CITIZEN A32 Programming & Orientation Manual
Rev. (02242009)
______________________________________________________ __________________________ ________________________________________________________ ______________________________ __
______________________________________________________ __________________________ ________________________________________________________ ______________________________ __
SWISS CONCEPT
CITIZEN SWISS TYPE TURNING CENTER
SLIDING HEADSTOCK
SPINDLE COLLET
GUIDE BUSHING (Stationary)
+
Z Axis
4
CONVENTIONAL BAR CHUCKER
SINGLE POINT CONTACT
BAR STOCK WHIP
CONVENTIONAL BAR CHUCKER
SINGLE POINT CONTACT
BAR STOCK WHIP
HARM ONICS / VIBRATION TRANSMITTED TO CUTTING AREA
VIBRATION / HARMONICS
5
SWISS TYPE TURNING CENTER
CUTTING FORCE
GUIDE BUSHING (Stationary)
SLIDING HEADSTOCK
SWISS TYPE TURNING CENTER
CUTTING FORCE
GUIDE BUSHING (Stationary)
SLIDING HEADSTOCK
SPINDLE COLLET NO DEFLECTION & VIBRATION
L DISTANCE
+
Z Axis
6
CONVENTIONAL CNC LATHE
CUTTING FORCE L DISTANCE
CONVENTIONAL CNC LATHE
CUTTING FORCE L DISTANCE
DEFLECTION & VIBRATION
7
SWISS TYPE TURNING CENTER WITH LIVE CROSS WORKING TOOLS
CUTTING FORCE
GUIDE BUSHING (Stationary)
SLIDING HEADSTOCK
SWISS TYPE TURNING CENTER WITH LIVE CROSS WORKING TOOLS
GUIDE BUSHING
CUTTING FORCE
(Stationary)
SLIDING HEADSTOCK
SPINDLE COLLET NO DEFLECTION & VIBRATION
L DISTANCE
+
Z Axis
8
CONVENTIONAL CNC LATHE WITH LIVE CROSS WORKING TOOLS
CUTTING FORCE L DISTANCE
CONVENTIONAL CNC LATHE WITH LIVE CROSS WORKING TOOLS
CUTTING FORCE L DISTANCE
DEFLECTION & VIBRATION
9
IDEAL PARTS FOR CNC SWISS TYPE TURNING CENTERS
LONG PARTS ( length / diameter ratio > 3 / 1)
HIGH ACCURACY ( tight tolerances in the tenths)
IDEAL PARTS FOR CNC SWISS TYPE TURNING CENTERS
LONG PARTS ( length / diameter ratio > 3 / 1)
HIGH ACCURACY ( tight tolerances in the tenths)
SECONDARY OPERATIONS ( complex parts) COMPLETE PARTS ( single setup) 10
SWISS TYPE MACHINES CAN HOLD 60% OF BAR STOCK TOL.
SWISS TYPE MACHINES CAN HOLD 60% OF BAR STOCK TOL.
IE: If bar stock varies by .001 The part can vary as much as .0006 Bar stock considerations Bar stock tolerance requirements will vary depending on the part tolerances you are trying to hold. Example- if you have .0003 tolerance on a dia. or .0003 tir concentricity you will want to use ground stock.
11
PROCESSING PARTS ON CNC SWISS TYPE LATHES
ALL I.D. WORK FIRST NO ROUGH AND FINISH (Due mainly to length of G/B locating surface)
PROCESSING PARTS ON CNC SWISS TYPE LATHES
ALL I.D. WORK FIRST NO ROUGH AND FINISH (Due mainly to length of G/B locating surface)
SEGMENT THE WORKPIECE
12
PULLING OUT OF THE GUIDE BUSHING
GUIDEBUSHING (Stationary)
SLIDING HEADSTOCK
PULLING OUT OF THE GUIDE BUSHING
GUIDEBUSHING (Stationary)
SLIDING HEADSTOCK
SPINDLECOLLET
L DISTANCE
+
Z Axis
13
PARTIALLY PULLING IN TO THE GUIDE BUSHING
1: BURR CREATE D BY
2: CLEAN UP BURR -TURN STOCK DIA.
PARTIALLY PULLING IN TO THE GUIDE BUSHING
2: CLEAN UP BURR -TURN STOCK DIA.
1: BURR CREATE D BY TURNING
3: PULL STOCK INTO GUIDE BUSHING ** NOT COMPLETELY OUT**
14
SEGMENT THE WORKPIECE
1
3
6
8
11
12
SEGMENT THE WORKPIECE
1
3
2
4
6
5
8
7
9
11
12
10
15
Machine Outline A32 VII
Machine Specifications w/Guide
Bushing
Machine Capacity 1.260 Bar stock max.(Spindle sleeve I.D. is Main Spindle 1.260 max (Spindle sleeve I.D. is . ”) Sub Spindle .394” MAX Drill .3125” MAX Tap Rotary 12.6 max (1 chuck) Length (main spindle) 5.90 max (2.56” sticking out) Length (sub spindle- with ejection)
RPM MAX Main 8,000 Spindle Sub 8,000 Spindle Rotary 4,000* 4,0 00*
H.P. 5.5/7.5 kW
Indexing .001 Deg. STANDARD
2.2/3.7 kW
.001 Deg. STANDARD
1.0 kW
* Constant RPM Tooling Guide Bushing TD32-NS ###, Collet (TF37SP ###) Collet (TF37SP ###) Smooth Bore .625 Shank T02 – T06 (T01 = .75” Shank) (4)ER16 Collets , T7 – T10 1.0” Shank T11 – T14 1.0” Shank T51 - T54, T31 – T34 23 (Positions) 6 4(3 Cross, 1 Face OPTIONAL) 4 9 (4 on Gang, 5 Backwork block)
Main Spindle Sub Spindle O.D. (static) O.D. (rotary) Front End-Work Back End-Work Number of Tools Turning Cross Drilling / Milling Front END Working Back END Working
Machine Weight 5511.5 Lbs, 2500kg Foot Print (inches) 48L x 98.8W x 70.1H Coolant Tank Cap.
46.2 Gallons
Power Power
208V 208 V , 3 phase phase,, 6KVA 6KVA
Air
.5MPa (72.5psi)
Barfeeder C332
by Edge Technologies
.”)
Bar Capacity
Lubricants Way Oil Vactra #2 Coolant (Oil) Hangsterfer`s, Hangsterfer`s, Blaser’s, Castrol W/ High pressure Blaser’s Vascomill 10 or pump 22 Coolan Coolantt (Water (Water Blaser- BLASOCUT Based) Valcool VNT 800 Air
Oil Same as cutting oil
Capacity
Tool Layout
A32 Type VII
Front EndWorking Tools
Back EndWorking Tools
Machine Layout
Axis Designation 5-axis control 1) Move the tool post vertically (X1 axis). 2) Move the tool post horizontally (Y1 axis). 3) Move the headstock longitudinally (Z1 axis). 4) Move the back headstock horizontally (X2 axis). 5) Move the back headstock longitudinally (Z2 axis).
PROGRAMMING CODES
CITIZEN A32VII
M-CODES
Note: Up
to 4 M-codes can be commanded in a single block. It saves time to command as many M-codes as possible in the same block. Some M-codes are macros and need to be alone on a single line. See (macro) below.
M00-
Program stop. Force the machine to stop. You can't re-start.
M0-
M01-
Optional stop M1- If the OPTIONAL STOP button is on (lit) the executing line $1 or $2 will stop until the CYCLE START button is pressed again, then operation in that line starts running again. If the OPTIONAL STOP button is not lit the M01 command is skipped.
M02-
One cycle stop M2- M2 will queue lines $1-$2 then stop execution of the program if in ONE CYCLE MODE.
M03M3-
Main spindle forward rotation "M3 S1=1000" If commanded wrong "M3 S1000" without "S1=" then the main spindle is commanded by default. 10000 RPM max 200 RPM min
M04M4-
Main spindle reverse rotation "M4 S1=500"
M05M5-
Main spindle stop
M06M6-
(macro) Collet close (main spindle) axis A1. Use it alone on the line because it is a macro! M6M3(M3 won't work) M3M6(Will work but as a habit, use M6 alone.)
-If a CAV barloader is used the A7 axis synchronization is turned on inside of the M6 macro. M07M7-
(macro) Collet open (main spindle) axis A1. Use it alone on the line!
M7M5(M5 won't work) M5M7(Will work but as a habit, use M7 alone.) or
M3S1=1000(or M5) M7 G4U.5(a dwell may be needed for some barloaders to change from sync to push)
-If a CAV barloader is used the A7 axis synchronization is turned off inside of the M6 macro.
M08M8- Short cut program. Used when using a bar loader. M8 shifts control of the BLOCK DELETE button to the bar loader end of bar switch. This lets one section of a program, or a sub-program, run only if the end of bar switch on the bar feeder is tripped.
Main Program M9(beginning- safety) " " O8000(BAR CHANGE SUB) G1X-.1F.002(CUT-OFF) M3S1=300M53 M8 G0 X#814+#815 W-2.(Z OUT OF GB/X ABOVE STOCK)(or X.85) M8(CONFIRM M8) M54(STOP BAR PUSH) /M98P8000(if EOB) M7 M9 M55(START LOAD/WAIT UNTIL DONE) M6 M3S1=#817(or S1=any RPM) (M26) (ONLY IF HEX OR SHAPED STOCK) G99G1W2.F.01 M52 X#824F#822(or X=-.1 F=.002) M99 Note: I used custom variables to have one program do all!
M108-(macro) This has the same function as the B12 series machines. Used when using a bar loader. If the loader sends a signal that the bar is done then the remnant is de-burred, pulled out, and a new bar is loaded. If the bar is still there then M108 is skipped. The RPM and IPR are taken from the Mach Data for the cut-off operation. M108 U.04 C.005 D.04 B.23 S1000 W1.5 F.02 A1. R1 t -CDB are used only if de-burring the remnant before removing from GB. U.04 = Amount above the stock size from the data page, to position before changing bars (diam value) C.005 = Feed in IPR(mm/rev) for de-burring. D.04 = Z axis movement for de-burring. B.23 = X axis position to go to for de-burring. S1000 = Spindle speed used while pulling out remnant. W1.5 = Z axis amount of pull back from GB to remove remnant. F.02 = Feed in IPR(mm/rev) for pulling out of GB. A1. = Dwell after bar load before closing collet. R1 = R1 or R0 If R1 then spindle runs during bar change.
-If any or all options are omitted then default values are used. If all defaults are OK, you can use M108U W S F R1 alone on the line. O1234(MAIN PROGRAM) M9 G99/M52 M6 G4U.5(SOME BARLOADERS) G50Z-.005 "" "" T100(CUT-OFF) G50W-.094 M3S1=3500M24S2=3500 G0Z.5T1 G650 !1!2L650 G231X-.1A-.03F.001 G50W.094 (STILL NEEDS TO BE TESTED BUT SHOULD NOT NEED M8 M8 / ) (M8) (M8) (/)M108 S200 W1.5 F.02 A1 R1 T1(S = less than 2000) M9 M7 G4U.5(SOME BARLOADERS) G0X-.05Z-.005T0 G999 (M6)(SOME BARLOADERS WANT THE COLLET CLOSED/NO DWELL IS NEEDED HERE) N999 M56 M2 or This style of code is from the manual and will also work but the 'M8 M8 / ' is not needed. M8 M8 /M108 S200 W1.5 F.02 A1 R1 T1(S = less than 2000) M9 M09M9- Cancels M8. Returns control of the BLOCK DELETE to the BLOCK DELETE button. If using M8 then put a M9 at the beginning of your program as a safety command if starting the program after a problem.
M10-(macro) Moves the knock-out pin forward to eject the part from the back spindle. If the back spindle is running or the collet is closed M10 won't work. M10 moves the knock out by an air cylinder. You can adjust the speed of knockout advance by the valve located on the front of the piston M11-(macro) Moves knock-out pin reverse. Back in! M11 moves the knock out by an air cylinder. If the back spindle is running or the collet is closed M11 won't work. You can adjust the speed of knockout retract by the valve located on the BACK of the piston
M15-(macro) Back spindle collet close. M16-(macro) Back spindle collet open. M18-(macro) (only with "C" axis option) References the "C" axis and goes to position specified. Only used if simple indexing in 1 deg increments and to enable the axis. M18 C0 G1 XYZ M18 C180.(M18 issued a G0 C?? internally) XYZ -If we want to use "C" axis and rotate it then M18 C0 G98G1C150.F1000.(feed=deg per min)(Feed command is wrong F36. = 360DPM) H120.(incremental)
M20- C-Axis cancel. Not needed but is used for backwards compatibility. Just by commanding M3 also cancels C-Axis. M23-Back spindle forward rotation "M23 S2=1000" 8000 RPM max min 200
M24-Back spindle reverse rotation "M24 S2=500"
M25-Back spindle stop
M28-(macro) (non "C" axis machine only) Spindle indexing. Not used any more because C-Axis is standard. 1 degree increments only. Only absolute commands. M28 S15 M28 S0 M28 S180 Incremental example... 24 indexes in a loop saves many program lines! #100=0 (SET VARIABLE TO 0) WHILE [#100 NE 360] DO1 (MACRO LOOP) G0 X Z (dummy move or you get macro alarm) M28 S#100 (INDEX DIFF. EACH TIME) G1 X.3 F6. (FEED TOOL INTO PART) G0 X.7 (RAPID OUT) #100=#100+15 (INCREMENT VARIABLE BY 15 DEG) END1 (LOOPS TO WHILE, UNTIL #100 IS NOT EQUAL TO 360) (#100 = 0,15,30,45,60,75,90,105,120,135,150,165) (180,195,210,225,240,255,270,285,300,315,330,345)
See the white Mitsubishi programming manual for more details on WHILE DO1 END1 in the macro section.
M31- Work conveyor on.(option). M31 is automatically commanded inside of the part ejection cycle M34. The time on is PLC Constant timer 18016=120 for 12 seconds M33-(macro) Parts collection and moving to the separation/collection position. Uses Basket attached to the sub spindle. M33 W...D...U...E... W= Retract position. When omitted spindle will go to zero. D= Feed rate (IPM) during "Z"retract. When omitted will rapid back! U= "X2" axis position. When omitted will go to "X0". E= Feed rate (IPM) during "X2"retract. When omitted will rapid back! SPECIFY THE VALUE WITH A DECIMAL POINT! ** W...D...U...E... CAN bo omitted.** ** You MUST choose "BASKET" for "BACK SPINDLE" on "MC DATA" screen.** $2 with basket connected to sub spindle (M88)(may be needed) M33 G0Z2.3 M23S2=100 G4U1. M25 M31 T3000 (M89)
$2 with part in sub spindle collet M25 M88 M33 G0Z2.63 M72 M16 M10 G4U.5 M11 M31 M73 T3000 M89
M34-(macro) Series of commands needed for parts ejection from the P.O. spindle all in one command. Collet open, parts catcher in/out, knock out forward, air ect. This can be commanded from $1 or $2 but has two very different functions. If M34 in $1 then dump the part from the catcher mounted on the sub spindle. If M34 from $2 then eject the part from the sub spindle into the parts box. There are many command options that can be used but usually just "M34" is all you need. See the different command options below.
If M34 from $1 and the part is in the catcher basket by using M32 then ... You must be in G600 mode. See M320. Also there can't be any "T3?00" in the $2 program or M34 will function like in $2 and try to knock out a part. M34 X W D U E Z F T S B M34 -nothing else on line then catcher moves away and dumps the part. X -X pos. to go to after collection. Normally not used. W -After the part is caught then the catcher moves back to Z0 or the amount of W from Z0. Used if Parts per 1/chucking is used to save time. Normally not used. D -Feed rate for Z2 to move away from GB. IPM U -Used to change the position of X2 at the dump position of ".156" . Normally don't use. E -Feed rate for X2 to move to the dump position. IPM Z -Move to Z position inside collection box. F -Feed rate when moving into position inside collection box. IPM T -Timer for rotation while back spindle is dumping the part. S -Spindle speed while dumping the part. RPM B -When finished dump, move Z2 to amount B from Z0. $1 G600 M34 (dump part in background of $1 early in the program) " (programming of part) " T100(Cut-Off) G0X1.1Z2.T1 M320X.2 G99G1X-.1F.002 M241 (catch the part but do not eject it) " "
If M34 from $2 and part is in the sub spindle then ... M34 W D U E Z F B T X M34 -nothing else on line then catcher moves away and ejects the part. W -After the part is caught then the catcher moves back to Z0 or the amount of W from Z0. Normally not used. D -Feed rate for Z2 to move away from GB. IPM U -Used to change the position of X2 at the dump position of ".156" . Normally don't use. E -Feed rate for X2 to move to the dump position. IPM Z -Move to Z position inside collection box. F -Feed rate when moving into position inside collection box. IPM B -When finished move Z2 to amount B from Z0. T -Timer for air blow after part is ejected. X -X pos. to go to after collection. Normally not used. $2 M25 M34
M38-(CAV)Bar loader synchronization on and torque off. Only used with special Citizen CAV bar loader. This will make the barfeed pusher, axis A7, mirror Z1. We don't have to use this command, it is used internally in the M6-M7 commands.
M39-(CAV)Bar loader synchronization off and torque on. See M38. This will now hold position. We don't have to use this command, it is used internally in the M6-M7 commands.
