 179798

[0006] Patent Document 2: Japanese Patent Application Publication No. 11-339071 Summary of the Invention

[0007] The problem that the invention aims to solve

[0008] However, without CAD data and target shape documentation for the workpiece to be machined at the machining site, it is often difficult to change target tolerances, cycle feeds, and path patterns. Furthermore, making these changes requires a high level of operator knowledge and significant time. Path patterns refer to tool movement modes such as parallel and spiral patterns. The workpiece to be machined will be referred to as the target workpiece.

[0009] The shape of the target workpiece can also be estimated through machining simulation. However, this estimation requires information about the tool shape and the shape of the raw material for the workpiece.

[0010] Therefore, the object of the present invention is to provide a machining program correction device that can correct the machining program of a specified tool path even without the shape data of the target workpiece, without requiring the operator to have high knowledge or spend a lot of time.

[0011] Methods for solving problems

[0012] The machining program correction apparatus disclosed herein is used in a numerical control device to correct a machining program that specifies the relative movement path between a tool and a workpiece. The machining program correction apparatus includes: a machining program parsing unit that parses the machining program and extracts a group of instruction points; an estimated machining surface generation unit that generates an estimated machining surface based on the group of instruction points; a tool path correction unit that corrects the tool path by moving, adding, or deleting instruction points based on the distance to the estimated machining surface; and a machining program output unit that transforms the tool path corrected by the tool path correction unit into a machining program and outputs it.

[0013] According to the machining program correction device disclosed herein, even without shape data of the target workpiece, the operator can correct the machining program of the specified tool path without requiring high knowledge or spending a lot of time. Attached Figure Description

[0014] Figure 1 This is a block diagram showing the general structure of the processing procedure correction device of this disclosure.

[0015] Figure 2 This is a block diagram illustrating a modified example of the processing procedure correction device of this disclosure.

[0016] Figure 3 This is a diagram showing a summary of the steps for generating the estimated machining surface in Example 1.

[0017] Figure 4 This is a diagram showing the outline of the addition of instruction points in Embodiment 1.

[0018] Figure 5A This is a diagram showing the modified processing procedure in Example 1.

[0019] Figure 5B This is a diagram showing the modified tool path after adding command points in Example 1.

[0020] Figure 6 This is a diagram showing the outline of the addition and deletion of instruction points in Embodiment 2.

[0021] Figure 7 This is a diagram showing the outline of the movement of the command point in Embodiment 3.

[0022] Figure 8 It is a flowchart that outlines the method for correcting the machining process. Detailed Implementation

[0023] (Processing program correction device)

[0024] The embodiments of this disclosure will be described with reference to the accompanying drawings. Figure 1This is a block diagram illustrating the general structure of the machining program correction device 10 according to an embodiment of the present disclosure. The machining program correction device 10 of the present disclosure corrects the tool path by adjusting the command point, etc., based on the distance to the estimated machining surface generated from the command point. The machining program correction device 10 is used in the numerical control device 1.

[0025] like Figure 1 As shown, the machining program correction device 10 includes a machining program analysis unit 12, an estimated machining surface generation unit 14, a tool path correction unit 16, and a machining program output unit 18. In the machining program correction device 10, the machining program analysis unit 12, the estimated machining surface generation unit 14, the tool path correction unit 16, and the machining program output unit 18 are connected in sequence.

[0026] The machining program parsing unit 12 is responsible for parsing the machining program 22 and extracting the instruction point group. The machining program 22 is input to the machining program parsing unit 12 from outside the machining program correction device 10. The estimated machining surface generation unit 14 is responsible for generating an estimated machining surface from the instruction point group extracted by the machining program parsing unit 12. The tool path correction unit 16 is responsible for correcting the tool path by moving, adding, or deleting instruction points based on the distance between the tool path and the estimated machining surface generated by the machining program parsing unit 12. The machining program output unit 18 is responsible for converting the tool path corrected by the tool path correction unit 16 into a machining program and outputting it. The machining program generated by converting and correcting the tool path is called the corrected machining program 24. Hereinafter, they will be described in sequence.

[0027] (Example 1)

[0028] Reference Figures 3 to 5B The following describes Embodiment 1 of the present disclosure. Figure 3 This is a diagram illustrating the outline of the steps for generating the presumed machined surface in Example 1. Figure 3 In this process, the generation steps are performed in the order from arrow 311 to arrow 313. In Embodiment 1, the correction method of the tool path correction unit 16 is to move, add, or delete instruction points to converge to a predetermined tolerance.

