Strippit HECC80 Control Punch Press Codes
N Optional Program-Line Block-Number. For Programmer's Convenience Only as
Control Does Not use Block Numbers for Anything. Example, Block 6 is N006
M00 Cycle Stop
M02 End of Program. Not usually used or needed.
M08 Tool Lube On, Activates Spray Mist Lubricator. Only on some 33-Station
Machines and No One uses. Who wants Operators to Breath Oil Fumes?
M09 Tool Lube Off
M30 Rewind. Rewind Stop-Code (a Percent Sign) % Must Appear in Program Before
M30 Code. Note that HECC80 Control does Not Need Rewind as Control will
Automatically Loop-Around to Beginning of Program. This Code is Carry-Over from
Old Paper-Tape Days when Paper-Tape Programs were "Rewind" to the Beginning.
M70 Low-Speed Press-Drive
M72 High-Speed Press-Drive. 2-Speed Press-Drive Machines automaticly go to hi-speed.
M74 Progressive Move "Canned-Cycle". Note, There are Several "Canned-Cycle"
Codes and it means a Whole Sequence of Events that are Performed by just 1 Code.
M75 Load Position. Axis Move to your Selected Positions, Turns-Off All Modal
Codes that were ON, and Stops Program for you to Load your Part-Sheet.
M81 Post Punch Delay. A Move-Delay After Punch of 100 or 250 msec. Selected by
Red-Switch on Front Panel Controller Board in Slot #7. This allows Extra Time for
Tool to Strip Out of Part, after Punch, so there is Less Change of a Part-Tool Jam.
A Modal Command, stays On & Active Until Turned-Off by Code.
M82 End Post Punch Delay.
G00 Point to Point Punching Mode. Used to go Back to Point to Point Punching
After a Nibble or Cutting Mode.
G01 Linear (Straight Line) Nibble Mode (Contouring)
G02 Circular Nibble (Contouring), Clockwise-Direction
G03 Circular Nibble (Contouring), Counter-Clockwise Direction
G60 Slow Feed, 750 Inch Per Minute Axis Speed. I Like Using "F" Feedrates than G60
G61 Remove Slow Feed, Go to Normal Full-Speed (Machine Dependent) Feedrate
G67 Turn the Punch Off
G68 Turn the Punch Back On
G69 Retract X & Y Axis to "Home" Position and T Axis (Tool Turret)
Retracts to Station T01. Not to be Confused with "Load Position".
G70 Dimensions are in Inch Input
G71 Dimensions are in Metric Input
G84 Tapping Head Canned-Cycle, No HECC80 Machine has Tapping Heads Anymore
G90 Absolute Input
G91 Incremental Input
G92 Absolute Preset
X X Axis Position Command. Dimensions are in .001 Inch or .01 Millimeter.
Assumed to be Positive Unless there is a Minus Sign.
Trailing Zeros can be used, but are Not needed.
There is Less Confusion if you Always use a Decimal Point.
Example, X 48 Inches. In 5-Digit Mode, The Following
are All the Same as far as HECC80 Control is Concerned;
X48 X+48 X48. X+48. X48000 X+48000 X48.000 X+48.000
I prefer X48. If you Always use Decimal Points, Control will Never be
Confused by 5 or 6 Digit Programs, or the 5 or 6 Digit Control-Switch Settings.
In 6 Digit Mode without a Decimal Point, Control would see X48 as 480 Inches.
Y X Axis Position Command. Same as X Above.
T Turret Tool Station Command. Expressed as T with 2 Digit Station Number
puts that Station Under the Punch-Ram. Example, Tool-Station #6 is T06
F F Codes are, In That Special Strippit-Way, Confusingly used in Different Ways.
In Normal Point to Point Punching,
F can (Feedrate is Optional) be used to Set Feedrate Speed on X and Y Axis,
in 1 Inch Increments between 1 Inch Per Minute and Full Speed.
For Example, on a FC1000/3 Machine the Axis Move at Normal Full-Speed of
3000 IPM unless a Feedrate is Specified. So I could Improve Accuracy or Keep
Large Parts from Pulling-Out of Workclamps by Slowing X and Y Axis Speed.
Perhaps I would use F15 for 1500 IPM, or F1 for 1000 IPM Feedrate Speed.
Add the F15 to the First Line of Code After Load-Position Block.
In Nibble Contouring Mode, F is Used to Set Actual Bite-Size of the Nibbling.
In Most HECC80/1 Machines you can use F040 to F200 Maximum which
corresponds to a Nibble-Bite-Size of .040 to .200 Inch. Undocumented, But
Decimal Points seem Ok with F.2 Same as F200 which is .200 Inch Bite.
In Metric Mode F100 to F500 Maximum corresponds to 1.00mm to 5.00 mm.
In Most HECC80/3 Machines, In Normal High-Speed Press-Drive Mode (M72)
you can use F040 to F200 Max. which is Nibble-Bite of .040 to .200 Inch.
In Optional Low-Speed Press-Drive Mode (M70) you can use F040 to F500
Max. which is Nibble-Bite of .040 to .500 Inch.
In some Laser and Plasma Continuous-Cutting Machines, F can be used as a
Operator-Added Feedrate-Override as a Percent % of Programmed Feedrate.
I Circular Interpolation Parameter for X-Axis. I Data is Distance from
Start-Point to the Center of Curvature of the Arc, and Must be Sined.
When in 5 Digit Mode, Values from 00000 to 99999 may be used.
In 6 Digit Mode (Including Metric), Values from 000000 to 999999 may be used.
J Circular Interpolation Parameter for X-Axis.
Similar to I Data word, Except J is Distance from Start-Point of Arc to
the Center of Curvature of the Arc Measured Parallel to Y-Axis.