SURFCAM has several canned drill cycles and three user definable custom drill cycles. Cycle names are used by post processors to access the canned cycles in the NC machines.
Cycle Type defaults to the type of cycle that would normally be used with the currently selected tool.
If you change the tool after you select a cycle type, you can inadvertently change the cycle type.
Drill
The tool moves to the bottom Z level at the Feed rate speed. The tool then retracts at the Rapid speed rate. This option is a G81 move on most NC machines.
Peck
This option is a peck operation. This option is a G83 move on most NC machines. The Peck Increment parameter is active when the Peck option is selected.
Chip Break
This cycle is used to break the drill chips. On most NC machines it is a G73 code.
Tap
This option is a standard tapping cycle. The tool moves to the bottom Z level at the Feed speed rate. The spindle direction reverses at the bottom of the hole. The tool then retracts to the top of the hole at the Feed speed rate. This option is a G84 move on most NC machines.
Tapping requires that the feed rate match the spindle speed. SURFCAM does this automatically. The tool library must indicate that the number of flutes on a tapping tool is one. The chip load per flute must be equal to the thread pitch of the tap. A 1/4-20 tap has a chip load value of 0.05.
Left Tap
This option is a left-hand tapping cycle like the Tap cycle, but with reversed spindle direction.
Rigid Tap
This option is a tapping cycle for a tap that is held tight in the spindle. The machine controller makes the spindle speed and feed rate match. The machine controller sets the spindle speed and feed rate values to the correct values.
Rigid Left Tap
This option is a left-hand tapping cycle like the Rigid Tap cycle, but with reversed spindle direction.
Ream
This option is like the Drill cycle except that the tool retracts from the hole at the Feed rate speed. This option is a G85 move on most NC machines.
Bore
This option is a bore cycle that will bore to the bottom of the hole. The spindle then stops. The tool is then moved away from the edge of the hole a small distance. The tool then retracts from the hole at the rapid speed rate. This option is a G86 move on most NC machines.
The Bore Side Clearance parameter is active when the Bore option is selected.
Back Bore
This option is a back-bore cycle that stops and adjusts the spindle orientation before the cycle starts. The tool moves at rapid speed to the bottom of the hole. The tool then moves at the feed speed rate toward the wall before the spindle is started. The tool then feeds to the top of the hole and bores the hole from the bottom to the top.
Bore Side Clearance parameter is active when the Back Bore option is selected.
Custom 1, Custom 2, Custom 3
These options are cycles that the user defines. These cycles are defined to use the unique or special capabilities of an NC machine. An example of a unique capability is the Chip-Break function.
Countersink
The Countersink option creates a countersink on a drill hole. When this option is selected, the Hole Depth parameter is changed to the Countersink Diameter. SURFCAM uses the Countersink Diameter parameter, the Clearance parameter value and the tool Tip Angle (from the Tool Library) to calculate the countersink depth.
Center Drill
The Center Drill option creates a hole to guide the next tool. A center drill tool with a center tip drills the guide hole.
Counterbore
The Counterbore option creates a hole with a square shoulder on the bottom.
Spot Drill
The Spot Drill option create a guide hole like the Center Drill option. A spot drill is used.