Fixed Cycles or canned cycles

                                  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)