3. Stock, origin and tools#

Two things have to be true before a toolpath means anything: the app has to know what is on your table, and it has to know what is in your spindle. Get these right once at the start of a project and everything downstream — depths, the simulation, the feeds, the warnings at export — follows from them.

Setup: the stock#

Setup is the third tab in the sidebar. It fills the panel and leaves the view visible, so edits show up live.

Dimensions#

Width (X), Height (Y) and Thickness (Z) are the actual piece of material. Thickness is the one that does real work: a profile cut to 12 mm through 12 mm stock is what separates the part, and the simulation carves a block of exactly this depth.

Work origin#

Two separate questions, and both matter more than they look.

X0 Y0 is the nine-position grid — which corner or edge of the stock the machine's zero corresponds to. Bottom left is the default and is what most hobby machines get jogged to. Pick centre if you locate work from the middle, which is common with a fixture or a rotary axis.

Z0 is where the tool's zero height is:

Top of stock is the usual choice — you touch off on the workpiece with a piece of paper or a Z-probe and go. Bottom of stock suits work where the material thickness varies but the finished depth from the table must not, such as surfacing a slab.

Whichever you choose, the export review restates it back to you before the file is written. Read that line against how you actually zeroed the machine. Getting this wrong is the fastest way to plunge a cutter through a spoilboard.

Material#

The material is not decoration. Each has a hardness factor that drives the automatic feeds and speeds:

Aluminium and brass additionally carry a maximum surface speed, because the failure mode in metal is not a broken cutter but a bit that overheats and welds swarf to its own edge. If your spindle cannot run slow enough to respect it, the export review says so.

The tool library#

The Tool Library tab across the top holds your cutters. It is saved with the project and kept in the browser between sessions, so a new project starts with the tools you already own.

Each row is one cutter. The little picture at the left is drawn from that tool's own numbers, so a taper really does taper and a V-bit really does come to a point — a quick check that a row says what you meant.

Type decides where a tool can be used#

If a cutter you expected isn't in an operation's list, it is the wrong type for that operation. Max Z does not hide a tool — ask for more depth than it has and the depth field warns Exceeds tool Max Z, leaving the decision to you.

The two angle conventions#

This trips people up because the trade itself is inconsistent, and the library follows the trade rather than tidying it up:

• A V-bit's angle is the included angle — the whole opening. A 60° V-bit has 30° on each side of the axis.
• A taper end mill's angle is per side, which is how the bits are sold.

And a taper's diameter column is its tip, not what it cuts. The library works out the rest for you: the shot above shows a 5°/side taper on a 2 mm tip, annotated Ø5.33 mm at depth · 10° incl. That is the real cutting diameter at its usable length, and the included angle for comparison against a V-bit.

The practical difference is at the bottom of a cut. A taper's tip is a small ball, so it can enter a groove narrower than itself and leave a round-bottomed cut instead of refusing the job — which is what makes it good for fine lettering and 3D finishing. A V-bit comes to a true point and closes tighter, which is why an inlay still wants one: a taper's rounded foot leaves a hairline gap at the finished face.

Feeds and speeds#

The bottom of the Setup panel decides how hard the machine is driven. Auto Feeds & Speeds is on by default, and it is the right default: it computes a feed, plunge feed, spindle speed and step-down per operation, from the tool, the material and your machine.

Machine rigidity#

The single most useful number here. It scales both how hard the app drives the chip and how deep a pass it takes:

Set it honestly. Too high and a flexy gantry chatters, deflects and leaves a wandering wall; too low and you spend hours cutting air-light passes. The status bar shows the icon at all times so an over-ambitious setting reads "hot" at a glance.

Spindle#

Set the min and max RPM to what your spindle can actually do — routers bottom out around 10 000. Auto mode picks a speed inside that range.

Then pick your spindle type. If you run a trim router rather than a VFD spindle, this is worth setting: the app knows the published speed charts for the DeWalt DW6xx / DWP611 and the Makita RT07 / RT0701C, and translates every RPM into the dial number you actually turn — dial 2, dial 2.5 — shown in the tool table, the simulation and the G-code comments. G-code S18000 is no use if your router has no idea what an S-word is.

Max feed rate#

A hard ceiling, in mm/min. Set it to what your machine can move without losing steps, and the app will not exceed it.

This one has a consequence worth understanding. Chip load is feed ÷ (RPM × flutes), and it does not depend on how deep the pass is. So when the machine cannot feed fast enough to reach a sensible chip load, the correct fix is to slow the spindle down, not to take a shallower cut — and that is what the app does. A bit that is fed too slowly for its speed doesn't cut; it rubs, heats and dulls.

The chip-load gauge#

Whether the numbers are right is answered while the simulation runs, in the readout under the stock:

On manual feeds the app also suggests the feed that would put you back in the band. This is the honest check on everything in this chapter: set the stock, set the tools, then watch the gauge on a simulated run before you cut anything.

The model produces sane starting numbers, not shop-certified values. It knows your tool, your material and how stiff you said your machine is; it does not know your cutter is dull, your stock is a knotty board, or your workholding is a bit optimistic. Treat its output the way you'd treat a manufacturer's chart — a place to start.

Next#

• 4. Operations — turning geometry into toolpaths
• 5. Profiles and pockets — cut side, tabs, and the five pocket strategies