1. F: Set Feed Rate
Fx - set the feed rate to x. x is usually in machine units (inches or millimeters) per minute.
2. S: Set Spindle Speed
Sx - set the speed of the spindle to x revolutions per minute (RPM).
The spindle will turn at that speed when a M3 or M4 is in effect. It is OK to program an S word whether the spindle is turning or not. If the speed override switch is enabled and not set at 100%, the speed will be different from what is programmed. It is OK to program S0, the spindle will not turn if that is done.
It is an error if:
the S number is negative.
As described in the G84 Section, if a G84 (tapping) canned cycle is active and the feed and speed override switches are enabled, the one set at the lower setting will take effect. The speed and feed rates will still be synchronized. In this case, the speed may differ from what is programmed, even if the speed override switch is set at 100%.
3. T: Select Tool
Tx - prepare to change to tool x.
The tool is not changed until an M6 is programmed (see Section M6). The T word may appear on the same line as the M6 or on a previous line. It is OK if T words appear on two or more lines with no tool change. Only the the most recent T word will take effect at the next tool change.
|When LinuxCNC is configured for a nonrandom toolchanger (see the entry for RANDOM_TOOLCHANGER in the EMCIO Section), T0 gets special handling: no tool will be selected. This is useful if you want the spindle to be empty after a tool change.|
|T0 When LinuxCNC is configured for a random toolchanger (see the entry for RANDOM_TOOLCHANGER in the EMCIO Section), T0 does not get any special treatment: T0 is a valid tool like any other. It is customary to use T0 on a random toolchanger machine to track an empty pocket, so that it behaves like a nonrandom toolchanger machine and unloads the spindle.|
It is an error if:
a negative T number is used,
T number is used that does not appear in the tool table file (with the exception that T0 on nonrandom toolchangers is accepted, as noted above).
On some machines, the carousel will move when a T word is programmed, at the same time machining is occurring. On such machines, programming the T word several lines before a tool change will save time. A common programming practice for such machines is to put the T word for the next tool to be used on the line after a tool change. This maximizes the time available for the carousel to move.
Rapid moves after a T<n> will not show on the AXIS preview until after a feed move. This is for machines that travel long distances to change the tool like a lathe. This can be very confusing at first. To turn this feature off for the current tool program a G1 without any move after the T<n>.