Output and the first cut

Exporting G-code

1. Check the status bar. The machine named there is the one the file will be written for.
2. Recalculate anything marked ⚠ recalc in the Toolpaths list.
3. Choose Manufacture ▸ Output ▸ Export G-code… for every toolpath, or Export Selected… for just the one selected in the list. Both are also in the toolbar's Export menu and in the Toolpaths menu.
4. The Export G-code window opens with the program in a preview pane.
5. Press Save G-code… and choose where to save it. In a project, the window starts in the project's G-code folder.

On the trial, step 3 stops with a message instead. Everything up to it works.

The export window

Controller

The post-processor the file is written with. It starts on the active machine's post. Changing it here affects this export only.

Units

Controller default uses the post's units. Millimetres or Inches overrides them for this file.

Preview

The program as it will be saved. Scroll through it to check the header, the first tool change and the first moves.

Files

One file writes the whole job as one program. One file per bit writes a program for each bit, in the order they cut: toolpaths that follow each other with the same bit share a file. One file per toolpath writes each operation as its own program. Files are named by their place in the sequence and their name, and the button reads Save files… and asks for a folder.

The file extension comes from the post.

Tools and tool changes

Tools are numbered in the order the program first uses them: the first bit is T1, the next different bit T2, and so on. Where the job changes bit, the post writes its tool-change block.

Whether the machine can act on that depends on the machine. One with an automatic tool changer swaps the bit itself. Without one, not every controller stops and waits, and none can set Z zero for the new bit. So when the active machine has no tool changer (Automatic tool changer in its settings) and the toolpaths use more than one bit, the export window starts on One file per bit. If you choose One file anyway, you are asked to confirm. A V-carve inlay with a clearing bit is the usual case: the pocket board needs two files, clearing and then V-carve, and so does the plug's.

Run the files in order. Before each one, fit its bit and set Z zero again.

Export writes the boards the Toolpaths list is showing. On This sheet that is the board in front of you. On All sheets, or with several boards Selected, every one of them is exported, and each board's files go in a folder named after the board. Each file is named for what it cuts and the bit it needs, for example 01_V-Inlay-Plug-clearing-1-4-Flat-End-Mill.

Manufacture ▸ Operations ▸ Merge Toolpaths reorders a job so that operations sharing a bit run together, which means fewer changes and fewer files.

The machine envelope check

Before writing, every move is checked against the active machine's travel. If anything is outside it you see Outside machine envelope, with each axis that overruns and by how much, and the choice to export anyway. Say no unless you know the machine setup in Carvect Pro is wrong. The check is only as good as the travel entered for the machine.

Exporting a double-sided job

A double-sided job is cut in two setups, so each face is exported as its own program. Export asks which to write: Side 1, Side 2 or Both. Side 2 is mirrored for the flip automatically, about the axis you chose in Job Setup, so you draw it as it will look and the program places it correctly after the board is turned over.

The same box reminds you how to zero Z. With Zero off same side on, keep the Side 1 zero and do not re-zero after the flip; Side 2 is offset by the stock thickness. With it off, zero on each side's own surface.

Run Side 1, turn the board over about the chosen axis, clamp it with the same datum corner in the same place, and run Side 2.

Running a new job

A new job, a new machine or a new post deserves a dry run.

1. Load the file on the machine's control.
2. Zero X and Y at the job's datum: the corner (or centre) you chose in Job Setup, plus any offset.
3. Set Z about 20 mm above where it should be, and run the program in the air. Watch that it traces the shapes you expect, in the right place, at sensible speeds.
4. Stop, re-zero Z on the surface you chose (the top of the material, or the bed), and run it for real.

Keep the job sheet beside the machine. It lists each operation and its tool in order, which is what you need when the program stops for a tool change.

Other files you can write

File ▸ Save As… also writes .svg and .dxf, for sending the vectors on the active sheet to another program. The Photo button in the simulation saves a picture of the carving, and the job sheet saves as an HTML page.