Setting up toolpaths

The app calculates the toolpaths from your drawing automatically whenever you change something. You only decide how each shape is cut. The toolpaths appear in blue on top of the drawing.

Cut type

Where do I set this?

• Cut popup: click a shape and a small window with cut type, depth, cut through and bit appears next to it.
• Properties → Cutting in the right panel: the same values, plus holding tabs.
• Layers: the default for all shapes on a layer (Layers).

A shape takes the values of its layer until you set something different. Like layer resets it.

Cut depth

The depth is measured down from the material surface. The app splits it into equal passes; how deep each goes depends on the bit's step down (Cutting data). Below the field you see, for example, “3 passes of 1 mm”.

Cut through goes through the whole material and by the overcut into the spoilboard. The depth then follows the material thickness automatically. When cutting through, the app adds holding tabs.

Depth 0 = mask: A shape with depth 0 is not cut. It does limit every pocket and V-carve it overlaps – only the area where both shapes lie on top of each other is machined. Handy for cutting just a section of a large area.

Project-wide settings

Use the Simple button (feather) at the top of the header bar to switch between Simple and Expert (also in the menu View → Expert mode). Simple shows only the bit, safe height and tabs; everything else is under More settings. Simple also hides pro features: special toolpaths, threads, form tools, photo engraving, two sides, rotary axis, toolpath templates, clamps as well as controller settings, calibration and macro buttons. The menus are shorter: among others, nesting, path, order, distribute, dimensions, symmetry, time and cost, cutting data, the fit comb and the split view are left out. In Simple mode a step bar below the header bar guides you through the workflow: Workpiece, Draw, Toolpaths and Machine. Clicking a step opens the matching window, Next goes to the next step, and in the last step Start carving starts the job. In an empty project in Simple mode, the start cards ask What would you like to make?: Name sign, Gift or decoration, For the kitchen, Crate or box, Game or puzzle, Logo or file, Draw it yourself and Mill a circuit board (in the laser Engrave a photo). Each card opens the matching assistant or the templates with the category preselected; Browse all templates shows the whole gallery. The command search (Ctrl+K) still finds them and then switches to Expert. A project that uses such a feature keeps showing it. Expert shows everything and is the default.

With nothing selected, Properties → Cutting shows the settings for the whole project:

• Cut direction: climb gives clean edges in wood and plastic; conventional is gentler on light machines with backlash and suits aluminium.
• Pocket clearing: offset (rings parallel to the wall) for complex shapes, zigzag (straight passes at an adjustable path angle, with a final pass along the wall) for large simple areas, adaptive (narrow strips from the inside out, helix entry) for deep pockets in hard material: sideways the bit only cuts a strip about a third of its normal stepover and steps down up to three times deeper instead, at most 90 % of the flute length. Between strips it stays down whenever the way leads through cleared material.
• Overcut: how far cutting through goes into the spoilboard.
• Retract: short lift within one shape.

Plunge angle

The bit ramps into the material along the path instead of drilling straight down. This is gentler on bit and machine. 0° means straight down; 2° to 5° are good values.

Lead-in and lead-out arcs

For outside and inside contours, the bit can arc in to the edge from the waste side on a quarter circle and arc away again at the end. It then never plunges on the finished edge, so no witness mark is left. The ramp from the plunge angle runs along the arc; if the arc is too short, the ramp goes back and forth on it.

• Arc radius: as a percentage of the bit diameter; 100 % is a good start. Where the arc does not fit, for example in small holes, it gets smaller on its own; if it does not fit at all, the shape is cut as usual and a notice names it.
• The entry point is in the middle of the longest straight edge, never under a holding tab.

Safe height

Between two shapes the bit rapids at this height above the material. It must be higher than all clamps, screws and hold-downs.

Order

The app cuts in a sensible order: engravings, then pockets, drill holes, inside contours and finally outside contours, so the part stays held until the end. Each bit becomes a separate part; in between the app asks you to change the bit.

The Cutting tab of the right panel lists all toolpaths per bit with their duration. Drag bits and toolpaths or use Alt+Up to reorder them. Order automatically restores the calculated order.

Toolpath templates

Do you often set up similar projects, such as signs with an “Engraving” and a “Cut-out” layer? Save the cut settings once as a toolpath template and apply them to the next project with one click.

• Save: Milling tab → Save as template, or menu Bits → Toolpath templates ▸ → Save as template …. Enter a name and tick the layers (layers that cut are ticked already). The bits used and the project-wide options are saved with it: cut direction, tabs, ramp, pocketing, goal, surfacing and lead-in/out arcs. The same name replaces the old template.
• Apply: Milling tab → Apply template, or Bits → Toolpath templates ▸, which also lists the five most recently saved templates to apply directly. The preview shows for each layer whether it already exists in the project or will be created.