[0029] First, the machining program parsing unit 12 reads the machining program 22. Alternatively, the machining program 22 is input into the machining program parsing unit 12. Figure 3 The machining program 301 represents an example of the machining program 22 before modification. Hereinafter, the situation before modification will sometimes be referred to as the original situation.

[0030] Next, the machining program analysis unit 12 analyzes the machining program 22 and extracts the instruction point group. Figure 3 In the example shown, the machining program parsing unit 12 extracts instruction points for the program block of machining program 22 whose mode is G01.

[0031] Figure 3 Table 302 represents the extracted command point group. The extracted command point group contains 6 command points, from command point n-2 to command point n+3. The position of each command point is represented by coordinates in the XYZ coordinate system.

[0032] Figure 3 Tool path diagram 303 shows the plotting of each command point 32 of the extracted command point group 30 in the XYZ coordinate system. In tool path diagram 303 and the following diagrams, the directions of each axis in the XYZ coordinate system are illustrated as needed. The path obtained by connecting each command point 32 in sequence is called tool path 60. The tool path 60 before correction shown in tool path diagram 303 is called tool path 61 before correction.

[0033] Figure 3 The machining surface diagram 304 represents a proposed machining surface 90 generated based on the extracted instruction point group 30. The proposed machining surface generation unit 14 generates the proposed machining surface 90 based on the extracted instruction point group 30. The method for generating the proposed machining surface 90 based on the instruction point group 30 is not particularly limited. For example, the technique shown in Patent Document 2 can be used to generate the proposed machining surface from the point group.

[0034] Reference Figure 4 The addition of command point 32 will be explained. The addition of command point 32 is performed by tool path correction unit 16 based on the distance between command point 32 and estimated machining surface 90. Figure 4 This is a diagram showing the outline of the addition of instruction point 32 in Embodiment 1. Figure 4 Tool path diagram 401 shows the tool path 61 before correction. Additionally, Figure 4 Command point diagrams 402 to 404, as shown by arrow 411, illustrate the addition of command point 32 within box 410 of tool path diagram 401. The addition steps for command point 32 proceed in the order of arrows 412 and 413. Furthermore, the points illustrated using command point 32 within box 410 as an example also apply to other command points.

[0035] The following explanation uses a target tolerance of 1 μm as an example to illustrate the addition of instruction point 32. Furthermore, various parameters related to toolpath correction used in machining program correction, such as the target tolerance, can be preset in the machining program correction device 10. Alternatively, parameters related to toolpath correction can also be set separately by the operator. (See reference...) Figure 2 Please provide an explanation.

[0036] Figure 2 This is a block diagram illustrating a modified example of the machining process correction device 10 of this disclosure. Figure 2 The machining program correction device 10 shown and Figure 1 Unlike the machining program correction device 10 shown, the tool path correction unit 16 allows the operator to input tool path correction parameters 26. Tool path correction parameters 26 specify at least one of the following: distance between the estimated machining surface 90 and the command point 32, target tolerance, periodic feed, and path mode. The tool path correction unit 16 can switch the tool path correction method based on the input tool path correction parameters 26. This allows for more flexible correction of the machining program to meet the operator's needs.

[0037] return Figure 4 The addition of instruction point 32 when the target tolerance is set to 1μm will be explained. First, as... Figure 4 As shown in the instruction point diagram 402, it is determined whether three consecutive instruction points 32 meet the target tolerance. In the instruction point diagram 402, the three consecutive instruction points 32 are designated as instruction point 32n-1, instruction point 32n, and instruction point 32n+1. The straight line connecting instruction point 32n-1 and instruction point 32n+1 is designated as line 421. The distance from instruction point 32n to line 421 is designated as distance 422. If distance 422 exceeds the target tolerance, an additional instruction point 32 is added.

[0038] Reference Figure 4 The instruction point diagram 403 illustrates a specific example of adding instruction point 32. Instruction point 32 is added by adding instruction point 32 between instruction points 32n and 32n-1, and between instruction points 32n and 32n+1. The line segment connecting instruction points 32n and 32n-1 is designated as line segment 431. Instruction point 32n-1' is added at the midpoint of line segment 431. The line segment connecting instruction points 32n and 32n+1 is designated as line segment 432. Instruction point 32n+1' is added at the midpoint of line segment 432.

