Manufacturing > Holemaking > Holemaking Cycle Types and Tabs
  
Holemaking Cycle Types and Tabs
Separate tools for drilling in the Mill mode and Turn mode are available. Mill mode drilling on a Mill/Turn Center work center is only available when a milling head is specified. Use options on the tab of the selected holemaking type to create a holemaking cycle. The procedure for creating a holemaking cycle is described in the topic To Create a Holemaking Cycle.
For example, if you select Standard on the Mill tab or Standard on the Turn tab, the Drilling tab opens. Use options on this tab to drill holes.
The following holemaking types are available and the tab that opens when you select a specific type is also listed in the table.
Category
Type
Mill Mode
Turn Mode
Tab Name
Description
Drill—Drill a hole. Depending on the additional option selected, the following statement will be output to the CL file
Standard
Drilling
CYCLE / DRILL
Deep
Drilling
CYCLE / DEEP
Constant
On the Parameters tab, select Constant in the Peck Type list.
Drilling
Variable Peck
On the Parameters tab, select Variable Peck in the Peck Type list.
Drilling
Break Chip
Drilling
CYCLE / BRKCHP
Web
Web Drilling
CYCLE / THRU (for multiple plates)
Back
Back Boring
A series of GOTO and SPINDLE statements to perform back boring.
Face
Face Drilling
Drill a hole with an optional dwell at final depth to help assure a clean surface at the bottom of the hole. The CYCLE / FACE statement will be output to the CL file.
Bore
Boring
Bore a hole to create a finish hole diameter with high precision. The CYCLE / BORE statement is output to the CL file.
Countersink
Countersinking
Drill a chamfer for a countersunk screw. The CYCLE / CSINK statement will be output to the CL file.
Back
Back Countersinking
The spindle is stopped as the tool traverses through hole to the hole where the spindle is engaged and the tool creates a countersink. If the Back option is selected, the system performs back countersinking.
Tap—Tap a threaded hole. Creo NC supports ISO standard thread output. The CYCLE / TAP statement will be output to the CL file. Two additional options are available:
Tapping
Tapping
The feed rate is determined by the combination of thread pitch and spindle speed.
Floating
On the Parameters tab, select Floating in the Tap Type list.
Tapping
Modify the feed rate using the parameter FLOAT_TAP_FACTOR.
Fixed
On the Parameters tab, select Fixed in the Tap Type list.
Tapping
Ream
Reaming
Create a precision finish hole. The CYCLE / REAM statement will be output to the CL file.
Custom
Custom Drilling
Create and use your own customized cycles for the current machine tool.
Tools Used for Holemaking Cycle Types
The table below summarizes which type of tool can be used for each cycle type:
TOOLS
CYCLE TYPES
Standard Drilling
Deep Drilling
Variable Peck Drilling
Breakchip Drilling
Web Drilling
Countersinking
Back Countersinking
Face Drilling
Boring
Back Boring
Reaming
Fixed Tapping
Float Tapping
Custom Drilling
Milling
End Mill
Bull Mill
Ball Mill
Drilling
Basic Drill
Countersink
Spot Drill
Tapping
Reaming
Boring
Center Drill
Boring Bar
Multi-Tip
Side Milling
Key Cutter
Lollipop
Plunge Milling
Back Spotting
 
* Drill type tools can also be used in Trajectory milling.