Program structure is nothing more then organizing your CNC program. Your programs will become easier to read, understand and follow by separating and labeling the individual operations. Next, break the program into the different program formats. There are three basic format groups (program, tooling &; operation), each being broken into two sub groups (start & end). Examples of each format group are given below.

Structure programming will save your company money. If you use the same format (structure) for all programs you write, you will be able to repeat past successes and eliminate common programming errors. Programs will be easier to write if there is a structure to follow. And, program structure can be used as your outline when training new employees.

PROGRAM START

:1190(FW-01305-08) ( REVISED 7/25/2000 ) B2190 N10(START UP) M97 G40G00T0G99G20G97/M08 M11 G300X0.750Z1.38T1414 G150Z0.539 M10 M3S2000 G00X2.283Z-.08

Program start includes all information needed to prepare the machine for operation. This example is a Swiss Style Screw machine. First two lines have main program number, part name and issue date. The next block of information is the program number for the proper sub program. The last block of information cancels out tool offset, shut off tool nose radius compensation, set the machine in rapid, IPR, and RPM mode. Since this is a Swiss style machine it opens the main collet, regrip the stock, reset the coordinate system, closes the collet and send the cutoff tool to home position.

PROGRAM END
X-.09F.001 G250 G160H9902 GOTO5 M2	Program end contains all information needed to close the program. In this example, spindle synchronization is cancelled, length of bar is checked to determine if new bar is needed and return to start of program.

TOOLING START

N40 ( form radius ) N45 T01 M06 N50 G64 G40 G54 G90 S2800 M03 N55 G00 X-0.217 Y-0.002 Z4.0 M08

Tooling start is everything needed to prepare the tool for machining. In this machining center example the first line is a description of the process about to be perform. The next line call up the tool and place it in the spindle. Line number 50 cancel cutter compensation, activate the correct WPC and start the spindle rotating at the speed programmed. Line number 55 positions the tool at rapid to start position for the machining process and turn coolant on.

TOOLING END
N155 G00 G40 Z1.0 M09 N160 G91 G28 Y0 Z0 M05 N165 G90	Tooling end is the information used to end machining when you are done using the tool. Line number 155 cancels tooling compensation and retracts the tool to a safe position while shutting off the coolant. It then sends the tool to tool change position and stops spindle rotation.

OPERATION START
M05 M50 ( MILL SLOT ) T1212 /M08 M24 S4000 G50 U0.0 Y0.0 W-.125 (DIA OF CUTTER )	Special operations start out different then the normal tooling start. This example shows the steps needed to use live tooling on a Swiss style screw machine. The spindle is stopped, C axis is activated, Tool is called up, Tool direction/rotation is started and offsets are applied. NOTE: the use of additional rem statements to give more detail information within the program.

OPERATION END
G50 U0.0 W0.032 G00 X2.283 M25 T0 G99 M51 M01	Special operations always deviate from the standard operating conditions. At the end of the operation the machine must be returned to it's normal state. This example shows the offsets that were applied being cancelled, live tooling rotation being stopped, feedrate being set back to IPR and C-axis being cancelled.

GB Custom Programming
2233 2nd Avenue West
Monroe, WI. 53566-2707
608-325-3745
E-mail: gabahn@wekz.net