HEIDENHAIN ITNC 530 - CONVERSATIONAL PROGRAMMING User Manual

HEIDENHAIN iTNC 530 581
15.1 Programming and Executing Simple Machining Operations
Example 1
A hole with a depth of 20 mm is to be drilled into a single workpiece.
After clamping and aligning the workpiece and setting the datum, you
can program and execute the drilling operation in a few lines.
First you pre-position the tool with straight-line blocks to the hole
center coordinates at a setup clearance of 5 mm above the workpiece
surface. Then drill the hole with Cycle 200 DRILLING.
Straight-line function: See “Straight line L” on page 218, DRILLING
cycle: See User’s Manual, Cycles, Cycle 200 DRILLING.
Y
X
Z
50
50
0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S2000 Call tool: tool axis Z
Spindle speed 2000 rpm
2 L Z+200 R0 FMAX Retract tool (FMAX = rapid traverse)
3 L X+50 Y+50 R0 FMAX M3 Move the tool at FMAX to a position above the hole,
spindle on
4 CYCL DEF 200 DRILLING Define DRILLING cycle
Q200=5 ;SETUP CLEARANCE Setup clearance of the tool above the hole
Q201=-15 ;DEPTH Total hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGN Feed rate for drilling
Q202=5 ;PLUNGING DEPTH Depth of each infeed before retraction
Q210=0 ;DWELL TIME AT TOP Dwell time after every retraction in seconds
Q203=-10 ;SURFACE COORDINATE Coordinate of the workpiece surface
Q204=20 ;2ND SETUP CLEARANCE Setup clearance of the tool above the hole
Q211=0.2 ;DWELL TIME AT DEPTH Dwell time in seconds at the hole bottom
5 CYCL CALL Call DRILLING cycle
6 L Z+200 R0 FMAX M2 Retract the tool
7 END PGM $MDI MM End of program

HEIDENHAIN ITNC 530 - CONVERSATIONAL PROGRAMMING Specifications

General

Brand	HEIDENHAIN
Model	ITNC 530 - CONVERSATIONAL PROGRAMMING
Category	Control Unit
Language	English