HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 264)

264
4.27 Milling Cy
cles
Parameters – milling
Q Cycle type (= milling location).
„ Open contour. If there is any overlapping, Q defines
whether the first area (as of starting point) or the entire
contour is to be machined.
„ Q=0: Milling center on the contour (without TRC)
„ Q=1: Machining at the left of the contour. If there is
overlapping, G840 machines only the first area of the
contour.
„ Q=2: Machining at the right of the contour. If there is
overlapping, G840 machines only the first area of the
contour.
„ Q=3: The contour is machined to the left or right
depending on H and the direction of cutter rotation (see
table). If there is overlapping, G840 machines only the
first area of the contour.
„ Q=4: Machining at the left of the contour. If there is
overlapping, G840 machines the entire contour.
„ Q=5: Machining at the right of the contour. If there is
overlapping, G840 machines the entire contour.
„ 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
NS Block number—beginning of contour section
„ Figures: Block number of the figure
„ Free open or closed contour: First contour element (not
starting point)
NE Block number—end of contour section
„ Figures, free closed contour: No input
„ Free open contour: Last contour element
„ Contour consists of one element:
„ No input: Machining in contour direction
„ NE programmed: Machining against the contour direction
H Cutting direction (default: 0)
„ H=0: Up-cut milling
„ H=1: Climb milling
I (Maximum) infeed (default: milling in one infeed)
F Infeed rate (depth infeed) – (default: active feed rate)
E Reduced feed rate for circular elements (default: current feed
rate)