Support Guides 09 of 11

Cut list, nesting and export

Parts (one cabinet)

Each cabinet's parts are in its editor: double-click the cabinet, then open the Parts tab. Every part is drawn with its machining:

ColourOperation
OrangeDado / rabbet
GreenNotch
Grey dotShelf pin (5 mm)
Blue dotHinge cup (35 mm)
Red dotHinge plate (5 mm)

Double-click a part to open it big, with every operation listed. You can pan and zoom it.

DXF ↓ this cabinet downloads the whole cabinet nested on its own, for a one-off. Downloads use the saved cabinet, so save your changes first.

Cut picked parts (recuts and offcuts)

A panel chipped or cut wrong, or you want a few parts out of a scrap:

The parts are grouped by material, and each material is its own cut: pick within a group, and that group gets its own sheet size and downloads. Pick all takes every part of that material (a whole cabinet's fronts, say).

  1. Click the parts you want. Each click ticks or unticks one.
  2. Set how many of each in the list below the parts.
  3. Sheet W × H: the piece you'll cut them from (H runs with the grain). Leave it blank for a full sheet of their material.
  4. The drawing shows how they fit, and warns if they don't.
  5. DXF ↓ or G-code ↓. For a styled door (shaker or groove) there are two files, cut in order: 1 · Back (hinge cups), then turn the piece over as the diagram shows, then 2 · Face (pocket, bevel or grooves).

Because each cut is one material, a ¼″ back never ends up on the same piece as ¾″ sides. Parts keep the job's machining and grain direction. A cut like this isn't added to Costing and doesn't change the job's Downloaded ticks.

The whole room's cut list, with glass pane sizes, prints on the Drawings set.

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:

LayerWhat's on itTypical toolpath
CUTOUTPart outlines and through-cutsProfile, outside, full depth (with tabs if you use them)
POCKETDados, rabbets, grooves and notchesPocket to the depth of the joint
UNDERMOUNTNotches for undermount drawer runnersPocket, through
DRILL_5MM (etc.)Holes, one layer per diameter, e.g. shelf pinsDrill
BORE_35MM (etc.)Large bores, e.g. hinge cupsDrill or pocket with a boring bit
GROOVESRough pockets for dovetail jointsPocket
MACHINE_PATHDovetail tails and sockets, already shaped for the bitFollow the line (no offset)
LABELPart names, sized to fit inside each partDon't cut. Hide it or engrave
SHEETThe sheet outlineDon't cut. Reference only

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 and Centroid CNC12 controllers, which covers Avid CNC machines. Pick yours in Shop settings. CNC12 output is in beta, so air-cut your first files. G-code 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. Zero Z where your Shop settings say: on the top of the material, or on the table.

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

Preview in 3D (in the Save list, or 3D beside one file) plays the files on the sheet: the paths drawn as the bit runs them (orange for rapids), and the sheet carved as it goes, with the line being run and the bit's position. Space plays and pauses; drag the slider to scrub. Under the view it lists any rapid that crosses the sheet below the top of the material, and any cut that goes into the table past the cut-through. Click one to jump to it. A viewer can't know your machine's real top of travel, so G53 Z0 is drawn 3″ above the sheet.

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:

StepWhat it cutsBit
Dovetail rough pocketsSides: clears the waste at both ends, half the side thickness deep. Front and back: clears a 0.5″ strip of sheet just past each end, as deep as the socketsDado and notch bit
Dovetail tailsThe tails, on the drawer sides only, cut right through the sideTail bit
Dovetail socketsThe sockets, on the drawer front and back only9282 insert

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 machine and bits. In Shop settings, pick your controller and where you zero Z. Then add your bits and pick the default bit for each operation. The tool numbers must match your controller's 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. Z zero goes on the top of the material or the table, whichever you picked under Machine. The first lines of each file state both, along with the sheet size. Zeroing on the table measures every depth up from it using the sheet thickness in Materials, so that thickness has to be right.
  5. Touch off Z for every bit. After each bit change, use your touch plate where you zero Z. On Mach4, 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 (Mach4) or to the top of the Z travel (CNC12), 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.
  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

Your machine and bits live in Shop settings (in the header), and every project uses them:

  • Machine: your controller and where you zero Z (Top of the material or Table / spoilboard), plus the rapid rate, tool-change time and sheet load time used for machine time on the Costing tab. Each Save G-code list shows which controller and Z zero its files are for.
  • Default tools: which bit runs each operation in every project.
  • Tool library: your bits. G-code uses them for its tool numbers, feeds and speeds.

