User manual · Chapter 6 of 9

Toolpaths

How a toolpath is made, the settings every one shares, each 2D, carving and 3D strategy in turn, and managing the list of operations.

Making a toolpath

Choose the Manufacture stage.
In the drawing, select the shapes to cut. (Surfacing, the photo carves and the 3D strategies work from the stock, a picture or a model and need less selecting; each section below says what it wants.)
Pick the strategy from 2D Toolpaths or 3D Toolpaths on the ribbon, or from the Toolpaths menu.
The form opens in the Properties tab on the right. Choose the Tool bit, then work down the cards.
Press OK. The toolpath is calculated, drawn over the job, and added to the list in the Toolpaths tab. Cancel closes the form without making anything.

To change a toolpath later, double-click it in the list (or right-click and choose Edit…), change what you need, and press OK again.

The Tool bit list shows the bits from the Tool Database whose shape suits the strategy: V-bits for a V-carve, flat and ball bits for a pocket, drills for drilling. Tick Show all tool bits to list the rest of the library as well. The small database button beside the list opens the Tool Database.

Once a bit is chosen, the fields it owns (its diameter, flutes and angle) are taken from the database and hidden from the form. The feed, plunge and spindle speed are filled from the job's material if automatic feeds are on, and from the bit if not. You can still change them for this operation.

Settings most toolpaths share

Name: What the operation is called in the list and in the G-code. Leave it and a name is made from the strategy. "Rough pocket 6 mm" is easier to find later than "Pocket 4".
Feed rate, Plunge rate, Spindle speed: How fast the bit moves while cutting, how fast it moves straight down, and how fast it turns. A spindle speed of 0 leaves the speed out of the file.
Cut depth: The total depth of the cut, measured down from the start depth. To cut a part free, go a few tenths past the stock thickness.
Start depth: How far below the top of the stock the operation begins. Use it when an earlier operation has already removed material, so the bit does not cut air on the way down.
Depth per pass: How much deeper each pass goes. 0 cuts the full depth in one pass. More than about half the bit's diameter per pass is heavy going in hardwood.
Passes: Force an exact number of passes. 0 lets the depth per pass decide.
Last pass depth: Make the final pass a light one of this depth; the passes above share the rest.

Depths are measured from the Z zero you set in Job Setup.

The Vectors card

Toolpaths that work from closed shapes have a Vectors card:

Machine / Follow: Vectors uses the shapes you selected. Areas uses the areas you picked with Select Areas.
Overlapping vectors: How several selected closed shapes combine. Keep separate is normal: a shape inside another is an island, and shapes that only overlap stay separate. Subtract the others from the boundary, Weld them into one shape and Only where they overlap combine them for this toolpath without changing the drawing.
Boundary vector: Which shape is the one being cut into, when the combine rule needs to know. Left alone it is the largest selected shape.

Rest machining

Rest machining (skip stock earlier toolpaths already cleared) makes a toolpath cut only what earlier operations left behind. It is what makes a large bit followed by a small one efficient: the small bit spends its time in the corners the large one could not reach instead of cutting air. It is not available on the first operation in a job.

Entries, ramps and allowances

Where a strategy has an Entry setting, Ramp or Helix takes the bit down while it moves, which is kinder to it than a straight Plunge. The ramp distance sets how far it travels on the way down. An allowance leaves material on the walls (a positive value) for a finishing pass or sanding, or cuts past the line (a negative value) to make up for a bit that measures small.

Profile

Cuts around a shape's outline: the operation that frees a part from the sheet or opens a hole. Select closed shapes (or open ones, for a cut on the line).

Side / offset: Outside for a part, so it keeps its drawn size. Inside for a hole. On line centres the bit on the line, cutting a slot one bit wide.
Direction: Climb usually leaves the cleaner edge. Conventional is safer on a machine with play in its drives.
Allowance offset: Material left on (positive) or cut past (negative) the line.
Separate last pass: Do a separate finishing pass leaves a thin skin (the Finishing allowance, 0.5 mm to start) and takes it off in one light pass at the end, which squares up a wall the roughing passes pushed out of true. Reverse finishing direction runs that pass the other way round.
Tabs: Add evenly-spaced tabs leaves small bridges holding the part to the sheet so the cutter does not throw it. Set the Tabs (count), Tab length and Tab thickness. You can also place tabs by hand by clicking on the outline; put them on straight edges, where they are easy to clean up.
Entry: Ramp length takes the bit down along the cut. 0 plunges.

