Sequence number techniques Most entry level programmers are taught in basic CNC courses to use sequence numbers (N words) to number the commands in the program Especially helpful with longer programs, this helps them confirm that they are on the correct line of the program before taking any action (modifying a command, rerunning a tool, etc) Most programmers that use sequence numbers also place them in a logical order We recommend, for instance, that programmers skip five numbers between lines (N5, N10, N15, and so on) to allow inserting additional commands if required Note first of all that sequence numbers are available for the programmer They are not required by the CNC control (except in special cases) They can be left out of the program entirely and can even repeat in the program Eliminating sequence numbers with limited memory capacity Since memory capacity is still at a premium with some CNC controls, CNC users sometimes find that they cannot fit all of the programs they want to in the control (sometimes they cannot place but one lengthy program in the control) Whenever CNC users face the problem of running out of memory, the first thing they ll do to shorten programs is eliminate sequence numbers Using for restart blocks It is often necessary to rerun tools And of course, the CNC setup person or operator must find the restart block for a tool as part of the restart procedure The programmer can make it very easy for setup people and operators if they place a special sequence number at the pickup block for each tool If, for example, the programmer has eliminated sequence numbers to conserve memory space, they can still use a restart block sequence number that corresponds to the tool station number Here is an example program that uses this technique O0008 (Program number) (Center drill) N1 G54 G90 S1000 M03 T02 (Select coordinate system, absolute mode, turn spindle on CW at 1000 RPM, get next tool ready) G00 X375 Y375 (Rapid over first hole) G43 H01 Z1 (Rapid down to just above work surface) G81 R1 Z-25 F3 (Center drill first hole) Y2625 (Center drill second hole) X25 Y15 (Center drill third hole) X4625 Y2625 (Center drill 4th hole) Y375 (Center drill last hole) G80 (Cancel canned cycle) G91 G28 Z0 (Return to tool change position) M01 (Optional stop) N2 T02 M06 (Change tools to 25 drill) 1
G54 G90 S1100 M03 T03 (Select coordinate system, absolute mode, turn spindle on CW at 1100 RPM, get next tool ready) G00 X375 Y375 (Rapid over first hole location) G43 H02 Z1 (Rapid down to just above work surface) G81 R1 Z-65 F25 (Drill first hole) Y2625 (Drill second hole) X4625 (Drill third hole) Y375 (Drill last hole) G80 (Cancel canned cycle) G91 G28 Z0 (Return to tool change position) M01 (Optional stop) N3 T03 M06 (Place 375 drill in spindle) G54 G90 S900 M03 T01 (Select coordinate system, absolute mode, turn spindle on CW at 900 RPM, get next tool ready) G00 X25 Y15 (Rapid over hole location) G43 H03 Z1 (Rapid down to just above work surface) G81 R1 Z-65 F40 (Drill hole) G80 (Cancel cycle) G91 G28 Z0 (Return to tool change position) M01 (Optional stop) G91 G28 X0 Y0 (Return to reference point in X-Y) T01 M06 (Place first tool back in spindle) M30 (End of program) If you do use sequence numbers in your program, you can use a variation of the technique Pick a series of special sequence numbers as restart block numbers Use, for instance, N9001 as the restart block for tool one, N9002 for tool two, and so on Note that many setup people and operators have learned a simple technique for finding the restart block without needing sequence numbers to do so They simply scan to the tool station number word that actually makes the tool change (normally the T word) and then back the cursor up to the beginning of the restart command Sequence numbers as statement labels Fanuc and Fanuc-compatible controls have special canned cycles that key on sequence numbers With the G70, G71, G72, and G73 turning center multiple repetitive cycles, for instance, P and Q words within the command specify starting block and ending block sequence numbers for the finish pass definition In this case, each sequence number being pointed to is called a statement label In a main program (not a subprogram), you can use statement labels in conjunction with an unconditional branching command And with standard Fanuc and Fanuc-compatible controls the unconditional branching word is M99 (note that when used as an unconditional branching command, the M99 must be in the main program) A P word in the M99 command points to the statement label The command N055 M99 P100 2
