HEIDENHAIN CNC Pilot 4290 - Manual (Page 134)

4 DIN PLUS 122
4.7 T
u
rning Cy
cles
Longitudinal roughing G810
G810 machines the contour area defined by “NS, NE.” The CNC
PILOT uses the tool definition to distinguish between external and
internal machining. With “NS – NE” you specify the machining
direction.
If the contour to be machined consists of one element, then:
■ If you program only NS: Machining in contour definition
direction
■ If you program NS and NE: Machining against the contour
definition direction
If required, the area to be machined is divided into several sections
(example: with contour valleys).
The simplest way of programming is specifying NS, NE and P.
Parameters
NS:
Starting block number (beginning of contour section)
NE: End block number (end of contour section)
P: Maximum infeed
I: Oversize in X direction (diameter value)—default: 0
K: Oversize in Z direction—default: 0
E: Approach behavior
■ E=0: Descending contours are not machined
■ E>0: Approach behavior
■ No input: Feed rate reduced depending on approach
angle—maximum reduction: 50%
X: Cutting limit in X direction (diameter value)—default: no
cutting limit
Z: Cutting limit in Z direction—default: no cutting limit
H: Type of contour smoothing—default:
■ H=0: smoothing after each cut
■ H=1: lift off at under 45°, smoothing after last cut
■ H=2: lift off at under 45°, no smoothing
Continued
Cycle run
1 Calculate the areas to be machined and the
cutting segmentation (infeeds).
2 Approach workpiece for first pass from starting
point, taking the safety clearance into account
(first in Z direction, then in X).
3 Move at feed rate to target point Z.
4 Depending on H:
■ H=0: Cut along the contour
■ H=1 or 2: Retract at 45°
5 Return at rapid traverse and approach for next
pass.
6 Repeat 3 to 5 until target point X has been
reached.
7 If required, repeat 2 to 6 until all areas have been
machined.
8 H=1: Smoothen contour.
9 Retract according to ”Q.”
4.7 Turning Cycles
4.7.1 Contour-Based Turning Cycles
Finding the block references:
Activate the contour graphics (GRAPHICS soft key)
Set the cursor to NS/NE and press the CONTINUE soft key
Using the horizontal arrow keys to select the contour element
The vertical arrow keys can be used to switch between contours
(also face contours, etc.)
Confirm the block of the contour element with ENTER
If you press the vertical arrow keys, the
CNC PILOT also considers contours that
are not displayed on the screen.