M46-(CAV) barloader torque set to 0%
M48-(macro) Back spindle "C" axis on. (only with "C2" axis option) References the "C" axis on the PO spindle and goes to position specified. Only used if simple indexing in 1 deg increments and to enable the axis. M48 C0 G1 XYZ M48 C180.(M48 issued a G0 C?? internally) XYZ -If we want to use "C" axis and rotate it then M48 C0 G98G1C150.F1000.(feed=deg per min)(Feed command is wrong F36. = 360DPM) H120.(incremental)
M50-Check cut-off tool breakage by spindle RPM. You command the main spindle and then use M50. M50 will check if S2 is turning, if so then alarm. If you don't have spindle sync. then you need to free wheel the sub spindle or you get alarms just turning the spindles off. (with spindle sync.) $1 T0100 G0Z2.T1 M3S1=2000M24S2=2000 G114.1H1D-2 S1=3500 G650 !L1
$2 T3000 G50Z0
G650 G0Z-.1 G98G1Z.5F50. M77 M15 !L1 G600 G50Z0
G1X-.1 M5M25 G113 M3S1=300 G4U.5 M50(IF S2 IS TURNING THEN CUT-OFF IS BROKE! ALARM) (ELSE IF S2 NOT TURNING THEN OK, SKIP OVER M50) G600 M5
(without spindle sync.) $1 $2 T0100 G0Z2.T1 G650
T3000 G650 G0Z-.1 G98G1Z.5F50. M15 !L1 G600 G50Z0
!L1 M3S1=100 G4U.7 M3S1=500 G4U.7 M3S1=1000 G4U.7 M3S1=1500 G4U.7 M3S1=2000 " " G1X-.1F.001(CUT-OFF PART) M5M25 G4U2. M3S1=300 G4U.5 M50(IF S2 IS TURNING THEN CUT-OFF IS BROKE! ALARM) (ELSE IF S2 NOT TURNING THEN OK, SKIP OVER M50) G600 M5
M51-(option) Tool breakage detection, by using a switch. After cut-off move Z back a little then position over the switch. This will check if the part is gone. If not then Alarm. M51 X.3 W-.2 X= The X position to move to after the switch is positioned above the bar stock. If no X is commanded then X-.04(1mm) is used. W= The INCREMENTAL amount to move so the switch contacts the proper spot of the part and away from the cut-off tool. If no Z is used then Z stays where it is for the check. $1 G50Z-.005 M6 M51 W-.02 X.3 T200 (continue on)
M52-Flood Coolant oil ON M53-Flood Coolant oil OFF M54-Bar loader feeding pressure stop -BAR LOADER ONLY
M55-Bar loader material replace -Tells bar loader to load a new bar. Then waits until the new bar is in position. See M8. M56-Counter- Increments parts counter by one if in CONTINUOUS CYCLE MODE This can be changed to ANY CYCLE MODE by changing Bit Select #1 bit 2 to a 1 . #6401 bit 2. M57-Cycle stop while in a sub program. Same as M2 but used in a sub program. If running multiple parts with one chucking, one cycle would be multiple parts. Use M57 only in the sub. M61M62M63M64M65-
EXTRA M-CODES FOR SPECIAL CUSTOMER USE
B1- B1 to B256 are also available if using a PLC to read the signals. With M61-M65 there are 5 possible functions. B has 256!
M72- Back spindle air blow ON -clears chips from P.O. collet surface. M73- Back spindle air blow OFF M77- Used with G114.1 to wait for spindle synch. confirmation. See G114.1 M78- (macro) Back spindle indexing 1 deg. "M78 S30." Incremental example... 24 indexes in a loop saves many program lines! #100=0 (SET VARIABLE TO 0) WHILE [#100 NE 360] DO1 (MACRO LOOP) G0 X Z (dummy move or you get macro alarm) M78 S#100 (INDEX P.O. DIFF. EACH TIME) G1 X.3 F6. (FEED TOOL INTO PART) G0 X.7 (RAPID OUT) #100=#100+15 (INCREMENT VARIABLE BY 15 DEG) END1 (LOOPS TO WHILE, UNTIL #100 IS NOT EQUAL TO 360) (#100 = 0,15,30,45,60,75,90,105,120,135,150,165) (180,195,210,225,240,255,270,285,300,315,330,345) See the white Mitsubishi programming manual for more details on WHILE DO1 END1 in the macro section.
M79- Back spindle indexing CANCEL (unlock). M80- Live tool spindle forward. "M80 S3=2000" 5000 RPM max with a 4000 RPM max suggested if running for long duty cycles. Live tool spindle forward. "M80 S3=2000" 4500 RPM max M81- Live tool spindle reverse. M82- Live tool spindle off. M86- Cutting Start interlock ENABLED. Cutting is not started until the spindle reaches the specified RPM.
M88- Interference check OFF. DISABLES crash protection.(Shuts off!) NOT recommended! Safety zones of all axis’ are turned off to work very close to the back spindle. M89- Interference check ON. Enables crash protection. Default condition. M92- Modal exact program stop. Used so corners are not rounded off while turning at high feed rates. This gives small dwells to confirm corners. See also G9 M93- Exact stop cancel. Cancels M92 M94- Back spindle fluctuation detection ON- Checks extra load on the spindle. If too much load, then alarm. M95- Back spindle fluctuation detection OFF (When power on is M94) If you will use G96(CSFM) or G84(rigid tap) then you must first command M95. M96- Main spindle fluctuation detection ON- Checks extra load on the spindle. If too much load, then alarm. M97- Main spindle fluctuation detection OFF (When power on is M96) If you will use G96(CSFM) or G84(rigid tap) then you must first command M97. M98- Sub program call. If commanded "M98 P1111 L5" from line $1 of a main program then the line $1 of sub program O1111 is looped 5 times. If "M98 P1111" is in line $2 of a main program then program line $2 of program O1111 is looped only one time. When the sub is finished M99 returns to the line after the M98 command in the main program. There is one other option to M98. "M98 H1" This command jumps down in the programming line you are in to sequence number N1 and returns when M99 is commanded, to one line after the "M98 H1" command. This is special to make the G999-N999 command easier. Search G999- Also if you use sub programs a lot, this helps to only have one program number to upload/download for your file storage system. -A new argument ,D1 allows to call a sub program stored on a flash card! M98 P H L ,D1 P = Sub Program Number to call H = Line Number in the main program to go to for the sub L = Loops or number of times to run the sub program. No L = L1 ,D1 = Used to enable the flash card to hold the sub program. O1234(main program)
O1111(sub program)
$1
$2
" M98P1111L5
"
$1 (loop 5 times)
M98P1111 " M2 M99
" M2 M99
$2
(loop 1 time) M99 (return to $1)
M99 (return to $2)
O1234(main program no sub) $1 G99M52
$2 M98H1 (goes to line sequence # N1) (M99 returns to here)
M56 G999 N999 M2 M99
G999(only if in one cycle mode) M98H1 (goes to line sequence # N1) (M99 returns to here) N999 M2 M99(returns to beginning of $2) N1 T3100 (CODES NEEDED TO COMPLETE THE PART) T3000 M99(return to line after M98H1)
NEW!!! M98P1234L3,D1 = ,D1 to run a program stored on an external Compact Flash Card. NOTE** The programs can be called and executed ONLY as a subprogram. They CANNOT be used as a main program. **Do NOT remove the CF card during operation!** M99- If commanded in sub program then return from sub program to main program. If commanded in the main program then return to the beginning. If using "M98 H1" then return to the line after "M98 H1" M100-(CAV)Barfeed gripper closed M101-(CAV)Barfeed gripper open M102-(CAV)Barfeed gripper open quickly(don't wait for confirmation) M103-(CAV)Barfeed release bar stock and slide channel forward M104-(CAV)Barfeed slide channel forward M105-(CAV)Barfeed slide channel back M106-(CAV)Barfeed stabilizer close M107-(CAV)Barfeed stabilizer open M108- ***See M8**** M122- Back spindle torque limit 25% ON. Used with G114.1 to help eliminate marking on the part from diff. spindle power. 75% of the torque of the back spindle is cut. M123- Back spindle torque limit 50% ON. Used with G114.1 to help eliminate marking on the part from diff. spindle power. 50% of the torque of the back spindle is cut. M124- Back spindle torque limit OFF. Cancel M122 or M123. Back to 100% M151- (macro) Gang tool post retract. Move the X1 axis to return position. After commanding M151 the X1 axis cannot be commanded until after the next G600 command. The "X" offset is CANCELED!
M160-M169 Are auto set from the G600 commands! M160- Main Spindle S1 cutting start interlock enabled.(ON) M161- Main Spindle S1 cutting start interlock disabled.(OFF) M162- Sub Spindle S2 cutting start interlock enabled.(ON) M163- Sub Spindle S2 cutting start interlock disabled.(OFF) M164- Gang Spindle S3 cutting start interlock enabled.(ON) M165- Gang Spindle S3 cutting start interlock disabled.(OFF) M168- S5 cutting start interlock enabled.(ON) M169- S5 cutting start interlock disabled.(OFF) M180- Back tool spindle forward. M180S5=####. 4000 RPM constant max. M181- Back tool spindle reverse.4000 RPM constant max. M182- Back tool spindle off/Stop. M190- C2-C1 superimpose ON. Used to hold parts with both spindles and be able to move C1 to do secondary work and C2 stays supporting. Inside M190 is "G156C2=C1" $1
$2
M80S3=3000 G98 T700 G0X1.1Z2.5+.59 M18C0 G650
!1!2L650 M190(C2 follow C1) G50W-.59 G0X1.1Z2.5T7 " G0 C180.(or M18C180.) " G0X1.1T0 G50W.59 M82 !1!2L651
M16 M48C0 G650 M72 G0Z-.05 G98G1Z.5F80. M15 M73 !1!2L650
!1!2L651 M191(off in $2) M79
M191- C2-C1 superimpose OFF
M204- Thread Chamfering On. To have an exit chamfer while threading with G92. Chamfering can also be turned on or off by operator switch #17. Using the "M204" code will allow setting changes from the program. M205- Thread Chamfering Off M241- Move Z2 to RETURN position.Command M241 in $1 or after G600 in $2 M260-M269 EXTRA M-CODES FOR SPECIAL RELAY ON/OFF. M320- (macro) Parts catcher used when not picking up with the sub spindle. A basket is mounted to the face of the sub spindle and Z2 will move up to catch the part, then back to dump it into the regular parts catcher. After M320 use M34 to dump the part. See M780 to setup the catcher in MDI. Also the basket to attach to the sub spindle is an option. M320X.2 X= Position to feed to before the basket is under the part. Used to eliminate chips in the catcher. Z= The position of the basket of absolute Z2. Usually not used but can be used to fine adjust catching for problem parts. If not used 165mm or 6.496 is used. F= Feed in IPM for movement of Z2 $1 G0 X.5 (all chamfer commands if needed must be done) (starting X must be more than M32X_) M320X.15 or M320X.15Z9. G1 X-.05 F.002 (when X reaches X.15 then the catcher comes in) M34(dump into ejector arm)
M350 -Rapid Feed Rate Setting The A32 rapid traverse for all axis except X1 is 45-MPM or 1772-IPM, this is extremely fast (fastest in the world!). The X1 rapid rate is 32-MPM or 1260-IPM. Many customers and many parts are normal or have a tolerance of more than or near (+- .0005-.001"). So the rapid rate is fine. But some customers desire to hold tighter tolerance and the thermal characteristics of the ball screws running at the fast rapid rate could possibly make longer warm-up times. Short time cutting and many tool changes could increase thermal growth. For these reasons we have the ability to program the NEW rapid feed rate. We do not have data yet as when exactly this is needed or not, as all part processes are different and more tool changes and less cutting vs low tool changes and long cutting creates totally different thermal conditions. If you have thermal issues, try this function. Also when used, the overall cycle time will increase but very small amounts. M350 X20000 Y20000 Z20000 X Y Z = mmpm (MM per minute feed rate)
$1 M350Z20000 (787IPM) T1200(drill) G0Z-.05T12 G83 Z1. F.003 Q.1 G80G0Z-.05T0 M351(set X1 Y1 Z1 back to full default rapid)
$2 M350Z20000 (787IPM) T3200(drill) G0Z-.05T32 G83 Z1. F.003 Q.1 G80G0Z-.05T0 M351(set X2 Z2 back to full default rapid)
M351 -Rapid Feed Rate Setting Reset Set the rapid rates for all axis back to default. Also when pressing RESET this is reset to default values. M360 -Rapid Feed Acceleration/Deceleration Time Constant Setting ON. This is used for X1-Y1-Z1 only. The A32 rapid traverse for Y1-Z1 axis is 45-MPM or 1772-IPM, this is extremely fast (fastest in the world!). The X1 rapid rate is 32-MPM or 1260-IPM. Many customers and many parts are normal or have a tolerance of more than or near (+- .0005-.001"). So the rapid accel/decel rate is fine. But some customers desire to hold tighter tolerance and the thermal characteristics of the ball screws running at the short time accel/decel could possibly make longer warmup times. Short time cutting and many tool changes could increase thermal growth. For these reasons we have the ability to program a change for the rapid accel/decal time constant. We do not have data yet as when exactly this is needed or not as all part processes are different and more tool changes and less cutting vs low tool changes and long cutting creates totally different thermal conditions. If you have thermal issues, try this function. Also when used, the overall cycle time will increase but very small amounts. M360 x3. Y3. Z3. X3. = set X1 accel/decel time multiplier to 3x or (90*3=270 msec) Y3. = set Y1 accel/decel time multiplier to 3x or (225*3=675 msec) Z3. = set Z1 accel/decel time multiplier to 3x or (158*3=474 msec)
M361-Rapid Feed Acceleration/Deceleration Time Constant Setting OFF Set the time constant, back to default on each axis. Also when pressing RESET this is reset to default values. X1= 90 msec Y1= 225 msec Z1= 158 msec
M430-M437 Special M-CODES for optional Medium pressure coolant pump. M452- Optional Medium pressure coolant pump ON. M453- Optional Medium pressure coolant pump OFF.
CITIZEN A32VII
G-CODES
G0- Rapid traverse G0 X.5; G0 Z1.; G0 X.875 Z0; G0 X.25 Y.45 Z1.56 G00G1- Linear interpolation G1 X.76 F.0015; G1 X.38 Z.05; G1 X.6 Y.29 Z2.457; G01G2- Circular interpolation clockwise direction. G02- When viewing the #1 gang tools, X1 and Z1. You can also use I J K giving the center of the arc from the position you start at before the G2. I=X J=Y K=Z. I, J, K is used when more than a 90 deg arc is needed, usually milling or turning a ball type part.
G0 X.85 Z0 G1 X-.04 F.002 X0 G2 X.5 Z.25 R.25 or G1 Z
G2 X.5 Z.25 I0 K.25
G0 X.85 Z0 G1 X-.04 F.002 X.42 G2 X.5 Z.2 I-.4 K.23 G1 Z
Circle Example... When milling with or without cutter comp(G41/G42), the feed rate given is not true. To get a proper feed rate you have to calculate using the radius desired and the tool radius. Cutting outside corners are different then inside pockets. Use this formula... Outside cutting: DesiredFeed=10 IPM CutRadius=.125 ToolRadius=.1875 Feed=DesiredFeed * ((CutRadius+ToolRadius)/CutRadius) Feed= 3 * ( .3125 / .125) Feed= * 2.5 Feed=7.5 See example on the following page
G19 (Y-Z PLANE SELECTION) G41 G1 Z-.0625 Y0 F10. G2 Z-.0625 Y0 K.3125 F7.5 (CUT A CIRCLE F7.5=F3. at cutting point) G1Y-.1 F10. G40 G18 Inside pocket cutting: DesiredFeed=10 IPM CutRadius=.25 ToolRadius=.125 Feed=DesiredFeed * ((CutRadius-ToolRadius)/CutRadius) Feed= 10 * ( .125 / .25) Feed=10 * .5 Feed=5 G19 G42G1Z.5Y0 F10. X?? G2Z.5Y0K.25 F5. (CUT A CIRCLE F5.=F10. at cutting point) G1X?? F10. G40 G18
G3- Circular interpolation counter-clockwise direction. G03- When viewing the #1 gang tools, X1 and Z1 -See G2
G0 X.85 Z0 G1X-.04 F.002 X.1 Z.08 G3 X .5 Z.28 R.2 F.0015 G1 Z
G4- Dwell G04- G4 can be used 3 different ways... G4 U1. (must have . or 1 = .0001) G4 X1. G4 P1000 (all three dwells = 1. second)
G9- Exact stop mode G09- G9 will make the axis stop after the program line. Used when no radius is allowed on an outside or inside corner. G9 is a one shot g-code. See also M92. G9 G1 Z.5 G10- Offset input from RS232C or program The way Mitsubishi worked this one is much better than Fanuc. If you choose I/O OUTPUT function and download "OFFSET" this will send a bunch of G10 and G11 commands to a file. This is all the offsets in a special code. To send it back to the machine later just pick I/O "tool data" and INPUT, and the offsets are loaded into the machine from the RS232. G10 L11 P1 X.001 Z.005 R.002 (P=offset number) You can also use G10 to set parameters. Please see the Mitsubishi manual for more details.
