GSK GSK980TDc, Manual

Page: 122 / 470

GSK980TDc Turning CNC System User Manual
104
Ⅰ
Progra
mming
value (radius value) of A1 point compared to Ad point. The X total cutting travel(radius
value) is equal to |
Δ i| in roughing, and X cutting direction is opposite to the sign of Δ i: Δ i
＞ 0, the system executes X negative cutting in roughing. It is reserved after Δ i specified
value is executed and the data is switched to the corresponding value to save to NO.053.
The No.053 value is regarded as X tool retraction clearance in roughing when U(
Δ i) is
not input.
Δ k: It is Z tool retraction clearance in roughing, and its range is ±99999999× least input
increment (radius, unit: mm/inch, with sign symbol) , Δ k is equal to Z coordinate offset
value (radius value) of A1 point compared to Ad point. Z total cutting travel(radius value)
is equal to |
Δ k| in roughing, and Z cutting direction is opposite to the sign of Δ k: Δ i
＞
0,
the system executes Z negative cutting in roughing. It is reserved after Δ k specified
value is executed and the data is switched to the corresponding value to save to NO.054.
The No.054 value is regarded as Z tool retraction clearance in roughing when W(
Δ k) is
not input.
d: It is the cutting times 1~9999 (unit: times). R5 means the closed cutting cycle is completed
by 5 times cutting. R (d) is reserved after it is executed and NO.055 value is rewritten to d
(unit: times). No.055 value is regarded as the cutting times when R(d) is not input. When
the cutting times is 1, the system completes the closed cutting cycle based on 2 times
cutting.
ns: Block number of the first block of finishing path.
nf: Block number of the last block of finishing path.
Δ u: It is X finishing allowance and its range is ±99999999× least input increment (diameter,
unit: mm/inch, with sign symbol) and is the X coordinate offset of roughing path
compared to finishing path, i.e. the different value of X absolute coordinates of A
1
compared to A. Δ u ＞ 0,it is the offset of the last X positive roughing path compared to
finishing path. The system defaults Δ u=0 when U( Δ u) is not input, i.e. there is no X
finishing allowance for roughing cycle.
Δ w: It is Z finishing allowance and its range is ±99999999× least input increment (diameter,
unit: mm/inch, with sign symbol) and is the X coordinate offset of roughing path
compared to finishing path, i.e. the different value of Z absolute coordinates of A
1
compared to A. Δ w
＞
0,it is the offset of the last X positive roughing path compared to
finishing path. The system defaults Δ w=0 when W( Δ w) is not input, i.e. there is no Z
finishing allowance for roughing cycle.
F: Feedrate; S: Spindle speed; T: Tool number, tool offset number.
M, S, T, F: They can be specified in the first G73 or the second ones or program ns
～
nf. M, S,
T, F functions of M, S, T, F blocks are invalid in G73, and they are valid in G70 finishing blocks.
Execution process: (Fig. 3-31)
① A → A
1
: Rapid traverse;
②
First roughing A
1
→ B
1
→ C
1
:
A
1
→ B
1
: Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in ns block
in G1;
B
1
→ C
1
: Cutting feed.
③
C
1
→ A
2
: Rapid traverse.
④
Second roughing A
2
→ B
2
→ C
2
:
A
2
→ B
2
: Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in ns block
in G1;