8 Basic CNC Programming
8.4 NC Codes
100
In the EIA-274 mode, arc centers are based on the selected coordinate mode: absolute (G90) or
incremental (G91). In contrast, arc center specifications in Fanuc mode (specified by the % code) are
always incremental, regardless of whether the system is set to absolute or incremental coordinate
mode.
The $ character must stand alone on the first line of the NC program in which it appears.
The default arc center mode is defined in the Run Settings window, accessed by clicking Setup | Run
Settings, in the Main Menu.
8.4.3.
\ Code: Skip
The Skip code causes the program line to be skipped when the program is run.
Place the code at the beginning of the line you wish to skip. When you run the NC program, the specified
line will be skipped.
You can also use the Skip code (\) with a parameter to instruct the control software to execute the line
of code every nth pass. Place the code at the beginning of the line you wish to skip. The syntax is: \n,
where n is the number of passes between executions.
For example, if you want to execute a block of code every 5 passes, place \5 as the first code at the
beginning of the block.
8.4.4.
/ Code: Optional Skip
The Optional Skip codes allow you to skip particular lines of code in your program.
Lines marked with the optional skip (/) code are skipped only when the Optional Skip parameter from
the Run Settings window is checked (see
5.6.2 Modifying Run Settings, pg. 67).
To use the Optional Skip code (/), place the code at the beginning of the line you wish to skip. Select the
Optional Skip option from the Run Settings window or the Operator Panel.
You can use the optional skip code with a parameter to instruct the control software to execute the line
of code every nth pass. Place the code at the beginning of the line you wish to optionally skip. The
syntax is: /n, where n is the number of passes between executions.
For example, if you want to execute a block of code every 5 passes, place /5 as the first code at the
beginning of the block.
8.4.5.
F Code: Feed Rate
The F Code is used to specify the velocity at which the tool moves (the feed rate). The feed rate is
specified in inches or millimeters per minute, depending on the selected unit of measure. For example,
F3 specifies a feed rate of 3 inch/min when using inch units or 3 mm/min when using metric units.
The feed rate should be set to a low value (up to 10 inch/min) for cutting operations. The feed rate
chosen depends on the combination of tool size, cut depth, and material type.
The control software limits the programmed feed rate so that it doesn’t exceed the maximum allowed
by the milling center.
The F Code is also used to specify the number of seconds to dwell when used with the G04 code. For
example, G04F5 causes the machine to dwell for five seconds. See
