2.8.20 PROGRAMMING OF ABSOLUTE ZERO POINT
(G 50) (Cent’d )
(3) Assume that the tool No. 01 is reference
tool, and perform the setting of the follow-
ing coordinate system for this tool:
G50 X80. z62. ;
then , select the tool No. 02 which has the
tool position compensation value shown in
the figure below and peroform the compen-
sation operation,
and the tool No. 02 moves
to point A.
N3 G50 x80. z62. ;
N4 GOO TO1O1 ;
N1O GOO T0202 ;
TOOL NO 02
‘H+
G50COMMAND
POSITION AT
=
40mm
TOOI NO 01
~;
+------+z
Fig. 2,36
If the coordinate system setting is performed
with
the reference tool and tool position com–
pensation is applied to the other tool as
shown above, the tool movement may be
programmed on a single coordinate system
for alltool noses.
Notes :
1.
2.
3.
62
When T , S and M commands are programmed
in
the block following that containing G50,
GOO should
be programmed in the block.
This designates
the traverse rate for tool
offset motion.
G50 X.. . Z.. . ;
GOO S500 M03 TO1O1 ;
G 50 is
a nonmodal G code which is valid only
in
the specified block.
Generally,
the other
G
codes, and M, S, and T codes cannot be
specified in the same block. Note that
G50 S.. .
;or G50
T.. .
;
command is a
separate feature and is not for coordinate
system setting.
G 50 should
be commanded after the tool off-
set and tool radius compensation are cancelled
4.
When
the power supply is turned on, the pre-
sent
position of tool is set to the coordinate
(o, o).
Therefore, the absolute coordinate
system should be set up before operation.
5. The current position of the tool in G 50 coor–
dinate system is shown in “POSITION
ABSOLUTE” of current position display.
6,
The coordinate system which was set is not
affected by reset operation. The cmrdinate
system is reset by one of the following oper-
ations:
(i)
(ii)
(iii)
The reset operation by ORG key (see
4.3.4.2,
POSITION ABSOLUTE) is per-
formed.
G50 XO ZO
; command is written in MDI
mode and
is executed.
The power
is turned on again.
7. When setting work coordinate system by G50,
parameter #6o 18
D7 can select whether Work
Coordinate
System Shift in 2.6.5 will be ef-
fective or not.
2.8.21 MAXIMUM SPINDLE-SPEED SETTING (G 50)t
This function is used for the control provided
with S 4–digit designation option.
(1) G50 S.. . ;
Four digits following
the address S
specifies
the upper limit of spindle speed
in rpm. If an S command exceeding the
limit is issued in subsequent blocks, the
spindle speed is governed at the upper limit,
(2)
In G 96 (Constant Surface Speed Control)
mode, when spindle speed rises up too fast
as the current X-coordinate of the tool is
too small, the spindle speed is clipped
the limit.
EXAMPLE
G50 S2000 ;
The maximum spindle speed is clipped at
2000 r/rein.
Notes :
1.
Maximum spindle speed specified by G50 can
be displayed on the CRT display. Refer to
4.3.2.1,“Command Data Display.”
2. The specified maximum spindle speed is not
cleared by reset operation.
3. In case of S 4-digit designation B , unit of
address S is not shown by rpm.
Refer to
machine tool builder’s manual.
For S 2-digit
designation,
this function cannot be used.
To Next Page
Loading...
