Programming Systems

Two types of programming modes are used for CNC, incremental and absolute. Both systems have applications in CNC programming, and no system is either right or wrong all the time. Controls on machine tools are capable of using both the incremental or absolute programming.

Incremental System

In the incremental system, dimensions or positions are given from a previous known position. Incremental dimensioning on a job print is shown in Fig. 36-8. The dimensions for each hole are given from the previous hole. One disadvantage of incremental positioning or programming is that if there is an error made in any location, this error is carried over to all the locations made after this point.

Command codes, tell the machine to move the table, spindle and knee are explained using a vertical milling machine as an example:

• X plus (X+) command moves the cutting tool to the right of the last point.

• X minus (X-) command moves the cutting tool to the left of the last point.

• Y plus (Y+) command moves the cutting tool toward the column.

• Y minus (Y-) moves the cutting tool away from the column.

• Z plus (Z+) command moves the cutting tool or spindle up or away from the workpiece.

• Z minus (Z-) command moves the cutting tool down or into the part.

In incremental programming, the G91 command indicates to the computer and MCU that programming is to be in the incremental mode.

Absolute System

Absolute program locations are always given from a single fixed zero or origin point, Fig. 36-9. The zero or origin point may be a position on the machine table, such as the corner of the worktable, or at any specific point on the workpiece. In absolute dimensioning and programming, each point or location on the workpiece is given as a certain distance from the zero or reference point. Therefore, in the absolute system of dimensioning or programming, an error in any dimension is still an error, but the error is not carried on to any other location.

• X plus (X+) command moves the cutting tool to the right of the zero or origin point.

• X minus (X-) command moves the cutting tool to the left of the zero or origin point.

• Y plus (Y+) command moves the cutting tool toward the column.

• Y minus (Y-) command moves the cutting tool away from the column.

In absolute programming, the G90 command indicates to the computer and MCU that the programming is to be in the absolute mode.

Positioning Systems

CNC programming falls into two categories: point-to-point and continuous path machining, Fig 36-10. A knowledge of both systems is necessary to understand the applications of each in CNC programming.

Point-to-Point Positioning

Point-to-point positioning is used when it is necessary to accurately locate the spindle, or the workpiece mounted on the machine table, at one or more specific locations to perform operations such as drilling, reaming, boring, and tapping.

• Point-to-point positioning is the process of positioning from one coordinate (XY) position or location to another, performing the machining operation and continuing this pattern until all the operations have been completed at all programmed locations, Fig. 36-11.

• As long as each point or hole location in the program is identified, this operation can be repeated as many times as required.

• Point-to-point machining moves from one point to another as fast as possible (rapid motion) while the cutting tool is above the work surface.

• Both XY axes move simultaneously and at the same rate during rapid traverse. This results in a movement along a 45° angle line until one axis is reached, and then there is a straight line movement to the other axis.

Continuous Path (Contouring)

Contouring, or continuous path machining, involves work that is produced on a milling machine or a lathe, where the cutting tool is in constant contact with the workpiece as it travels from one programmed point to the next. Continuous path is the ability to control the motion of two or more machine axes simultaneously to keep a steady cutter workpiece relationship. The programmed information must accurately position the cutting tool from one point to the next and follow an accurate path at a programmed feed rate to produce the form or contour required, Fig. 36-12.

The method by which contouring machine tools move from one programmed point to the next is called interpolation. This is the ability to merge individual axis points into a predefined tool path. There are five methods of interpolation: linear, circular, helical, parabolic, and cubic. All controls are capable of both linear and circular interpolation. Helical, parabolic, and cubic interpolation are used by industries that manufacture parts that have complex shapes, such as aerospace parts dies and molds for car bodies.

Linear Interpolation

Linear interpolation consists of any programmed points linked together by straight lines, whether the points are close together or far apart, Fig. 36-13. Curves can also be produced with linear interpolation by breaking them into short, straight-line segments. This method has limitations, because a very large number of points would have to be programmed to describe the curve in order to produce a contour shape.

A contour programmed in linear interpolation requires the coordinate positions for the start and finish of each line or segment. Therefore, the end point of one line or segment becomes the start point for the next segment, and so on, throughout the entire program.

The accuracy of a circle or contour shape depends on the distance between each two programmed points. Any complex forms on two axes can be generated by using circular interpolation.