HEIDENHAIN ITNC 530 User Manual page 86

3.1 Programming and Executing
Simple Machining Operations
The Positioning with Manual Data Input mode of operation is
particularly convenient for simple machining operations or pre-
positioning of the tool. It enables you to write a short program in
HEIDENHAIN conversational programming or in ISO format, and
execute it immediately. You can also call TNC cycles. The program is
stored in the file $MDI. In the Positioning with MDI operating mode,
the additional status displays can also be activated.
Positioning with Manual Data Input (MDI)
Select the Positioning with MDI mode of operation.
Program the file $MDI as you wish.
To start program run, press the machine START key.
Limitation
FK free contour programming, programming graphics and
program run graphics cannot be used. The $MDI file must
not contain a program call (PGM CALL).
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 in L blocks (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 1 PECKING.
0 BEGIN PGM $MDI MM
1 TOOL DEF 1 L+0 R+5
2 TOOL CALL 1 Z S2000
3 L Z+200 R0 FMAX
4 L X+50 Y+50 R0 FMAX M3
5 CYCL DEF 200 DRILLING
Q200=5 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
86
Z
Y
50
Define tool: zero tool, radius 5
Call tool: tool axis Z
spindle speed 2000 rpm
Retract tool (F MAX = rapid traverse)
Move the tool at F MAX to a position above the
hole,
spindle on
Define DRILLING cycle
Set-up clearance of the tool above the hole
Total hole depth (Algebraic sign=working direction)
3 Positioning with Manual Data Input (MDI)
X
50