On the CNC Milling and machining centers the most common
operation done is the drilling, tapping and boring the holes. The standard
center drilling, spot drilling and drilling are used together with related
operations such as reaming, tapping, single point boring, countersinking and
counter boring operations. Always machining a simple hole requires only a single drill
but the complex hole may require several tools to be completed. All CNC control manufacturers have incorporated
the programming methods for machining holes in their control systems. These
methods are called canned cycles or fixed cycles. Machining holes are operated with point to point machining;
the detailed of Point to point machining is explained as below:
POINT-TO-POINT Machining:
While
machining the holes actual cutting takes place is along a single axis i.e., the
Z=axis. This type of machining is commonly called as point-to-point machining.
This method involves the rapid motion in X and Y-axis for positioning to centre
of hole and then the cutting take place in Z-Axis with machining federate. Some motions along Z axis may also include
rapid motion till the tool reaches the part for machining hole. The programming
structure for point to point machining can be grouped into four general steps
as shown below:
Step1: Rapid
motion to the hole position along X and/or Y-axis.
Step2: Rapid motion to the starting point of the cut along the Z
axis.
Step3: Feedrate
motion to the specified depth along Z axis
Step4: Return to
a clear position along the Z axis.
These
four steps represent the minimum number of blocks required to program a
drilling for a single hole using manual programming method, without using fixed
cycles or canned cycles. If you have one or two holes in a part with same
diameter then the program is very simple with the minimum tool. Suppose you
have a more holes with different diameter then we may have to call more
tools to finish all the holes.
Fixed Cycles or canned cycles:
Most of
the time consuming task in programming point to point operation is the
repetitive information written in the program, this can be overcome by using
the fixed cycles, here once the drilling cycle is called and the next the
inputting the position of holes is
enough, the controller repeats the drilling cycle until it is cancelled by the
G-code. This method is called the canned or fixed cycle.
The
canned cycle is designed by the control manufacturers to eliminate the repeated
data in manual programming and allow an easy program data changes at the
machine. A number of identical holes may share the same starting point, same
feedrate and the same depth, only the X and Y coordinates are different for
each hole on the part. The specified values become modal for the duration of the
cycle and do not have to be repeated, unless there is a change in them.
These canned cycles are called in the program by a G command
as following canned or fixed cycles.
G73 = High speed peck
drilling cycle.
G74 = Left hand Tapping cycle.
G76 = Boring cycle
G80 = cancel of any kind of canned cycles.
G81 = general drilling or simple drilling cycle.
G83 = Peck drilling cycle.
G84 = Right hand tapping cycle.
G85 = Simple Boring Cycle.
G86 = Boring cycle with spindle stop
G87 = Back boring cycle.
Programming Format for the canned cycle:
General format for the canned cycle is a series of values
specified by the unique address. The format is as shown below:
N... G... X...Y... R... Z... P... Q... I... J... F... K…
Whereas,
N = Block Number
G= Cycle Number eg: G81, G83 etc.
X = Hole position in X-axis
Y= Hole position in Y-Axis
R = Start position or the return Level
Z= depth of the hole
P= Dwell time (1s=1000ms)
Q = Depth of the peck drill
I = shift amount in X-direction for boring cycles.
J= shift amount in Y-direction
for boring cycles.
F= Feed rate
K = number of repetitions.
Programming example for Point to point position and canned cycles:
Manual
Programming with Points: Programming with Fixed cycles or canned cycles:
O1000 O1000
N100 G20 G17 G40 G80 N100
G20 G17 G40 G80
N101 G90 G54 G00 X5.9 Y1.89 S1000
M03 N101 G90 G54 G00 X5.9
Y1.89 S1000 M03
N102 G43 Z1 H01 M08 N102
G43 Z1 H01 M08
N103 Z0.5 N103
G99 G81 R0.5 Z-2 P300 F5
N104 G01 Z-2 F5 N104
X3.87 Y3.4
N105 G04 P300 N105
X2.047
N106 G00 Z0.5 N106
G80 G28 Z0 M09
N107 X3.87 Y3.4 N107
M30
N108 G01 Z-2 F5
N109 G04 P300
N110 G00 Z0.5
N111 X 2.047
N112 G01 Z-2 F5
N113 G04 P300
N114 G00 Z0.5 M09
N115 G28 Z0
N116 M30
General rules to be followed by the fixed cycles or canned cycles:
è Absolute
or incremental mode can be programmed anytime in the fixed cycle or before the
fixed cycle. i.e., G90 for absolute mode and the G91 for Incremental mode
è If
both X and the Y-axis Omitted in the canned cycle mode then the cycle will be
executed at the current position of the tool. If one of the axis is omitted,
the cycle will be executed in the specified location of one axis, without
changing the other axis.
è If
you miss to select G98 or G99, the control system will select the default command
set ny a system parameter, usually G98 is default command.
è Address
P for the dwell cannot be used with the decimal points, dwell is always
programmed in milliseconds.
è The
command G80 should be always used to cancel the canned cycles, no any other
canned cycles can be called in the same line.
Canned or fixed cycle cancellation
Any canned or the fixed cycle that is active can be
cancelled with the G80 Gcode command. When the machine calls the G80 Gcode the
control mode is automatically transferred to the rapid motion mode G00.
Code line for G81 Drilling cycle:
N100 G98 (G99) G81 X... Y... R... Z... F...
N110 G80 (Canned
cycle cancel)
N120 G0 Z… (To the
safety plane)