Postprocessor Statements aptcodes

                        Statements that refer to the operation of the machine rather than to the geometry of the part or the motion of the cutter about the part are called postprocessor statements. APT postprocessor statements have been standardized internationally.Some common statements and an explanation of their meaning follow:

SEQNO/N,incr,k,m ==> This command controls the output sequence line number of the NC programs, Where as N is the initial sequence number, k is the increment desired, if sequence numbers are on desired at rapid motions then m=0, if sequence numbers are desired in all blocks then m=1.   

SEQNO/OFF ==> This command terminates or turn off the sequence number output in the program.

PARTNO/ ==>  This command identify the Program Number given to the Number, Most of the Program number start with the Letter O in the output NC program. 
Example: PARTNO/100 Apt code gives the output of O100 in NC program which defines the program number. 

PPRINT/ ==> This command is called postprocessor print, The character following the command will be printed in the post processor output. the maximum number of characters used can be 66. 
For example: if you want to operator to check the diameter of the hole at M00 you can print a message after M0 as PPRINT/(Check the hole diameter 10mm) ; and your program will appear ad below.
N00001 M00;
N00002 (Check the hole diameter 10mm) ;

MACHIN/ ==> Specifies the postprocessor that is to be used. Every postprocessor has an identity code, and this code must follow the slash mark (/). For example: MACHIN/Fanuc

TOOLNO/ ==> Specifies the tool parameters use in the post processor, define the diameter and the length of the tool used in the programming. 
for example: TOOLNO/100,MILL,10,0,50. Where as 10 is the diameter of the tool, 0 is the radius of the tool and 50 is the length of the tool.

SPINDL/ ==> Refers to spindle speed. If in revolutions per minute (rpm), only the number needbe shown. If in surface feet per minute (sfm), the letters SFM need to be shown, for example:SPINDL/ 100SFM. this command gives the output gcode M03. and SPINDL/OFF gives the output of M05.

LOADTL/ ==> Describes which tool to be loaded to the spindle, the tool magazine as several number of tool with the numbers, this command calls the tool number which is loaded in the magazine. 
Example: LOADTL/12, Calls the tool number 12 and loads into the spindle in case of automatic tool changer. this command gives the output gcode T12 M06

FEDRATE/ ==> Denotes the feed rate. If in inches per minute (ipm), only the number need be shown. If in inches per revolution (ipr), IPR must be shown, for example: FEDRAT/.005,IPR

COOLNT/ ==> This command defines the control of cutting fluid into the machine. 
Example: 
COOLNT/ON - this command gives the output gcode M07.
COOLNT/MIST -this command gives the output gcode M08.
COOLNT/FLOOD - this command gives the output gcode M18 ( Changes in some machine control)
COOLNT/OFF -this command gives the output gcode M09.

TURRET/  ==> Used to call for a selected tool or turret position

CYCLE/ ==> Specifies a cycle operation such as a drilling or boring cycle. An example of adrilling cycle is: CYCLE/DRILL,RAPTO,.45,FEDTO,0,IPR,.004. The next statement might be GOTO/PI and the drill will then move to P1 and perform the cycle operation. The cycle will repeat until the CYCLE/OFF statement is read.. 
CYCLE/DRILL - Drilling cycle, it gives the output of Gcode  G81.
CYCLE/REAM - Drilling cycle, it gives the output of Gcode  G85.
CYCLE/TAP - Drilling cycle, it gives the output of Gcode  G84.
CYCLE/OFF - Drilling cycle, it gives the output of Gcode  G80.


RAPID ==> Means rapid traverse and applies only to the statement that immediately follows it. this command gives the output gcode G00.

END ==> Stops the machine but does not turn off the control system, this command stops all the operations including the coolant, spindle and the machine. its like end of the program or operation. this command gives the Output of M02.

FINI ==> This command ends the programs and resets the program to the beginning of the program, it give the output of gcode M30  

STOP ==> This Command stops the program and let the operator to check the dimensions on the part, and cycle start to continue the program, it gives the out put of mcode M0.

OPSTOP==> This Command Halts the program Similar to STOP, and cycle start to continue the program, it gives the out put of mcode M1. to check the difference go to mcodes section.

INSERT ==> Inserts the command directly into the program, ignoring the postprocesser, use this command carefully, Example INSERT M01, it gives the out put of mcode M01 without calling OPSTOP command.

ORIGIN/ ==> This Apt command gives the origin defined by programmer, 
Example: ORIGIN/54, gives the out put of mcode G54.

FROM/X,Y,Z ==>  FROM Statement initializes the spindle start position from the coordinate system. if the FROM command not used the postprocesser will assume the start point coordinates are X0,Y0,Z0. most of the postprocesser developed gives the warning message for not using FROM command.

ROTABL/ATANGL ==> This command rotates the table at a specified defined angle. 
for example: ROTABL/ATANGL,45 in an 4axis horizontal table machine this command rotates the table at B45, it takes the shortest angle of rotation to reach B45 degrees it may be either clockwise or the anticlockwise.

ROTABL/INCR,45 ==> This command rotates the table 45 degrees incremental from its current position in clockwisse direction.

ROTABL/ATANGL,45,(A)(B)(C)AXIS ==> This command rotates the table 45 degrees in the specified axis either A or B or C as per the programmer commands.


There are several apt commands for the NC Programming, we will be updating one by one to cover all the code list. 

Enjoy learning CNC Programming and APT Programming.