CNC programming and alarms
Fadal G-code list (CNC 88 and 88HS vertical machining center controls)
G-codes for Fadal VMCs running the CNC 88 or 88HS control; confirm against your machine's programming manual and format setting.
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
| G-code | Group or modal | Function | Notes |
|---|---|---|---|
| G0 | Motion, modal | Rapid positioning | Moves at the rapid rate. Not a cutting move. |
| G1 | Motion, modal | Linear interpolation | Straight-line move at feed rate F. |
| G2 | Motion, modal | Circular interpolation, clockwise | Direction is viewed from the positive side of the axis normal to the active plane. |
| G3 | Motion, modal | Circular interpolation, counterclockwise | Direction is viewed from the positive side of the axis normal to the active plane. |
| G4 | Non-modal | Dwell | Pauses for the programmed time, in that block only. |
| G17 | Plane, modal | XY plane selection | Sets the plane for arcs and cutter compensation. |
| G18 | Plane, modal | XZ plane selection | Sets the plane for arcs and cutter compensation. |
| G19 | Plane, modal | YZ plane selection | Sets the plane for arcs and cutter compensation. |
| G28 | Non-modal | Return to machine home (reference) | Goes through an intermediate point on the way home. |
| G40 | Cutter compensation, modal | Cutter compensation cancel | Cancel on a move clear of the part. |
| G41 | Cutter compensation, modal | Cutter compensation left | Tool on the left of the path, looking in the direction of travel. |
| G42 | Cutter compensation, modal | Cutter compensation right | Tool on the right of the path, looking in the direction of travel. |
| G43 | Tool length compensation, modal | Tool length compensation | The H word selects the length offset. |
| G49 | Tool length compensation, modal | Tool length compensation cancel | Cancels G43. |
| G53 | Non-modal | Machine coordinate positioning | Positions in machine coordinates for that block only. |
| G73 | Canned cycle, modal | High-speed peck drilling | Chip-breaking pecks. Check the manual for the retract amount. |
| G74 | Canned cycle, modal | Left-hand tapping | For left-hand taps. Feed = RPM / TPI. |
| G80 | Canned cycle, modal | Canned cycle cancel | Ends G73 to G85. |
| G81 | Canned cycle, modal | Drilling | Feed to depth, rapid out. |
| G82 | Canned cycle, modal | Spot drill or counterbore with dwell | Dwells at the bottom of the hole. |
| G83 | Canned cycle, modal | Deep-hole peck drilling | Q sets the peck depth. |
| G84 | Canned cycle, modal | Right-hand tapping | Feed = RPM / TPI in inches per minute mode. |
| G85 | Canned cycle, modal | Boring, feed in and feed out | Feeds in and feeds back out at the feed rate. |
| G90 | Distance mode, modal | Absolute positioning | Positions read from the work zero. |
| G91 | Distance mode, modal | Incremental positioning | Positions read from the current location. |
| G98 | Canned cycle return, modal | Return to the initial plane | Clears clamps between holes. |
| G99 | Canned cycle return, modal | Return to the R plane | Shorter moves between holes on open work. |
Modal codes stay active until another code in the same group replaces them. Non-modal codes act in their own block only. Functions are paraphrased; the programming manual is the reference.
Source: Fadal CNC 88/88HS programming manual (cited by control series, not reproduced)
Format 1 and format 2 change how some codes read; check the control's setting before running a program from another machine.
How to read the table
Codes are grouped the way the control treats them: motion, plane, compensation, canned cycles and modes. One code from each group is active at a time. The same G-code can mean different things on different controls: G92 is a threading cycle on a Fanuc lathe but sets the coordinate system on many mills. Read every code with the control named.
Tapping feed for G84 and G74
IPM = RPM / TPI
| Symbol | Meaning | Unit |
|---|---|---|
| IPM | Feed rate, inches per minute | in/min |
| RPM | Spindle speed | rev/min |
| TPI | Threads per inch of the tap | 1/in |
Source: Machinery's Handbook (tapping feed equals pitch per revolution)
Worked example: G84 feed for 1/4-20
Tapping a 1/4-20 hole with G84 at 500 RPM on a Fadal VMC, feed in inches per minute.
- Pitch: 1 / 20 = 0.0500 in per revolution.
- Feed: IPM = RPM / TPI = 500 / 20 = 25.0 IPM.
- Check: 500 RPM x 0.0500 in per revolution = 25.0 IPM.
Result: F25.0 with S500 for 1/4-20. A starting point; check the tap maker's speed for the material.
Shop notes
- Functions are paraphrased. The Fadal CNC 88/88HS programming manual is the reference for block format and word addresses.
- This list does not cover inch and metric selection, fixture offsets, G92 or the Fadal pocket and frame cycles. Take those from the manual for your control.
- Before running a program written for a Fanuc-style mill, check the format setting and every canned cycle block.
- G98 and G99 decide where the tool goes between holes. On work with clamps, G98 keeps the tool at the initial plane.
FAQ
What is G83 on a Fadal?
Deep-hole peck drilling on the Fadal CNC 88 and 88HS VMC controls. Q sets the peck depth. The peck drilling calculator gives Q for your drill.
Does G84 on a Fadal need a tapping feed?
Yes. Feed = RPM / TPI in inches per minute mode: 500 RPM on 1/4-20 is 500 / 20 = 25.0 IPM.
What cancels a canned cycle on a Fadal?
G80. It ends any active canned cycle, G73 to G85 in this list.
Is G92 the same on a Fadal and a Fanuc lathe?
No. On a Fanuc lathe with G-code system A, G92 is a threading cycle; on many mills G92 sets the coordinate system. Check the Fadal programming manual for how G92 reads on your control, and always read a G-code with the control named.
Last updated