[0039] Reference Figure 4Command point diagram 404 explains the movement of command point 32 in the Z-axis direction, etc. The additional command points 32n-1' and 32n+1' shown in command point diagram 403 are positioned without considering the distance from the estimated machining surface 90. That is, command points 32n-1' and 32n+1' are temporarily positioned, essentially temporary command points 32. Therefore, command points 32n-1' and 32n+1' are moved in the Z-axis direction, etc., as needed. This movement brings command points 32n-1' and 32n+1' into contact with the estimated machining surface 90, or positions them at a predetermined distance away from the estimated machining surface 90. In other words, command points 32n-1' and 32n+1' are moved to a position a certain distance away from the estimated machining surface, for example, +0.1 μm.

[0040] This movement, for example as shown by lines 411 and 422 in command point diagram 404, can be set to a movement in the Z-axis direction regardless of command point 32.

[0041] Alternatively, the movement can be set to a movement in the tool axis direction that can be known based on the machining program 22 or the settings of the numerical control device 1. The tool axis direction refers to, for example, the direction orthogonal to the tool path at each command point 32. For example, angle 471 is 90 degrees. The tool axis direction varies depending on each command point 32. Lines 461, 463, and 465 represent the tool axis direction relative to the corresponding command points 32n-1, 32n, and 32n+1, respectively.

[0042] The tool axis directions of the added command point 32n-1' and command point 32n+1' can be determined, for example, by the following method: The tool axis direction of command point 32n-1' is represented by line 462, and the tool axis direction of command point 32n+1' is also represented by line 462. The tool axis directions of the added command point 32n-1' and command point 32n+1' can also be the tool axis direction of the original command point 32 (before or after the added command point). That is, for example, the direction of line 462 can be the same as the direction of line 461 or line 463.

[0043] Alternatively, the tool axis directions of the additional command points 32n-1' and 32n+1' can also be the average of the tool axis directions of the command points 32 before and after the addition of the command points. That is, for example, the direction of line 464 can also be calculated by averaging the directions of line 463 and line 465.

[0044] By moving the additional command points 32n-1' and 32n+1' in the tool axis direction, the new command point 32 can be configured at a position closer to the midpoint of the adjacent uncorrected command point 32 compared to the case of moving it in the Z-axis direction.

[0045] As described above, the tool path correction unit 16 adds command points 32, etc., to generate a corrected command point group 30. The corrected tool path is then created using the corrected command point group 30.

[0046] The machining program with the added instruction point 32 is called the modified machining program 24. (See reference...) Figure 5A The revised processing procedure 24 is explained. Figure 5A This is a diagram representing the corrected processing procedure 24, etc.

[0047] Figure 5A The instruction point group table 501 represents the instruction point group after being corrected by adding and moving instruction points. The instruction points n-1' and n+1', indicated in bold, are instruction points 32 added by the tool path correction unit 16, etc.

[0048] Figure 5A Machining program 502 represents the modified machining program 24. As shown by arrow 511, the machining program output unit 18 transforms the tool path shown by the instruction point group corrected by the tool path correction unit 16 into the modified machining program 24. The parts indicated in bold in the modified machining program 24 correspond to the added instruction points n-1' and n+1'. The machining program output unit 18 outputs the transformed modified machining program 24, and the series of processes ends.

[0049] Figure 5B This is a diagram illustrating an example of the modified toolpath 62 after the addition of command points. Figure 5B In box 511 shown, command points 3201, 3202, and 3203 are the command points before correction. Command points 3211, 3212, and 3213 are the added command points after correction. For example, by adding command point 3211 between command points 3201 and 3202, a toolpath corresponding to the change in the target tolerance is obtained. Furthermore, as shown by command points 3212 and 3213, the number of command points 32 added between command points 32 is not limited to one. Two or more command points can also be added between command points 32. Additionally, if the target tolerance is met, it is also possible not to add new command points 32 between command points 32.

[0050] Furthermore, if the target tolerance is met even after deleting instruction point 32, then instruction point 32 can be deleted. Deleting instruction point 32 reduces the burden on information processing. When there are many instruction points 32 before correction, deleting instruction point 32 is an effective method.

