2 Applications When Using Incremental Mode is Better

While there are a number of ways to manipulate the coordinates being used in a CNC program, such as polar coordinates and coordinate rotation, there are only two positioning modes: absolute mode and incremental mode. With absolute mode, coordinates are specified from the current program origin (often called program zero for the workpiece coordinate system). With incremental mode, coordinates are specified from the cutting tool’s current position.

For machining centers, absolute mode is commanded by G90; incremental by G91. All coordinates following a G90 will be taken from the program zero point. Coordinates following a G91 will be taken from the cutting tool’s most recent position. For most turning centers, the positioning mode is implied by the letter address used to specify the coordinate. X and Z, for example, specify the absolute positions. U and W specify incremental movements.

Featured Content

Automation is for Everyone READ MORE

Why Add TASC to Your List? READ MORE

Choosing the Right Drill Type READ MORE

Most programmers would agree that absolute mode is better than incremental mode for two important reasons:

• Absolute coordinates are easier to calculate and understand since they are taken from a common origin. By comparison, a series of incremental positioning movements can be difficult to follow since each position is taken from the cutting tool’s previous position.
• Mistakes are not compounded when using the absolute mode. When an incorrect coordinate is used, only one positioning movement will be wrong. With incremental mode, when a mistake is made, all positioning movements from the point of the mistake will be incorrect.

For these reasons, most programs are developed using the absolute mode exclusively. Indeed, some programmers have never used the incremental mode. That said, there are at least two times when using incremental mode can be more advantageous.

When programming sculptured surfaces

This is a popular application for four- and five-axis machining. A CAM system creates a series of very tiny positioning movements that cause the cutting tool to form a complex surface. The smaller the motions, the finer the resolution the surface will have. Using incremental mode for these tiny motions can dramatically shorten a program’s length.

Consider making a 0.004-inch motion from 10.0182 to 10.0122 in the X-axis. With the absolute mode, this positive direction movement requires eight characters (X10.1022). The same motion in the incremental mode will require only three characters (X40), assuming fixed format programming is being used (commonly a parameter setting). All other axes — Y, Z and the rotary axes — will experience similar reductions, meaning the incremental version of a sculptured surface program will be well less than half the length of the absolute version. This can be an important concern, even with modern FANUC-controlled machines since memory capacity is limited. It requires, of course, the CAM system to be configured to generate incremental using fixed format.

For certain hole-machining canned cycle applications

When programming hole-machining canned cycles in the absolute mode, each hole requires one command. Each command could cause many motions. A chip-breaking drilling cycle (G73 for a FANUC CNC), could cause hundreds of motions per hole, depending on the depth of the hole and the depth of each peck. But still, one command is required for every hole.

In contrast, multiple holes can be specified per command when programming in the incremental mode. The limitation is that the holes must be equally spaced, as is commonly the case with the holes required in a manifold.

Consider 100 holes in a 10.0-inch by 10.0-inch grid that are equally spaced at 1.0-inch apart. 100 commands will be required to machine these holes if working in the absolute mode. With the incremental mode, almost an entire row/column of holes can be programmed per command, reducing the number of required commands to about twenty (example shown using FANUC method):

• G90 G00 X1.0 Y1.0 (Move to first hole)
• G43 H01 Z0.1 (Instate tool length compensation)
• G91 G73 X0 Y0 R0 Z-1.1 Q0.1 F6.0 (Machine first hole)
• X1.0 L9 (Machine the rest of the equally spaced holes in the first row)
• Y1.0 (Machine the first hole in the second row)
• X-1.0 L9 (Machine the rest of the holes in the second row)
• Y1.0 (Machine the first hole in the third row)
• X1.0 L9 (Machine the rest of the holes in the third row)
• Y1.0 (Machine the first hole in the fourth row)
• X-1.0 L9 (Machine the rest of the holes in the fourth row)
• Y1.0 (Machine the first hole in the fifth row)
• X1.0 L9 (Machine the rest of the holes in the fifth row)
• Y1.0 (Machine the first hole in the sixth row)
• X-1.0 L9 (Machine the rest of the holes in the sixth row)
• Y1.0 (Machine the first hole in the seventh row)
• X1.0 L9 (Machine the rest of the holes in the seventh row)
• Y1.0 (Machine the first hole in the eighth row)
• X-1.0 L9 (Machine the rest of the holes in the eighth row)
• Y1.0 (Machine the first hole in the nineth row)
• X1.0 L9 (Machine the rest of the holes in the nineth row)
• Y1.0 (Machine the first hole in the tenth row)
• X-1.0 L9 (Machine the rest of the holes in the tenth row)
• G80 G90 (Cancel canned cycle, back to absolute mode)

The L word specifies the number holes to be machined per command. If the L word is left out, the CNC assumes one hole.