big overhaul

nc_files/OFFSETS.md

@@ -0,0 +1,137 @@
+# Offsets Quick Reference
+
+## Coordinate Stack
+
+```
+What you see = machine position + work offset (G54...) + G52/G92 + tool length offset (G43)
+```
+
+`G53` bypasses everything and moves in machine coords.
+
+## Work Offsets (G54–G59.3)
+
+9 available coordinate systems. G54 is default. Persist across power cycles (stored in `linuxcnc.var`).
+
+### Touching off work zero
+
+**In GMOCCAPY**: Jog to desired zero, click the axis letter (X/Y/Z) in the DRO, enter `0`. Done.
+Internally: `G10 L20 P0 <axis> 0`
+
+**Pendant**: Macro 5/6/7 = zero X/Y/Z. Macro 1/2 = halve X/Y (center-finding: zero one edge, jog to other edge, halve).
+
+**In G-code**:
+```gcode
+G10 L20 P1 X0 Y0 Z0    ; set G54 origin to current position
+G10 L20 P0 X0           ; set current system's X to 0
+```
+
+### Switching systems
+
+```gcode
+G55    ; all coords now relative to work offset 2
+```
+
+In GMOCCAPY: Offset page > click row > "Set Active".
+
+### Editing numerically
+
+In GMOCCAPY: Offset page > double-click a cell > type value. This uses `G10 L2` (absolute set), not touch-off.
+
+### Temporary offsets
+
+```gcode
+G52 X1 Y1    ; shift on top of active G5x (good for pattern repeats)
+G52 X0 Y0    ; cancel
+```
+
+Avoid `G92` — it persists across program runs and causes confusion. Use `G92.1` to clear if needed.
+
+## Tool Length
+
+### Setting up a tool (first time)
+
+1. In GMOCCAPY Tool page: set diameter (D column) and any known Z offset. Click "Apply Changes".
+2. Or in G-code: `G10 L1 P1 Z-2.5 R0.125` (R = **radius**, stored as D = diameter = 2R)
+
+### Loading a tool
+
+```gcode
+T1 M6    ; select + change (pops up dialog, operator confirms)
+G43      ; activate its Z offset — REQUIRED or Z is wrong
+```
+
+### Touching off tool length
+
+Jog tool tip down to top of workpiece, then in MDI:
+
+```gcode
+G10 L10 P1 Z0    ; "tip is at Z=0, calculate and store the offset"
+G43               ; activate it
+```
+
+Or: GMOCCAPY DRO > click Z letter > enter `0` (but this sets the **work offset**, not the tool offset — different thing).
+
+### Canceling
+
+```gcode
+G49    ; cancel tool length offset
+```
+
+Standard practice: `G49` before each tool change, `G43` after.
+
+## Cutter Radius Compensation (G41/G42)
+
+Offsets the toolpath left or right of the programmed line by the tool's radius. Program the actual part edge; the machine handles the rest.
+
+```gcode
+G41      ; offset LEFT of path (climb milling outside profiles)
+G42      ; offset RIGHT
+G40      ; cancel
+```
+
+The D word in G41/G42 is a **tool number** (not a diameter): `G41 D1` looks up tool 1's diameter from the table. Omit D to use the current tool.
+
+Rules:
+- Lead-in move after G41/G42 must be >= tool radius
+- Lead-out move with G40 must be >= tool radius
+- Must be in G17 (XY plane)
+
+```gcode
+G41                  ; comp on
+G1 X0 Y0 F10        ; lead-in (this IS the first compensated move)
+G1 X2 Y0            ; cut along part edge — tool rides 1 radius to the left
+G1 X2 Y2
+G40                  ; comp off (next linear move is lead-out)
+G0 X-1 Y-1
+```
+
+Dynamic variant: `G41.1 D0.250` — D is a literal diameter value, not a tool number.
+
+**Our macros** handle radius compensation internally via `#<_td>`. Don't use G41/G42 with macro calls.
+
+## Tool Table Columns (mill)
+
+| Column | Meaning |
+|--------|---------|
+| T | Tool number |
+| P | Pocket (we use P = T) |
+| Z | Length offset |
+| D | Diameter (not radius) |
+
+## DRO Modes (click axis value to cycle)
+
+| Mode | Color | Shows |
+|------|-------|-------|
+| Relative | Black | Work coords (what G-code sees) |
+| Absolute | Blue | Machine coords (G53) |
+| DTG | Yellow | Distance to go |
+
+Green digits = homed. Red = unhomed.
+
+## Named Parameters
+
+| Parameter | Value |
+|-----------|-------|
+| `#<_current_tool>` / `#5400` | Tool in spindle |
+| `#5410` | Current tool diameter |
+| `#<_td>` | Our macros' tool diameter (user-set, not built-in) |