Yaskawa YASNAC PC NC Programming Manual - Manual (Page 222)

4 - 85
YASNAC PCNC Programming Manual Chapter 4: Enhanced Level Commands
Therefore, if the parameters are not set correctly, operation is not performed as pro-
grammed. If axis move commands are specified for the axis not set for parameters,
they are disregarded. This does not cause an alarm.
• G41, G42, and G40 should be specified in the area enclosed by “HON” and “HOF”
codes. If the high-speed cutting mode is started with G41, G42, or G40 specified
before such area, alarm 0189, “OFS ABNORMAL ERROR” (tool radius offset error)
or alarm0181, “RADIUS OFS END ERROR” (tool radius offset end error) occurs.
• For the G41, G42, or G40 program specified in the high-speed cutting mode, only the
following G codes can be specified.
G00, G01, G02, G03, G90, and G91
If G codes other than these G codes are specified, alarm “0)181” occurs. The follow-
ing G codes can be specified in high-speed cutting: G01, G02, G03, G41, G42, G90
andG91. In addition to these G codes, G00 specified in the tool radius offset mode is
treated as G01 to execute high-speed cutting.
Axis move commands specified with a G code other than those indicated above are not
converted into segment data and thus they are processed in normal mode. Note that
designation of G20, G21, G25, G50, G51, G50R, G66, G67, G68 and G69 causes
alarm “0163”.
• When the setting for a parameter is made so that “the tool radius offset C cancel is
made”, alarm “0189” occurs if the HOF code is specified immediately after the desig-
nation of G40. Therefore, to specify G40 in the high speed cutting mode, either insert
a G01 mode block between the G40 and HOF blocks or enter an axis move command
in the G40 block.
4.2.6 Chamfering and Corner Rounding Commands *
For the continuous linear interpolation blocks or circular interpolation blocks, chamfering or cor-
ner rounding are executed by specifying “P” or “Q” command. If P and “Q” are specified in the
same block, chamfering is executed.
(1) Programming Format
Both P and Q commands are non-modal commands and should be specified with an absolute
value. If a minus sign is used, processing is executed based on the absolute value of the spec-
ified value.
If chamfering or corner rounding command is specified n the incremental mode (G91), the
programmed commands are treated as if the chamfering or corner rounding commands were
not specified.