G12.1- Converts C axis degrees and X axis movement to work like a milling machine. Program X-Y axis and the control converts all the commands to degrees automatically. X and Y are programmed in radius values and zero is at the center of the part, like a milling machine. Tool nose rad comp is also needed to use G12.1 correctly. Thinking about the direction for G2/G3 and G41/G42 is backwards! You have to imagine you are back behind the guide bushing looking to the cutter. If you can't do this, then just do everything opposite! There are some new options while calling G12.1. We used to have to change parameters to use G12.1 #1125 Mill_AX and #1126 MillC , now we can set these while calling G12.1 . See also G16 below. G12.1 (no arguments uses C commands same as G12.1 D1 E=C)
G12.1 D0 E=C D0 -You can use "C" or "Y" as the virtual axis while in G12.1 The manual suggests using "D1" to use "C" but I don't agree. If in G17 X-Y plane, then I suggest you use "D0" to use Y". Your choice, it makes no difference which you use! If D is not on the G12.1 line then "C" is default. Always have "D" first on the G12.1 line! E=C -This will set the axis number of the system to use as the polar axis. This depends if you are using the gang plate in $1 or the U121B option in $2 or $3. Setting E=C will set the proper axis automatically. If you don't use E=C on the line then $1 C axis is default. For safety, always use E=C
(MILL A .3 SQUARE WITH .02R CORNERS) T1000(Live face mill/.25" cutter /1/2"bar) (M5) M18C0 G98M80S3=1200 G0X.8Z.1T10 G12.1 D0 E=C G17 G41G0X.15Y.3 G1Y-.15,R.02F8.(or use G2) X-.15,R.02 Y.15,R.02 X.15,R.02 Y.1 G40G0X.4Y0 G13.1 G18G99M82
G13.1- cancels G12.1 by setting control of the C axis back to C and H G16 - Plane select Y-Z cylindrical machining. To use this plane you need the option of G12.1 milling interpolation. G16 is used to convert polar C axis degrees to linear Y when machining "J" slots or cylindrical cams. Most of these part prints are dimensioned with linear and radial values, not degrees. Also the prints usually show the part cut and spread flat. Radii are hard to program and adjust without G16 and tool nose radius comp. G41-G42. Programming would be linear "Z Y". The polar "C" axis is converted to a linear "Y" axis. Another use of G16 is to chamfer a cross hole equally all the way around the hole. G16C.15 C= Position of X axis to calculate from if the actual cutting position is different. This is in radial value. C.15 = X.3 (MILL A J SLOT Sample program not tested yet but should work) T900(.125" cutter / 1/2"bar/ to cut .156 slot) (M5) M18C0 G98M80S3=2500 G50W-.59 G0X.6Z-.1T9 X.3(to depth of J slot) G12.1 D0 E=C G16 (C.15) G41G1Z-.02Y.078F6. G1Z.1,R.02(or use G2) Y.187 G3Z.256K.078 G1Y-.078,R.078 Z-.02 G13.1 G40G0X.6Y0 G50W.59 G18G99M20M82
G17- Plane select- X-Y used when milling with "Y" on the Gang Tools G18- Plane select- X-Z normally used for turning. G18 is when power on. G19- Plane select- Y-Z
G28- Automatic reference return. Usually use the incremental command for each axis. "G28 U0 W0". You probably won't use G28 very often. G32- Threading- G32 locks the feed-rate override at 100% and turns off the single block mode. Then G32 looks to find an exact spot on the spindle to start feeding. G32 is canceled by a G00 command. It's uses are for multiple angle threads (bone screws, worm gears) or we commonly use G32 when we tap a part with the main spindle, or the PO spindle. G32 won't work on the secondary spindles because there is no encoder on S3 or S4. If you are cutting a special OD thread always start G32 on a Z move. If you start G32 on an X move, the spindle zero will pick up in a different Z position each time. Position "X" first then "G32 Z" or keep the X distance from start to cut the same distance. To do this each start X will vary, calculated from the current cut X position. If you are 'continuous threading' or moving X and Z like a worm gear or bone screw thread, usually we set the param Control #8053=8D to eliminate the issues of thread mis-match. Also don't use 'On Mach Prg Check' while checking, cutting this kind of thread. Run it in auto cycle. G32 can also adjust the spindle zero for double start threads. G32 Q180000 = Q180.? 180. deg from spindle zero. G600 (tap example 10-32 .4” deep) T2100 M3S1=500 G0 X0 Z-.06 T?? (position to center of part)
Start 2 thread leads before the face of the part G32 Z.48 F.025 (locks feed-rate 100% and turns off single block) Feed in at 80% (.03125 x .80 = .025) of the pitch of the tap. This pulls the tap in and allows for Z axis error during spindle reverse and feed out.
Z-.06 F.0313 M4
(still locked feed and no single block)
Feed out at 100% of the tap’s pitch G4U.5 G0 Z-.1 T0
(feed and single block are usable again)
M3
G34- Variable lead threading. This command is the same as G32 but has the "K" value for the amount of pitch change per revolution. See G32G34 X Z F.03 K.05 X= Position to go to in X Z= Position to go to in Z F= Feed rate in IPR K.05= Amount of change in pitch per revolution. Can be growing pitch if plus value or reducing pitch if minus value. First rev will be F.03 2nd rev is (.03+.05) 3rd rev is (.08+.05) and so on.
G35- Arc threading (cw) Used to cut a radius while threading. G35 X Z R F (Q) (IJK) G32 X Z F
G36- Arc threading (ccw) see above
G40- Tool nose radius compensation CANCEL. Turns off G41 or G42
G41- Tool nose radius compensation LEFT. Usually used when front turning on Cincom machines in a Z positive direction. There are 8 quadrants of the radius to be used. 1= Boring 3= Back turning 4= Front turn 8= Profile 0= Endmill
G42- Tool nose radius compensation RIGHT. Not used as often turning. G42 could be used when traveling in a Z negative direction. See G41
Rules of tool nose radius compensation: 1) Turn compensation on and off in feed not rapid 2) If you turn compensation on during rapid stay at least one nose radius away from the part 3) Make sure compensation is fully loaded in both axes before cutting 4) Don’t change direction after compensation is turned on 5) Compensation reads six lines ahead so the line you alarm on might not be the problem
T0202 G0X .725 Z0 G1X-.04 F.0015 G0 X.08 Z-.03 G41 G1 X.14 Z0 X.3 Z.08 Z.45 X.465 X.725 W.13 G40 G0 X.725 T0 Front turning tool with a nose radius of .0156”. Tool number P=4
G43-Feed per revolution in $2 on S1. IPR and CSF is read off of the main spindle. This is used when in G650 and programming from $2 but feeding IPR to S1. The default is G43 so feeding in $1 and $2 is IPR off the main spindle. G44-Feed per revolution in $2 on S2. IPR and CSF is read off of the sub spindle. Used to single point thread with the pick-off spindle, tap, or any IPR feeding needed to be done from the S2 spindle. This code is unique to each side $1 and $2. Probably you will only use G44 in $2 because you normally don't need to feed from S2 on the front side program unless using G650. $1
$2 G44(G43 is default) G99 G99 M23S2=1000 T0200 T3100 G0X Z T G0X.27Z-.05T31 G1 Z1.F.002(READ OFF S1) G92X.3Z.4F.05(READ OFF S2) X.31 T0300 X.32 G0X Z T X.33 G1 X Z F.001 G0X.27
G50- Coordinate system setting. Used to either set the position p osition of an axis absolutely to a known k nown value, or to shift the position of an axis incrementally over a specified amount. The axis doesn't move but the position screen changes. Also used for spindle speed clamp. G50 Z0
Changes the current position position of Z axis to zero but there is no movement of Z. Usually Used at the start of the program to define d efine the face of the part pa rt as Z zero.
G50 W-.5905 shifts the Z coordinate system for temporary use then it would be shifted back by by programming G50 W.5905
T2200 (index boring bar) G50 U.1 (X coordinate shift)
T1212 (index saw) G50 U.062 G0 X0
G50 S4000 max RPM=4000 only in G96 mode (If in $1 or $2 the clamp is for the local spindle) (You can Use G50S2000 or G50S1=2000) $1 G50 Z-.005 M9 M52 M6 G0X.725 Z-.03 M3 S1=4000 G99 T0202 (FRONT TURN) G0 X.725 Z0 G50 S7000 G96 S1=450 G1 X-.04 F.002 G0 X.725 Z-.03 T0 G97 S1=3000
M5 M80 S3=3000 G98 T1111 (1/4 MILL) M28 S0 G50 W-.5905 G0X.725 Y-.875 Z.5 X.487 G1 Y.875 F6. G0X.725 T0 G50W.5905 M82 M20 M3 S1=3000 G99
G53 – Machine coordinate command. Rapids specified axis to commanded location according to the MACHINE Coordinate system NOT the Work Coordinate system. Sometimes used after running multiple parts per chucking. G53Z-[#818*#819] #818= mach len #819= parts per chucking G53 Z-1.5(Rapid Z to machine position -1.5 not program position) G53 Z3. ,F80. The ",F" is a new feature that enables a feed rate command for G53. If used the ",F" is a one shot feed rate command, not changing modal "F".
G65- Calling a macro program. Same as M98 but we pass variables to a macro sub-program. Example: Peck drilling macro. Z-AXIS ALL ARE IN RADIAL VALUE G65 P8999 A.05 B.03 C.02 S0 R-.03 Z1. W.01 F.0005 D.5 E3. X-AXIS A,B,C,U IN RADIUS VALUE S,R,X IN DIAMETER VALUE G65 P8999 A.05 B.03 C.02 S1. R1.1 X.1 U.01 F8. D.5 E3. A. FIRST PECK B. SECOND PECK C. THIRD AND ALL FINAL PECKS S. START POINT W/U. RETURN POINT (RAPID IN) Z/X. ENDING Z POSITION OR X POSITION R. RETREAT POINT (OUT OF HOLE) F. FEED RATE D. DWELL E. DWELL EVERY ? PECKS P8999 is the macro sub-program O8999 and the rest is information passed to the macro to drill the hole.
G66 Macro modal call A G66.1 Macro modal call B G67 Macro modal call A/B cancel
G70- Finish turning/Boring/Facing cycle G71- Rough turning/Boring cycle G71 U____ R____ G71 P___ Q____ U____ W____ F____ S1=____ T____ N_____ Finish machining Tool Path N_____ U – Infeed amount. R – Escape distance in the X axis. P – Starting line number of the finishing program Q – Ending line number of the finishing program U – Finish allowance in the X axis, radial, sign is required (+ for OD, - for ID) W - Finish allowance in the Z axis, sign required F – Feedrate S1= Spindle speed T – Offset number N – Line number
T0400 G0 X.6 Z-.03 T04 G71 U.04 R.02 G71 P1000 Q2000 U.005 W-.002 F.002 S1=3000 N1000 G0 X.08 G1 Z.12 F.0015 X,2 X.27 Z.28 Z.39 X.32 X.42 Z.47 N2000 X.6 G70 P1000 Q2000 F.001 S1=5000 G0 X.6 T0
G70- Finish turning/Boring/Facing cycle G72- Rough Facing cycle G72 W____ R____ G72 P___ Q____ U____ W____ F____ S1=____ T____ N_____ Finish machining Tool Path N_____ ** Parameters same as “G71” above. **
G73- Closed loop or “Pattern” cutting cycle. Used for Shaped material to minimize cutting. (Rarely used)
G74- Fixed face Groove plunge cycle. (Face groove or drilling) Used to peck groove to break chips but will also plunge as many repetitions as needed to complete the groove width. T1300(.2w face groove with .094 tool Groove starts at x.225 and ends at X.625) G50U.? G0X.225Z-.04T13(X.225+(.094+.094)=.413) G74 R.01 G74 z.15 X.625 P.05 Q.08 (R NOT USED) F.003 G0z-.04T0 G50U-.? R.01 = First Line G75R sets the return amount in X axis radial value. This is the amount the tool moves away for each peck. X.3 = Final X axis position to go to Z.15= Final Z axis position to groove to. P.05 = Cut amount radius designation/ incremental Q.08 = Z cut amount radius designation/ incremental (less than tool width) R = When reaching Z bottom, X axis would retract R amount before rapid out and moving over Q amount. F.003= Feed rate
G75- Fixed OD Groove/Cutoff cycle. Used to peck groove to break chips but will also plunge as many repetitions as needed to complete the groove width. T500(.325w groove with .094 tool Groove starts at Z.3 and ends at Z.625) G0X.6Z.419T5(Z.325+.094=.419) G75 R.01 G75 X.3 Z.625 P.05 Q.08 (R NOT USED) F.003 G0X.6T0 R.01 = First Line G75R sets the return amount in X axis radial value. This is the amount the tool moves away for each peck. X.3 = Final X axis position to go to Z.625= Final Z axis position to groove to. P.05 = Cut amount radius designation/ incremental Q.08 = Z cut amount radius designation/ incremental (less than tool width) R = Might be used for cut-off. When reaching X bottom, Z axis would retract R amount "-" before rapid up and moving over Q amount. F.003= Feed rate
G76- Canned threading cycle G76 P010060 Q0020 R0005 (first G76 sets parameters for threading. No decimals allowed) G76 X Z P Q F R (cuts the thread)
The first G76 isn't needed but is recommended. - G76 P Q R
P010010 sets 3 things - first 2 digits is the amount of finish passes - 01
- second 2 digits is number of leads before the end of the thread to begin chamfering out 00 = no chamfer, thread to ending Z position and rapid out at 90 degrees.
99 = 9.9 leads before ending Z position to begin chamfering out. Default angle is 45 degrees. - third 2 digits are the angle of infeed - 60 00, 29, 30, 55, 60, and 80 are valid angles
Q0020 sets the minimum cut amount during threading .002 but no decimal (Q00200 for sub inch)
R0005 sets the cut amount of the last pass .0005 but no decimal (R00050 for sub inch)
The second G76 cuts the thread. -G76 X.1876 Z.3 P0302 Q0010 F.05 (R-.002) FOR 1/4-20 X.1876 =Minor Dia. of thread Z.3 or (W) =The ending Z of the thread P0302 =Height of thread in radius (Maj-Min)/2 (.0302) (No decimal allowed) (P03020 for sub inch) Q0100 =Amount of the first cut. All the rest of the cuts are calculated. (No decimal allowed) (.01) (Q01000 for sub inch) F.05 =Feed-rate 20 TPI 1/20=.05 R = R is optional for tapered threading. R is the change in X from start to finish. R is radial. A negative value will begin threading at smaller X position and thread in the plus direction. A positive value will begin threading at a lager X position and thread in the minus direction.
G79- (G83.2) Face drilling Deep hole cycle. ExampleG0 Z-.05 T12 G79 Z1. R.03 I.1 K.05 A.01 Q100 J200 F.001 Z1. =Z position of the bottom of the hole R.03 =Rapid from current Z position the R amount incrementally. If starting at Z-.05 and R=.03 then the Z axis rapidly positions to "Z-.02" and after every peck Z retracts to the same position "Z-.02". If you use "R-.03" it is the same as "R.03". Leave R out to start from current Z position. I.1 = Depth of FIRST infeed in a radial value
K.05 = Depth of SECOND and successive infeeds in a radial value.
A.01 = Drill STOP safety distance in radial value from last depth completed.
Q100 = Dwell length at the BOTTOM of the hole.
J200 = Dwell length at the RETURN position BEFORE re-entry.
F.001 =Feed in IPR or IPM
,F30= This was added! Now you can change the rapid moves to a feed if desired.
G80-Cancel G8? series codes. G83- Peck drilling cycle. There are (2) parameters related to G83. Control Param #8125 "G83 Rapid" if ON then the pecks do NOT come out of the hole, they only back up the amount of Setup1 Param "G83 Retract" to break the chip and then start feeding again. Setup1 Param "G83 Retract .02" is the amount to rapid back into the hole from the last peck for clearance. I suggest... Setup1 Param "G83 Retract"=.02 Control Param #8125 "G83 Rapid"=OFF ExampleG0 Z-.05 T22 G83 Z1. F.001 R.03 Q.04 P0 Z1. =Z position of the bottom of the hole F.001 =Feed in IPR or IPM R.03 =Rapid from current Z position the R amount incrementally. If starting at Z-.05 and R=.03 then the Z axis rapidly positions to "Z-.02" and after every peck Z retracts to the same position "Z-.02". If you use "R-.03" it is the same as "R.03". Leave R out to start from current Z position. Q.04 =Peck amount P0 =Dwell amount at the bottom of the hole. You can just leave P off the command line if you want K4 =If face off center drilling use K for the amount of holes Just leave K off the command if only one. H90. =If you have C axis option and using K ,F30= This was added! Now you can change the rapid moves to a feed if desired.
G84- rigid tapping. Main Z1-S1 or sub Z2-S2 T1300 M97(M95 for S2 fluctuation detection off) M3S1=500 G0Z-.05T13 G84 Z.5 R.03 D1 F.05 S500 ,R1 G80
G84 Z.5 F.05 D1 R.03 S500,R1 Z1. =Z position of the bottom of the hole D1 =spindle 1=S1,2=S2,3=S3,5=S5 -1=S1 rev for left hand taps F.05 =Feed in IPR R.03 =Rapid from current Z position the R amount incrementally. If starting at Z-.05 and R=.03 then the Z axis rapidly positions to "Z-.02" the same position "Z-.02". If you use "R-.03" it is the same as "R.03". Leave R out to start from current Z position.
S500=RPM K4 =If more than one feature use K for the amount of holes. Just leave K off the command if only one. H90. =If you have C axis option and using K ,R1=Synch. tap ,R0=Non Synch. tap ,R2=Re-Synch. tap -Use ,R2 in both cycles if you will tap then later, re tap. ,R2 will home the live tool or spindle so the tap starts in the same rotational location. Q200 = option- High speed removal. 100-500 200=200% feed removal rate. ,F30= This was added! Now you can change the rapid moves to a feed if desired.
G87- Peck drilling cycle X axis. See G83 G87 X.1 Q.2 F5.K4 H90.
G88- Cross rigid tapping. If using T700 or any 1/2 speed live tool holder you need to double the spindle speed to get the proper RPM and then 1/2 the feed rate to get the proper feed.
T800(1/4-20 tap) M80S3=0 G50W-.59 G0X.8Y0Z1.5T8 G88 X0 R.05 F.05 D3 S500 K4 H90. ,R1 G80 or
T700(1/4-20 tap in 1/2 speed tool position) M80S3=0 G50W-.59 G0X.8Y0Z1.5T7 G88 X0 R.05 F.025(F.05) D3 S1000 K4 H90. ,R1 (feed is 1/2 and RPM is double) G80 or
T800(1/4-20 peck tap) M80S3=0 G50W-.59 G0X.8Y0Z1.5T8 G88 X.4 R.05 F.05 D3 S500 K4 H90. ,R1 X0 (,R1)(second peck tap) X-.4 (,R1)(third peck tap) G80
X0 R.05
=Ending X position of tap =Distance from position point to tap start point in radius. Leave R out to start from current X position.
F.05
=Feed rate.
D3
=spindle 3 use -3 for left hand taps.
S500 K4
H90.
=RPM =If more than one use K for the amount of holes. Just leave K off the command if only one. =If you have C axis option and using K
,R1=Synch. tap ,R0=Non Synch. tap ,R2=Re-Synch. tap -Use ,R2 in both cycles if you will tap then later, re tap. ,R2 will home the live tool or spindle so the tap starts in the same rotational location. Q200 = option- High speed removal. 100-500 200=200% feed removal rate. ,F30= This was added! Now you can change the rapid moves to a feed if desired.
G90- Rough turning cycle used like G92 G92- Threading cycle. Straight infeed only. G92 X.22 Z.3 F.05 (R-.002) X.21 X.2 X.19 thread 1/4-20 X.188 X.1876 X.1876 G0 X.5 Z-.05 (ENDS G92 CYCLE. IF NO G0 THEN ALARM!) X.1876 = Each cutting pass Z.3 or (W) =The ending Z of the thread F.05 =Feed-rate 20 TPI 1/20=.05 R = R is optional for tapered threading. R is the amount of difference in X from start to finish in Z. When cutting threads moving Z and X in a positive direction R is a negative value.