For a through cut, set the cut depth slightly past the stock thickness. Cutting exactly to thickness usually leaves a skin, because neither the sheet nor the spoilboard is perfectly flat.

Pocket

Clears all the material inside a closed shape to a depth. A shape fully inside another is left standing as an island.

Stepover: How far the bit steps sideways between passes, as a fraction of its diameter. 0.4 is a normal clearing cut.
Clearing pattern: Offset (concentric) follows the walls. Raster (zig-zag) is quicker in open areas. Spiral (continuous) joins the offset loops into one path so the bit enters once and never steps into solid material twice in the same place; on a pocket with an island it falls back to offset by itself.
Cut direction, Raster angle: Climb or conventional, and the direction of the raster lines (0 runs along X).
Profile pass: A final loop round the wall, Last (after clearing) or First (before clearing). It cleans off the scallops the clearing leaves. Choose First for thin walls that might break out.
Entry: Helix (spiral bore-in) or Plunge (straight down), with the ramp distance.
Pocket allowance: Material to leave on the walls.

2D Adaptive Clearing

Clears a pocket with a cut that holds the load on the bit constant, so it is never buried in a corner. The bit takes a deep, narrow cut, which spreads wear along the flutes and lets the feed go up.

Optimal load: How much of the bit's diameter is in the material at any moment. It is a different quantity from a pocket's stepover: 0.1 to 0.2 is normal here and is not slow.
Depth per pass: Because the load is controlled, this can be most of the flute length.
Wall taper: Lean the walls by an angle. 0 is straight.
Finish allowance: Material left for a finishing pass.
Trochoidal corner loops: Loop through inside corners instead of turning into them, with the Loop radius as a multiple of the stepover.
Entry: Ramp or plunge.

Trochoidal Clearing

Clears a closed shape with the bit cutting in light half-circle loops, each one taking only a sliver. On an open line it cuts a slot. The walls are cut first, the loops shrink to fit every corner, and the bit never crosses the shape's edge.

Loop width: The width of each loop. 0 picks one from the bit (1.8 times its diameter).
Radial engagement: How far the cutter advances on each loop, as a fraction of its diameter. 0.05 to 0.15 is usual. Above about 0.25 there is little point cutting this way.
Direction: Climb or conventional.
Cut full depth in one pass: Ignore the depth per pass and loop at full depth.

Surface

Skims a face flat with a wide bit: flattening a spoilboard or truing rough stock before the real work.

Face: Whole job stock, or Selected area for a shape you have selected.
Overhang past edge: How far the bit runs past the edge. Running out into free air avoids a mark at the boundary. Half the bit's diameter is a good start.
Pattern: Raster (parallel) or Offset (concentric).
Stepover, Raster angle, Cut direction: As for a pocket. Along the grain leaves the better finish on wood.
Zig-zag: Cut in both directions. Off returns to the same side each pass.

Chamfer

Runs a V-bit along an edge to bevel it. Select the outline.

Width W: How wide the bevel is, measured across. The depth follows from the bit's angle: a 90° bit cutting 3 mm wide goes 3 mm deep.
Overcut: Extra depth below the bevel so it meets the face below cleanly.
Side: Outside bevels the outer edge of a part, Inside the rim of a hole or pocket.
Slope: Slope downwards or Slope upwards.
Cut direction: Climb or conventional.

Round Over

Softens an edge to a radius with a round-over bit. There is no radius to type: the bit cuts its own.

Shoulder / flat above: A flat lip left above the curve. 0 runs the round right up to the face.
Overcut: Extra depth below the curve.
Side: Outside edge, or Inside edge (hole or pocket).
Cut direction: Climb or conventional.

Fluting

Cuts decorative grooves along lines, usually with a ball-nose or round-nose bit, easing in and out at the ends.

Flute depth, Depth per pass: How deep the groove is, and in how many steps. Alternate direction each pass saves travel.
Flute width: 0 makes the groove one bit wide. Wider grooves are cut in several side passes, their Cross-section either Flat bottom or Coved / scalloped, with a Side-pass stepover.
Ramp ends: Ramp both ends, Ramp at start, Ramp at end or No ramp (constant depth), with a Ramp shape of Smooth (cosine) or Linear.
Ramp length / Ramp (% of length): A fixed ramp length, or 0 to use a percentage of each flute (25% to start).

