Calling a cycle in connection with point tables
8.3 Drilling Cycles
The TNC offers 9 (or 13) cycles for all types of drilling operations:
Cycle Soft key
2nd setup clearance, chip breaking, and decrement G204 BACK BORING
With automatic pre-positioning, 2nd set-up clearance
G205 UNIVERSAL PECKING
(only with TNC 426 and TNC 430 with NC software 280 474-xx) With automatic pre-positioning,
2nd setup clearance, chip breaking, advanced stop distance
8.3 Dr illing Cy cles
Cycle Soft key
G84 TAPPING
With a floating tap holder G85 RIGID TAPPING
Without a floating tap holder G86 THREAD CUTTING (not in TNC 410) G206 TAPPING NEW
(only with TNC 426, TNC 430 with NC software 280 474-xx)
with floating tap holder automatic pre-positioning, 2nd setup clearance G207 RIGID TAPPING NEW
(only with the TNC 426, TNC 430 with NC software 280 474-xx)
Without floating tap holder, with automatic pre-positioning, 2nd setup clearance G208 BORE MILLING
(only with the TNC 426, TNC 430 with NC software 280 474-xx)
With automatic pre-positioning, 2nd set-up clearance
PECKING (Cycle G83)
1The tool drills from the current position to the first plunging depth at the programmed feed rate F.
2When it reaches the first plunging depth, the tool retracts in rapid traverse to the starting position and advances again to the first plunging depth minus the advanced stop distance t.
3The advanced stop distance is automatically calculated by the control:
■At a total hole depth of up to 30 mm: t = 0.6 mm
■At a total hole depth exceeding 30 mm: t = hole depth / 50 Maximum advanced stop distance: 7 mm
4The tool then advances with another infeed at the programmed feed rate F.
5The TNC repeats this process (1 to 4) until the programmed total hole depth is reached.
6After a dwell time at the hole bottom, the tool is returned to the starting position in rapid traverse for chip breaking.
Before programming, note the following:
Program a positioning block for the starting point (hole center) in the working plane with RADIUS
COMPENSATION G40.
Program a positioning block for the starting point in the tool axis (set-up clearance above the workpiece surface).
The algebraic sign for the cycle parameter TOTAL HOLE DEPTH determines the working direction.
úSetup clearance (incremental value): Distance between tool tip (at starting position) and workpiece surface
úTotal hole depth (incremental value):
Distance between workpiece surface and bottom of hole (tip of drill taper)
úPlunging depth (incremental value):
Infeed per cut. The tool will drill to the total hole depth in one movement if:
■ The plunging depth is equal to the total hole depth
■ The plunging depth is greater than the total hole depth
The total hole depth does not have to be a multiple of the plunging depth.
úDwell time in seconds: Amount of time the tool remains at the total hole depth for chip breaking úFeed rate F: Traversing speed of the tool during
drilling in mm/min
DRILLING (Cycle G200)
1 The TNC positions the tool in the tool axis at rapid traverse to the set-up clearance above the workpiece surface.
2 The tool drills to the first plunging depth at the programmed feed rate F.
3 The TNC returns the tool at rapid traverse to the setup clearance, dwells there (if a dwell time was entered), and then moves at rapid traverse to the setup clearance above the first plunging depth.
4 The tool then advances with another infeed at the programmed feed rate F.
5 The TNC repeats this process (2 to 4) until the programmed total hole depth is reached.
6At the hole bottom, the tool path is retraced to set-up clearance or, if programmed, to the 2nd set-up clearance in rapid traverse.
Before programming, note the following:
Program a positioning block for the starting point (hole center) in the working plane with RADIUS
COMPENSATION G40.
The algebraic sign for the depth parameter determines the working direction.
úSet-up clearance Q200 (incremental value): Distance between tool tip and workpiece surface. Enter a positive value.
úDepth Q201 (incremental value): Distance between workpiece surface and bottom of hole (tip of drill taper)
úFeed rate for plunging Q206: Traversing speed of the tool during drilling in mm/min
úPlunging depth Q202 (incremental value):
Infeed per cut The TNC will go to depth in one movement if:
■ the plunging depth is equal to the depth
■ the plunging depth is greater than the depth The depth does not have to be a multiple of the plunging depth.
úDwell time at top Q210: Time in seconds that the tool remains at set-up clearance after having been retracted from the hole for chip release.
úWorkpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
X
N70 G200 Q200=2 Q201=-20 Q206=150 Q202=5 Q210=0 Q203=+0 Q204=50*
ú2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision between tool and workpiece (clamping devices) can occur.
The TNC 426, TNC 430 with NC software 280 474-xx also provides:
úDwell time at depth Q211: time in seconds that the tool remains at the hole bottom
REAMING (Cycle G201)
1The TNC positions the tool in the tool axis at rapid traverse to the input set-up clearance above the workpiece surface.
2The tool reams to the entered depth at the programmed feed rate F.
3If programmed, the tool remains at the hole bottom for the entered dwell time.
4The tool then retracts to set-up clearance at the feed rate F, and from there — if programmed — to the 2nd set-up clearance in rapid traverse.
Before programming, note the following:
Program a positioning block for the starting point (hole center) in the working plane with RADIUS
COMPENSATION G40.
The algebraic sign for the depth parameter determines the working direction.
úSet-up clearance Q200 (incremental value): Distance between tool tip and workpiece surface.
úDepth Q201 (incremental value): Distance between workpiece surface and bottom of hole
úFeed rate for plunging Q206: Traversing speed of the tool during reaming in mm/min
úDwell time at depth Q211: Time in seconds that the tool remains at the hole bottom
úRetraction feed rate Q208: Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the tool retracts at the reaming feed rate.
úWorkpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
ú2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision between tool and workpiece (clamping devices) can occur.
N80 G201 Q200=2 Q201=-20 Q206=150 Q211=0.25 Q208=500 Q203=+0 Q204=50*
BORING (Cycle G202)
Machine and control must be specially prepared by the machine tool builder to enable Cycle 202.
1The TNC positions the tool in the tool axis at rapid traverse to set-up clearance above the workpiece surface.
2The tool drills to the programmed depth at the feed rate for plunging.
3If programmed, the tool remains at the hole bottom for the entered dwell time with active spindle rotation for cutting free.
4The TNC then orients the spindle to the 0° position with an oriented spindle stop.
5If retraction is selected, the tool retracts in the programmed direction by 0.2 mm (fixed value).
6The TNC moves the tool at the retraction feed rate to the set-up clearance and then, if entered, to the 2nd set-up clearance at rapid traverse. If Q214=0 the tool point remains on the wall of the hole.
Before programming, note the following:
Program a positioning block for the starting point (hole center) in the working plane with RADIUS
COMPENSATION G40.
The algebraic sign for the cycle parameter TOTAL HOLE DEPTH determines the working direction.
After the cycle is completed, the TNC restores the coolant and spindle conditions that were active before the cycle call.
úSet-up clearance Q200 (incremental value): Distance between tool tip and workpiece surface.
úDepth Q201 (incremental value): Distance between workpiece surface and bottom of hole
úFeed rate for plunging Q206: Traversing speed of the tool during boring in mm/min
úDwell time at depth Q211: Time in seconds that the tool remains at the hole bottom
úRetraction feed rate Q208: Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the tool retracts at feed rate for plunging.
úWorkpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
ú2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision between tool and workpiece (clamping devices) can occur.