Tool Radius Compensation Analysis

This paper starts from the errors that occur when students apply tool radius compensation programming during the CNC programming teaching process, and discusses the errors in the application of the tool radius compensation function. It strives to find out the problem through error analysis, so that the operator can accurately apply the tool radius compensation function to ensure the processing accuracy of parts processing.

CNC machining has the characteristics of high machining accuracy, high efficiency and stable quality. Reasonable mastery of tool compensation methods, flexible application of tool compensation functions and reasonable setting of tool radius compensation values ​​are important factors to ensure accuracy and stable quality. However, in the process of CNC programming, some errors in the application of tool radius compensation functions often occur. Therefore, it is necessary to discuss the tool radius compensation method of CNC machining.

1. Tool radius compensation principle

During the machining process, the CNC machine tool controls the trajectory of the tool center. Therefore, when programming CNC, programming can be performed according to the trajectory of the tool center. This programming method is called tool center programming. Since there is a margin in rough machining, the dimensional accuracy of the parts is not greatly affected. Tool center trajectory programming can be used for simple graphics. However, when the shape of the part to be machined is more complex, if tool center programming is used, it will bring a lot of workload to calculate the key points, and the calculation error of the key points often affects the interpolation operation of the machine tool, which in turn generates an alarm and prevents the machining from proceeding normally. Therefore, theoretical contour programming can be used, that is, programming according to the contour of the graphics. When using theoretical contour programming, it is necessary to pre-set the offset parameters in the system. The CNC system will automatically calculate the tool center trajectory so that the tool deviates from the contour of the graphics by a tool value, so that the tool can process the actual contour of the graphics. This function is the tool radius compensation function.

2. Tool Compensation Process

The tool compensation of the numerical control system is to hand over the process of calculating the tool center trajectory to the CNC system for execution. The tool radius is not considered during programming, and programming is performed directly according to the contour shape of the part, while the actual tool radius is placed in a programmable tool radius offset register. During the processing, the CNC system automatically calculates the tool center trajectory based on the programmed program and the tool radius in the tool offset register to complete the processing of the part. When the tool radius changes, there is no need to modify the part program, only the tool diameter value in the tool radius register needs to be modified.

Today's CNC systems are generally equipped with 16, 32, 64 or more programmable tool offset registers, and the tools are numbered for tool compensation. When performing CNC programming, you only need to call the register number corresponding to the tool compensation parameter to perform processing. During processing, the CNC system takes the tool radius value corresponding to the number from the register, performs compensation calculations on the tool center trajectory, and generates the actual tool center trajectory. When tool radius compensation is executed, the intersection calculation method is used, that is, before each program execution starts, the system will first read in two segments and calculate their intersection, and then automatically add the tool compensation vector path on the left or right side of each forward direction according to the vector of the startup phase.

Analysis of incorrect application of tool radius compensation #e#3. Analysis of incorrect application of tool radius compensation

1. Correct use of tool radius compensation instructions

Use G41 or G42 to create a tool compensation command, and use G40 to cancel a tool compensation command. The format is:

G01 G41(G42)G17(G18, G19)X___Y___D___,

G01 G40 X___Y___

Among them, G41 is the left tool compensation, which is clockwise when processing the outer contour and counterclockwise when processing the inner contour; G42 is the right tool compensation, which is counterclockwise when processing the outer contour and clockwise when processing the inner contour.

First, the compensation plane should be specified. The CNC system generally defaults to G17, which can be omitted. If compensation is to be performed on the YOZ or XOZ plane, it must be specified and cannot be omitted. In addition, the switch of the tool radius compensation plane must be performed in the compensation cancellation mode. The establishment and cancellation of tool radius compensation can only be done with G00 or G01, but not G02 or G03.

For the cutting outer contour shown in Figure 1, an alarm will be triggered if the following procedure is used.

34

N10 G54 G90 G00 X20 Y0 S800 M03

N20 G41 G03 X20 Y20 R10 D01 F200

N30 G02 X20 Y60 R20

N40 G01 X50 Y60

N50 G02 X50 Y20 R20

N60 G03 X50 Y0 R10

N70 G40 G00 X0 Y0 M05

N80 M30

The reason for the error is that in the N20 program segment, G03 is used in the radius compensation instruction in the hope of preventing feed marks from being produced on the surface of the part, but this program will alarm and terminate.

2. Undo tool compensation settings

When tool compensation is canceled, G02 or G03 cannot be used to cancel tool compensation. For example, if the N60 segment in the above program is changed to "N60 G40 G03 X50 Y0 R10", an alarm will still be triggered when the program is executed to this segment.

3. Pay attention to the feed position when the dry run reaches the tool compensation position

When cutting into the workpiece from the straight edge for processing, the tool compensation instruction should pay attention to setting the end point coordinates and the processed section on the same straight line to avoid alarms due to overcutting. The so-called overcutting here refers to the phenomenon that the system will think that the cutting inner contour produces tool interference when the tool is running in the empty stroke. For example, if the trajectory shown in Figure 2 is processed according to the program "g89", the system will alarm. Because in this program, the processing trajectory is OEAB, since OE and EA (as shown in Figure 2) form an angle less than 90°, the system will think that the tool has interfered. If N20 and N30 are changed to a program segment "G41 G00 X20 Y20 F200D01" (that is, the processing trajectory is OAB), or N20 is changed to "G41 G00 X20 Y10", and N30 and N40 are changed to "G01 X20 Y60 F200", the program can be executed correctly.

g89

N10 G54 G90 G00 X0 Y0 S800 M03

N20 G41 G00 X30 Y10 D01

N30 G01 X20 Y20 F200

N40 Y60

N50 X60

N60 Y20

N70 X20

N80 G40 G00 X0 Y0 M05

N90 M304. Overcutting of inner contour tool compensation

When machining the inner contour, if the angle between the two straight lines of the inner contour is less than 90°, when the tool radius is too large and the radius compensation instruction is used for manual programming, overcutting will occur. As shown in Figure 3, the programming trajectory is AB →BC →CD, which is the intersection of the tool center trajectory corresponding to AB and BC. When the programming trajectory CD is read in, the upper trajectory must be corrected to determine that the tool center should be moved from point to point . At this time, overcutting will inevitably occur as shown in the shaded part of the figure.

5. Inner arc tool compensation setting

When machining inner arc contours, the set tool radius should not be larger than the arc radius required for machining, otherwise the system will prompt "overcutting or collision risk, tool interference" etc.

3. Example Analysis

The blank is a 120mm×60mm×10mm plate. The 5mm deep outer contour has been roughly processed, leaving a 2mm margin around it. It is required to process the outer contour and Ф20mm hole as shown in Figure 4. The workpiece material is aluminum (here only the outer contour processing is taken as an example).

U66 (zero point at 0 o'clock)

N10 G54 G90 G00 X0 Y-20 S800 M03

N20 Z-5

N30 G01 G41 Y-10 D01 F200