Layers are matched by name (upper and lower case do not matter). Missing layers are created so you can draw into them right away. Settings that differ on individual shapes stay as they are. A bit that already exists in the project with the same values is reused; otherwise a copy is added. Applying is one step, Ctrl+Z undoes it.

Toolpath templates are kept in your account and are available on every device (up to 200). The app already combines toolpaths with the same bit into one program, even across layers; a bit change only happens between different bits.

Carving a relief

The app carves a relief in two steps, optionally with a third. Set all of them in the relief's properties under Milling:

• Roughing with the roughing bit (ideally a large flat end mill): rows in steps of the depth per pass until the finishing allowance is left above the surface, on the slopes too. Without a roughing bit, the finishing bit clears in steps itself if the relief is deeper than its depth per pass. In rows moves the bit across the relief row by row. In levels clears the area height by height from the inside out, like a pocket, and flat areas get a level of their own. This is gentler on the bit for tall 3D models and is the default for STL and STEP models.
• Finishing with the finishing bit (ideally a ball-nose bit): close rows that follow the surface. The row spacing in % of the diameter sets how smooth it gets; Both directions one after the other are even smoother but take twice as long. In rows suits shallow reliefs. On steep walls the rows end up far apart; Waterlines work better there: height by height around the model, from top to bottom. Steep and shallow combines both: areas steeper than Steep from (default 45°) in waterlines, shallower ones in rows, and the two areas overlap by 5°. Steep and shallow is the default for STL and STEP models (more).
• Rest machining with the rest machining bit (optional, a smaller ball-nose or tapered ball-nose bit): after finishing, it only machines the spots the finishing bit could not reach, such as narrow valleys, fine edges and steep walls. Where a lot was left, it goes down in steps of its depth per pass. The rest machining bit must be smaller than the finishing bit.

At every point the bit only goes down until its cutting edge touches the surface: it never cuts too deep, not even with its side. It cannot reach into valleys narrower than the bit; the rest machining bit helps there. Roughing comes first, then finishing, and rest machining last. The Milling tab lists all toolpaths with their time, and the 3D view shows the result with the real bits.

Milling 3D models exactly

A relief made from an STL or STEP model keeps its triangle mesh. Roughing, finishing, rest machining, the simulation and the 3D view then work exactly on the triangles instead of on a height map: at every point the bit goes down until its tip, ball or flank touches a triangle, an edge or a corner. Fine edges and small lettering stay as sharp as they are in the model. The properties then show Milled exactly on the 3D model with the number of triangles. The app reduces very large models to at most 200,000 triangles when inserting them.

Recessed, smoothed or with a fading edge, the app mills from the height map; the note in the properties says why. After editing with the brush or with Relief from shape, the model no longer applies; Undo brings it back. Profile bits also mill from the height map.

Waterlines, steep and shallow

With Waterlines, the tip of the finishing bit follows, height by height, the line where it just touches the surface, like the contour lines of a map. The app picks the height spacing from the row spacing: on walls from 45° (with Steep and shallow, from the threshold angle) the paths on the surface are at most one row spacing apart. On a 3D model the app moves each line exactly onto the triangles; where it would pass over a bump between two points, the bit lifts, so it never cuts too deep. On shallow areas waterlines are far apart, which is why rows take over there with Steep and shallow. Short steep pieces under two row spacings are left out; the rows pass over them anyway.

Pencil pass

Rows and waterlines only cross valleys and inside corners and leave small ridges there. With the Pencil pass switch below the rest-machining bit, the app runs once exactly along the valleys after finishing, where the bit touches the surface on two sides at once. It uses the rest-machining bit, or the finishing bit if there is none. In the Carving tab the pencil pass appears as its own operation after finishing. Any spot tighter than one and a half times the bit radius counts as a valley; gentle hollows are cut cleanly by rows and waterlines anyway. If the relief has no valleys, the app shows a note.

Engraving on the relief

A line, text or shape with the cut type On line, Pocket, V-carve or Contour that lies over a carved relief follows its finished surface: the cut depth counts from the relief surface below, so the engraving is equally deep everywhere on a dome. Beside the relief it stays on the top of the material. The app cuts the engraving after the relief, even if it has its own bit; in the Carving tab it appears as Engraving on the relief or, for example, Pocket on the relief. With V-carving the groove depth counts from the surface, so crests and lettering on a dome are equally wide everywhere. Toolpaths cut through do not follow the relief. For fine lettering on steep spots, a pointed bit or a small ball-nose bit works best.

