G81 Drilling Canned Cycle / G80 Cancel Canned Cycle
OBJECTIVES
After completing this unit, you should be able to:
- Identify and describe G81 Drill Canned Cycle for CNC code
- Identify and describe G80 Cancel Canned Cycle
- Identify Z-depth for a center drill
- Calculate Z-axis (part thickness + radius of drill) for thru holes
- Write a three-part CNC program using G81 canned cycle code
G81 Drill Canned Cycle
Variables in G81
G99 – R-plane Return after the drilling operation is complete
F = Feedrate in inches per minute (IPM) or Metric (mm)
R = Position of the R plane for drilling operation to begin (tool out of the hole, above the part)
X = X-axis motion
Y = Y-axis motion
Z = Position of the Z-axis at the bottom of hole
G81 Uses
The CNC code G81 is used with center drills and drilling operations. These would be different tools in the CNC machine, so two sections of the program would use G81. One section for the center drill. Another section for the drill tool.
One block (of code) is for the center drill. The following block (of code) is for drilling.
The operation drills to center of tool. The program will not use G41 or G42.
The drill is 118°. The tip of the center drill is used. This makes sure that all surfaces on the second cut with the drill tool will have contact with workpiece. A 118° center drill has more surface contact than a 60° drill.
The Z is only -.05, which will only use the tip of the center drill. This is the depth for the center drill.
G80 Cancels Canned Cycles
A canned cycle is modal and must be cancelled. G80 deactivates all canned cycles. The code appears in the footer.
For example:
| T1 M06 (5 CD) [Center Drill = CD]
G90 G54 X .75 Y -1 (hole #1) S1000 M03 G43 H01 Z1.0 M08 |
Header |
| G81 G99 R.1 [start feed] Z-.05 [described above] F10 [drills 1st hole]
X # Y# [coordinates for other holes] |
Body |
| G80 G00 Z1.0 M09 [Cancel canned cycle]
G28 G91 Z0 M05 M01 [program is not ending because we need to drill.] |
Footer |
Above is just the center drill.
Holemaking is a two-step operation.
The drilling operation, the second step, is below.
| T02 M06 (1/2″ drill)
G90 G 54 G00 X Y [hole location] S???? M03 [Use CNC speed chart from lab portion of class] G43 G02 Z1.0 M08 |
Header |
| G81 G99 R .1 Z -.625 F20 [canned cycle command for drilling operation.]
X Y [locations for all holes] |
Body |
Drill Depth (Z-.625 above) explanation
The code must compensate for the angle on the tip of the drill.
For a thru-hole, the Z (depth) needs to push the tip of the drill past the opening on the bottom of the part. That part of the hole must also keep its measurement.
To keep calculations simple, let’s calculate the angle of the tip of the drill to 90°. It is easy math.
The calculation is this: part thickness + radius of drill = Z for thru hole.
In the example above, the thickness of the workpiece is .500 (it was not given above) and the radius of a 1/2″ drill is .125.
Therefore, .500 + .125 = .625 for the Z in the negative (-.625).
Shop Talk
T