Basics Of Feed Function; Rapid Traverse; Cutting Feed (F Command) - Siemens Sinumerik 802D sl Programming Manual

04.07
1.2

Basics of feed function

This section describes the feed function that specifies feedrate (distance per
minute, distance per revolution) of a cutting tool.
1.2.1

Rapid traverse

Rapid traverse is used for positioning (G00) and manual rapid traverse (RAPID)
operation. In the rapid traverse mode, each axis moves at the rapid traverse rate
set for the individual axes; the rapid traverse rate is determined by the machine
tool builder and set for the individual axes by using parameters. Since the axes
move independently of each other, the axes reach the target point at different time.
Therefore, the resultant tool paths are not a straight line generally.
1.2.2

Cutting feed (F command)

The feedrate at which a cutting tool should be moved in the linear interpolation
(G01) mode or circular interpolation (G02, G03) mode is designated using address
characters F. The axis feed mode to be used is selected by designating the feed
function G code (G94 or G95) as indicated in Table 1-3. Select the required feed
mode by designating the feed function G code before specifying an F code.
Table 1-3
G code
G94
G95
See 1.2.3 "Switching between feed per minute mode and feed per revolution
mode" for details of these G codes. The F code is modal and once designated it
remains valid until another F code is designated. If feed mode designation G codes
are switched between G94 and G95, however, it is necessary to designate the
F code again. If no new F code is designated, alarm 10860 "No feedrate program-
med" occurs.
Feed per revolution mode (G95)
A feedrate of a cutting tool per revolution of the spindle (mm/rev, inch/rev) can be
designated by a numeral specified following address character F.
Note: The upper limit of feedrates could be restricted by the servo system and the mechani-
cal system. For the actual programmable feedrate range, refer to the manuals pub-
lished by the machine tool builder.
© SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning - - 04.07 Edition
Cutting feed mode G codes
Designation of feed per minute (mm/min) mode
Designation of feed per revolution (mm/rev) mode
1.2 Basics of feed function
Function
Programming Basics
Group
05
05
1-17