G94- Facing cycle used like G90/92 but feeds down on X.
G96- Constant surface footage on. You should turn off before any T???? code or you force the spindle up and down. So index to the tool then turn on. When finished turn off, and then index to the next tool. If you use G96 without S?= then the last G96 S? value is used.
SPINDLE S1-$1 G50 S5000 Q1000 (clamp max rpm and Q= min RPM) M97 G96 S200 M3 (CSFM on at 200 SFM) (TURNING) G97 S1=2000 (CSFM off and spindle 2000 RPM) SPINDLE S2-$2 G50 S5000 Q1000 (clamp max rpm and Q= min RPM) M87 G96 S200 M23 (CSFM on at 200 SFM) (TURNING) G97 S2=2000 (CSFM off and spindle 2000 RPM)
G97- CSFM off. ( Cancels G96 ) Maybe have at the beginning of your program as a safety command. G97 S1=1000 is allowed.
G98- Feed commanded in Inch Per Minute designation. IPM used for milling. IPM=RPM*IPR G99- Feed commanded in Inch Per Revolution designation. IPR used for turning. IPR=IPM/RPM G113- SPINDLE SYNCHRONIZE CANCEL G114.1 G114.1- SPINDLE SYNCHRONIZE. Used to exactly lock the P.O. spindle and the main spindle. G96 can be used also. We can also phase shift so we can pick up odd shapes while the spindles are running. See G814 also. G114.1 H1 D-2 R0 (if 'R' is used then 'M77' is needed) (if 'R' is not used you can skip 'M77') - H1= Commanding spindle 1 for S1 main spindle - D-2= Following spindle 2 for S2 PO spindle - ROTATION like M24 - R0= Degrees of rotation -picking up odd shapes. Example to pick-off a round part with CSFM... T100 G50W-.094S5000 (MAKE SURE PO WONT GO OVER 5000 RPM) G0X1.1Z4.T1 M97M87 M3S1=1000M24S2=1000 G114.1 H1 D-2 (not using G814 or M77 to save time) G96 M3 S200(MAIN SPL COMES ON AND PO SPL ALSO COMES ON LIKE M24) G650 (PO SPL COMES OVER THE PART -SEE G650) !L1 (WAIT PO SPL CHUCK CLOSE)
G1X-.05F.0015 X-.1F.003 G50W.094 G97M5M25 G113 M96M86 G600 Example to pick-off a HEX part or front/back phasing with CSFM ... ($1) ($2) T100 G50W-.094S5000 (PO 5000 RPM) G0X1.1Z4.T1 M97M87 M3S1=500M24S2=500 G114.1 H1 D-2 R0(or G814 -CHANGE R FOR OFFSET/ see G899) (M77) G96 M3 S200 G650 G650Z-.1 !L2 G98G1Z1.F50. (G231) M77 (WAIT FOR SYNCH) G1X-.05F.0015 M15 X-.1F.003 !L2 G50W.094 G97M5M25 G113 M96M86 G600 G600
G814-(macro) Same as G114.1 but you don't need all the codes on the command line. You can use the R command for phase shifting. Citizen added this macro just to make it easier to use spindle sync. See G114.1 and G113. You may save time by not using G814. G814 even with no 'R' argument will internally use 'R0' and this will force a phase shift for spindle sync, needing also to use M77. To save time use G114.1 without the R value. G814 R10. same as
G114.1 H1 D-2 R10.
G814 (no R) same as
G114.1 H1 D-2 R0
G114.2- Polygon machining command. There are many unique ways to use polygon machining. Not just for hex or square shapes. Side slots, Phillips screw driver shapes and whatever else can benefit from the live tool synchronized with the part while cutting. Use G113 to cancel. G114.2 H3 D1 E3 L6 (R15.) H3 = Master spindle or S3(gang live tool) S4 U121B option D1= Slave spindle. Could be 1,-1, 2, -1 - is for direction. E3 = Rotation rate. Number of teeth of the cutter. L6= Number of flats to be cut on the part. R15. = Phase shifting amount in degrees.
G114.3- Gear hobbing command. With a special holder this command will time the cutter(S3) and spindle(S1C1) to constantly hold position so all we do is feed across the part as if we were turning and a gear shape is cut. A "C" axis is also needed! Use G113 to cancel. G114.3 H3 D-9 E1 L18 (P0) (Q1.) H3 = Master spindle or S3(gang live tool) D-9= Slave spindle or 9= Caxis -9 = reverse E1 = Rotation rate. Always set to one. Not sure exactly why! L18= Number of gear teeth to be on the part. P0 = Helix angle -89.000 to 89.000 for helical gears. Leave off or set to P0 for spur(straight) gears. Q1.= Gear module. For helical gears only.
G115- Start point queuing (Type 1) or Queuing during an axis movement (Type 1) The programming system that G115 is in waits until the other system reaches a specified axis position Then continues. See G116 below. Example... getting P.O. spindle over the part while still turning. $1 (TURN CUT OFF SAME TOOL) G650 G0X.5Z.45T1S1=4000 G1X.4Z.5F.002 !L10 Z1.3 (G231) X-.1 G600
$2 T3000 G650 Z-.1(SUPERIMPOSE Z2 TO Z1) M24S2=4000M16 G115 Z1. !L10 (WAIT FOR Z1 TO PASS POS 1.000) G1Z.75F.02(FEED Z2 OVER PART .75) M15 G600 M25
G116- Start point queuing (Type 2) or Queuing during an axis movement (Type 2) G116 puts into memory a queue but instantly starts the next machining command. When the position is met in the same system then a queue is sent to the other system to continue. $1 G1 X.2 Z.5 G116 Z1. !1!2L10 G1 Z1.5 F.001
$2 !1!2L10 (Z1. is greater than Z.5 and less than Z1.5)
Z1. = let queue begin when Z axis of the programming line that G116 is in reaches Z1. while still moving to Z1.5 . Also position Z1. has to be passed on the next CNC command line. !1!2L10 = just like queuing
Example... getting P.O. spindle over the part while still turning. $1 (TURN CUT OFF SAME TOOL) G650 G0X.5Z.45T1S1=4000 G1X.4Z.5F.002 G116 Z1. !L10 Z1.3 (G231) X-.1 G600
$2 T3000 G650 Z-.1(SUPERIMPOSE Z2 TO Z1) M24S2=4000M16 !L10 (WAIT FOR Z1 TO PASS POS 1.000) G1Z.75F.02(FEED Z2 OVER PART .75) M15 G600 M25
G117- Execution of CNC codes during an axis movement. Usually an M code G117 X.1 M?? D1 X.1 = when X passes .1 the M?? is automatically commanded. Also X.1 has to be passed on the next CNC line. M?? = any M-code S-code B-Code D1 = offset #. Normally not used
G140- Arbitrary Axis Change Command. Normally not used. G140 will assign which axis are programmed in each line $1-$2. Following is an example to move control of "C" axis to $2 and back to $1 again. Any axis can be called any name and used in any system. Very powerful! $1 !1!2L10
$2 !1!2L10 G140X=X2Z=Z2C=C1 (programming C1)
!1!2L20
!1!2L20
G140X=X1Z=Z1Y=Y1C=C1 (programming C1)
G141- Cross Machining cancel. If you used a small sub with G140 to change all the axis around, you can use G141 to set it back. $1 (before has X1-Z1-Y1-C1) G140 X=X2 Z=Z1 (has X2-Z1) G141 (has X1-Z1-Y1-C1 again)
G149- End position queuing during an axis movement. Similar to G116 except G149 is smart and will calculate how long it will take to move to the desired position and finish moving at the queuing point. G149 is used in "M32 X.1" and will have Z2 and the catcher basket under the part when X=.1 . Z2 won't start coming in at X.1 but will start sooner to be there when X gets to .1 . You also need to add special line labels to mark the lines to end at. "BNxxx" $1 !1!2L10 G149 Q100 X.1 G1 X.3 F.002 BN100 G1 X-.1 F.002
$2 !1!2L10 Q200 BN200 G1 Z3. F50.(BN200 done when X1=.1)
G156- Mirroring two axis. Used automatically in G610 to lock Y1 to X2 so the drills can't hit the turning tools while using T2?00 stations. You won't normally use G156. If you don't command the other axis, it just follows. G156 Y1=X2 ON G156 Y1 OFF
G156- Superimpose one axis onto another. G650/G620 uses G156 to make the Z2 axis follow Z1. You normally won't need G156. If you command the other axis, it follows but also move simultaneously. See also -G620/G650 G156 Z2=Z1 turns on Also queue $1 and $2 before G156 G156 Z2
turns back off
G160- Axis torque sensing command. This is used internally by Citizen for the auto collet adjusting and auto guide bushing adjustment. Possible uses could be to check the Z2 torque while positioning over the part when picking off. If the turning tool has failed and the size is big, the collet could jam on to the part! G160 will feed to the desired position at the commanded feed but if the torque is reached the axis will stop short of the commanded position. We can then use macro to determine where it stopped. G160 is a one shot code and after G160 is done or if the torque was met, then 100% of torque is set back to the commanded axis. I tested and I used G160 with a shank of a tool and checked the turned size of a part and had .0003" repeating! Maybe this is not good for all jobs but could be used as part of an auto offset macro! G160 will not work on a superimposed axis. So if you have a CAV, A7 is superimposed on Z1 and G160 can not be used on Z1. Instead just use Z2 for the motion if needed.(no problem)
G160 Q20. Z1. F20. IF[#5022EQ1.] GOTO 10 #3000=1( ERROR -CHECK PART SIZE) N10(GO ON)
Q = Torque % of motor to stop feeding. It takes 5-10% to get moving. Z1.= Axis and position. Could be X, Y, or C or even U, V, W . F = Feed #5021= Macro variable for "X" current axis "Machine" position #5022= Macro variable for "Z" current axis "Machine" position #5023= Macro variable for "Y" current axis "Machine" position #5024= Macro variable for "C" current axis "Machine" position #5041= Macro variable for "X" current axis "Relative" position #5042= Macro variable for "Z" current axis "Relative" position #5043= Macro variable for "Y" current axis "Relative" position #5044= Macro variable for "C" current axis "Relative" position Check a drill to see if broken by inserting a pin (drill chucked backwards). If there was a gun drill from the front side drilled through and a larger drill drilled from the sub side. T3300(CHECK-GUNDRILL/and Back Drill) G0Z-.05 G98 G160Z.4Q30.F10. #100=#5042 (set #100 to Z pos) G0Z-.05T0 #523=0(reset broken gundrill flag) IF[#100EQ.4]GOTO3300 (if it made it to .4 then both are good, continue) #523=-1 (set flag drill broke at end of cycle) (#3000=999)(-GUNDRILL-IS-BROKEN) (didn't want to alarm here in cycle) IF[#100GE.14]GOTO3300 (check to see if back drill is broken) #3000=999(-PRE-DRILL-IS-BROKEN) N3300(GUNDRILL-OK/PRE-DRILL-OK)
G164- Spindle Superimpose. This is used for differential speed sync. tapping. The one spindle follows the other but can be commanded for example 500RPM and it would go 500 More than current. Use G113 to cancel G164. M3S1=2000 M84S3=0 G164 H1 D-3(-3= live tool reverse direction) M77 (Confirm completion of sync. before advancing. G84 Z.3 F.0312 D3 S500, R1 (500 is 500 more than currant) G80 (Cancel G84) G113 (Cancel sync.)
G173- Inclined Coordinate Rotation. Used with helical interpolation to perform thread milling on an angle. It will also let you program angle peck drilling easier, or milling at an angle.
G173 Y0 Z0 D5. or G173 X0 Z.5 D5. G173 no arguments cancels the G173 command.
Y0 = Center of rotation position of Y Z0 = Center of rotation position of Z X0 = Center of rotation position of X D5.= Angle of rotation. Remember to use G173 again with no arguments to cancel.
G231- (macro)Pick-off cancel. This was added to save time during the ending of the program. G231 is used after G650 and when done cutting off G231 will automatically cancel the G650 superimpose and send the Z2 home, all in one command. You then don't need to end with G600's. This can save 1-1.5 seconds on each cycle! G231 X-.1 F.002 A-.02 Z? X= Cut-off end position F= IPR feed rate for cut-off A-.02= When the cut-off is at "X" axis position -.1 then automatically bring the sub spindle Z2 away. This will cancel the G650 “superimposition”. Z1.= If you want Z2 to go to some position, not all the way back. It will position to the Z2 machine position specified. Z1. is 1" from return position. Example... $1
$2
T100(cut-off) G50W-.125 M3S1=3000 G0X.5Z2.T1 G50W.125 G650
G650Z-.1
!1!3L650 G50W-.125 (moving Z1) " G231X-.1A-.02F.001 (G600 NOT NEEDED) G50W.125 S1=1500M25 M7 G0X-.1Z-.005T0 M56 G999 N999 M2 M99
G1Z1.F.05(feed over) M73M15(close collet) !1!3L650(let $1 continue)
(G600 NOT NEEDED)
G999 N999 M2 M99
G600-CODES G600's- The G600's commands are Citizen's way of making a very complex multi axis machine, very easy to program. These G600's commands are called mode selections. G600,G630,G650,G660. All of these commands select each axis and make coordinate system settings in each of the two systems. G650 enables superimposition between Z1 & Z2. This is the ability of one axis to follow (slave) another axis but still be fully programmable. For example we can support the part WHILE it s being turned, cutoff, etc.. Because all the G600 modes are working with all the axis, the two systems are queued with each other by commanding the code in both systems for the mode change. There are also different arguments possible for each command that can change the axis movements as desired. See each code and it's arguments below...
G600 Machining pattern cancel G600 cancels the machining patterns G610 to G660. (Power-on state) Also G600 is the default mode before the program starts and after the G999 command at the end of the program. G600 will queue with both lines $1-$2 then X1-Z1-Y1-C1 are now controlled from $1,and X2-Z2-C2 is controlled from $2. Also when in MDI, Mode G600 is in affect. $1 $2 G600
G600W0
Macro specification
Command code
G600
Name:
Machining pattern cancel
Axis control group Axis of axis control group Superimpose Coordinate system Argument Spindle with which synchronous feed is enabled Spindle with which constant surface speed control is enabled Cutting block interlock
T commands available
Others
$1 X1, Y1, Z1, C1 Cancels Superimpose Main spindle Main spindle
$2 X2, Z2, C2 Cancels Superimpose W0 : The back headstock (Z2 axis) does not move. Back spindle Back spindle
Main spindle
Back spindle
T0100~T1000 T1100~T1400 T5100~T5400 T0100~T1000 K2**
T3000 T3100~T3500 T5100~T5400 *
-
-
* To use T5100 – T5400 for back machining be sure to use queing between $1 & $2 because the T50s are mounted on the gang tool post and another gang tool MUST NOT be selected during machining with T50s. ** When K2 argument for T command is specified, care MUST be taken for interference between the back headstock ,Front/back drilling holder, and back tool post.
G630 Front/back parallel machining Use this machining pattern to perform outer diameter machining OR end working drilling/boring with a tool on the tool post No. 1 in $1, and independently perform back drilling/boring with a tool on the back tool post in $2. Front Back parallel machining mode. Basicly G630 is the same as G600. G630 will queue with both lines $1-$2 then X1-Z1-Y1-C1 are now controlled from $1,and X2-Z2-C2 is controlled from $2. $1 G630
$2 G630W0
Macro specification
Command code
G630
Name:
Front/Back Parallel Machining pattern
Axis control group Axis of axis control group Superimpose Coordinate system Argument Spindle with which synchronous feed is enabled Spindle with which constant surface speed control is enabled Cutting block interlock T commands available Others
$1 X1, Y1, Z1, C1 Cancels Superimpose Main spindle Main spindle Main spindle T0100~T1000 T1100~T1400 -
$2 X2, Z2, C2 Cancels Superimpose W0 : The back headstock (Z2 axis) does not move. Back spindle Back spindle Back spindle T3000 T3100~T3500 -
G650 Pick-off, Center-support This machining pattern enables the back spindle to pick off the workpiece and support the center of the workpiece. Machining mode change to superimpose Z2 on to Z1. G650 will queue with both lines $1-$2 then make Z2 follow Z1 but Z2 can also be programmed independently. Example -when we pick up a part and chamfer it while we have the back spindle collet closed on the part. Also if we are using Z2 as a work support.
Macro specification
Command code Name:
G650 Pick-off, Center support Machining pattern $1 X1, Y1, Z1, C1
$2 X2, Z2,C2
Superimpose
-
Coordinate system
-
Argument
-
Z2 superimposed on Z1 Z2 : Alignment of the face of the back headstock cap nut with the end face of the workpiece on the FRONT SIDE. U0 : The back headstock (X2 axis)does not move. W0 : The back headstock (Z2 axis) does not move. Z___ : The back headstock (Z2 axis) moves to the position specified by Z___.
Axis control group Axis of axis control group
Spindle with which synchronous feed is enabled Spindle with which constant surface speed control is enabled T commands available Others
Main spindle
Back spindle
Main spindle
Back spindle
T0100~T0900 -
T3000 -
* If a numeric value is entered to machining data “Back chuck extend length” , command Z-.1 for $2 AFTER G650 and Z2 will move to the position at which the “Extended nose collet chuck” will rapid .100” in front of the work piece.
Note- Any shift, "G50W-.125", on Z1 must be canceled, "G50W.125", before G650 or, G650 won't find the face of the part!
See Example on next page...
Pickoff Example...
