HEIDENHAIN CNC PILOT 640 User Manual page 423

DIN/ISO programming | Milling cycles
G840 – deburring
G840 deburrs when you program Chamfer width B. If there is
any overlapping of the contour, specify with cycle type Q whether
the first section (as of starting point) or the entire contour is to be
machined. Program only the parameters given in the following table.
Parameters:
Q: Cycle type – milling location
Open contour. If there is any overlapping, Q defines whether
the first section (as of starting point) or the entire contour is to
be machined
Q = 0: Center of milling cutter on the contour (hole position
= starting point)
Q = 1: Machining at the left of the contour. If there is any
overlapping, only the first area of the contour is machined
Q = 2: Machining at the right of the contour. If there is any
overlapping, only the first area of the contour is machined
Q = 3: Not allowed
Q = 4: Machining at the left of the contour. If there is any
overlapping, the entire contour is machined
Q = 5: Machining at the right of the contour. If there is any
overlapping, the entire contour is machined
Closed contours
Q = 0: Center of milling cutter on the contour (hole position
= starting point)
Q = 1: Inside milling
Q = 2: Outside milling
Q = 3 to 5: Not allowed
ID: Milling contour – name of the milling contour
NS: Starting block no. of contour – beginning of contour section
Figures: Block number of the figure
Free closed contour: First contour element (not starting point)
Open contour: First contour element (not starting point)
NE: Contour end block no. – end of contour section
Figures, free closed contour: No input
Open contour: last contour element
Contour consists of one element:
No input: Machining in contour direction
NS = NE programmed: Machining against the contour
direction
E: Reduced feed for circular elements (default: active feed rate)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
423