Cut list, nesting and export

Cut list

In a room, open Cut list & Export. Each cabinet is listed with its number, size, type and face (e.g. #3 Sink base — 33 × 34.5 × 24 in · base · 2-door).

Click Parts to expand the cabinet. Every part is drawn with its machining:

Click a part to enlarge it and see its operations.

Each cabinet also has its own DXF ↓ link, useful for a one-off.

Nesting

Nesting lays every part out on your sheets. It's on the project's Nesting tab (whole project) and on each room's Nesting tab (starts with just that room ticked).

1. Rooms to nest: tick the rooms to include.
2. Materials to nest: tick the materials. Each material nests separately.
3. Between parts: the gap between parts. Make it at least your cutter diameter plus a margin.
4. Sheet edge margin: how much of the sheet edge to keep clear.
5. The preview updates as you change these. The gaps are saved for the project when you click out of the box.

Your ticked rooms and materials, and which materials are collapsed, are remembered for each project in this browser, so they're still there when you come back.

Each material shows its sheet count and % yield (how much of the sheet ends up as parts).

• Click a sheet (⤢ open) to see it full size.
• Numbers on the parts match the table underneath: number → room → part → qty → size.
• Click a piece or a row to see its machining.

"Parts won't fit this sheet"

If a part is bigger than the sheet allows at your gaps, you'll see a red warning listing the parts and the largest size that fits. Export is blocked until every part fits, so you never get a short file. To fix it:

• reduce the part or edge gap
• use larger sheet stock (set in Materials)
• split the part, e.g. make a tall end panel two pieces

Export

Each material has a DXF ↓ link, with one file per material covering all its sheets. Each sheet also has its own DXF and G-code downloads.

DXF

Labelled DXF of every nested sheet, for Vectric VCarve/Aspire or any CAM that reads DXF. You set the toolpaths in your CAM. The file is always drawn in inches, whatever units you design in, so set your CAM job to inches when you import it.

Each kind of cut is on its own layer, so you can make one toolpath per layer:

Layers only appear when they're used. A sheet of doors has no POCKET layer, for example.

Each label is the fullest name that fits inside its part, e.g. Kitchen #2 Base 3 drawer - D1 Left side, shortening to #2 D1 Left side on a narrow part. D1 means drawer 1.

G-code

For Mach4 controllers, including Avid CNC machines. It isn't written for other controllers; on those, export DXF and toolpath it in your CAM. G-code needs a subscription or the trial.

On the Nesting tab, click Save… on the sheet you're about to cut. Each sheet is saved as one file per bit: every cut on the same bit goes in one file, and the cutout is always its own file, last (or as one file with tool changes, for a machine with a tool changer). Zero Z on the top of the material.

Check every file before you run it, and test on scrap the first time, especially tool numbers, feeds, speeds and depths.

Vortex 9282 dovetail drawers add three steps. They run in this order; the rough pockets are on your dado bit, so they go in the same file as your dados and notches:

The rough pockets are cleared like a dado, with the edge of the bit kept on the pocket's walls, so any size of straight bit cuts the same pocket. On the sides the bit runs off the end of the board. On the front and back the strip is the clear space the 9282 bit drops into before it moves into the board, since a dovetail bit can't plunge into solid wood. The nest leaves that strip free of other parts. Your dado bit must be 0.5″ or smaller to fit it; the Save G-code list warns you if it isn't.

On a dovetailed box the front and back run the full width of the box, out to the outside faces of the sides, since the whole side thickness sits in the sockets. Their bottom groove starts in line with the floor of the sides' groove, and the runner notch starts at the inside face of the side. The sides are cut a little shorter than the drawer depth, by the wood left behind the sockets at each end, so the finished box comes out to the depth you set.

Drawers on undermount runners have a notch cut in the bottom of the back at each end. To keep the narrow strip of back beside the notch solid, those boxes start the joint higher, the same amount at the top and bottom, so the lowest socket clears the notch by ⅛″. Their tails and sockets are also 0.15″ wider, to fill the larger spacing. Fronts and backs get the same layout, so every corner matches. Drawers on side-mount runners have no notch and keep the standard layout.

Your first G-code cut

Check your own machine's routine against these steps, and test on scrap first. Each file calls a tool length offset, then moves the machine, so a wrong Z setup can drive a bit into the work.

1. Measure the sheet. Enter its real thickness in Materials, measured with calipers. Depths and through cuts are worked out from it.
2. Set up your bits. On the Nesting tab, add them to CNC tools and assign one to each operation. The tool numbers must match your Mach4 tool table.
3. Check each bit's numbers. Look over its RPM, feed, plunge and pass depth. They start as general values, not values for your bit, spindle and material.
4. Set your zeros. X and Y zero go on the bottom-left corner of the sheet, and Z zero on the top of the material. The first lines of each file state both, along with the sheet size.
5. Touch off Z for every bit. After each bit change, use your touch plate on top of the material. Each file also calls G43 with its tool number, which adds that tool's length from your tool table, so keep those lengths at 0 if you touch off.
6. Check the clearance. Each file goes to Z4 above your Z zero, then to X20 Y20 before it starts cutting, and back there at the end. Make sure that path is clear.
7. Run the numbered files in order. Before each one, put in the bit it names and touch off. The cutout is always last, because it frees the parts. If you touch off by hand, use the separate files rather than the single file with tool changes.
8. Flip when told to. A sheet with shaker or groove doors has two programs, back and face. Cut the back first, then roll the sheet as the file's notes describe.

Air-cut the first file above the sheet if you want to be extra careful.

CNC tools

The tool library and tool assignment (which bit runs each operation) are above the nest, on a subscription or the trial. G-code uses them for its tool numbers, feeds and speeds.

If you export DXF, set your bit diameters in your CAM as usual. DXF geometry doesn't depend on them, with one exception: dovetail drawer joints are drawn for a new ¼″ tail bit.

Which export should I use?

• Mach4 or Avid machine: G-code if you want to load the file and cut. Zero Z on top of the material.
• Any other machine, or you prefer your own CAM: DXF, into VCarve/Aspire or your usual CAM.
• One cabinet, not the whole job: the per-cabinet DXF links on Cut list & Export.