HEIDENHAIN TNC 620 User Manual page 185

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | POLYGON STUD (Cycle 258, DIN/ISO: G258,
software option 19)
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of stud. Input range
-99999.9999 to 99999.9999
Q202 Plunging depth? (incremental): Infeed per
cut; enter a value greater than 0. Input range 0 to
99999.9999
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while moving to depth.
Input range 0 to 99999.999; alternatively fmax,
FAUTO, fu, FZ
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999; alternatively PREDEF
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999; alternatively PREDEF
Q370 Path overlap factor?: Q370 x tool radius =
stepover factor k. Input range: 0.0001 to 1.9999
alternatively PREDEF
Q215 Machining operation (0/1/2)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing
Side finishing and floor finishing are only machined
when the specific allowance (Q368, Q369) is
defined
Q369 Finishing allowance for floor?
(incremental): Finishing allowance for the floor.
Input range 0 to 99999.9999
Q338 Infeed for finishing? (incremental):
Infeed in the spindle axis per finishing cut.
Q338=0: Finishing in one infeed. Input range 0 to
99999.9999
Q385 Finishing feed rate?: Traversing speed of
the tool in mm/min during side and floor finishing.
Input range 0 to 99999.999, alternatively FAUTO,
fu, FZ
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
Q215=0 ;MACHINING OPERATION
Q369=0 ;ALLOWANCE FOR FLOOR
Q338=0 ;INFEED FOR FINISHING
Q385=500 ;FINISHING FEED RATE
9 L X+50 Y+50 R0 FMAX M3 M99
5
185