Shank and collet nut

In deep reliefs it is often not the bit that hits, but the collet nut or the spindle above it. The app checks every relief toolpath against the finished surface (with the finishing allowance when roughing) and against the top of the material around it. Under Shank and collet nut, enter the stick-out of the finishing bit (from the tip to the collet nut) and the collet nut Ø (19 mm for ER11, 28 mm for ER16, 35 mm for ER20). If the stick-out is left empty, the app uses the longest possible length (overall length minus clamping) and tells you in a note how far the bit must at least stick out. Roughing and rest-machining bits are always checked at their longest possible length. If the collet nut hits, a warning marks the spots on the canvas. With Keep collet nut clear, the bit stays high enough there to keep 1 mm of clearance; material is left at those spots. The app also warns if the shank rubs against the relief above the flutes. For the spindle body it assumes Ø 52 mm from 15 mm above the collet nut.

For pockets, contours, engravings and drill holes the app checks the collet nut too: if a toolpath is deeper than the bit can stick out of the collet (overall length from the bit library minus at least 12 mm clamping), it warns, because beside the path the material stands up to the top. This warning then replaces the one about the flute length.

Height steps

Instead of 3D toolpaths, a relief can also be cut in height steps, like the layers of a contour map. In the properties under Height steps, choose the number of steps and click Split into … steps. Each step becomes its own layer with a pocket at its depth, cut with the roughing bit (or the largest end mill in the project). No step cuts deeper than the relief, so terraces remain. The relief itself is hidden and kept; Undo brings it back. With a cut-out, the cut-out shape trims the steps.

Finishing allowance

Under Settings → Carving you set the finishing allowance (0 to 5 mm, default 0 = single pass). For the cut types Outside and Inside the app then cuts two passes: first with the allowance (listed as “Name (+0.5 mm)”), then to size. This is easier on the bit and gives clean edges, because the last cut removes little material. Since it only removes the allowance sideways, the finishing pass uses twice the depth per pass (at most the flute length) and is correspondingly quick. Roughing always runs before finishing the same shape. For pockets the app clears the area leaving the allowance at the wall, then runs once around the wall to size (“Name (+0.5 mm)”).

Rest-machining bit for pockets and inside contours

A large bit clears a pocket quickly but leaves material in corners and curves. For the cut type Pocket you can also choose a rest-machining bit (a smaller flat or ball end mill). The large bit clears the area, then the small one cuts only what is left. For the cut type Inside the small bit cuts only the corners the large one cannot reach. In the Carving tab it appears as its own program “Name (Rest Ø x)”; the carve wizard guides you through the bit change. If the rest-machining bit is not smaller than the pocket bit or is not a flat or ball end mill, the app shows a note and does not use it.

Cut out a group as one part

Group the shapes of a workpiece (Ctrl+G), for example a board with a round head and lettering on it. In the group's Properties or in the carve window, turn on Cut out as one part. The app then cuts out the shared outline of all shapes along the outside, by default through the material and with tabs. Set depth, cut-through and bit there.

The shapes in the group keep their cut type: pockets, engraving and V-carving are carved as usual. Only their own Outside contour is dropped, because the group's outline replaces it. If one part group sits inside another, the outer one applies.

If the part should not be cut exactly along the outline but with a margin and without bays (like a sticker), click Shrink wrap as outline … there. The shrink wrap becomes the bottom shape of the group, is not carved itself and then is the outline along which the group is cut out.

Carving goal: fast or fine

At the top of the Milling tab you choose what matters for the whole workpiece. Each option shows how long carving takes with it and how many percent faster or slower that is than the selected option.

• Fast: about a third more depth per pass and stepover (at most up to the flute length, the bit diameter and 60 % stepover), coarser relief rows and V-carve flanks, no finishing pass. Good for rough parts, test cuts and parts that will be sanded anyway.
• Balanced: carves with the bits' cutting values as set in the bit library. This is the default.
• Best quality: about 20 % less depth per pass and 30 % less stepover, finer relief rows and V-carve flanks, and a finishing pass with at least 0.2 mm allowance on outside and inside contours.

The carving goal does not change feed rate or spindle speed: they suit your machine and appear like that in the carving assistant. The bits' values in the project stay the same; the goal only applies when the toolpaths are calculated and is saved with the project. Undo restores the previous goal.

Chamfer and deburring

With Chamfer outside and Chamfer inside a V-bit (or chamfer bit) breaks the top edge: outside all around a part, inside on holes and cut-outs. Instead of the cutting depth you enter the chamfer width; the app works out the depth from the bit angle (at 90° as deep as it is wide). For deburring 0.3 to 0.5 mm is enough.

