Programming

Sun, Jun 6, 2010

Control Tips, Expert Tips

Programming
Program Beginning & End Format – 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 Programming a program received via floppy or RS-232 (which will be the first line the operator sees) must be Onnnnn, 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.

M19 (Orient Spindle) with a P or R Value

This feature works on any vector drive mill. Previously, the M19 command would orient the spindle to only one position – that suitable for a tool change. Now, a P or R 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 value, the P command is used and no decimal point is needed. P270.001 (or any other fraction) will be truncated to P270. Also, P365 will be treated as P5. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.21 and above)

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 requires a decimal point: if you program M19 R60, the spindle will orient to 0.060 degree. Previously, R commands were not used for this purpose; only integer P values could be used. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.29 and above)

G150 Pocket Milling with 40 Moves

In the G150 command line, a P command (P12345) calls up a subprogram (O12345) that defines the geometry of a pocket. This pocket geometry must be defined in 40 moves (strokes) or less (any Mill Control ver. 11.11 and above). In software versions previous to 11.11, G150 Pocket Milling could only accommodate a subprogram with 20 moves or less.

Duplicating a Program

In 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 (Onnnnn), and then pressing F1. You can also duplicate a program in the Advanced Editor, using the Program menu and the Duplicate Active Program item.

Tapping: G84 or G74 Spindle Commands

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 use M03 or M04. The control will stop the spindle and turn it back on again to get the feed and speed in sync. The operator just needs to define the spindle speed.

G84 Quick Reverse

This feature allows the spindle to back out faster than it went into a tapped hole. This is specified 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 generated. 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)

G84 or G74 Tapping Back into a Hole

You can go back into a tapped hole to go deeper if you have the Rigid Tapping option and if you have not moved the tool or part. Parameter 57 bit 6, REPT RIG TAP, must be set to 1 (On). Edit the Z depth to go deeper, or offset down by the amount of one thread pitch to rerun a tapped hole. NOTE: If you move, offset, or change the starting position of the part or tap and it is not equal to one pitch of the thread, you will cross-thread the hole.

G84 or G74 Peck Tapping

You can also peck tap into a hole to go deeper (for tough/hard material) if Parameter 57 bit 6, REPT RIG TAP, is set to 1 (On). Then all you would need to do is repeat the tapping cycle at the same XY location, going deeper in the Z axis on each command line. See the following examples.
Example 1:
G90 G54 X1.5 Y-0.5
S450
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
G84 Z-0.5
G84 Z-0.75
G00 Z1. M09

Example 2:
G90 G54 X1.5 Y-0.5
S450
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
X1.5 Y-0.5 Z-0.5
X1.5 Y-0.5 Z-0.75
G00 Z1. M09

Note: On Mill software versions12.09 and above, REPT RIG TAP has been moved from the Parameters to Setting 133. This is now an On/Off setting that is much easier for the user to change.

|| More
, ,