HEIDENHAIN TNC 620 Programming Station, Руководство пользователя

Страница: 552 / 695

Positioning with Manual Data Input
15.1 Programming and executing simple machining operations
15
552
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
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 with
a few lines of programming.
First you pre-position the tool above the workpiece with straight-
line blocks and position with a safety clearance of 5 mm above the
hole. Then drill the hole with Cycle
G200
.
%$MDI G71 *
N10 T1 G17 S2000*
Call the tool: tool axis Z,
spindle speed 2000 rpm
N20 G00 G40 G90 Z+200*
Retract the tool (rapid traverse)
N30 X+50 Y+50 M3*
Move the tool at rapid traverse to a position above the hole.
Spindle on.
N40 G01 Z+2 F2000*
Position the tool to 2 mm above the hole
N50 G200 DRILLING
Define Cycle G200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Set-up clearance of the tool above the hole
Q201=-20 ;DEPTH
Hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGNG
Feed rate for drilling
Q202=10 ;PLUNGING DEPTH
Depth of each infeed before retraction
Q210=0 ;DWELL TIME AT TOP
Dwell time at top for chip release (in seconds)
Q203=+0 ;SURFACE COORDINATE
Workpiece surface coordinate
Q204=50 ;2ND SET-UP CLEARANCE
Position after the cycle, with respect to Q203
Q211=0.5 ;DWELL TIME AT DEPTH
Dwell time in seconds at the hole bottom
Q395=0 ;DEPTH REFERENCE
Depth referenced to the tool tip or the cylindrical part of the
tool
N60 G79*
Call Cycle G200 PECKING
N70 G00 G40 Z+200 M2*
Retract the tool
N9999999 %$MDI G71 *
End of program
Straight-line function:
Further Information: "Straight line in rapid traverse G00 or straight
line with feed rate F G01", page 253