CNC tools above the nest shows your machine, with a link to Shop settings, and the tool assignment for this project only: leave an operation blank to use your Shop settings default.

Costing and purchase orders

The project's Costing tab works from the nest of every room:

  • Sheets to order: each material's sheet count from the nest. Set how many to order (for spares or stock on hand), the price per sheet and the supplier. A price or supplier you enter is kept on this job and offered again on your next one.
  • Purchase order: one per supplier, with your shop name, logo and delivery address (Shop settings). Print it or save it as PDF, or copy it as an email to paste into your mail.
  • Edge banding: worked out from the front edges of the case parts (sides, tops and bottoms, shelves, front stretchers). Doors, drawer fronts, end panels, fillers and the kick face are painted, so they aren't counted. Add an extra percentage and the job rounds up to whole rolls (500 ft by default). Add a line for each colour; type your own feet for a finished end.
  • Additional materials: anything bought for the job, like glass or LED strip. With glass doors, a glass line fills in the square footage, and its purchase order lists each pane. + Paint & primer starts at both faces of everything cut from the front material (doors, fronts, end panels, fillers); switch it to gallons if you buy by the can. + Shop supplies (screws, nails, sandpaper, glue) is a percentage of the sheet goods and never goes on a purchase order.
  • Job cost: the sheets, the machine time at your shop rate, the Cabineo connectors, hardware, labour, banding, additional materials and overhead: what an hour of your shop costs you, charged on every machine and labour hour. Base cost per hour is that time cost over the job's hours. Machine time is read from each sheet's G-code at your bits' feed rates, plus tool changes and loading each sheet. Rates start from Shop setup and can be changed for one job.

Ordering doors and drawers

If you buy your doors, drawer fronts, drawer boxes or end panels from another shop, the Order tab (after Costing, in the project and in every room) writes the order for you. It covers the whole job, every room.

  1. Send out: tick what you're buying. Nothing else changes: the parts stay in your nest and G-code, so you can still cut any of them yourself.
  2. Supplier, Doors & fronts, Drawer boxes: the fields start with the job's own settings (door style, front material and thickness, drawer box materials and joinery). Type what the other shop needs instead: a 1″ beaded door, a species, the Colour code and sheen. A room in another colour (an island) gets its own colour on its lines.
  3. Print / save PDF, or Copy as email and paste it into your mail.

What the order lists, all worked out from your design:

  • Doors: width × height, the hinge side, and the hinge cup centres from the bottom of the door (the top and bottom hinges sit the same distance from each end, so it reads the same from the top). Untick Bore the hinge cups to leave the boring to you.
  • Drawer fronts and false fronts: width × height.
  • Drawer boxes: outside width × depth × height, fitted to your runner, with the runner's rear notch when it's an undermount.
  • End panels & fillers: finished ends and backs, appliance end panels, fillers and the corner cover. Untick it if you cut your own ends.

DXF · doors & fronts shows the doors, fronts and panels nested on each material's standard sheet, with their outlines, hinge cups and the same labels as the order, before you download. Download one material at a time, or one sheet. The free plan gets one sheet.

+ Add this order to the job cost puts the order on the Costing tab, under Additional materials, in square feet and by the box; set the prices there.

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, CNC12 or Avid machine: G-code if you want to load the file and cut. Zero Z where your Machine setting says.
  • Any other machine, or you prefer your own CAM: DXF, into VCarve/Aspire or your usual CAM.
  • One cabinet, not the whole job: open the cabinet, Parts tab, DXF ↓ this cabinet.
  • One damaged part, or a few from an offcut: pick them in the Parts tab and cut them on the size you give.