tells the control to jump to line N100 (specified by the P word) Note that if your control has parametric programming capabilities, a GOTO word can be used as the unconditional branch Looping with block delete In a previous lesson related to the block delete function, we give an example for trial boring on a machining center A subprogram is called four times, giving the setup person four tries to get the boring bar sized If it is not sized after the fourth try, the program will bore to depth, regardless of the boring bar size Here are the commands giving four tries N255 T04 M06 (23750 boring bar) N260 G54 G90 S450 M03 T05 (Select coordinate system, absolute mode, start spindle, get next tool ready) N265 G00 X40 Y40 (Move to first hole location) N270 G43 H04 Z01 M08 (Instate tool length compensation, move to Z position, start coolant) N275 F25 (Ensure that trial boring program uses desired feedrate) /N280 M98 P1000 (Jump to trial boring sub program) /N285 M98 P1000 (Give second trial boring try) /N290 M98 P1000 (Give third trial boring try) /N295 M98 P1000 (Give fourth trial boring try) N300 G86 R01 Z-10 F25 (Bore hole to depth) Consider these commands: N255 T04 M06 (23750 boring bar) N260 G54 G90 S450 M03 T05 (Select coordinate system, absolute mode, start spindle, get next tool ready) N265 G00 X40 Y40 (Move to first hole location) N270 G43 H04 Z01 M08 (Instate tool length compensation, move to Z position, start coolant) N275 F25 (Ensure that trial boring program uses desired feedrate) /N280 M98 P1000 (Jump to trial boring sub program) /N285 M99 P280 N290 G86 R01 Z-10 F25 (Bore hole to depth) In line N285, if block delete is turned on (trial machining), the M99 P280 is telling the control to go back to line N280, which will execute the subprogram to trial bore Notice that the control is stuck repeating line N280 until the setup person or operator turns on the block delete switch, at which point the control will skip line N285 3
Changing machining order There may be times during a program s verification that severe mistakes in process are discovered For example, say a program is prepared for a turning center that follows this process 1) Rough turn 2) Finish turn 3) Drill 2" hole 4) Rough bore 5) Finish bore Experienced machinists would agree that you should rough everything before you finish anything In this process, the Finish turning is being done before the drilling and rough boring It is quite likely that during these operations, the workpiece will be deformed slightly, meaning the turned diameter will probably not be concentric to the bored diameter While this may be a relatively obvious processing mistake, there may be many times you wish to change machining order right on the machine You may, for example, wish to test a change in process that you hope will cause a burr to be thrown in a different direction Unless your CNC control has mass editing capabilities like cut and paste (many current model controls don t have these editing capabilities), the programmer must go back to the office and change the program within a CNC text editor Using cut and paste techniques, they will modify the original program to reflect the process change and download the corrected program to the CNC machine tool Depending on the availability of the programmer, the programmer s aptitude, whether the computer is available, and how quickly programs can be transferred, this wasteful on-line task could take from fifteen to forty-five minutes Keep in mind that newer CNC controls have very powerful text editors which allow