$1 G600 T100(cut-off) G50W-.125 !1!3L100 M3S1=3000 M24S2=3000 G0X.5Z2.T1 G50W.125 G650 !1!3L650 G50W-.125 (moving Z1) " G1X-.1F.001 G600 G50W.125 S1=1500 M7 G0X-.1Z-.005T0 M56 G999 N999 M2 M99
$2 G600 (eject part) !1!3L100
G650 G0 Z-.1(bring Z2 to Z1 -.1) G1Z1.F.05(feed over) M15(close collet) !1!3L650(let $1 continue)
G600(bring Z2 back) M25
G999 N999 M2 M99
G660 Front/back simultaneous machining Use this machining pattern to perform front drilling with a tool on the tool post No. 1 in $1, and simultaneously perform the back drilling with a tool on the back tool post in $2. Machining mode change to use the front ID tools (T11-T14) and also the back side T51-T54) at the same time. G660 will queue with both lines $1-$2 then set auto queuing between tool calls of T11-T51, T12-T52, and T13,T53.. after G660 $1 controls X1-Y1-Z1-C1 and $2 has Z2-C2. The Z2 position is set to program the sub spindle part zero to the back side drill zero. Example... $1
$2
G660 T1100 G0 Z-.05 T21 (peck drilling 8 sec)
G660X2 T5100 G0Z-.05T? (peck drill 15 sec)
T1200 (queues with T5200)
T5200
T1300 (queues with T5300)
T5300
G600
G600
Macro specification
Command code
G660
Name:
Front/Back Simultaneous Machining pattern
Axis control group Axis of axis control group Superimpose
$1 X1, Y1, Z1, C1 Cancels Superimpose
Coordinate system
-
Argument
-
Spindle with which synchronous feed is enabled Spindle with which constant surface speed control is enabled T commands available Others
Main spindle Main spindle
$2 X2, Z2, C2 The X2 axis is superimposed onto the Y1 axis. Z2: The coordinate system for the Z2 axis is established at the “standard” tool point of the vertical end face drilling holder. X2: The X2 axis is “superimposed”onto the Y1 axis. Back spindle Back spindle
Gang Tool Post (Drilling Tool)
Gang Tool Post (Drilling Tool)
T1100~T1400 -
T5100~T5400 -
Machining patterns, axis’ of axis control groups, and available tools Machining pattern name
Command code
$1
$2
Operation: X2: No operation Z2: Movement to return position (Argument W0(Specifying no operation of Selectable tool numbers: Z2) is available) T0100 to T1000 Selectable tool numbers: T1100 to T1400 T3000 *T5100 to T5400 T3100 to T3500 *T5100 to T5400 Axis available: Axis available: X1, Z1, Y1, C1 X2, Z2, C2 (NOTE: that the axis available are switched to X1, Y1 and Z2 when T5100 to T5400 are (NOTE: that the axis available are switched to X1, Y1 and Z2 when T5100 to T5400 are called.) called.) •
Operation: X1, Y1and Z1: No operation
•
•
Free Pattern (Machining pattern Cancel)
•
G600
•
•
•
Front/back parallel machining
G630
•
•
Operation: X1, Y1and Z1: No operation Selectable tool numbers: T0100 to T1000 T1100 to T1400 Axis available: X1, Z1, Y1, C1
Operation: X2: No operation Z2: Movement to return position (Argument W0(Specifying no operation of Z2) is available) Selectable tool numbers: T3000 T3100 to T3500 Axis available: X2, Z2, C2 •
•
•
Operation: X2: No operation (Argument U0(Specifying no operation of X2) is available) Z2: Movement to return position (Argument W0(Specifying no operation of Z2) is available) Selectable tool numbers: T3000 Axis available: X2, Z2 and C2 Superimpose: Z2 superimposed on Z1 •
•
Pick-off, center support
G650
•
•
Operation: X1, Y1and Z1: No operation Selectable tool numbers: T0100 to T1000 Axis available: X1, Z1, Y1, C1
•
•
•
• •
Front/back simultaneous machining
G660
•
•
Operation: X1, Y1and Z1: No operation Selectable tool numbers: T1100 to T1400 Axis available: X1, Z1, Y1, C1
•
•
•
Operation: X2 and Z2: No operation Selectable tool numbers: T5100 to T5400 Axis available: X2, Z2 and C2 Superimpose: X2 superimposed on Y1
N o t e s A machining pattern is a modal G code that remains valid until another machining pattern is called. •
Before selecting the needed machining pattern, be sure to cancel ANY coordinate system shift (G50) and tool compensation (Offset). **For selection of G650, however, it is not necessary to cancel the compensation.
SPINDLE SYNC.
G813-(macro) Same as G113, to turn off spindle synchronization. G814-(macro) Spindle synchronization on. See also G113 and M77 (confirm synchronization complete)
M3 S1=300 M24 S2=300 G814 M77 M3 S1=4000
(Slow RPM BEFORE Sync.)
(After Sync Adjust RPM for cutting)
Example to pick-off a round part with CSFM... ($1)
($2)
(NORMAL STARTUP SEQUENCE AND PART MACHINING OMITTED) T100 (CUT OFF) M3 S1=300 G0 X.85 Z4.125 T1 G650 (M24S2=300) G50 W-.125 S5000 G96 S1=67 G814 G0 X.85 Z4.0 !1!2L2 G96S1=200 (Adjust) G1X-.05F.0015 X-.1F.003 G50W.125 G97 G813 M5 M25 G600
Program M24 here if the cut off is waiting
Program M24 here if the pick off is waiting
M24 S2=300 G650 M95 G0Z-.5 G98G1Z1.F50. M77 M15 !1!2L2
G600
Spindle Synchronization control command (G814 R0); When non-conforming material phase adjustment (G899) has been performed to control clamping location, “G814 (G114.1H2D-2) R0” MUST always be specified. If the “R” argument is not specified the orientation of angular phase is not matched. You must also follow this command with M77 BEFORE clamping the second spindle onto the part to ensure the spindles wait for completion of the “phase adjustment”. Following these procedures will allow angular orientation to be consistent between the two spindles. See G114.1 for an explanation of the arguments.
G899 - Phase adjustment. Used for hex stock and alignment of Main and sub spindles. Put material through the Main spindle and into the Sub spindle. Execute G899 R1 C1 from MDI. There is also a K1 that can be added to prevent the sub spindle from closing. G899 R1 = Phase S1 and S2. G899 R1 K1= Phase S1 and S2 AND do NOT close sub spindle collet. G899 R1 C1= Phase C1 and C2. You need the option "G114.1" to use "G899 R1".(Standard option now) After you have done this when your program calls G114.1H1D-2R0(or G814) M77 The spindle will sync together. You MUST use M77! Common MDI process after manually moving Z2 over the special shaped work piece. M18C0 G899R1C1 *** NOTE: *** G899 command is for adjustment. Use this command in MDI mode ONLY. Should NOT be written in the part program.
G999- Finish last part. Finishes the part in the P.O. spindle if you are running in SINGLE CYCLE MODE. While the machine is running usually the work on the P.O. spindle is completed while the front of the part is also working. When the counter is full or the bar stock is empty or, if we are in ONE CYCLE MODE, then we can finish the part by using G999 and N999 in our program. If in regular CONTINUOUS CYCLE MODE then the CNC statements between G999 and N999 are skipped but if in ONE CYCLE MODE or the counter is full or there are other operator alarms then the CNC statements between G999 and N999 are read and performed. G999 has to be in all programming lines $1 $2. If using G999 and at some time you want to turn off this function then turn off soft key in auto mode "Lastprt" and the codes between G999 and N999 are always skipped no mater what MODE your in. Mode G600 is in affect at the beginning of G999 by default. The code "M98 H_" does not work for this command. $1
$2
M56 G999 G630 G600 M5M53 N999 M2 M99
G999 G630 G600 N999 M2 M99
sample using macro #100 O1234(main program no sub) $1 G99M52 G610 G630 G600 G650 G600 M56 G999 G610 G630 G600 N999 M2 M99
$2 #100=10 GOTO H100 (goes to line sequence # N100) N10(M99 returns to here)
G650 G600
G999(only if in one cycle mode) #100=20 GOTO100 (goes to line sequence # N100) N20(M99 returns to here) N999 M2 M99(returns to beginning of $2) N100G610 G630 (CODES NEEDED TO COMPLETE THE PART) G600 GOTO#100(M99)(return to line after call)
Wait (Queing) Commands !1!2L1- Queuing between lines $1-$2. Used as waiting commands to make $1 wait for $2. !1= line $1 !2= line $2 L1= queuing reference #. 1-9999. Also "L" does not have to be in order. Example... O1234(queuing example) $1 $2 !1!2L5
!1!2L1
(10 seconds of CNC commands) !1!2L5 ($2 and $1 wait until on !1!2L5 then continue) !1!2L1 ($2 and $1 wait until on !1!2L1 then continue)
-You can also use it this way, leaving out the "!?" for the line you are in. O1234(queuing example does the same as above) $1 $2 !2L5
!2L1
(10 seconds of CNC commands) !1L5 ($2 and $1 wait until on !1!2L5 then continue) !1L1 ($2 and $1 wait until on !1!2L1 then continue)
T-Tool selection Each tool call will rapid to position point of the old tool and then to the position point of the new tool. A four digit code is a tool call and a two digit code is an offset. If you have arguments on the T-call line they have different meanings depending on which set of tools are called. The A20 also does a calculation when using the gang. It will take the largest diam. setting from the tool set page and add this to each tool while indexing, then come down to the position point for the tool. T100 tool call T101 tool call with offset T1 offset call T0 cancel offset (** X## Z## T0; ; ** NOT alone, NOT followed by a modal command ***)
Special options T0100-T1000 T0200 X Y Z H Q1 K2 E
X. = Specify the workpiece coordinate of X1 axis after tool selection. If the argument is omitted, the tool moves to “Position Point”. Y. = Specify the workpiece coordinate of Y1 axis after tool selection. If the argument is omitted, the tool moves to “Position Point”.
Z. = Specify the workpiece coordinate of Z axis after tool selection. If the argument is omitted, the Z axis does NOT move. (If “K2” argument is specified, the “Z2” axis is used. ) Q1 = Quick index. This will not move to safe position then index, It will move from where it is to the new tool in a straight line. Be careful! H. = Specify this argument to change “Position Point” temporarily. The machine will add this value to the Stock Dia. According to to the Machining Data and move to next tool selection. E. = Specify this argument to index the spindle to the specified angle. This argument is valid in the transition from the turning to secondary machining process. If used WITH the “K2” argument the BACK spindle will be indexed to specified angle. K2 = can only be used in G600 and can be in $1 or $2 After the Tool is called, the Z2 axis is the commanded Z axis. Also the C2 axis is called up. X1,Y1,Z2,C2 are commanded from either $1 or $2 depending where you called it from . The next T__00 call changes it back. If a live the Z2 shift is automatically set to the center of the tool to the part face. If a OD turn tool then the Z2 shift is automatically set to the LH(back) tool tip of the tool (from MachData Tool Block) to the part face (5/8" or 3/4").
Special options T1100-T1400 T1100 X Y Z A E
X. = Specify the workpiece coordinate of X1 axis after tool selection. If the argument is omitted, the tool moves to “CENTER Point” of workpiece For “Front/Back Simultaneous machining” (G660) specify “X” argument with T11##’s. Y. = Specify the workpiece coordinate of Y1 axis after tool selection. If the argument is omitted, the tool moves to “CENTER Point” of workpiece For “Front/Back Simultaneous machining” (G660) specify “Y” argument with T11##’s. Z. = Specify the workpiece coordinate of Z axis after tool selection. If the argument is omitted, the Z axis does NOT move. E. = Specify this argument to index the spindle to the specified angle. This argument is valid in the transition from the turning to secondary machining process. A. = Select one of the following when using “G660” “Front/Back Simultaneous machining”command. A – without argument: DIA and CORE data stored in front machining tool (T11##’s) and back machining tool (T51##’s) are added to the X1 and Y1 axes. See Below examples. A1 – DIA and CORE data stored in front machining tool (T11##’s) is added to the X1 and Y1 axes. A5 – DIA and CORE data stored in back machining tool (T51##’s) is added to the X1 and Y1 axes.
Using A
Using A1
Using A5
Note: Before commanding a tool T1100 – T1400 or T5100 – T5400 the “Z1” barstock axis and the “Z2” back spindle should be retracted to prevent collisions.
Special options T5100-T5400 T5100 X Y Z W Q1
Q3 E
X. = Specify the workpiece coordinate of X1 axis after tool selection. If the argument is omitted, the tool moves to “CENTER Point” of workpiece For “Front/Back Simultaneous machining” (G660) specify “X” argument with T11##’s. Y. = Specify the workpiece coordinate of Y1 axis after tool selection. If the argument is omitted, the tool moves to “CENTER Point” of workpiece For “Front/Back Simultaneous machining” (G660) specify “Y” argument with T11##’s. Z. = Specify the position to which the back headstock (Z2 axis) is moved (absolute move distance from the machine zero point of Z2 axis). If the argument is omitted, the back headstock (Z2 axis) moves to the position separated from the maximum nose protrusion length by 5.0mm. W. = Specify the retract point of the back headstock (Z2 axis) (incremental move distance from the back headstock of (Z2 axis) from the current position. If the argument is omitted, the back headstock (Z2 axis) moves to the position separated from the maximum nose protrusion length by 5.0mm. Q1 = Select a tool without moving the back headstock (Z2 axis). If the argument is omitted, the back headstock (Z2 axis) moves to the position separated from the maximum nose protrusion length by 5.0mm. Q3 = Select a tool after moving the back headstock (Z2 axis) to the “positioning Point. If the argument is omitted, the back headstock (Z2 axis) moves to the position separated from the maximum nose protrusion length by 5.0mm. E. = Specify this argument to index the spindle to the specified angle. This argument is valid in the transition from the turning to secondary machining process.
Note: *Arguments Z, W and Q cannot be specified together. If specified together, an alarm occurs. **Tool call note T3_00's for proper offset cancel. T3300 (don't use T3333) G0Z-.05T33 "" G0Z-.05T0 (If T0 is left out offsets will add together!! *******) X.4 or X0(U0) (If you don't move the X axis after a offset cancel they will also add together! Always cancel offsets moving X-Z *******)
Back ID tools T3100-T3500 T3100 X Z W Q1 Q3 E T3100 X.5
Rapids to X.5 work coordinate after tool change. If omitted X moves to center of the workpiece.
T3200 Z-.05
Rapids to position specified from Z0 of BACK workpiece. If omitted, Z2 will rapid 5mm from part face.
T3400 W3.
-If W is on the command then Z2 moves to W amount from current position. W is NOT from the face of the part! If omitted, Z2 will rapid 5mm from part face.
T3500 Q1
Allows tool selection without retracting Z2 axis. If omitted, Z2 will rapid 5mm from part face.
T3100 Q3
Forces full retracting of Z2 axis. If omitted, Z2 will rapid 5mm from part face.
T3200 E90.
-While the Tool is called, the C2 axis is positioned at the same time to the E value.
Back Spindle (T3000) T3000 Z W Q1 E T3000 Z-.05
Rapids to position specified from Z0. Absolute position from machine zero of Z2 axis. If omitted, Z2 will rapid 5mm from part face.
T3000 W3.
-If W is on the command then Z2 moves to W amount from current position. W is NOT from the face of the part! If omitted, Z2 will rapid to return position.
T3000 Q1 T3000 E90.
Allows spindle selection without retracting Z2 axis. If omitted, Z2 will rapid to return position. -While the Tool is called, the C2 axis is positioned at the same time to the E value.
**Tool call note T3?00. T3100 (don't use T3131Z-.05) G0Z-.05T31 "" G0Z-.05T0 (If T0 is left out offsets will add together!!) Note- Any other codes must be before the T command on the line. Also if you are using G96 you must cancel with G97 before any T???? command. S1=2000 T200 X.3 Z.15 Q1 G96 S300 " " " G97 T303
(T200 S1=2000
NO GOOD)
Wait (Queing) Commands NOTE: Queing or wait commands are used when using the sub spindle to pick-off or for support. They will stop the main spindle side or sub spindle side of the machine from moving until you want them to. You need to have a cueing command in $1 and $2 that matches otherwise the machine will hang up. Which ever $ sign gets to the cueing command first waits until the corresponding cueing command is read in the other $ sign then both $ signs will continue.
$1
$2
!L1 (Would wait until $1 got to!L1 to continue) !L2(Would wait until $1 got to!L1 to continue) !L1(Would wait until $2 got to!L1 to continue) Any commands in between these to cueing Commands would be executed while $2 is Held at !L2 until $1 gets to !L2.
!L2(Would wait until $2 got to!L2 to continue) $1 AND $2 WOULD NOW BE RUNNING INDEPENDENTLY
$1 AND $2 WOULD NOW BE RUNNING INDEPENDENTLY
Circular Interpolation (G2, G3) Pic #1 & #2 - G2, R value would be tool rad plus part rad. G3, R value would be tool radius minus part rad.
PIC #1
PIC #2
G2
G3
G3
G2
Pic #3
T07-T10 T11 – T14
G3
G3 G2
Pic #3 - G2, R value would be tool rad minus part rad. G3, R value would be tool radius plus part rad.
G2
Tool Nose Radius Compensation (G41 & G42) Note: General rules for tool comp., start (G41, G42)at least 2X the tool radius in X and at least the tool radius in Z and cancel it (G40) with same rule. Ex.- if using a .031 rad. Tool start the comp(G41,G42) at least .062 from the cut in X and .031 from the cut in Z. If you don’t you will cause a under cutting or over cutting alarm. When you cancel (G40) make sure the G40X__ value is at least .031 from the last move or if you cancel it using G40Z__ the Z move should be at .031.
#1
#2
.
G E D 5 3
F O R P
#3
.
R E LI
5 5 H R
G E D
H R
#4
#5
N R U T K C A B
L.H. BORE
R.H. BORE
P1
P8
TOOL #1
P4
#3
P4
P0 OR P9
P3
#2
#6
TOOL #4
NOTE: As long as your moving in X+ and Z+
G41
direction with Tools 1-3 its G41
( O.D. BOSS)
TOOL #5
TOOL #6
G42
(TOP VIEW)
G41
G41
G41
G41 G42 (I.D. POCKET)
G42
G41
79
G50Z (absolute setting) Example G50- Coordinate system setting. Used to either set the position absolutely (x,y,z) to a known value, or to shift the position of an axis incrementally (u,v,w) a specified amount. The axis doesn’t move but the position screen changes. It’s also used to clamp the spindle speed. NOTE: G50Z____ is used in the beginning of the program to establish part zero (Z0). This is about the only time you will see a G50 with an absolute command (x,z). What we normally do on this G50Z____ line for a RH CUT-OFF tool is use G50Z-.005 instead of G50Z0 for a .005 facing allowance. This will set the coordinate system to Z-.005 instead of Z0. The cut-off tool should be in front of the stock (PIC #2). For a LH CUT-OFF tool the stock is sticking out passed the Z0 plane. Looking at PIC #3 the stock is sticking out .400 (.500-.100, PIC #1). The G50Z value would be the width of the tool shank (.500, PIC #1) minus the width of the insert (.100, PIC #1) minus .005 (facing allowance). In this case the G50Z value would be .395 (G50Z.395). The cut-off tool should be in front of the stock (PIC #3).
