4.11 Programming Examples; Example: Thread Milling - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Tapping / Thread Milling | Programming Examples

4.11 Programming Examples

Example: Thread milling

The drill hole coordinates are stored in the point table
TAB1.PNT and are called by the TNC with CYCL CALL
PAT.
The tool radii are selected so that all work steps can be
seen in the test graphics.
Program sequence
Centering
Drilling
Tapping
0 BEGIN PGM 1 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S5000
4 L Z+10 R0 F5000
5 SEL PATTERN "TAB1"
6 CYCL DEF 240 CENTERING
Q200=2 ;SET-UP CLEARANCE
Q343=1 ;SELECT DIA./DEPTH
Q201=-3.5 ;DEPTH
Q344=-7 ;DIAMETER
Q206=150 ;FEED RATE FOR PLNGNG
Q11=0 ;DWELL TIME AT DEPTH
Q203=+0 ;SURFACE COORDINATE
Q204=0 ;2ND SET-UP CLEARANCE
10 CYCL CALL PAT F5000 M3
11 L Z+100 R0 FMAX M6
12 TOOL CALL 2 Z S5000
13 L Z+10 R0 F5000
14 CYCL DEF 200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Q201=-25 ;DEPTH
Q206=150 ;FEED RATE FOR PLNGNG
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
HEIDENHAIN | User's manual for cycle programming | 10/2017
Definition of workpiece blank
Call tool: centering drill
Move tool to clearance height (enter a value for F): the TNC
positions to the clearance height after every cycle
Definition of point table
Cycle definition: CENTERING
0 must be entered here, effective as defined in point table
0 must be entered here, effective as defined in point table
Cycle call in connection with point table TAB1.PNT, feed rate
between the points: 5000 mm/min
Retract the tool, change the tool
Call tool: drill
Move tool to clearance height (enter a value for F)
Cycle definition: drilling
4
155