[0051] (Example 2)

[0052] Reference Figure 6 Embodiment 2 of this disclosure will be described. Figure 6 This diagram illustrates the general outline of the addition and deletion of command points 32 in Embodiment 2. The description of Embodiment 2 focuses on aspects that differ from Embodiment 1. Matters not specifically described in Embodiment 2 may be the same as in Embodiment 1. In Embodiment 2, the correction method of the tool path correction unit 16 involves moving, adding, or deleting command points 32 to converge to a predetermined periodic feed.

[0053] The process of analyzing machining procedure 22 until the estimated machining surface 90 is generated is the same as in Example 1.

[0054] In Example 2, after the estimated machining surface 90 is generated, the tool path correction unit 16 calculates the periodic feed based on the instruction point group 30. (Refer to...) Figure 6 Tool path diagram 601 illustrates periodic feed. Tool path diagram 601 represents the tool path 61 before correction. Periodic feed refers to the distance between paths.

[0055] As shown in tool path diagram 601, tool path 60 includes a main path and connecting paths. A main path is the path corresponding to the main movement in tool path 60, such as the path from command point 201 to command point 204. A connecting path is the path that connects two adjacent main paths, such as the path from command point 204 to command point 205. The distance of the connecting paths is called the periodic feed.

[0056] Before the correction, tool path 61 included four main paths from main path 101 to main path 104. Additionally, tool path 61 included three connection paths from connection path 141 to connection path 143. Connection paths 141, 142, and 143 had the same distance (length).

[0057] In toolpath diagram 601, double arrows 631 represent the periodic feed of the unmodified toolpath 61. The periodic feed 631 of the unmodified toolpath 61 is 10 μm.

[0058] Here, we explain how to calculate the periodic feed. First, we explain how to determine if two line segments are on the same path. Regarding the line segments connecting command points, if the angle between two consecutive line segments is less than 30 degrees, they are considered to be on the same path. If the angle between consecutive line segments is greater than 30 degrees, they are considered to be on different paths.

[0059] Furthermore, if the angles between each end of a line segment and a consecutive line segment are both greater than 30 degrees, it is determined that there is movement along a path within that line segment. Additionally, it is determined that the two command points at the two ends of the line segment are not on the same path. If the angles are less than 30 degrees, the opposite determination is made.

[0060] For example, in Figure 6 If both angles 621 and 622 exceed 30 degrees, it is determined that there is movement between paths within line segment 142. Furthermore, in this case, it is determined that command point 207 and command point 208 are not on the same path.

[0061] Additionally, the length of line segment 142 is used as the periodic feed. That is, the distance 631 between command point 207 and command point 208 is the periodic feed 631. Figure 6 In the example shown, the length of the original periodic feed 631 before the change was 10 μm.

[0062] In Example 2, the cases of extending the length of the periodic feed and shortening the length of the periodic feed are described. Figure 6 Arrow 611 represents an example of path change when extending the cycle feed. Figure 6 Arrow 612 represents an example of path change when shortening the cycle feed.

[0063] First, refer to Figure 6 The tool path diagram 602 illustrates the path change when extending the cycle feed. Figure 6 Tool path diagram 602 shows the modified tool path 63 with a longer periodic feed. Modified tool path 63 changes the periodic feed of the original tool path 61 from 10 μm to 15 μm. The double arrow 632 in tool path diagram 602 represents the periodic feed of the modified tool path 63. The length of the periodic feed 632 is 15 μm.

[0064] First, let's explain the common aspects when extending and shortening the cycle feed. When changing the cycle feed, the path is added or removed, i.e., command points are added or deleted, to make the cycle feed the target value. In this case, the paths at both ends of the tool path remain unchanged. When changing the path from the unmodified tool path 61 shown in tool path diagram 601 to the modified tool path 63 shown in tool path diagram 602, the main path 101 from command point 201 to command point 204 and the main path 104 from command point 209 to command point 210 remain unchanged. Main paths 101 and 104 are represented by thick lines. When changing the cycle feed, the path between main paths 101 and 104 is changed.

[0065] The case of extended cycle feed is explained. In the case of extended cycle feed, the path is reduced, that is, the command point is deleted, to achieve the desired cycle feed. In the example shown in tool path diagram 602, the number of main paths configured between main path 101 and main path 104 is reduced from 2 to 1. Before the correction, tool path 61 included two main paths, main path 102 and main path 103. In contrast, after the correction, tool path 63 only includes main path 111.

