Positioning On Freely Programmable Positions And Position Patterns; Freely Programmable Positions - Siemens SINUMERIK 840D Operation/Programming Manual

3
10.04

3.7.8 Positioning on freely programmable positions and position patterns

Machining sequence and
tool travel path
Including/skipping
positions
Rotary axis
 Siemens AG, 2004. All rights reserved
SINUMERIK 840D/840Di/810D Operation/Programming ShopMill (BAS) – 10.04 Edition
After you have programmed the machining technologies, you must
program the positions. ShopMill offers a variety of positioning
patterns, i.e.:

• Freely programmable positions

• Position on a line, on a matrix or box
• Position on a full or pitch circle
Several position patterns can be programmed in succession (up to 20
technologies and position patterns together). They are traversed in
the order in which you program them.
The programmed technologies and subsequently programmed
positions are automatically chained by the control.
The first tool in the program traverses all programmed positions, e.g.
center all positions. Machining of the positions always starts at the
reference point.
In the case of a matrix, machining is performed first in the direction of
the 1st axis and then back and forth. The box and hole circle are
machined counterclockwise. The second tool in the program then
machines all programmed positions, etc. This process is repeated
until every programmed drilling operation has been performed at
every programmed position.
Inside a position pattern or on the approach from one position pattern
to the next, the tool is retracted to safety clearance in the case of
optimized retraction, or otherwise to the return plane (see also Sec.
"Creating new program; defining a blank"). The new position is then
approached at rapid traverse.
If the position pattern consists of only one position, the tool is
retracted to the retraction plane after machining.
You can include or skip any positions.
If an A or B axis is set up on your machine, this is supported during
drilling (any position pattern, full circle, and pitch circle).
Please also refer to your machine manufacturer's instructions.
In the A or B axis is present, it makes sense to define a work offset
with
X = end face of the cylinder
Y = center point of the cylinder
Z = center point of the cylinder
The "cylinder" in this case refers to any part that is clamped in the A/B
axis.
Programming with ShopMill
3.7 Drilling
3
3-245