G50Z (absolute setting) Example G50- Coordinate system setting. Used to either set the position absolutely (x,y,z) to a known value, or to shift the position of an axis incrementally (u,v,w) a specified amount. The axis doesn’t move but the position screen changes. It’s also used to clamp the spindle speed. NOTE: G50Z____ is used in the beginning of the program to establish part zero (Z0). This is about the only time you will see a G50 with an absolute command (x,z). What we normally do on this G50Z____ line for a RH CUT-OFF tool is use G50Z-.005 instead of G50Z0 for a .005 facing allowance. This will set the coordinate system to Z-.005 instead of Z0. The cut-off tool should be in front of the stock (PIC #2). For a LH CUT-OFF tool the stock is sticking out passed the Z0 plane. Looking at PIC #3 the stock is sticking out .400 (.500-.100, PIC #1). The G50Z value would be the width of the tool shank (.500, PIC #1) minus the width of the insert (.100, PIC #1) minus .005 (facing allowance). In this case the G50Z value would be .395 (G50Z.395). The cut-off tool should be in front of the stock (PIC #3).
Z+
. 10 0 W I D E INSERT
PIC #1 (TOOL)
Z+
PIC #3
PIC #2
$1 $1 M118 G99M6 G99M52M6 /M52 G50Z.395 G50Z.395 G0X1.0Z-.03M3S1=4000 G0X1.0Z-.03 M3S1=4000
$$1 1 M 118 G99M6 G 9 9M52M6 /M52 G50Z-.005 G50Z-.005 G0X1.0Z-.03M3S1=4000 G0X1.0Z-.03 M3S1=4000
80
G50W (incremental shift) Example G50- Coordinate system setting. Used to either set the position absolutely (x, y, z) to a known value, or to shift the position of an axis incrementally (U, v, w) a specified amount. The axis doesn’t move but the position screen changes. It’s also used to clamp the spindle speed. NOTE: G50 shifts keep the numbers in the program matching those that are on the print, therefore making the program easier to follow. They can be used at any point in the program
.100 WIDE INSERT
XO
XO
ZO
PIC #1
PIC #2
TEMPORARY Z0
ZO
PIC #3
G50W (incremental shift) Example G50- Coordinate system setting. Used to either set the position absolutely (x, y, z) to a known value, or to shift the position of an axis incrementally (U, v, w) a specified amount. The axis doesn’t move but the position screen changes. It’s also used to clamp the spindle speed. NOTE: G50 shifts keep the numbers in the program matching those that are on the print, therefore making the program easier to follow. They can be used at any point in the program
XO
.100 WIDE INSERT
XO TEMPORARY Z0
ZO
PIC #1 (TOOL)
ZO
PIC #2 (NO SHIFT)
PIC #3 (WITH SHIFT)
EX. If starting out at Z0 (PIC #2) and you programmed G50W-.100 the stock would not move but the position screen would read Z-.100. Next you program G0Z0 then the stock would move forward .100 giving you the result in PIC #3. This would be your temporary Z0. If your given a dim. On the print that your holding on this side of the tool, this will allow you to use the exact dim’s from the print in your program. EX. N5(GROOVE) M3S1=3000 T0200 G50W-.1 (Changes position screen, stock will not move) G0X.6Z0T02 (Will move stock out .100 from where it is)
81
G50W (incremental shift) Example cont.
.100 WIDE INSERT
FIRST GRV. N5(FIRST GRV.) (USING SHIFT) M3S1=3000T0200 G50W-.1 G0X.7Z.3T02
SECOND GRV. N5(SECOND GRV.) M3S1=3000T0200 G0X.7Z1.0T02 G99G1X.4F.003 G0X1.0T0
G50W (incremental shift) Example cont.
.100 WIDE INSERT
FIRST GRV. N5(FIRST GRV.) (USING SHIFT) M3S1=3000T0200 G50W-.1 G0X.7Z.3T02 G99G1X.4F.003 G0X1.0T0 G50W.1
SECOND GRV. N5(SECOND GRV.) M3S1=3000T0200 G0X.7Z1.0T02 G99G1X.4F.003 G0X1.0T0
OR N5(FIRST GRV.) (USES NO SHIFT) M3S1=3000T0200 G0X.7Z.4T02 G99G1X.4F.003
82
,A ,A- The control can use commands with angles instead of X & Z moves. ( You must be in the G1mode with either Z or X move on the line following the ,A_ or you will get an alarm)
SideView, Front Turn Ex.
Z0,90 deg.
45 deg. Z Feed
X0, 0 deg.
PART
G1X.25,A90. Z.5,A0. X.5,A30. (Calculates ending Z point) Z____
,A ,A- The control can use commands with angles instead of X & Z moves. ( You must be in the G1mode with either Z or X move on the line following the ,A_ or you will get an alarm)
SideView, Front Turn Ex.
Z0,90 deg.
45 deg. Z Feed
X0, 0 deg.
PART
315 deg.
G1X.25,A90. Z.5,A0. X.5,A30. (Calculates ending Z point) Z____
30 deg
Z0,270 deg.
Top View, Bore Ex.
Z0,90 deg.
G1 X.3,A330.0,C.04F.003 (Calculates beginning X and ending Z points) Z______ 45 deg.
Z Feed X0, 0 deg.
0 or 180 deg.
315 deg. Z0,270 deg.
PART
30 deg X .04
,R ,R- Put a radius on the part but the control does all of the calculations. It will only generate a 90 deg. radius. (You must be in the G1mode with either Z or X move on the line following the, R _ or you will get an alarm)
G1 X.5, R.015 Z1.
.5
G1 X.5 ,A30. , R.030 Z1.
,C , C- same as ,R but chamfers instead. It will only generate a 45 deg chamfer. (You must be in the G1mode with either Z or X move on the line following the, C _ or you will get an alarm)
G1X.5, C.03F.002 Z1.0
Programming Examples
Program Example #1 Typical Beginning & End Note: The following is a TYPICAL example. There may be variations to the beginning due to added options and operations etc. The ending may vary also due to options and differences in the Cut off operation due to part processing and geometry.
BEGINNING $1
BEGINNING $2
0001 (Program number/name) G50Z-.040 (Sets the Z absolute position. If you have a RH cutoff tool and leaving .005 on for facing the Z would be Z-.005. If using a LH cutoff tool and leaving .005 on for facing the Z would be (tool shank width – tool insert width - .005. ( Ex. .500-.094-.005)Z=.401)
T3000 (Calls Sub Spindle,”X” into position in line with Main Spindle)(“Z” axis goes to Ref Point) G50Z0 (Sets the Z absolute position)
M9 (SAFETY, Barchange cancel command. Added at top of the program in case there had been a Barfeeder alarm) M6 ( M6- Closes main spindle collet) /M52 ( Turns on FLOOD coolant) G0X.4331Z-.05 (Rapids the Z back .050 off the face of the part. The X value would be stock size + approx..05,) G630 (Sync) - (Front/Back Machining Mode ON)
G630 (Sync) - (Front/Back Machining Mode ON) (Allows simultaneous Front and Back Machining)
G99 (Inches per rev. feed) M3S1=2500 (Starting the MAIN spindle clockwise at 2500 rpm) T1100(SPOT-FRONT) T1200(DRILL-BACK) G600 (Sync) – (Machining Mode CANCEL )
G600 (Sync) – (Machining Mode CANCEL )
T0300(FACE/TURN) T0100(CUTOFF)
M23S2=2500 (Starting the SUB spindle clockwise at 2500 rpm
ENDING $1
T0100(CUTOFF) (Call cutoff tool into position)
ENDING $2
T3000 (SUB-SPINDLE) (Call pickoff into position)
G0X0.4331Z1.635T1 (RAPID stock to Cutoff position using offset #1 ) G650 (Sync) – (Super-Impose Machining Mode ON )
G650 (Sync) – (Super-Impose Machining Mode ON ) M16 (Opens SUB spindle collet) M72 ( Turns ON air blast through knockout BEFORE clamping on part) G0Z-.1 (Rapid sub-spindle .1” from face of part on main spindle side) G98G1Z.7F80. (G98= IPM,)(G1 Z.7 F80. = Feed over part for clamping) M15 (Closes SUB spindle collet) M73 ( Turns OFF air blast through knockout AFTER clamping on part)
!2L651 (WAIT, for $2 queing)
!1L651 (WAIT, for $1 queing)
G99G1X-.05F0.0008 (G99= IPR,) (G1 X-.05 F.0008 = cutoff part for Separation) G630 (Sync) - (Front/Back Machining Mode ON)
G630 (Sync) - (Front/Back Machining Mode ON)
(Cancels G650 mode)
(Cancels G650 mode)
M25 (Stops SUB spindle RPM)
M5 (Stops MAIN spindle RPM)
G999 (BEGIN « Last Part Off ») M98H100 (Run Backwork Sub Program) M53 (Flood Coolant OFF) N999 (END « Last Part Off ») M2 (End of program)
M7 (Opens MAIN spindle collet)
M99 (LOOP in continuous Cycle)
G0X-.05Z-.040T0 (RAPID to “START POSITION” with collet OPEN and NO offset active )(From Beginning)
N100(BACK-SUB) G99G44 (IPR, IPR on Backspindle)
M56 (Parts counter advance)
T3100(DRILL.375)
M2 (End of program)
T3200(BORE)
M99 (LOOP in continuous Cycle)
M99 (Return to Main Program)
G99G1X-0.08F0.002 (Cutoff to end point position from M/C Data)
Program Example #2 CODE DESCRIPTION
$1
(Beginning of Main Side Program)
0001011 (WIDGET) (Program number / Name) G50 Z-.005 (Sets the Z Work Coordinate position.) ( If you have a RH cutoff tool and leaving .005 on for facing the Z would be Z.005. If using a LH cutoff tool and leaving .005 on for facing the Z would be (tool shank width – tool insert width - .005. ( Ex. .500-.094-.005)Z=.401)
M9 (SAFETY, Barchange cancel command. Added at top of the program in case there had been a Barfeeder alarm) G813 (SAFETY, Spindle SYNC. Cancel) M6 ( M6- Closes main spindle collet) /M52 ( Turns on FLOOD coolant ) G99G0 X.425 Z-.05 (Inches per rev. Rapid,“ Z” to .050 off the face of the part, X to stock size + approx..05 over stock dia.) M3 S1=2500 (Start the MAIN spindle clockwise at 2500 rpm) M96 (MAIN Spindle Speed Fluctuation Detection ON ) G630 ( Mode setting, .”Front/Back Parallel Machining” ) (***Will Sync. With $2***) T1400 ( Tool call, Endworking tools will go to X0 & Y0 unless given other end coordinates to go to. ) G0 Z-.02 T14 (Rapid, Stock Close to Tool , Call offset #14 ) G1 Z.090 F.0028 (Feed, Depth, feedrate ) G0 Z-.05 T0 (Rapid, Retract position, Cancel offset ) M3 S1=3000 (Starting/Adjusting the MAIN spindle clockwise at 3000 rpm) T0300 (FRONT-TURN) ( Tool call, Front “Gang” tool. ) G0 X.435 Z0 T3 (Rapid, Tool ABOVE stock dia., Stock to ZERO position for facing operation, Call offset #3 ) G1 X.04 F.0008 (Feed, Cut Face of part into spot, Feedrate per rev. ) X.1567 F.004 (Feed UP face to start of angle cut, Feedrate per rev. ) X.2321 Z.0039 F.0012 (Feed UP Angle, Feedrate per rev. ) (Slower Feedrate to maintain finish) Z.2362 F.002 (Feed along length, Feedrate per rev. ) X.378 (Feed UP shoulder) X.4094 W.0157 F.0012 (Feed UP Angle, Feedrate per rev. ) (Slower Feedrate to maintain finish) G0 X.435 T0 (Rapid, Retract position, Cancel offset) M3 S1=1000 (Starting/Adjusting the MAIN spindle clockwise at 1000 rpm) G4 U.5 ( DWELL, .5 seconds. )
Code description cont.
T0400 (THREAD) ( Tool call, Front “Gang” tool. ) G50 W-.0625 (Co-Ordinate shift for tool Tip location from “STANDARD ZERO”) G0 X.435 Z-.078 T4 (Rapid, Tool ABOVE stock dia., Stock to starting position for Threading operation, Call offset #4 ) G92 X.228 Z.1772 F.0394 (Threading mode, “X” 1st pass dia., “Z” ending position, Feedrate per rev.”Pitch” ) X.2165 (“X” 2nd pass dia. ) X.1992 (“X” 3r d pass dia. ) X.189 (“X” 4th pass dia. ) X.1854 (“X” 5th pass dia. ) X.185 (“X” 6th pass dia., Finish MINOR Dia. ) G0 X.435 T0 (Rapid, Retract position, Cancel offset ) G50 W.0625 (CANCEL, Co-Ordinate shift for tool Tip location) M3 S1=3000 (Starting/Adjusting the MAIN spindle clockwise at 3000 rpm) T0300 (FRONT-TURN) ( Tool call, Front “Gang” tool. ) G0 X.435 Z.2205 T3 (Rapid, Tool ABOVE stock dia., Stock to Safe position for turning operation, Call offset #3 ) G1 X.2598 F.004 (Feed, Angle start position, Feedrate per rev. ) X.315 W.0276 F.0012 (Feed UP Angle, Feedrate per rev. ) (Slower Feedrate to maintain finish) Z.5512 F.002 (Feed along length, Feedrate per rev. ) G4 U.008 ( DWELL, .008 seconds., Create fillet radius around circle ) X.3543 F.0012 (Feed UP shoulder) G2 X.3858 Z.5669 R.0157 F.0008 (C.W. Arc, “X & Z” endpoints, Radius size, Slow Feedrate per rev. ) G1 Z.748 F.0016 (Feed along length, Feedrate per rev. ) X.4094 W.0118 F.0012 (Feed UP Angle, Feedrate per rev. ) G0 X.435 T0 (Rapid, Retract position, Cancel offset) M5 (Stop Main Spindle RPM) G98 (FeedRate, Inches Per MINUTE) M80 S3=2500 (Start “Live” spindle FWD. Direction, RPM) M28 S0 (Engage Indexer, Position at “0”)
Code description cont.
T0700 (X-MILL) (Tool call, , Front “Gang” LIVE tool) G50 W-.5905 (Co-Ordinate shift for tool Tip location from “STANDARD ZERO”) G0 X.435 Z.6299 T7 (Rapid, Tool ABOVE stock dia., Stock to Safe position for turning operation, Call offset #7 ) Y-.5457 (Position “Y” axis beside material, Left Side ) G1 X-.1181 F7.87 (Feed, Plunge “X” position, Feedrate per Minute. ) G0 X.435 (Rapid, Retract position) Y.5457 (Position “Y” axis beside material, Right Side ) G1 X-.1181 F7.87 (Feed, Plunge “X” position, Feedrate per Minute. ) G0 X.435 T0 (Rapid, Retract position, Cancel offset) G50 W.5905 (CANCEL, Co-Ordinate shift for tool Tip location) M20 (DIS-Engage Indexer) M82 (STOP live tool spindle) G99 (Inches per rev. feed mode ) M3 S1=2500 (Start the MAIN spindle clockwise at 2500 rpm) T0500 (BACK-TURN) ( Tool call, Front “Gang” tool. ) G50 W-.1476 (Co-Ordinate shift for tool Tip location from “STANDARD ZERO”) G0 X.435 Z.6693 T5 (Rapid, Tool ABOVE stock dia., Stock to Safe position for turning operation, Call offset #5 ) G3 X.3858 Z.6929 R.0236 F.0012 (C.C.W. Arc, “X & Z” endpoints, Radius size, Feedrate per rev. ) (Re-Engage into cut) G2 X.353 Z.7087 R.0157 F.0008 (C.W. Arc, “X & Z” endpoints, Radius size, Slow Feedrate per rev. ) G1 X.315 (Feed, into start dia. position ) G4 U.008 ( DWELL, .008 seconds) (Hesitate before starting turn, for accuracy) Z.9764 F.002 (Feed along length, Feedrate per rev. ) X.2913 Z.9882 F.0008 (Feed UP Angle, Feedrate per rev. ) X.4094 F.004 (Feed UP shoulder) G0 X.435 T0 (Rapid, Retract position, Cancel offset) G50 W.1476 (CANCEL, Co-Ordinate shift for tool Tip location) M24 S2=300 (Starting the SUB spindle COUNTER clockwise at 300 rpm) M3 S1=300 (Starting the MAIN spindle clockwise at 300 rpm) G814 ( Spindle SYNC. ON)
Code description cont.
