Hurco winmax, Руководство по программированию, Страница: 174 / 254

4 - 60 ISNC G Codes
704-0115-307
WinMax Lathe NC Programming
G76 - Multiple Threading Cycle
G76 performs single edge ID and OD thread cutting. The cutting amount per depth is
held constant.
Default—No
Modal—Yes
Cancels:
• G32 - Constant Lead Thread Cutting
• G33 - Threading
• G77 - Outer Diameter/Inner Diameter Cutting Cycle
• G78 - Threading Cycle
• G79 - Stock Removal in Facing Cycle
This cycle can be interrupted. If either the Feed Hold or Interrupt Cycle button is
pressed, the tool will retract to Z start after completing the lead-out move for the current
depth of cut.
Format
G76 Pxxxxxx Q ____ R ____
G76 X(u) ____ Z(w) ____ R0 P ____ Q ____ F ____
Parameters
• P—first line with P, P contains 6 digits. Moving from left to right, the digits
represent the following values:
•
The first two digits represent the number of repetitive passes for the
finish pass. The value ranges from 1 to 99.
• The second two digits represent the chamfering distance along the Z axis
for the lead-out move. This value ranges from 0.1 to 9.9 in increments of
0.1 expressed as a value from 00 to 99 and is a multiple of the thread
lead specified by F.
• The last two digits represent the angle of the tool tip.
For example 2 finish passes, a chamfer of 1.5F using a tool tip angle of 55
would be expressed as: P021555
• Q—minimum depth of cut.
• X indicates Absolute X and (u) indicates Incremental X.
• Z indicates Absolute Z and (w) indicates Incremental Z.
Please refer to Sign of U and R, on page 4 - 62 for information about
determining the angle of the taper.