HEIDENHAIN CNC Pilot 4290 - Manual (Page 164)

4 DIN PLUS 152
4.11 Milling Cycle Group
Contour milling G840
G840 mills, finishes, engraves or deburrs figures or ”free contours”
(open or closed) in the following program sections:
■ FRONT
■ REAR SIDE
■ SURFACE
NS/NE defines the contour section and the contour direction. NE is
not programmed for closed contours. For a single contour element,
you can program NS and NE to reverse the contour direction.
You can change the machining direction and the cutter radius
compensation (TRC) with the ”cycle type Q,” the ”cutting direction
H” and the rotational direction of the tool (see following table).
Deburring
G840 deburrs if ”chamfer width B” is programmed. The ”milling depth
P” defines the plunging depth of the tool – preempting the ”infeed I.”
”Preparation diameter J” (see illustration):
■ Open contour – J programmed: The contour is deburred all
around. Prerequisite:The deburring tool has a smaller diameter than
the milling cutter.
■ Open contour – deburring tool and milling cutter have equal
diameter: J is omitted
■ Closed contour: The side programmed with ”cycle type Q” is
deburred; J is omitted.
Other parameters are usually programmed in the same way as milling
contours.
Approach and departure
For closed contours, the point of the surface normal from the tool
position to the first contour element is the point of approach and
departure. If no surface normal intersects the tool position, the
starting point of the first element is the point of approach and
departure.
For figures, you can select the approach/depart element or machine
parts of the figure by selecting ”Begin, End Element Number D, V.”
Oversize
A G58 oversize ”shifts” the contour to be milled in the direction given
in ”cycle type.” ”Inside milling” (closed contour) contracts the
contour, while an ”outside milling” type expands it. For open contours,
the contour is shifted to the left or right, depending on the cycle type.
Continued
4.1
1 Milling Cy
cles
■ With ”cycle type Q=0,” oversizes are
not taken into account.
■ G57 and negative G58 oversizes are not
taken into account.
Cycle run
1 Starting position (X, Z, C) is the position before the
cycle begins.
2 Calculate the milling depth infeeds.
3 Move to the safety clearance and plunge to the first
milling depth.
4 Mill the contour.
5 ■ For open contours and for slots whose width =
tool diameter: Plunge to the next milling depth and
mill the contour in the opposite direction.
■ For closed contours and slots: Retract by the
safety clearance, return and cut to the next milling
depth.
6 Repeat steps 4 and 5 until the complete contour is
milled.
7 Retract to ”return plane K.”