CNC Export

Generates the machining files for the panels in the model in SVG, DXF or G-code format: outer contour, cutouts, pockets, grooves, rabbets, drillings and engravings.

How it works

1. Optionally select the parts to machine, then launch the command from the CNC toolbar (or the Adwood menu)
2. Wait while the panels are prepared; a click in the view interrupts the processing in progress
3. In the window, check the list of panels to export and the grouping mode
4. Choose the export format (SVG, DXF or G-code) and set its options
5. Assign at least a tool for contour and cut-out; pockets and engraving are optional
6. Set the export folder if you do not want to write next to the SketchUp file
7. Click Export

A profile stores all of these settings and recalls them from one model to the next.

Profile bar

At the top of the window, it remembers a complete set of settings (format, options, tools, folder).

• Profile (list) — “New profile” as long as no profile is selected
• Load this profile (down arrow) — applies the selected profile to the whole window
• Save current profile (floppy disk) — asks for a name and saves the current settings; reusing an existing name overwrites it
• Delete this profile (trash) — deletes the selected profile, after confirmation
• Import from file / Export to file (on the right) — exchanges profiles as a .json file, to share them between workstations or workshops

“Panels to export” section

• Entire model / Selection (radio buttons) — only appears if a selection existed when the command was launched; each choice shows its panel count
• Counter — number of checked panels and total of the corresponding machinings
• Panel list — one checkbox per part, all checked by default. Beyond five parts the list is collapsed: click “… and N more” to unfold it
• Machining grouping (list):
  • Separate machinings — one file (or two, face and back) per part
  • Group facing machinings — all parts nested in a single file, face side
  • Group back machinings — same on the back side
• Nesting clearance (mm) — only visible in grouped mode. The actual spacing between parts equals the tool diameter plus this clearance (Ø8 mm tool + 0.2 mm clearance = 8.2 mm)

“Export format” section

Three buttons — SVG, DXF, G-code — only one of which is active at a time. The chosen format drives the display of the options below: whatever does not apply is hidden.

Two settings remain common to all three formats:

• Export circular arcs as arcs (recommended) — checked, arcs are output as true arcs (G2/G3 in G-code, A command in SVG); unchecked, they are output as line segments, exactly as in SketchUp
• Toolpath direction (machining) (collapsible block) — clockwise (CW) or counter-clockwise (CCW) for the outer contour, the inner contours, the pockets / rabbets / grooves and the cutouts. Default: CCW outside, CW everywhere else, which corresponds to climb milling

SVG

Format for checking and simple cutting: a to-scale vector drawing readable by any cutting or drawing software. A preview opens in the browser once the window is closed.

No specific option: only the common settings apply (panels, grouping, arcs, toolpath direction, tools, export folder).

DXF

Exchange format for wood CAM software (woodWOP, BiesseWorks, WoodStore, CADWork, WoodCAD|CAM…), which selects the tool from the layer name and colour.

• DXF version:
  • R2000 (AC1015) — recommended, colored layers, LWPOLYLINE; suits every modern CNC program
  • R14 (AC1014) — POLYLINE/VERTEX/SEQEND, for older machines or proprietary controllers
• Help by brand (link) — table of recommended versions depending on the software or machine
• Apply tool offset — checked, Adwood computes the tool-center path and the file already contains the radius offset; unchecked, the path follows the nominal contour of the part exactly

G-code (beta)

Complete machining program, directly executable by the machine. This is the most configurable format: the settings below only appear when it is selected.

Toolpaths and tool radius

• G-code arc format — R (radius, recommended) or I/J (center vector)
• Apply tool offset — offset computed by the software (works on any machine)
• Cutter compensation (G-code) — None (software offset), Left — G41 or Right — G42: the machine then applies the radius through its offset register (D). Mutually exclusive with the software offset on the outer contour: enabling G41/G42 disables it automatically, otherwise compensation would be applied twice

Advanced export

• Use drilling cycles G81/G83 — instead of expanded G0/G1 moves
• Generate one file per tool — for machines without an automatic tool changer
• Generate an operator summary (.txt) — summary sheet of tools and operations to hand to the workstation