[0066] When extending the cycle feed, if the changed cycle feed can be achieved by deleting the main paths contained in the original tool path 61, the unnecessary main paths are deleted to generate the revised tool path 63. Conversely, if the changed cycle feed cannot be achieved by deleting the main paths contained in the original tool path 61, a new main path is added after deleting the unnecessary main paths. In the revised tool path 63, a new main path 111 is added after deleting the main paths 102 and 103 contained in the original tool path 61. Then, the main paths 101 and 111 are connected by the connection path 161, and the main paths 111 and 104 are connected by the connection path 162, thereby generating the revised tool path 63.

[0067] Furthermore, the location of the additional main path can be determined, for example, by dividing the main path 101 and main path 104 equally according to the periodic feed. The addition of the main path will be explained in detail later.

[0068] Similar to the command points added in Example 1, the main path, and consequently the command points, configured according to the modified periodic feed, are in a so-called temporary placement state where the distance to the estimated machining surface 90 is not optimized. Therefore, the position relative to the estimated machining surface 90 is optimized using the same method as described in Example 1. That is, the command points are moved in the Z-axis direction, etc., so that the path (command points) contacts the estimated machining surface 90. Thus, the modified tool path 63 is obtained. Then, a machining program is generated from the modified tool path 63, and the series of processes ends.

[0069] Next, refer to Figure 6 Tool path diagram 603 illustrates the path changes when shortening the cycle feed. The following explanation focuses on the differences from the case of extended cycle feed. Unless otherwise specified, the same procedures apply as with extended cycle feed.

[0070] Figure 6 Tool path diagram 603 shows the corrected tool path 64 with a shorter periodic feed. The corrected tool path 64 changes the periodic feed of the original tool path 61 from 10 μm to 5 μm. The double arrow 633 in tool path diagram 603 represents the periodic feed 633 of the corrected tool path 64. The length of the periodic feed 633 is 5 μm.

[0071] When shortening the cycle feed, additional paths, i.e., additional command points, are added to achieve the target cycle feed. In the example shown in tool path diagram 603, the number of main paths configured between main path 101 and main path 104 increases from 2 to 5. Main paths 102 and 103, configured between main paths 101 and 104, are the main paths included in the original tool path 61.

[0072] In the revised tool path 64, a new main path portion 121 is added between main paths 101 and 102, a new main path portion 122 is added between main paths 102 and 103, and a new main path portion 123 is added between main paths 103 and 104. Furthermore, the revised tool path 64 is generated by sequentially connecting adjacent main paths with connecting paths 151 and 152, etc.

[0073] The method for adding command points to the main path is explained. When adding command points, the position of the added command point can be determined using the difference between the command points that constitute the original path. The difference between command points is also called the increment. In the tool path diagram 601, the difference between command points is represented by arrow 661. The difference 661 is the difference between command point 201 and command point 202. When adding command points, the new command point can be added by referring to the difference at the corresponding position in the tool path 61 before the modification. This will be explained in detail below.

[0074] When determining the position of command point 223 shown in tool path diagram 603, the difference between command point 201 and command point 202, i.e., difference 661, is used to determine the position of command point 223. Specifically, the position where command point 224 has been moved by difference 661 is set as the position of command point 223.

[0075] Furthermore, instruction point 224 can be determined based on instruction point 201 of the tool path 61 before modification, and on the distance of the changed periodic feed 633, etc.

[0076] Similarly, the locations of other command points on main path 121, as well as command points on additional main paths 122 and 123, can be determined.

[0077] Furthermore, the method for determining the position of the additional command point 202 is not limited to the method described above. For example, the position of the additional command point 202 can be determined not based on the difference between two adjacent command points, but based on the two command points sandwiching the additional command point. The following explanation uses command points 203 and 206 of the tool path 61 before correction as an example. The line segment connecting command points 203 and 206 is designated as line segment 651. The midpoint of line segment 651 is designated as midpoint 652.

[0078] When a new main path is added between the main path 101 containing command point 203 and the main path 102 containing command point 206, the midpoints of the other command points of the main paths 101 and 102 are also calculated in the same way. Furthermore, by connecting the calculated midpoints, a new main path can be generated.