T0100 (CUT-OFF) ( Tool call, Front “Gang” tool. ) (1.0 + .0625 + .005 = 1.0675)
G0 X.435 Z1.0675 T1 (Rapid, Tool ABOVE stock dia., Stock CUTOFF position*, Call offset #1 ) (*OAL + Insert + Facing) G650 ( Mode setting, .”Pickoff, Center Support Machining” ) (***Will Sync. With $2***) !2L20 ( Wait, Queing command ) (Will wait for $2 to get to MATCHING wait “L20” then continue)(Pickoff will grab part) M3 S1=2500 (ADJUST the spindle to 2500 rpm)(In Sync. BOTH spindles will adjust) G1 X-.04 F.0012 (Feed, CutOFF part, Feedrate per rev. ) G630 ( Mode setting, .”Front/Back Parallel Machining” ) (***Will Sync. With $2***) (Cancels G650 mode) G813 (SAFETY, Spindle SYNC. Cancel) M5 (Stop Main Spindle RPM) M25 (Stop SUB Spindle RPM) M7 (Open Main Spindle Collet) M56 (Advance counter) G0 X-.1181 Z-.005 T0 (Rapid, to “START POSITION”, NO OFFSET) (“X” from “MDATA”, “Cutoff End Position” ( “Z” from Beginning of program, “Z Work Coordinate position”) (This “LOOP” allows continuous cycles, by sending the axis’ back to where they were located at the BEGINING of the program)
G999 (Start of “Last Part Off”) (***Will Sync. With $2***) (When the program is formatted correctly this will allow you to do ALL the Backwork WITHOUT running the front end again) (This cycle will minimize scrap when setting up or changing tools)
N999 (END of “Last Part Off) (***Will Sync. With $2***) M2 (End of program) (***Will Sync. With $2***)
$2
(Beginning of SUB Side Program)
G630 ( Mode setting, .”Single Machining” ) (***Will Sync. With $1***) T3200 ( Tool call, Endworking tools will go to X0 unless given other end coordinates to go to. ) M23 S2=2000 (Starting the SUB spindle Clockwise at 2000 rpm) G99 G44 (Feed “Inches Per Rev., Calculate IPR per SUB Spindle RPM) G0 Z-.05 T32 (Rapid, Part face .05” from tool tip, Turn ON offset #32) G1 Z.0984 F.0024 (Feed, Depth, feedrate ) G0 Z-.05 T0 (Rapid, Retract position, Cancel offset ) M25 (Stop SUB Spindle RPM)
Code description cont.
M34 (Macro) (Part Ejection routine)
Cutoff / Pickoff routine
T3000 (Tool Call to position PickOff Spindle BEFORE Pickoff) G650 ( Mode setting, .”Pickoff, Center Support Machining” ) (***Will Sync. With $1***)(Re-Calc.) M95 (Fluctuation Detection OFF) (Allows spindle sync. (change) from $1) M16 (OPEN Sub Spindle Collet) M72 (Air Blast thru Sub Spindle ON) G0 Z-.1 (Rapid, Sub Spindle collet .100” from Face of part on Barstock ) G98 G1 Z.4724 F80. (IPM Feed ,”Z” Pickoff position, feedrate ) M77 (Spindle Sync. Wait for confirmation) G4 U.012 ( DWELL, .012 seconds ) M15 (CLOSE Sub Spindle Collet) M73 (Air Blast thru Sub Spindle OFF) G4 U.008 ( DWELL, .008 seconds ) !1L20 ( Wait, Queing command ) (Will wait for $1 to get to MATCHING wait “L20” then continue)(Pickoff has grabbed part) G630 ( Mode setting, .”Single Machining”) (***Will Sync. With $1***)(Cancels G650 mode & sends Z2 HOME) G999 (Start of “Last Part Off”) (***Will Sync. With $1***) (When the program is formatted correctly this will allow you to do ALL the Backwork WITHOUT running the front end again) (This cycle will minimize scrap when setting up or changing tools)
T3200 ( Tool call, Endworking tools will go to X0 unless given other end coordinates to go to. ) M23 S2=2000 (Starting the SUB spindle Clockwise at 2000 rpm) G99 G44 (Feed “Inches Per Rev., Calculate IPR per SUB Spindle RPM) G0 Z-.05 T32 (Rapid, Part face .05” from tool tip, Turn ON offset #32) G1 Z.0984 F.0024 (Feed, Depth, feedrate ) G0 Z-.05 T0 (Rapid, Retract position, Cancel offset ) M25 (Stop SUB Spindle RPM) M34 (Macro) (Part Ejection routine) N999 (END of “Last Part Off) (***Will Sync. With $1***) M2 (End of program) (***Will Sync. With $1***)
Formulas General Formulas: 1) SFM = Surface Feet per Minute 2) RPM = Revolutions per Minute 3)IPR = Inches per Revolution 4) IPM = Inches per Minute
1) SFM = RPM x DIA. (Tool or Part) / 3.82 2) RPM = SFM x 3.82 divided by DIA. (Tool or Part) 3) IPM(Drilling,Tapping ect.) = RPM x IPR 4) IPM(Milling) = RPM x IPR x Number of flutes.) 5) IPR = IPM divided by RPM
Trig Formulas: Triangles U S I D R A
Known
Find Sine
SINE
Radius & @
@
Cos COS
Formula
Radius x Sine of @ (input @ in calc ulator . and press the sin button take that value and multiply it by the Radius)
Radius x Cosine of @ (input @ in calc ulator . and press the cos button take that value and multiply it by the Radius)
b x Tangent of @ U S I D R A
@ & b
c
@&c
b
c
@
b
(input @ in calc ulator . and press the tan button. Take that value and multiply it by b
c divided by Tangent of @ (input @ in calculator and press tan button. Now take c and divide by this no.
U S I D R A
Radius & b
b
The square root of radius squared – b squared.
b
The square root of radius squared – c squared.
c
Radius & c
@
c
Formulas
Triangles
S I U D R A
Con`t
Known
Find
Formula
@&b
Radius
b divided by the Cosine of @
@ & c
Radius
c divided by the Sine of @
b &c
@
c
@
b
U S I D R A
c
c divided by b = Tangent of @ ( after dividing c by b press Tan-1 button on calculator)
@
Radius & b
b
S I U D R A @
b
c
Radius & c
@
@
b divided by Radius = Cosine of @( after dividing b by rad press Cos-1 button)
c divided by Radius = Sine of @ (After dividing c by the Radius press the Sine-1 button on the calculator)
Define the Process (Process considerations)
A) DETERMINE WHAT IS THE FRONT OF THE PART 1) Is I.D. work required a) Must be done before O.D. work 2) Is front work required a) Turning is done in one pass due to guide bushing land width b) If having to pull part back into G/B keep in mind the G/B land width 3) Is back turning required 4) Is cross milling or cross drilling required 5) Is there back end work required 6) Where is the tightest tolerance (front is more accurate) 7) Is a special guide bushing required a) You can have extended land guide bushings made (up to .375 longer) b) Do I need a meehinite instead of a carbide (Meehinite will help with scoring problems but will wear out quicker) 8) Can cycle be reduced by using the sub spindle
B) SUB – SPINDLE WORK
1) Where do I hold the part at pick-off 2) Is a special collet required a) extended nose collet ( For extremely short parts) b) tapered collet c) dead length shoulder d) over-grip collet e) key for orientation (picking off on non round dia.) f) special shape collet 3) Will chips from machining process get into collet (if so high pressure coolant is recommended to blast chips out of collet.)
4) How does part get ejected
Process Examples
4
1 2 3
1
2
3
4 5 5
6
Spot Drill Tap Face & Turn Thread Major Thread Turn
6
4
1
2
3
7
6
8
9
5
1
Spot
2
Drill
3
Bore
4
Face & Turn
5
Slot (Saw)
6
Re-Bore to Deburr
7
Re-Turn to Deburr
8
Re-Slot to Deburr
9
Turn
Process Examples Con`t EX. # 1
Turn Groove Groove
1
1
2 3
2 3
4
3
Turn Groove Groove
41
Turn
1 1
2
EX. # 2
2 3
Note: Examples above are based on using .625 dia. Guide Bushing which has approximately .800 carbide pad length. In Ex. #1 the part was turned complete before grooving. You can turn complete then groove in this example without coming out of the guide bushing when you retract the Z-Axis to do the grooves after turning. In Ex. #2 you would come out of the guide bushing if you were to turn complete then retract the Z- Axis to do the grooves.
2
3
1 2 3
1
4
Turn Groove Cross Drill Turn
4 2 3
3
Turn Cross Drill Groove
4
Turn
1 2
1
4
Class Program creation Part Examples for programming
Turn, Thread, Pick-off T 02
3
T 01 4
T 02 1
T 03
.025 x 45 deg.
2 3/8-24 x .375 long (.3228 Minor)
( Spot, Drill, Bore)
.575
.425 .250
Knockout Pin
.03 x 45 Deg .031 Rad
1/8 -27 Npt x .38 deep
10-32 Thread
7
6
3 1B
1
2B
2
3B 4 5
Front 1 2 3 4 5 6 7
T22 - Spot T23 - #36 Drill T2 - Face &Turn T3 - Thread T2 - Turn T7 - Mill Flats T1 - Cut-off
Back 1B T31 - Drill 2B T32 - Bore 3B T33 - Thread
T01- L.H. Cut-off T03- R.H. 55 Deg. Turning Tool T05- R.H. Threading Tool T14- .250 Dia. End Mill T21- .250 Dia. Spot Drill T23- #36 (.1065) Drill
T32- Boring Bar T33- (.295) Drill T34- Single Point Threading Tool
.625 Dia. Bar Stock
102
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____________ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _______________________ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP 0
0
0
0
0
0
0
0
0
collet
Holder
Insert
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____________ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _______________________ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP
collet
Holder
Insert
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
Notes: 103
104
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____________ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _____ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP 0
0
0
0
0
0
0
collet
Holder
Insert
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____________ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _____ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP
collet
Holder
Insert
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0 105
106
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _____ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP 0
0
0
0
0
0
0
0
0
collet
Holder
Insert
A32VII Tool Sheet Barfeed: _____ Collet : ____________ Torque setting: ____%
Part #: __________________________ Program #: _______________ Bar Stock: ________________________ Main Spl Collet –TF37SP: ____ Guide Bushing- _TD32_____________ Sub Spl Collet- TF37SP: ___________ Knockout: _____ Cutting Oil: _______________________ Cycle Time: __________________ Operation
Tool
Off
CUTOFF
1
1
T i p 0
BACKWORK
Rad
0
Len Core
Diam
0
0
HP
collet
Holder
Insert
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
Notes: 107
108
Class Program
Class Program
Class Program
Class Program
Class Program
Class Program
Class Program
SECONDARY MACHINING During secondary machining we stop rotating the material and rotate the tool instead.
The Process: Stop the main spindle
(M5)
Engage the C axis
(M18 or M28)
Start the rotary tools
(M80, M81)
Switch to inch per minute feed
(G98)
Turn on your tool shift
(G50 W-.5905)
Execute secondary machining Turn off your tool shift
(G50 W.5905)
Stop the rotary tools
(M82)
Disengage the C axis
(M20)
Start the main spindle to continue turning
(M3, M4)
Don’t forget to go back to inch per minute feed
(G99)
Example: Milling two flats
T0808 ………………………….. Index tool 08 and call offset 08 G50 W-.59 …………………….
Turn on tool shift
M5 ……………………………… Stop the main spindle M18 C0 ………………………… Index the C axis M80 S3=2500 ……………
Start the rotary tool
G0 Y-.52 Z.6875 ……………… Rapid to position in Y and Z X.375 …………………………..
Rapid to position in X
G98 G1 Y .52 F8. …………………..
Feed across, inch per minute feed
G0 C180. (H180.) …………….
Index the C axis 180 degrees
G1 Y-.52 ………………………
Feed across
G0 X.56 T0 ……………………
Rapid out and cancel the tool offset
M82 ……………………………
Stop the rotary tools
M20 ……………………………
Disengage the C axis
G50 W.59 ……………………..
Turn off the tool shift
M3 S1=5000 G99 …………….
Start the main spindle and switch back to inch per revolution feed
Example: Milling a key using circular interpolation and tool nose radius compensation
T08 - 5/32” (.15625”) DIAMETER ENDMILL
Process: Mill across the front to remove some material (no TNRC) 1 - 2 Mill the key (with TNRC) 3 - 8 Remove the material behind the key (no TNRC) 9 - 12 Index and mill the ¼” flat (no TNRC) 13 - 15
T0808 M5 G50 W-.5124 (.5905 - .0781) M18 C0 M80 S3=3000 G19 G0 Y.56 Z.12 X.28 G98 G1 Y-.56 F4. G50W-.0781 G41 Y-.2 Z.225 Z.775 G2 Y.2 R.1 G1 Z.225 G2 Y-.2 R.1 G40 G1 Y-.56 G50 W-.0781 G0 Z1.03 G1Y.56 G50W.1562 G0 Z1.25 G1 Y-.56
Index tool 08 and call offset 08 (R=.0781 (.156/2)) Stop the main spindle Turn on tool shift to the front of the tool Engage the C axis Start the rotary tools Switch to the YZ plane, rapid to start position (1) Rapid to milling position in the X axis Feed across (2) , inch per minute feed Shift to the center of the tool for TNRC Turn on TNRC and feed to the start position (3) Feed in Z axis (4) Clockwise radius (5) Feed in Z axis (6) Clockwise radius (7) Turn of TNRC and feed off the part (8) Shift to the back of the tool Rapid to position (9) Feed across (10) Shift to the front of the tool Rapid to position (11) Feed across (12)
G0 C180. X.36 G1 Y.56 G50 W-.1562 G0 Z1. G1 Y-.56 G18 G0 X .56 T0 G50 W.6686 M82 M20 M3 S1=3000 G99
Index 180 degrees to mill the ¼” flat Rapid to milling position in the X axis Feed across (13) Shift to the back of the tool Rapid to Z position (14) Feed across (15) Switch to the XZ plane, rapid out , cancel offset Turn off tool shifts (-.5124 + -.1562 = -.6686) Stop the rotary tools Disengage the C axis Start the main spindle, inch per revolution
Cross drilling through maximum stock diameter Always be sure you have enough drill to drill through the stock diameter. Normally, we try not to over extend the tooling so we have maximum rigidity. When setting the gang tools we try to have no value in diameter.
With DIA at zero the drill extends about ½” from collet X axis over travels at X -.19 so a drill set at zero can’t drill through maximum stock diameter. To calculate the shift required for a .125” diameter drill to drill through .75” first calculate the X position the drill tip has to be programmed to break through the stock OD and include the drill point. The drill point is about 1/3 the drill diameter. So, .125” x .3 = .0375” drill point. Double it because the X axis is in diameter .0375” x 2 = .075” The X position to program to is stock diameter plus the drill point in diameter .75” + .075” = X-.825” Calculate how far past over travel you need to go to reach this position .825” - .19” = .635” So, the minimum shift to get this drill through .75” stock is .635”. With this shift in DIA it is not necessary to program a tool shift, i.e. G50 U-.635. If you prefer to program G50, after setting the tool the .635 in DIA would have to be deleted.
Control
***Note***** To view a button-by-button description PLEASE refer to the Cincom A32 “OPERATOR’S MANUAL”.
Control Con`t
Operation Panel & Alpha Numeric Key Pad
Soft “Menu” Keys
Maintenance
There are required periodical checks for the machine AND the bar feeders.
Below are samples from the machine manual.
PLEASE refer to the respective manuals for a complete set of instructions.
**** SEE THE MAINTENANCE MANUAL FOR A COMPLETE LISTING **
Machine Operations
Power Up 1) Release E-Stop 2) Turn on the main circuit breaker located on the Back of the machine. 3) Press the power on button located in the top left corner on the control panel After the preparation screen appears. 4) Make sure main collet is closed, bar feeder is turned on and switched into auto cycle. 5) Press the preparation button.
6) Close main spindle collet ( light is on when closed)
7) Press the arrow button to cursor to the cutoff tool (should always use T01) 8) Press
soft key.
9) Press and hold the green start key in until cycle is completed 11) Press
soft key.
12) Press and hold the green start key until cycle is completed 13) Turn on the coolant 14) Press the Cut-off soft key and the Start button at the same time 15) Open the main spindle collet 16) Press the
soft key
17) Press and hold the green start key until cycle is completed 18) Close the main spindle collet
Power Down 1) Press the power off button located in the top LEFT corner on the control panel 2) Turn off the main circuit breaker located on the front lower right side of the machine
Jogging
Using the MPG handle; 1) Press the “Manual Operation” button.
2) Cursor to axis you want to jog using arrow keys (Axis will be highlighted)
3) Select jog increment **Selecting “X10” and “X100” TOGETHER will allow faster movement.
4) Turn hand wheel to move axis
Cut-off 1. Make sure main collet is closed, bar feeder is turned on and switched to auto cycle. 2. Press the “Preparation” Button.
3. Close main spindle collet ( light is on when closed) 4. Press
soft key.
5. Press the arrow button to cursor to the cutoff tool (should always use T01) 6. Press and hold the green start key in until cycle is completed 7. Press
soft key.
8. Press and hold the green start key until cycle is completed 9. Turn on the coolant 10. Press the
soft key and the Cycle Start button at the same time
Start Position 1. Perform cutoff procedure. (above) 2. Open the main spindle collet 3.
Press the
soft key
4.
Press and hold the green start key until cycle is completed
5.
Close the main spindle collet
Restarting (when machine stops in cycle) If sub is clamped on the part, prior to cut-off:
1) Press Reset (Do not press spindle stop button) 2) Stop spindles if they are still running 3) Press the “Preparation” button 4) Open Sub spindle collet 5) Jog the Z2 axis away from the stock ( Jog shown on previous page) 6) Jog the X1 axis away from the stock 7) Jog stock out past last cut 8) Run the cut-off procedure ( shown on previous page) 9) Run the start position procedure ( shown on previous page )
Machine Setup
Guide Bushing ( Installation)
Figure #2 Figure #1
Removing Guide Bushing: 1) Insert the Guide Bushing adjustment wrench (Figure #2) onto the draw bar and loosen the clamp screw. Use the spanner wrench on the guide bushing sleeve to prevent spindle from turning. (Figure #1) 2) Rotate the draw bar counter clockwise until the Guide Bushing comes out.
Installing Guide Bushing: 1) Put the new Guide Bushing in, lining up the key way. 2) Rotate the draw bar clockwise to tighten. 3) Push the bar stock through the Guide Bushing. (Finish adj. MUST be done manually, continue with step#2 above.)
Main Spindle Collet (Installation & Manual Adjustment)
Figure #1
Figure #2
Installation: Removing Collet
1) Open Collet 2) Remove spindle cap nut (Figure #1) 3) Pull collet out (Figure #2) Installing Collet
1) Put new collet into spindle (Make sure spring is in collet sleeve) 2) Tighten spindle cap nut. (***COLLET MUST BE IN OPEN POSITION***)
Main Spindle Collet Adjustment 1) 2) 3) 4) 5) 6) 7) 8) 9)
Remove headstock cover. Open Main Spindle collet. Loosen the lock screw on the Chuck Adjustment Nut. Turn adjustment nut to get the appropriate chucking pressure. Remove the connecting shaft. Use the chuck wrench to check the tension. Put connecting shaft back in when setting is complete. Tighten the adjustment nut lock screw. Replace the headstock cover plate.
