1 3 6
G Codes
96-8000 rev R June 2007
C
ANNED
C
YCLES
Introduction
Canned cycles are used to simplify programming. They are used for repetitive operations, such as drilling, tapping,
and boring. The canned cycle is executed every time an X and/or Y-axis motion is programmed.
Using Canned Cycles
The positioning of a canned cycle in the X and/or Y-axes can be done in either absolute (G90) or incremental (G91).
Incremental (G91) motion in a canned cycle is often useful with a loop count (Lnn) which will repeat the canned
cycle operation that many times with each incremental X or Y move for the canned cycle.
Example:
G81 G99 Z-0.5 R0.1 F6.5 (This will drill one hole at the present location)
G91 X-0.5625 L9 (This will drill 9 more holes .5625 equally spaced in the minus direction)
If a canned cycle is defined without an X or Y and a loop count of 0 (L0), the cycle will not be performed initially.
The operation of the canned cycle will vary according to whether incremental (G91) or absolute (G90) positioning is
active. Incremental motion in a canned cycle is often useful as a loop (L) count as it can be used to repeat the
operation with an incremental X or Y move between each cycle.
Example:
X1.25 Y-0.75 (center location of bolt hole pattern)
G81 G99 Z-0.5 R0.1 F6.5 L0 (L0 on the G81 line will not drill a hole in the bolt hole circle)
G70 I0.75 J10. L6 (6-hole bolt hole circle)
Once a canned cycle is commanded, that operation is done at every X-Y position listed in a block. Some of the
canned cycle numerical values can be changed after the canned cycle is defined. The most important of these are
the R plane value and the Z depth value. If these are listed in a block with XY commands, the XY move is done and
all subsequent canned cycles are performed with the new R or Z value.
The positioning of the X and Y-axes prior to a canned cycle is done with rapid moves.
G98 and G99 change the way the canned cycles operate. When G98 is active, the Z-axis will return to the initial
start plane at the completion of each hole in the canned cycle. This allows for positioning up and around areas of
the part and/or clamps and fixtures.
When G99 is active, the Z-axis returns to the R (rapid) plane after each hole in the canned cycle for clearance to
the next XY location. Changes to the G98/G99 selection can also be made after the canned cycle is commanded,
which will affect all later canned cycles.
A P address is an optional command for the some of the canned cycles. This is a programmed pause at the
bottom hole to help break chips, provide a smoother finish and relieve any tool pressure to hold closer tolerance.
Note that if a value for P is entered for one canned cycle it will be used in others unless cancelled (G00, G01, G80
or the Reset button).
An S (spindle speed) command must be defined in, or before the G-code line of code.
Tapping in a canned cycle needs a feed rate calculated. The Feed Formula is:
Spindle speed divided by Threads per inch of the tap = Feedrate in inches per minute
Canned Cycles also benefit from the use of Setting 57. Turning this setting ON will perform an exact stop between
rapids. This is useful to avoid nicking the part at the bottom of the hole.
NOTE: The Z, R, and F addresses are required data for all canned cycles.
Canceling a Canned Cycle
The G80 code is used to cancel all canned cycles; note that a G00 or G01 code will also cancel a canned cycle.
Once selected, a canned cycle is active until canceled with G80, G00 or G01.
Содержание Mill
Страница 12: ...96 8000 rev R June 2007 Safety 5 ...
Страница 14: ...96 8000 rev R June 2007 Safety 7 LATHE WARNING DECALS ...
Страница 15: ...8 Safety 96 8000 rev R June 2007 ...
Страница 17: ...10 Introduction 96 8000 rev R June 2007 ...
Страница 117: ...110 4 5 Axis Programming 96 8000 rev R June 2007 ...
Страница 199: ...Settings 192 96 8000 rev R June 2007 ...
Страница 213: ...206 Maintenance 96 8000 rev R June 2007 ...
