Need Help!- Z feed rate change

[haastm2]

We have a TM-2. After writing a program using the rectangle pocketing cycle (IPS). The line that is produced starts with G150. The feed rate that the machine inputs on that line is used for all movements (XYZ). Can you change the plunge feed rate (Z) for that cycle and have a different (XY) feed rate, if you do not have a pre drilled hole for a 2 flute end mill. We are plunging with the same tool that is used for the pocket milling.

Any help

Thanks

[Geof]

Have you actually run the pocket routine? I understood the pre-drilled center hole is mandatory and the few times I have used G150 it seems the feed down into this hole is a rapid.

[maccam cnc]

You are correct in your original statement in that the cycle will feed down in Z at the same feed as you want to use in X and Y axis.

The work around for this is to place a G01 line feeding to depth at a sensible feed for this move and then feed back to the top of the part BEFORE calling the G150

G01 Z-.5 F4. ;
G01 Z.05 F20. ;
G150 Z-.5 etc.

[Caue]

Directly from Haas Mill Operator's Manual (pay special attention to the end notes):

"G150 General Purpose Pocket Milling (Group 00)

D Tool radius/diameter offset selection
F Feedrate
I X-axis cut increment (positive value)
J Y-axis cut increment (positive value)
K Finishing pass amount (positive value)
P Subprogram number that defines pocket geometry
Q Incremental Z-axis cut depth per pass (positive value)
R Position of the rapid R-plane location
S Optional spindle speed
X X start position
Y Y start position
Z Final depth of pocket

The G150 starts by positioning the cutter to a start point inside the pocket, followed by the outline, and completes with a finish cut. The end mill will plunge in the Z-axis. A subprogram P### is called that defines the pocket geometry of a closed area using G01, G02, and G03 motions in the X and Y axes on the pocket. The G150 command will search for an internal subprogram with a N-number specified by the P-code. If that is not found the control will search for an external subprogram. If neither are found, alarm 314 Subprogram Not In Memory will be generated.
Note: When defining the G150 pocket geometry in the subprogram, do not move back to the starting hole after the pocket shape is closed.
An I or J value defines the roughing pass amount the cutter moves over for each cut increment. If I is used, the pocket is roughed out from a series of increment cuts in the X-axis. If J is used, the increment cuts are in the Yaxis.
The K command defines a finish pass amount on the pocket. If a K value is specified, a finish pass is performed by K amount, around the inside of pocket geometry for the last pass and is done at the final Z depth. There is no
finishing pass command for the Z depth.
The R value needs to be specified, even if it is zero (R0), or the last R value that was specified will be used.
Multiple passes in the pocket area are done, starting from the R plane, with each Q (Z-axis depth) pass to the final depth. The G150 command will first make a pass around pocket geometry, leaving stock with K, then doing passes
of I or J roughing out inside of pocket after feeding down by the value in Q until the Z depth is reached.
The Q command must be in the G150 line, even if only one pass to the Z depth is desired. The Q command starts from the R plane.
Notes: The subprogram (P) must not consist of more than 40 pocket geometry moves.
The Q command must be in the G150 line, even if only one pass to the Z depth is desired. The Q command starts from the R plane.
It may be necessary to drill a starting point, for the G150 cutter, to the final depth (Z). Then position the end mill to the start location in the XY axes within the pocket for the G150 command."