Sub Spindle Collet (Installation & Manual Adjustment)
Figure #1
Installation: Removing Collet
1) 2) 3) 4)
Open Collet Remove the spindle cap (Figure #1) Remove the spindle cap nut (Figure #1) Pull collet out (Figure #2)
Installing Collet
1) Put new collet into spindle (Make sure spring is in collet sleeve) 2) Tighten spindle nut 3) Install the spindle cap (Make sure oil hole is facing down)
Figure #2
Sub Spindle Collet Adjustment
Adjustment (Manual): 1) 2) 3) 4) 5) 6) 7) 8) 9)
Remove headstock cover. Open Sub Spindle collet. Loosen the lock screw on the chuck adjustment Nut. Turn adjustment nut to get appropriate chucking pressure. Remove the connecting shaft. Use the chuck wrench to check the tension. Put connecting shaft back in after setting is complete. Tighten the adjustment nut lock screw. Replace headstock cover.
Machining Data
#1 Bar Stock O.D.- Stock size #2 Tool Positioning Point (Dia.)- This is the tool index point (X1 axis) for the gang tools. The actual position is the stock size plus this setting. In the view above all indexing would be at .855. #3 Cut-off Tool- This should always be tool # 1 #4 Cut-off Speed- This rpm value is used when you do an automatic cut-off operation in the Prep mode. #5 Cut-off Feed- This feed value is used when you do an automatic cut-off operation in the Prep mode. #6 Cut-off End (Dia.)- This value is used whe n you do a automatic cut-off operation in the Prep mode. In the view above the automatic cut-off would end at X-.05 (Physically .025 below center line) #7 Machining Length- This is the amount of head stock stroke you need to complete one part. (Calculation involved is Part Length + Cut-off Tool Shift + Face amount ) #8 Pieces /1Chuck- 99% of the time this would always remain a 1 #9 Tubing Bar Stock I.D.- If using solid bar stock this should always be a 0 #10 Back Chuck extend length- Length of EXTENDED NOSE COLLET, if using one. #11 Back Work extend length- What you are doing here is telling the machine how much the part is sticking out of the sub spindle after the pick-off is complete. (Calculation involved is Part Length minus feed onto the part with the sub ) #12-14- 99% of the time you will not have to change these. This is the physical equipment mounted on the machine
Tool Setting “CORE” (T01 – T06) CORE SETTING 1.
IMPORTANT !
You MUST verify that the current MC DATA is correctly showing the stock diameter. Your tool settings will be INCORRECT if it is not.
2. Install and adjust the collet and GuideBushing. ( as shown in previous section) 3. Call tool to “Position Point” (WAIT). ( as shown in previous section) 4. Measure the distance from the tool shank(A) to the tool tip(B) , record this value.
5. With the stock retracted; Press “T-SET” then “CORE” Softkey, then press “CYCLE START” and hold until all movement is complete. ( ADJUSTMENT (CORE)) will flash on screen. 6. Insert the tool into the tool pocket with the shank down in line with the stock and slide the stock out past the tool. If the stock pushes the tool away, reset and enter -.050” into “core” field and try again.
7. Place a shim between the tool shank and the stock and turn pulse wheel clockwise until the shim is pinching the shim. PRESS INPUT to add/subtract the value you moved the tool.
8. You must now ADD in TWICE the width of the shim(x2). Press “CORE” Softkey and key in the value. 9. You must now ADD/SUBTRACT in TWICE the measurement(x2) you got from step #4 above. (If the tip is HIGHER than the shank you will subtract…)
10. REMOVE the tool and retract the stock into the GuideBushing.
Tool Setting (DIA.) (T01 – T10) DIAMETER SETTING
1.
IMPORTANT !
You MUST do “CORE” setting above FIRST. (T01 – T06)
2. Call tool to “Position Point” (WAIT). ( as shown in previous section) 3. With the tool OUT or the stock retracted; Press “T-SET” then “DIA.” Softkey, then press “CYCLE START” and hold until all movement is complete. ( ADJUSTMENT( DIA).) will flash on screen.
4. Insert the tool into the tool pocket and slide the stock out under the tool tip. (T07-09 Insert tool into collet push back and snug into place.)
5. Slide the tool down/out onto the stock dia. WHILE pressing the tool SQUARLY into the pocket. 6. TIGHTEN the tool into place EVENLY by alternating back and forth between the two bolts. *** When using carbide tip tools you should “SNUG” the tool into place and retract the “X” axis before ** When tightening T07-09 the tool will pull back. You will then need to use a shim to SET the Dia..
Tool Setting (Long.)
(T11 – T14)
LONGITUDE SETTING 1.
Assemble your tools in sleeves or collet chucks with enough tool length to reach your needed depth.
2. Slide these sleeves into the desired pockets a nd set them back so there is **** LESS THAN 1.9” sticking out of the pocket **** (Longer will HIT during index) 3. FIRST, You must call your facing tool to “Wait” Point and face the bar using the “Cutoff” procedure. (***This will CREATE “Z” ZERO ***)
Without moving the stock. 4. Call first tool to be set to “Position Point” (WAIT). ( This will position the pocket at “X0” and “Z2” BACK ) 5. Now press the “soft key” “T-SET” (screen “soft keys”will change) 6. Press “LEN” Softkey. 7. Press and HOLD “CYCLE START” this will bring the sub spindle to the “set” position. 8. Slide the tool OUT against the face of the stock and tighten the bolts down on the sleeve or chuck. 9. To set the next tool, REPEAT #4 thru #8. 10. Repeat for each T11- 14 tool.
Tool Setting (Long.)
(T31 – T35)
LONGITUDE SETTING 1. Assemble your tools in sleeves or collet chucks with enough tool length to reach your needed depth. 2. Slide these sleeves into the desired pockets a nd set them back so there is **** LESS THAN 2.0” sticking out of the pocket **** (Longer will HIT during index)
3. CLEAR THE BAR STOCK TO PREVENT CRASH DURING INDEX. 4. You will need a part in the spindle that was picked off by the programmed cycle OR a gage block the exact length you will have protruding from the collet. 5. Call first tool to be set; from “PREP” mode P ress page down 6. Press the “WAIT” soft key > (screen “soft keys”will change) 7. Now press the “soft key” “T-SET” (screen “soft keys”will change) 8. Press “LEN”. 9. Press and HOLD “CYCLE START” ( This will position the chosen pocket at “X0” and “Y0” ) THEN, this will bring the sub spindle to the “set” position.
ONCE ALL MOVEMENT HAS STOPPED 10. Slide the tool OUT against the face of the stock and tighten the bolts down on the sleeve or chuck.
LONGITUDE MEASUREMENT When your tool is too short or too long: Do steps #1 thru #9 then; 11. You will use the “MPG” or pulse wheel to crank the spindle towards the tool WHILE holding a shim in between them. Once the part and the tool “pinch the shim you will stop and press ‘INPUT” . (this will enter the location of the tip into the “LEN” register.
12. To set the next tool select new tool number. 13. Call this tool to “LEN” **(the tool will slide sideways to next tool)** WATCH CLEARANCE!! 14. Now follow STEP #10 or #11 above to set length. 15. Repeat for each T3# tool.
Tooling
Guide Bushing & Collets
Types of Guide Bushings:
1) Southwick & Meister- #TD32 2) KEB Industries, inc - # 3) Hardinge
(Phone no. 1-203-237-0000, Fax no. 1-203-634-4509 ) (Phone no. 1-866-394-4438, Fax no. 1-440-953-9209) (Phone no. 1-800-843-8801, Fax no. 1-607-734-3886)
Carbide- Steel bushing with a carbide pad surface. Generally used for round Stock only. Has best wear life.
Steel- Always used rotating. Primarily used for hexes,squares, and special shapes. Can be used for round stock, wear life is less than carbide.
Meehanite- Has less tendency to “pick-up” or weld to the barstock than carbide and steel. When used stationary allows higher R.P.M without seizing. When used rotating can run polished stock without scratching.
X.P. (Extra Precision)- Held to closer concentricity tolerances. Extended Land- Will add up 3/8” of pad length.Used for special applications when you have to pull back into G/B and std. length is not sufficient.
Bushing Insert- A meehanite bushing is pressed into the tail end. Used for special applications and extra support and or pulling back into the G/B. Used with ground stock .Bushing is ground a couple of tenths above stock size.
Guide Bushing & Collets
Con`t
Note: Collets for the main and sub spindle have the same number designation. The collets come with a smooth bore up to .500. When ordering sub spindle collets over .500 specify smooth bore.
1)Southwick & Meister- #TF37SP ( Phone no. 1-203-237-0000, Fax no. 1-203-634-4509 ) 2) KEB Industries, inc - # (Phone no. 1-866-394-4438, Fax no. 1-440-953-9209) 3) Hardinge (Phone no. 1-800-843-8801, Fax no. 1-607-734-3886) Types of Collets:
-
Hex, Square, Special shape These collets are made to the same tolerance as the standard collets. The gripping surface rather than being ground is put in with an E.D.M
Eccentric- Collets can be provided with the gripping surface offset to spindle center line. EXT.
Extended
DIA.
Tappered Extended Nose
Standard
You must specify tapered dia. and amount of extension when ordering. Used to pickoff extremely short pc`s
Overgrip- sometimes it is necessary to pass the sub-spindle collet over a large diameter and close it on a smaller dia. A standard collet will only pass over a diameter that is about .005 bigger than its normal size. An overgrip collet is used to pass over a larger diameter difference. There are many factors involved in determining the maximum amount of overgrip, such as: nominal size, amount of land permissible, stroke of collet sleeve and the nose diameter.Therefore , these collets are only sold upon review of application.Note concentricity is usually poor. (Hardinge Phone no. 1-800-843-8801, Fax no. 1-607-734-3886)
X.P. (Extra Precision)- Held to closer concentricity tolerances. Incline Slotted- Used for picking off on non round material with a round collet.
O.D. Tooling (Static, Rotary) Note: Only tooling where the edge of the insert doesn`t extend out past the edge of the tool holder can be used(Figure #1), otherwise the insert could hit the guide bushing(Figure #2).
NO
YES
Z0
Z0
Figure #1
Figure #2
1) Mitsubishi Materials 1-800-523-0800 (www.mitsubishicarbide.com) 2)Sandvik- (Cutoff) 1-800-726-3845 3) Genevieve Swiss -(Tooling and Holders) 413-562-4800 (www.genswiss.com) 4)Iscar- (Turn,Groove,Cutoff) 1-717-620-3010 5)Valenite- 1-800-544-3336 6)NTK -( Backturn) 1-201-371-6499 7)Thinbit- (Small Grooving) 1-219-484-3620 8)Micro 100- (Boring and Cutoff) 9)Fette- (Thread Rolling) 1-800-225-0852 (www.lmtfette.com) 10) Robbjack- (Saws & Endmills – 1.25 dia. max saw ) 1-800-527-8883(www.robbjack.com) 11) Kyocera - (Micro tools) 1-888-848-8449 (www.kyoceramicrotools.com) 12)MicroCut – (Small carbide tooling) 1-866-426-3300 (www.microcutUSA.com) 13)Kennametal- (Turn,Groove,Backturn,Thread,Cutoff) 1-800-446-7738
I.D. Tooling (Front & Back) Collets/Chucks: 1) Msc (ER16 Collets) 2) Southwick & Meister (MPC 16 Collets) 1-203-237-0000 (Ct.) 3) Rego Fix 1-800-999-7346 (Indiana) 4) Centaur Drills: 1) Mitsubishi Carbide 800-523-0800 (www.mitsubishicarbide.com) 2)Titex 1-413-774-6561 3) Msc 4) Genevieve Swiss -(Tooling and Holders) 413-562-4800 (www.genswiss.com) 5) Guhring 1-414-784-6730 (Wisconsin)
Boring Bars: 1) Mitsubishi Carbide 800-523-0800 (www.mitsubishicarbide.com)
2) Genevieve Swiss -(Tooling and Holders) 413-562-4800 (www.genswiss.com) 3) Micro 100 4) Ph Horn 1-800-356-1111 5) Circle Tools (J&L-Windsor, Ct) 6) Kennametal (J&L-Windsor, Ct)
Start-up Tooling examples General Tooling : (OD Turning Tools .625 Square Shank Holders) (CutOff can be .750”) (I.D. front(T11-14) and back (T31-35) are ER20 collets with 1” shank holders. The Rotary Tools (T07-10) use ER16 collets) Turning: Mitsubishi : SVJBR1616M11-SM (35 R.H. Profile)(Insert-VBMT-2 Profile)(Insert-VBMT-221MV 21MV UE6020) Grooving: Mitsubishi: TTAHR/L 1616 1616 (Insert # TTAT####) TTAT####) Kennametal : NASR-102B (Insert-NG-2R) Threading: Mitsubishi: TTAHR/L 1616 1616 (Insert # TTAT####) TTAT####) Kennametal : 1) NASR-102B (Insert-NT-2R) (Insert-NT-2R) 2) LSASR-103 (Insert LT-16ER) BACK Turning : Mitsubishi : BTAHR1616-50 (Insert –BTBT604501R-B –BTBT604501R-B VP15TF) Cutoff: (***** The Cutoff tool position can accept 5/8” tools ***) Mitsubishi: CTDHL1616-350 (Insert-GTDT2535002N-B VP15TF) Iscar : 1) DGTR-16B-2D32 (Insert-DGR-2000P) (Insert-DGR-2000P) 2) DGTL-16B-2D32 (Insert-DGR-2000P) (Insert-DGR-2000P)
END Work A32 (T11-14) & (T31-T35) : Turning/Boring : Mitsubishi: 1) 25M-FSDUCL07 25M-FSDUCL 07 (Insert # 21.5##) 2) 25M-FSDUCL11 25M-FSDUCL 11 (Insert # 32.5##) 3) RBH1930 N (Insert # CB04RS VP17TF) Kennametal : 1) A16-TSCLCR/L3 (Insert-CPMT-32.5) (Right-hand) Grooving / Threading : 1) A16-NEL2 (Insert-NG-2R/NT-2R) (Insert-NG-2R/NT-2R) NOTE :
This is a generic list of of tool holders used on the A32. Grades , tool nose radius radius , width and insert geometry should be based on specific applications .
A32VII A32VII Tool Shee Sheett
Part #: Program # Bar Stock: Main Spl Collet –TF37SP Guide Bushing- TD32: Sub Spl Collet- TF37SP: Knockout: Cutting Oil: Cycle Time: BACKWORK
Operation Cut-Off
Tool
Off
T i p
Rad
Len Core
Diam
HP
collet
Holder
Insert
1 2 3 4 5 6 7
ER20
8
ER16
9
ER16
10
ER16
11 12 13 14 31 32 33 34 Notes: T51 T52 T53 T54 151
-
-
152
A32VII Tool Sheet
Part #: Program # Bar Stock: Main Spl Collet –TF37SP Guide Bushing- TD32: Sub Spl Collet- TF37SP: Knockout: Cutting Oil: Cycle Time: BACKWORK
Operation Cut-Off
Tool 1 2 3 4
Off
T i p
Rad
Len Core
Diam
HP
collet
Holder
Insert
A32VII Tool Sheet
Part #: Program # Bar Stock: Main Spl Collet –TF37SP Guide Bushing- TD32: Sub Spl Collet- TF37SP: Knockout: Cutting Oil: Cycle Time: BACKWORK
Operation Cut-Off
Tool
Off
T i p
Rad
Len Core
Diam
HP
collet
Holder
Insert
1 2 3 4 5 6 7
ER20
8
ER16
9
ER16
10
ER16
11 12 13 14 31 32 33 34 Notes: T51 T52 T53 T54 153
-
-
154
A32VII Tool Sheet
Part #: Program # Bar Stock: Main Spl Collet –TF37SP Guide Bushing- TD32: Sub Spl Collet- TF37SP: Knockout: Cutting Oil: Cycle Time: BACKWORK
Operation Cut-Off
Tool 1 2 3 4
Off
T i p
Rad
Len Core
Diam
HP
collet
Holder
Insert
A32VII Tool Sheet
Part #: Program # Bar Stock: Main Spl Collet –TF37SP Guide Bushing- TD32: Sub Spl Collet- TF37SP: Knockout: Cutting Oil: Cycle Time: BACKWORK
Operation Cut-Off
Tool
Off
T i p
Rad
Len Core
Diam
HP
collet
Holder
Insert
1 2 3 4 5 6 7
ER20
8
ER16
9
ER16
10
ER16
11 12 13 14 31 32 33 34 Notes: T51 T52 T53 T54 155
-
-
156
Class survey
Class: We’d like to thank you for attending this class and we hope you enjoyed it and you are leaving MCC with a better understanding of Citizen Machines. In an effort to continually improve our training classes we ask that you fill out the following survey. This survey is not mandatory and you do not have to fill in your name unless you choose to.
CLASS SURVEY
NAME (OPTIONAL) :
___________________________________________
Class survey
Class: We’d like to thank you for attending this class and we hope you enjoyed it and you are leaving MCC with a better understanding of Citizen Machines. In an effort to continually improve our training classes we ask that you fill out the following survey. This survey is not mandatory and you do not have to fill in your name unless you choose to.
CLASS SURVEY
NAME (OPTIONAL) :
___________________________________________
Please select an answer indicating how much you agree with the statement on the left.
Instructor was well prepared.
1
2
3
Strongly Disagree
Instructor had thorough kn owledge of the subject matter.
1
2
1
2
3
1
2
3
1
2
Strongly Disagree
5
4
3
4
5
4 Neutral
6 Strongly Agree
5
Neutral
3
6 Strongly Agree
Neutral
Strongly Disagree
Handout materials contr ibuted to class.
4
6 Strongly Agree
Neutral
Strongly Disagree
The instructor provided excellent answers to student’s questions.
5
Neutral
Strongly Disagree
The class was w ell organized.
4
6 Strongly Agree
5
6 Strongly Agree