cut and paste techniques to be done right on the CNC control When available, these editors should be used to minimize the CNC machine s downtime Most are simple enough to use that the setup person may be able to make the required program changes without needing the programmer s help For those machines that do not have cut and paste features, you can use unconditional branching to change machining order The setup person can quickly and easily change the program to match the desired machining order Here is an example to stress how easy it is First we show the incorrect program based on the previous process O0008 (Program with incorrect process) N005 T0101 M41 (Rough turning tool) N010 G96 S400 M03 (Start spindle CW at 400 SFM) N015 G00 X3040 Z01 (Rapid to rough turn diameter) N020 G01 Z-1995 F0017 (Rough turn) N025 X325 (Feed up face) N030 G00 X60 Z50 (Rapid to tool change position) N035 M01 (Optional stop) N040 T0202 M42 (Finish turning tool) 4
N045 G96 S600 M03 (Start spindle CW at 600 SFM) N050 G00 X3 Z01 (Rapid to diameter to be turned) N055 G01 Z-20 F0006 (Finish turn) N060 X325 (Feed up face) N065 G00 X60 Z50 (Rapid to tool change position) N070 M01 (Optional stop) N075 T0303 M41 (2" drill) N080 G97 S300 M03 (Start spindle CW at 300 RPM) N085 G00 X0 Z01 (Rapid to position) N090 G01 Z-26 F009 (Feed to depth) N095 G00 Z01 (Rapid out of hole) N100 G00 X60 Z50 (Rapid to tool change position) N105 M01 (Optional stop) N110 T0404 M41 (15" rough boring bar) N115 G96 S400 M03 (Start spindle CW at 400 SFM) N120 G00 X2085 Z01 (Rapid to rough bore diameter) N125 G01 Z-1995 F0010 (Rough bore) N130 X20 (Feed down face) N135 G00 Z01 (Rapid out of hole) N140 X60 Z50 (Rapid to tool change position) N145 M01 (Optional stop) N150 T0505 M42 (15" finish boring bar) N155 G96 S600 M03 (Start spindle CW at 600 SFM) N160 G00 X1125 Z01 (Rapid to position) N165 G01 Z-20 F0006 (Finish bore) N170 X20 (Feed down face) N175 G00 Z01 (Rapid out of hole) N180 G00 X60 Z50 (Rapid to tool change position) N185 M30 (End of program) Here is the corrected version of the program that uses the desired process O0008 (Program with incorrect process) N005 T0101 M41 (Rough turning tool) N010 G96 S400 M03 (Start spindle CW at 400 SFM) N015 G00 X3040 Z01 (Rapid to rough turn diameter) N020 G01 Z-1995 F0017 (Rough turn) N025 X325 (Feed up face) N030 G00 X60 Z50 (Rapid to tool change position) N035 M01 (Optional stop) N038 M99 P075 (Jump to line N075) N040 T0202 M42 (Finish turning tool) N045 G96 S600 M03 (Start spindle CW at 600 SFM) N050 G00 X3 Z01 (Rapid to diameter to be turned) 5
N055 G01 Z-20 F0006 (Finish turn) N060 X325 (Feed up face) N065 G00 X60 Z50 (Rapid to tool change position) N070 M01 (Optional stop) N073 M99 P185 (Jump to end of program) N075 T0303 M41 (2" drill) N080 G97 S300 M03 (Start spindle CW at 300 RPM) N085 G00 X0 Z01 (Rapid to position) N090 G01 Z-26 F009 (Feed to depth) N095 G00 Z01 (Rapid out of hole) N100 G00 X60 Z50 (Rapid to tool change position) N105 M01 (Optional stop) N110 T0404 M41 (15" rough boring bar) N115 G96 S400 M03 (Start spindle CW at 400 SFM) N120 G00 X2085 Z01 (Rapid to rough bore diameter) N125 G01 Z-1995 F0010 (Rough bore) N130 X20 (Feed down face) N135 G00 Z01 (Rapid out of hole) N140 X60 Z50 (Rapid to tool change position) N145 M01 (Optional stop) N150 T0505 M42 (15" finish boring bar) N155 G96 S600 M03 (Start spindle CW at 600 SFM) N160 G00 X1125 Z01 (Rapid to position) N165 G01 Z-20 F0006 (Finish bore) N170 X20 (Feed down face) N175 G00 Z01 (Rapid out of hole) N180 G00 X60 Z50 (Rapid to tool change position) N183 M99 P040 (Go back to line N040 to finish turn) N185 M30 (End of program) With three simple commands (lines N038, N073, and N183) we have quickly changed the machining order to match our desired process Admittedly, this program is rather difficult to follow since it is not executed in sequential order For this reason, we still recommend that the programmer eventually changes it in the conventional manner But since the machine is running production, this can be done at the programmer s leisure 6