4.11 Programming Examples; Example: Thread Milling - HEIDENHAIN TNC 620 User Manual
Hide thumbs
Also See for TNC 620:
- User manual (840 pages) ,
- User manual (695 pages) ,
- User manual (488 pages)
Table of Contents
Advertisement
4
Fixed Cycles: Tapping / Thread Milling
4.11 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 Y+0
3 TOOL CALL 1 Z S5000
4 L Z+10 R0 F5000
5 SEL PATTERN "TAB1"
6 CYCL DEF 240 CENTERING
Q200=2
Q343=1
Q201=-3.5
Q344=-7
Q206=150
Q11=0
Q203=+0
Q204=0
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
Q201=-25
Q206=150
Q202=5
Q210=0
Q203=+0
132
;SET-UP CLEARANCE
;SELECT DIA./DEPTH
;DEPTH
;DIAMETER
;FEED RATE FOR PLNGNG
;DWELL TIME AT DEPTH
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;SET-UP CLEARANCE
;DEPTH
;FEED RATE FOR PLNGNG
;PLUNGING DEPTH
;DWELL TIME AT TOP
;SURFACE COORDINATE
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
0 must be entered here, effective as defined in point table
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015
Advertisement
Table of Contents
