Haas Automation VF Series, Книга управления

Страница: 121 / 127

114
January 2004
PROGRAMMING
D Program Format at the Beginning and End - Programs written on a PC and sent to the control from a
floppy disk or through the RS-232 port must start and end with a % sign, on a line by itself. The second line in
a program received via floppy or RS-232 (which will be the first line the operator sees) must be O nnnnn, a six-
character program number that starts with the letter O followed by five digits. When you create a program on
the Haas control the percent (%) signs will be entered automatically, though you won’t see them displayed.
D Program Format with M06 - It is not necessary to turn off the coolant (M09), stop the spindle (M05), or
move the Z axis home (G28) prior to a tool change. The control will do these tasks for you during a tool change
M06 command. However, you may decide to program these commands anyway for convenience and timely
execution of a tool change sequence. If you’re using Single Block to step through a program you will be able to
see the commands when you stop on that line.
D M19 (Orient Spindle) with a P Value - This feature works on any vector drive mill. Previously, the M19
command would simply orient the spindle to only one position — that suitable for a tool change. Now, a P value
can be added that will cause the spindle to be oriented to a particular position (in degrees). If a whole number
is used for the P value, no decimal point is needed. For example, M19 P270 will orient the spindle to 270
degrees. Note that P270.001 (or any other fraction) will be truncated to P270, and P365 will be treated as P5.
(Any Mill Control ver. 9.49 and above. Any Lathe Control ver. 2.21 and above.)
D M19 (Orient Spindle) with a Fractional R Value - This feature works on any vector drive mill. An M19
R123.4567 command will position the spindle to the angle specified by the R fractional value; up to 4 decimal
places will be recognized. This R command now needs a decimal point : if you program M19 R60, the spindle will
orient to 0.060 of a degree. Previously, R commands were not used for this purpose and only integer P values
could be used.
(Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.29 and above.)
D G150 Pocket Milling with 40 Moves - In the G150 command line, it calls up a subprogram with a
P command (P1234) which is calling up a separate program (O1234) that defines in it, the geometry of a
pocket. This pocket geometry must be defined in 40 moves (strokes) or less. In software ver. 11.11, the G150
Pocket Milling was increased to 40 strokes. In all previous versions, the control could only accommodate a
G150 Pocket Milling subprogram with 20 moves or less.
(Any Mill Control ver. 11.11 and above)
D Duplicating a Program in LIST PROG - In the LIST PROG mode, you can duplicate an existing program
by cursor-selecting the program number you wish to duplicate, typing in a new program number ( O nnnnn), and
then pressing F1 . You can also go to the Advanced Editor menu to duplicate a program, using the PROGRAM
menu and the DUPLICATE ACTIVE PROGRAM item.
D G84 or G74 Tapping - When tapping, you don’t need to start the spindle with an M03 or M04 command.
The control starts the spindle for you automatically with each G84 or G74 cycle, and it will in fact be faster if
you don’t turn on the spindle with an M03 or M04. The control stops the spindle and turns it back on again in the
G84 or G74 tapping cycle to get the feed and speed in sync. The operator just needs to define the spindle speed.
D G84 Rigid Tapping Cycle Quick Reverse - This feature for rigid tapping has the spindle back out faster
than it went into a tapped hole. The way to specify this is with a J code on the G84 command line. J2 retracts
twice as fast as the entry motion; J3 retracts three times as fast, and so on, up to J9. A J code of zero will be
ignored. If a J code less than 0 or greater than 9 is specified, Alarm 306 — “INVALID I, J, K or Q” — is gener-
ated. The J code is not modal and must be specified in each block where this effect is wanted. The J value
should not contain a decimal point.
(Any Mill Control ver. 10.13 and above.)