[0079] The instruction point 222 of the main path 121 in tool path diagram 603 is at the same position as the midpoint 652 shown in tool path diagram 601 as described above. Similarly, the positions of other instruction points of the main path 121, as well as the instruction points of the additional main paths 122 and 123, can be determined.

[0080] With the cycle feed shortened, the position relative to the estimated machining surface 90 is optimized for command points that are temporarily placed, just as with the cycle feed extended. Then, a machining program is generated from the modified toolpath 63, and the series of processes concludes.

[0081] (Example 3)

[0082] Reference Figure 7 Example 3 of this disclosure is described below. Figure 7 This is a diagram illustrating the outline of the movement of command point 32 in Embodiment 3. The description of Embodiment 3 focuses on aspects that differ from Embodiment 1. Matters not specifically described in Embodiment 3 may be the same as in Embodiment 1. In Embodiment 3, the correction method of the tool path correction unit 16 is to move, add, or delete command points 32 in a manner consistent with a predetermined path pattern.

[0083] The process of analyzing machining procedure 22 until the estimated machining surface 90 is generated is the same as in Example 1.

[0084] In Embodiment 3, after the estimated machining surface 90 is generated, the tool path correction unit 16 moves the command point 32 in a manner consistent with the target path pattern. Then, the command point is further moved in the Z-axis direction so that the moved command point 32 contacts the estimated machining surface 90. The following will describe these steps in sequence.

[0085] Figure 7 Tool path diagram 701 is a diagram showing a path pattern with a fixed Y-axis scan line. In the path pattern with a fixed Y-axis scan line, the Y-axis coordinate values ​​of all command points determined to be on the same path are changed to the same Y-axis coordinate values ​​as the starting point of the path, and then the tool path moves in the Z-axis direction in a manner that contacts the estimated machining surface 90. Furthermore, the determination of whether command points 32 are on the same path can be performed in the same way as in Embodiment 2. That is, if the angle between the two ends of the line segment connecting the two command points is less than 30 degrees, the two command points are determined to be on the same path.

[0086] The following is a detailed explanation with reference to the accompanying drawings. Referring to tool path diagram 701, the path pattern with a fixed Y-axis, i.e., the modified tool path 65, will be explained. Command point 250 is the starting point of the path. In the main path 261 (the path indicated in bold) from command point 250 to command point 253, the coordinate values ​​of each command point are transformed to have the same Y-axis coordinate values ​​as the Y-axis coordinate values ​​of command point 250; that is, the Y-axis coordinate values ​​are not changed, only the X-axis and Z-axis coordinate values ​​are moved. Thus, the main path 261 becomes a path with a scan line whose Y-axis is fixed.

[0087] After transforming the coordinate values ​​of one main path as described above, the coordinate values ​​of the next main path that is connected via a connecting path such as connecting path 262 are transformed in the same way.

[0088] After completing the transformation of the coordinate values ​​of all command points, similar to Example 1, the distance between the command points and the estimated machining surface is adjusted by moving the command points in the Z-axis direction to contact the estimated machining surface.

[0089] In the corrected tool path 65 under the path mode with the Y-axis fixed, the main paths, such as main paths 261 and 263, move primarily in the X direction. Furthermore, these main paths are connected by connecting paths 262 and 264, thus forming a tool path.

[0090] Next, referring to tool path diagram 702, the path pattern with a fixed X-axis, i.e., the modified tool path 66, will be explained. Command point 250, like the modified tool path 65, is the starting point of the path. In the main path 271 (the path indicated in bold) from command point 250 to command point 259, the coordinate values ​​of each command point are transformed to have the same X-axis coordinate values ​​as the X-axis coordinate values ​​of command point 250; that is, the Y-axis and Z-axis coordinate values ​​are moved without changing the X-axis coordinate values. Thus, the main path 271 becomes a path with a scan line whose X-axis is fixed.

[0091] After transforming the coordinate values ​​of one main path as described above, the coordinate values ​​of the next main path that is connected via a connecting path such as connecting path 272 are transformed in the same way.

[0092] After completing the transformation of the coordinate values ​​of all command points, similar to Example 1, the distance between the command points and the estimated machining surface is adjusted by moving the command points in the Z-axis direction to contact the estimated machining surface.

