Fanuc Post-Processor

The figure shows the eight properties, below the common properties, on the Postprocessor tab of the Machine Editor.

The next figure shows the two Job-scope properties in the Postprocessor Properties group of the Post-Processing Dialog.

The fanuc Post changes the defaults of these common properties. Each other common property has the default that Machine gives.

The fanuc Post also changes the help text of Pre-Rotary Move, Post-Rotary Move and Tilted work plane: align. Work Planes describes the values for a Fanuc control.

Each section of the output starts with the % line when Tape Marks (%) is checked. The O line follows when Program Number is more than 0. These two lines come before the header.

When comments are enabled, the O line also has the Job label as a comment. The Post removes each parenthesis from the label. With Program Number set to 12 and a Job with the label "Bracket", the output starts with these lines:

When Park Empty Spindle at End is checked, the Post writes the park block before the postamble. With the default Empty-Spindle Retract, the park block is:

The last % line follows the postamble.

The fanuc Post writes each drill cycle and each tapping cycle as a native canned cycle. Each block of a sequence of holes has the cycle word and all its parameters. A control that is set to non-modal cycles thus gets a complete block for each hole.

When Rigid Tapping (M29) is checked, the Post writes M29 S<rpm> as a separate block before each G84 or G74 block. The S value is the S word of the tapping cycle. When the cycle has no S word, the S value is the last spindle speed that an M3 or M4 command gave. The G84 or G74 block does not have an S word. The Post writes G80 after a sequence of tapping blocks.

The F word of a tapping cycle is the thread pitch multiplied by the spindle speed. This applies when Rigid Tapping (M29) is checked and when it is unchecked.

The export stops with an error when Rigid Tapping (M29) is checked and no spindle speed is available for a tapping cycle. The message names the Operation and the cycle command.

The Sanity Check of the fanuc Post gives a WARNING Squawk for the same condition. The Squawk applies to an active Operation that taps with no S word, when its Tool Controller also has a Spindle Speed of 0. The Sanity Check does not do this check when Rigid Tapping (M29) is unchecked.

When Dwell in Milliseconds is checked, a dwell of 1.5 seconds is G4 P1500. A dwell of 0.5 seconds in a G82 cycle is P500.

After a tool change, the fanuc Post writes G43 H<n>, where <n> is the number of the Tool Bit. When Parametric Tool Length Offset is checked, the Post writes these two lines as an alternative:

The system variable #4120 is the active T code. The control gets the length of Tool Bit number n from the variable #[2000+n].

The fanuc Post does not change the default of Generated Parameter Order for GCode. The common order XYZABCUVWFSIJKTQRPDHL has the K word.

The fanuc Post follows the arc plane (G17, G18, G19) of each arc. An arc has the two center words of its arc plane and no center word along the plane normal. A G17 arc has no K word. A G18 arc keeps the K word and has no J word. A G19 arc keeps the K word and has no I word. Postprocessor Customization gives the arc plane rule.

After a G18 command, an arc command with the center words I5, J0 and K-5 gives this line:

A helical arc gives its pitch through the axis word along the plane normal. In the G17 arc plane, that word is the Z word.

The fanuc Post can emit the dwo and twp values of the Machine’s Rotation Strategy. Machine lists the conditions for an Operation on a tilted Work Plane.

These common properties have values that are specific to a Fanuc control:

A Work Plane can name a Fixture. A Fixture is a G54 to G59.9 selection, not the workholding. The fanuc Post also accepts G54.1 and writes its P word as an integer offset number.