The bit tip runs exactly on the edge (a flat tip runs beside it by its radius). If the chamfer is wider than the bit's cone can reach, the app cuts the largest possible width and warns. When you choose a chamfer, the app takes a V-bit from the project if there is one. The chamfer is cut before cutting out, while the part is still held.

More cut types

Below the usual cut types, More opens four special toolpaths and the thread, each with a small preview image. You find them in the cut window on the shape, in the properties and on the layers. The app calculates each toolpath from the real shape of the cutter: the bit never goes deeper than intended, not even with its side. The 3D view shows the result before you cut. If you do not need the group, switch it off under Settings → Features → More cut types; with Ctrl+K you can also find each toolpath by name and choose it for the selected shapes.

Prism

Raised letters or shapes with a sharp ridge: the V-bit cuts the sides at its angle from the edge up to the centre. Height (max.) limits how deep the sides start at the edge. If it does not reach the ridge, a flat top remains and the app tells you the height needed for a sharp ridge. Lower the background afterwards with a pocket so the shape stands free. V-bit only.

Fluting

A groove along the line whose depth fades out smoothly at the start, end or both ends, as on columns, frames and trims. Length is the length of each fade in percent of the line. Open lines work too. A ball-nose bit gives round grooves, a V-bit pointed ones. If the groove is deeper than one step down, the bit runs back and forth several times.

Texture

Fills an area with a hammered pattern (short, staggered dimples as if made by a hammer) or waves (continuous grooves whose depth rises and falls gently), for example as a background for a sign. Spacing is the distance between rows; about two thirds of the bit diameter looks even. The texture is random but stays the same for each shape every time it is calculated. It looks best with a ball-nose bit or V-bit; a flat end mill leaves square dimples.

Moulding

A profile runs along the edge of an area: roundover (convex), cove, ogee (S-shape) or bevel. Profile height and width set its size. With Edge: Part the profile lies inside the shape (table top, sign); with Opening it lies around the outside of the shape (picture frame). Next to the edge the bit cuts a little deeper so the profile ends crisply at the bottom; cut the part out afterwards with Outside contour. Best with a ball-nose bit. If part of the profile is tighter than the bit can reach, the app tells you how much remains there.

Thread

The app mills a thread on a circle: the circle is the nominal diameter, so for M8 a circle of Ø 8 mm. The thread mill (60° profile on a slim neck, in the library under Thread mill) follows a helix and enters and leaves smoothly along a half circle.

• Internal thread cuts a nut thread into a hole. The core hole must be milled first, for example with Inside contour or Pocket on a second circle: nominal diameter minus pitch (M8: Ø 6.8 mm). The app shows the value below the settings.
• External thread cuts a bolt thread around a standing boss with the nominal diameter, which has been cleared beforehand.
• Thread length: how deep the thread reaches from the surface. It must not be longer than the neck of the cutter.
• Pitch: Coarse uses the metric coarse pitch for the diameter (M6 = 1 mm, M8 = 1.25 mm, M10 = 1.5 mm), Custom allows fine threads such as M10 × 1.
• Hand: right (standard) or left. Passes: in this many rounds the cutter reaches the full thread depth; more rounds are gentler on the cutter and the machine.

The app climb-mills if the project is set that way and chooses from that whether the helix runs bottom-up or top-down. Every pass starts at the same point so all rounds hit exactly the same pitch. Programs with threads always come last, so the core hole and boss are already finished. Thread milling can be switched off under Settings → Features → Thread milling. It works best in aluminium, brass and plastics; in wood a thread only holds in very hard wood.

Surface facing

If the board is not quite flat or the top is rough, Surface facing mills it smooth first. The switch is in the Carve tab below the carving goal.

• Remove: how much is taken off the whole top, usually 0.3 to 1 mm.
• Facing bit: ideally a surfacing bit or a large flat end mill. Without a choice the app takes the largest flat end mill in the project.

The bit runs in rows along the longer side across the whole material and plunges next to the material. Facing is always the first program in the list. All depths then count from the faced surface: a 4 mm pocket is 4 mm below the new top, cutting through still goes into the spoilboard. With Z zero on top, the carving assistant probes Z again on the faced surface after facing, even if the bit stays the same.

Notes and warnings

Whatever cannot be cut is shown in red: spots the bit does not fit into, shapes that are too narrow, paths outside the material. The list of notes is under “Ready to carve”, in the Cutting tab and in the cut popup; clicking one selects the affected shapes. Usually a smaller bit or a different cut type helps.