[0093] In the corrected tool path 66 under the path mode with the X-axis fixed, the main paths, such as main paths 271 and 273, move primarily in the Y direction. Furthermore, these main paths are connected by connecting paths 272 and 274, thus forming a tool path.

[0094] exist Figure 7 In the example shown, both the modified toolpath 65 and the modified toolpath 66 target the same presumed machining surface 90, but their endpoints are different.

[0095] By changing the path pattern in this way, a tool path that is consistent with the characteristics of the device can be obtained, such as high or poor movement accuracy in a predetermined direction.

[0096] in addition, Figure 7 The path pattern shown is an example. Other path patterns include spiral paths and contour paths that maintain a constant height (Z-axis coordinate value). Tool paths can also be generated using the same method described above for these path patterns.

[0097] Alternatively, after making the aforementioned path pattern change, the target tolerance and periodic feed described earlier can also be changed.

[0098] Furthermore, the machining program correction device 10 can also be configured using a computer equipped with a memory such as ROM (read-only memory) or RAM (random access memory), a CPU (control processing unit), and a communication control unit interconnected via a bus. The functions and operations of each of the aforementioned functional units are realized through the cooperation of the CPU, memory, and control program stored in the memory mounted on the computer. Additionally, the machining program correction device 10 can be configured as a CNC (Computer Numerical Controller), PLC (Programmable Logic Controller), or connected to a host computer that outputs machining programs and machining conditions.

[0099] (Methods for correcting machining procedures)

[0100] Reference Figure 8 This describes the machining program correction method implemented by the machining program correction device 10 of this disclosure. Figure 8 This is a flowchart outlining a method for correcting a machining process. Figure 8 In the following explanation, S1 represents step 1. This also applies to other steps.

[0101] Figure 8 This refers to changes in the target tolerance, periodic feed, and path pattern in the correction methods performed by the tool path correction department. In the machining program correction methods, S1 to S3 and S4 to S5 are common to the three correction methods mentioned above.

[0102] In the machining program correction method, the machining program is first read into the machining program parsing unit, etc., as S1. Then, the machining program is parsed and the instruction point group is extracted, as S2.

[0103] Next, as S3, in the estimated machining surface generation unit, an estimated machining surface is generated based on the instruction point group.

[0104] Following S3, in the case of a change in the target tolerance, as S11, the tolerance from the command point group is calculated in the tool path correction unit, etc. Next, as S12, temporary command points are added between command points that exceed the target tolerance. Additionally, in S12, command points can also be deleted as needed.

[0105] If the periodic feed is changed after S3, as in S21, the periodic feed from the command point group is calculated in the toolpath correction unit, etc. Then, as in S22, command points are added or deleted based on the changed periodic feed, thereby increasing or decreasing the toolpath.

[0106] When the path mode is changed after S3, as S31, the coordinate values ​​of the command points that are consistent with the predetermined path mode are transformed in the tool path correction unit, such as fixing the coordinate values ​​of the predetermined coordinate axes in the XYZ axes.

[0107] After completing the steps corresponding to each correction method, the process proceeds to S4. In S4, a temporary command point is moved based on the distance to the estimated machining surface in the toolpath correction unit, etc. This optimizes the distance between the command point and the estimated machining surface. Next, in S5, a machining program is generated based on the corrected toolpath in the machining program output unit, etc. This concludes the flow of the machining program correction method.

[0108] As explained above, in the machining program correction apparatus 10 of this disclosure, instruction point group 30 is extracted from machining program 22 to generate estimated machining surface 90. Then, the tool path 60 is corrected by moving, adding or deleting instruction points 32 so that the distance from the estimated machining surface 90 converges to a predetermined range.

[0109] Specifically, command points can be moved or added as follows: convergence to a predetermined tolerance (change in target tolerance), convergence to a predetermined periodic feed (change in periodic feed), and consistency with a predetermined path pattern (change in path pattern).

[0110] When moving or adding command point 32, it is preferable to set the distance from the estimated machining surface 90 to 0 mm, and move or add it in such a way that command point 32 contacts the estimated machining surface 90. The distance of command point 32 from the estimated machining surface 90 is not limited to 0 mm, and can also be set to a predetermined distance. In addition, the direction of movement of command point 32 or the direction of distance from the estimated machining surface can be calculated in the Z-axis direction or the tool axis direction, etc.

