User's Manual TNC 360 (from 259 900-11) - heidenhain

7 Programming with Q Parameters
7.1 Q Parameters Instead of Numerical Values
7-4
Example for exercise: Full circle
Circle center CC: X = 50 mm
Beginning and end
Y = 50 mm
of circular arc C: X = 50 mm
Y = 0 mm
Milling depth: Z = –5 mm
Tool radius: R = 15 mm
Part program without Q parameters
0 BEGIN 360074 MM ............................................ Start of program
1 BLK FORM 0.1 Z X+0 Y+0 Z–20 ........................ Blank form definition
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 6 L+0 R+15 ...................................... Tool definition
4 TOOL CALL 6 Z S500 ......................................... Tool call
5 CC X+50 Y+50 .................................................... Coordinates of circle center CC
6 L Z+100 R0 FMAX M6 ....................................... Insert tool
7 L X+30 Y–20 FMAX ............................................ Pre-position tool
8 L Z–5 FMAX M3
9 L X+50 Y+0 RR F100 .......................................... Move to first compensation point with radius compensation
10 C X+50 Y+0 DR+ ................................................ Mill circular arc C around circle center CC; coordinates of end
point: X = +50 mm and Y = 0; positive direction of rotation
11 L X+70 Y–20 R0 FMAX
12 L Z+100 FMAX M2
13 END PGM 360074 MM ...................................... Retract tool and end program
Part program with Q parameters
0 BEGIN PGM 3600741 MM
1 FN 0: Q1 = +100 ................................................ Clearance height
2 FN 0: Q2 = +30 .................................................. Start pos. X
3 FN 0: Q3 = –20 ................................................... Start-End pos. Y
4 FN 0: Q4 = +70 .................................................. End pos. X
5 FN 0: Q5 = –5 ..................................................... Milling depth
6 FN 0: Q6 = +50 .................................................. Center point X
7 FN 0: Q7 = +50 .................................................. Center point Y
8 FN 0: Q8 = +50 .................................................. Circle starting point X
9 FN 0: Q9 = +0 .................................................... Circle starting point Y
10 FN 0: Q10 = +0 .................................................. Tool length L
11 FN 0: Q11 = +15 ................................................ Tool radius R
12 FN 0: Q20 = +100 .............................................. Milling feed rate F
13 BLK FORM 0.1.Z X+0 Y+0 Z–20
14 BLK FORM 0.2 X+100 Y+100 Z+0
15 TOOL DEF 1 L+Q10 R+Q11
16 TOOL CALL 1 Z S500
17 CC X+Q6 Y+Q7
18 L Z+Q1 R0 FMAX M6
19 L X+Q2 Y+Q3 F MAX
20 L Z+Q5 F MAX M3
21 L X+Q8 Y+Q9 RR FQ20
22 C X+Q8 Y+Q9 DR+
23 L X+Q4 Y+Q3 R0 FMAX
24 L Z+Q1 FMAX M2
25 END PGM 3600741 MM
Y
50
–5
Z
CC
50
Blocks 1 to 12:
Assign numerical values to the Q
parameters
Blocks 13 to 24:
Corresponding to blocks 1 to 12
from program 360074
X
TNC 360