HEIDENHAIN TNC 360 User Manual - Manual (Page 153)

7-19 TNC 360
7 Programming with Q Parameters
Continued...
Workpiece blank; define and insert tool
Assign the sphere data to the parameters
7.8 Example for exercise
Three-dimensional machining (machining a hemisphere with an end mill)
Notes on the program:
• The tool moves upwards in the ZX plane.
• You can enter an oversize in block 12 (Q12)
if you want to machine the contour in
several steps.
• The tool radius is automatically compensated
with parameter Q108.
The program works with the following values:
• Solid angle: Start angle Q1
End angle Q2
Increment Q3
• Sphere radius Q4
• Setup clearance Q5
• Plane angle: Start angle Q6
End angle Q7
Increment Q8
• Center of sphere: X coordinate Q9
Y coordinate Q10
• Milling feed rate Q11
• Oversize Q12
The parameters additionally defined in the
program have the following meanings:
• Q15: Setup clearance above the sphere
• Q21: Solid angle during machining
• Q24: Distance from center of sphere
to center of tool
• Q26: Plane angle during machining
• Q108: TNC parameter with tool radius
Part program
0 BEGIN PGM 360712 MM
1 FN 0: Q1 = + 90
2 FN 0: Q2 = + 0
3 FN 0: Q3 = + 5
4 FN 0: Q4 = + 45
5 FN 0: Q5 = + 2
6 FN 0: Q6 = + 0
7 FN 0: Q7 = + 360
8 FN 0: Q8 = + 5
9 FN 0: Q9 = + 50
10 FN 0: Q10 = + 50
11 FN 0: Q11 = + 500
12 FN 0: Q12 = + 0
13 BLK FORM 0.1 Z X+0 Y+0 Z–50
14 BLK FORM 0.2 X+100 Y+100 Z+0
15 TOOL DEF 1 L+0 R+5
16 TOOL CALL 1 Z S1000
17 L Z+100 R0 FMAX M6
18 CALL LBL 10 ...................................................... Subprogram call
19 L Z+100 R0 FMAX M2 ....................................... Retract tool; jump to beginning of program