[0111] Then, the modified toolpath 60 is transformed into a machining program, namely the modified machining program 24, and output. Thus, the toolpath can be modified without using a post-processor or the like.

[0112] In the machining program correction apparatus 10 of this disclosure, even without shape data of the target workpiece, the machining program, i.e., the tool path, can be corrected without requiring high levels of operator knowledge or excessive operation time. This results in shorter cycle time, improved machining accuracy, and improved surface quality. Typically, these three effects are sometimes traded off. In this respect, the machining program correction apparatus 10 of this disclosure achieves these effects at a high level. Furthermore, compared to the case where the shape of the workpiece is estimated through machining simulation, the machining program correction apparatus 10 of this disclosure does not require information on the tool shape and the shape of the raw material of the workpiece. Therefore, path correction can be easily implemented.

[0113] Furthermore, this disclosure is not limited to the above-described embodiments, examples, and variations. Any variations or improvements within the scope of achieving the purpose of this disclosure are included in this disclosure.

[0114] Regarding the above-described embodiments, the following notes are further disclosed.

[0115] (Note 1)

[0116] A machining program correction device 10 corrects the relative movement path between a tool used in the machining program correction device 10 and a workpiece. The machining program correction device 10 includes: a machining program parsing unit 12 that parses the machining program and extracts a group of instruction points; an estimated machining surface generation unit 14 that generates an estimated machining surface based on the group of instruction points; a tool path correction unit 16 that corrects the tool path by moving, adding, or deleting instruction points based on the distance to the estimated machining surface; and a machining program output unit 18 that converts the tool path corrected by the tool path correction unit into a machining program and outputs it.

[0117] (Note 2)

[0118] In the machining program correction device 1 described above, the correction method of the tool path correction unit 16 is to move, add or delete instruction points to converge to a predetermined tolerance.

[0119] (Note 3)

[0120] In the machining program correction device 1 described above, the correction method of the tool path correction unit is to move, add, or delete command points to converge to a predetermined periodic feed.

[0121] (Note 4)

[0122] In the aforementioned machining program correction device 1, the correction method of the tool path correction unit is to move, add, or delete instruction points to match a predetermined path pattern.

[0123] (Note 5)

[0124] In the machining program correction device 1 described above, the tool path correction unit switches the tool path correction method based on information such as the distance to the estimated machining surface, the target tolerance, the periodic feed, and the path mode, i.e., the tool path correction parameters.

[0125] Explanation of reference numerals in the attached figures

[0126] 1 Numerical control device

[0127] 10. Machining program correction device

[0128] 12 Machining Program Analysis Department

[0129] 14 Estimated Machining Surface Generation Section

[0130] 16 Tool Path Correction Department

[0131] 18 Machining Program Output Department

[0132] 22 processing procedures

[0133] 24. Modified machining program

[0134] 30 instruction point group

[0135] 32 instruction points

[0136] 60 Tool Path

[0137] 61. Tool path before correction

[0138] Tool paths revised in sections 62-65

[0139] 90 Estimated Machining Surface

[0140] 100 main path

[0141] 140 Connection Path.

Claims

1. A machining program correction device, used in a numerical control device, for correcting a machining program of a specified relative movement path between a tool and a workpiece, characterized in that, The machining process correction device includes: The machining program analysis unit analyzes the machining program and extracts the instruction point group. The estimated machining surface generation unit generates an estimated machining surface based on the instruction point group; A tool path correction unit that corrects the tool path by moving, adding, or deleting instruction points based on the distance to the estimated machining surface; and The machining program output unit transforms the tool path corrected by the tool path correction unit into a machining program and outputs it.

2. The machining program correction device according to claim 1, characterized in that, The correction method of the tool path correction unit is to move, add, or delete instruction points to converge to a predetermined tolerance.

3. The machining program correction device according to claim 1, characterized in that, The correction method of the tool path correction unit is to move, add, or delete command points to converge to a predetermined periodic feed.

4. The machining program correction device according to claim 1, characterized in that, The correction method of the tool path correction unit is to move, add, or delete command points to match the predetermined path pattern.

5. The machining program correction device according to any one of claims 2 to 4, characterized in that, The tool path correction unit switches the tool path correction method based on information such as the distance to the estimated machining surface, target tolerance, periodic feed, and path mode, i.e., tool path correction parameters.

Images