Safety height and auxiliary outputs

• Z1 - Safety plane (mm) — height of rapid moves (G0) above the part between two operations
• Enable M7 (blow / mist) and Enable M8 (suction / coolant) — each with a customizable label and code, to match the actual wiring of the machine
• Auxiliary stop code — sent at the end of the program if M7 or M8 is active (M9 by default)
• Dry-run mode — program without M3 and without M7/M8, at reduced speeds; the speed factor (0.3 = 30%) sets the slowdown

Tool change

• Automatic tool magazine (ATC) — checked, the machine changes tools on its own with M6; unchecked, the program stops (M0) at every change for a manual operation
• Tool change format — T1 M6, M6 T1, T01 M06 or none
• Include tool name as comment — then choose the template: (Tool: Fraise_D8), (Fraise_D8) or ; Tool: Fraise_D8
• Tool length compensation — G43 H{n}, G43 H{n} Z{z1} or none
• H number identical to T number — otherwise enter an H offset
• Spindle / speed order — S18000 M3 or M3 S18000
• Delay after spindle start — none, G4 P1, G4 P2 or a custom command

5-axis machine

• Not a 5-axis machine — no command added (3-axis machines)
• B+C, A+C, A+B — inserts G0 B0 C0, G0 A0 C0 or G0 A0 B0 at the top of the program to bring the tool back to vertical
• Custom (free field) — your own line, for example M129 G0 B0 C0 to disable RTCP before the reset

G-code format

• Comment type — semicolon, parentheses, or no comments
• Clean special characters — strips accents and Unicode from the comments
• Decimal places — 2 (12.50) or 3 (12.500)
• Remove trailing zeros — writes 12.5 instead of 12.500
• Number the lines — with an increment of 1, 5 or 10
• Machine-safe filename — no accents or spaces

Header / End of program

• Full modal header — writes G90 G94 G17 G21 G40 G49 G80… at the beginning of the file
• Output units — millimeters (G21) or inches (G20)
• Work coordinate — none, G54, G55 or G56
• End of program code — M30 (recommended), M2 or custom
• Return height at end of program — safety height (G0 Z{Z1}), machine zero (G53 G0 Z0) or none
• XY return at end of program — none, part origin, parking position (X/Y to enter) or machine zero
• Insert an information block — descriptive header at the beginning of the file (part, tools, dimensions)

“CNC tools” section

• Manage CNC tools (button) — opens the tool manager, where the router bits, drill bits and engravers of your inventory are created and edited
• Tool for contour and cut-out — required: without it the Export button stays inactive
• Additional cutting depth (mm) — extra depth below the panel thickness to guarantee a clean through cut (0.2 mm by default)
• Machining strategy (G-code only):
  • Progressive depth-first (default) — thick panels, medium rigidity
  • Progressive linear — simultaneous depth and offset progression
  • Direct — a single full pass, for thin panels and rigid machines
• Max depth per pass (mm) (G-code, except the Direct strategy) — 3 mm per pass on a 19 mm panel gives 7 passes
• Tool for pockets and Tool for engraving — optional
• Eye (to the right of each list) — unfolds the tool data sheet: type, diameter, description, speed XY, speed Z, rotation

“Export folder” section

• Browse… — chooses the destination folder for the files
• Red cross — clears the choice and returns to the default behaviour: the files are written to the folder of the SketchUp file

Window footer

• Export — starts the generation. The button stays inactive as long as no contour tool is selected or no panel is checked
• Cancel — closes the window without writing anything

Keys

• Enter = start the export (if the Export button is active)
• Click in the view = interrupt the preparation of the panels before the window opens
• Esc = Cancel the operation

Tips

• Create one profile per machine: format, tools, tool change and auxiliary codes are then fixed once and for all, and the exported .json file can be shared with the workshop
• Select the parts in the model before launching the command: the “Selection” choice then appears in the window
• Export to SVG first to visually check the contours and drillings, then run the export again as G-code once the result is validated
• When in doubt about the DXF version, stay on R2000: every recent wood CAM program accepts it
• Never enable G41/G42 together with a software offset: the radius would be counted twice — the window handles this, but check the result on the machine
• Before a first program on an unknown machine, enable dry-run mode: the toolpath runs without spindle or suction, at reduced speed
• Grouped mode (nesting) only makes sense if all the checked parts share the same board and the same thickness