138 lines
3.7 KiB
Markdown
138 lines
3.7 KiB
Markdown
# 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) |
|