Drill

Drills a hole at the centre of each selected circle or point.

Cut depth: The hole depth. For a through hole, add a little for the drill's point.
Depth per pass: The peck: how far to drill before coming out to clear chips. 0 drills in one plunge. Set it for any hole deeper than about two diameters.
Retract: Where the drill lifts to between pecks: Retract above start depth, Retract above previous pass (with a Retract gap), or Retract to safe Z.
Deep-hole (advanced): A different First peck, a Peck reduction so each peck is shorter than the last, and a Minimum peck.
Dwell at bottom: Pause at full depth, in seconds.
Breakthrough / overshoot: How far past the far face to go, so the hole is fully open.
Use vector selection order: Drill in the order you clicked the circles instead of the shortest route.

Engrave

Follows lines with the bit, cutting along them. The cut is centred on the line, so open vectors are fine: lettering, layout marks, decorative line work. Set the depth and passes; there is nothing else to decide.

V-Carve

Carves with a V-bit so the cut widens as it deepens. The carve goes deep where the shape is wide and shallow where it is narrow, which gives lettering its chiselled look. Select closed shapes: letters converted to curves, or any artwork.

Use flat depth / Flat depth: Stop carving at this depth and give wide areas a flat floor instead of letting them run to a point.
Carving pass step: How closely the carving passes are spaced. Smaller is smoother and slower.
Area clearance: With a flat depth, a flat bit clears the floor first. Choose the clearance bits, the Clearance stepover, Clearance depth/pass, Clearance pattern and direction, whether to ramp in, and whether the Clearance area is Flat areas only or the Whole pocket. Rough with clearance tool first takes the bulk out before the V-bit runs, which saves the V-bit's tip. Corner sharpen drives into inside corners to leave them as square as the tool allows.
Use vector start points: Start each cut at the shape's own start point, so the entry mark goes where you want it.

The depth of a V-carve comes from the shape and the bit's angle. To limit it, use the flat depth.

Inlay

Makes a matching pocket and plug so one piece of wood can be set into another. One operation cuts both halves: the pocket into the board the design is drawn on, and a mirrored plug onto a board of its own. Run it from the pocket's board. Design ▸ Modify ▸ Set up Inlay (Plug + Pocket) prepares a selected design for it.

Joint: V wedge cuts angled walls with a V-bit. The plug wedges tight as it seats, with no gap at the sides, and corners are as sharp as the bit's point. Straight wall cuts vertical walls with an end mill. It is quicker, but the plug has to be made smaller than the pocket, leaving a visible glue line, and inside corners take the bit's radius.
Fit clearance per side: How much smaller the plug is than the pocket on each side, so it goes in. A tenth or two suits most timber.
Generate: Pocket + plug, Pocket only or Plug only.
Pocket depth Dp: How deep the pocket is.
Plug surface gap Sp: How far the plug's face sits below the face of its own board. It lets the finished inlay stand proud, to be sanded flush when the glue is dry.
Plug wall height Fp: How tall the plug's wall is. Set it a little under the pocket depth so there is room for glue at the bottom.
Wall pass step, Wall step override, Floor clearance step: How finely the walls and floor are cut. Finer on the walls gives a better fit.
Plug outer boundary: Clear the plug's surroundings across The whole board (job stock) or only A moat around the design of a set Moat width. A moat must be wider than the bit.

A separate clearing bit can be chosen to take out the floor. If you later want the plug cut differently, Toolpaths ▸ Regenerate Plug Only re-cuts it from the pocket as it stands, so the two halves cannot drift apart.

Photo V-Carve

Carves a picture as grooves whose width follows the picture's brightness, like a halftone. Import the picture first (Import Image…). High-contrast images with a clear subject work best.

Max carving depth: A limit on how deep the grooves go.
Stepover retract: How far the bit lifts when it moves to the next line.
Pattern: Raster (parallel lines), Hatch (crossed) (a second set at right angles, which darkens the shadows and doubles the time), or Selected vectors to follow lines you drew.
Line spacing: The distance between lines. Closer lines give a finer, shallower picture. On a V-bit the spacing also caps the depth, since a groove cannot be wider than the gap between lines.
Sample step, Line angle, Min cut depth: How finely the picture is read along each line, the direction of the lines, and a depth below which nothing is cut.
Invert (light cuts deep): Swap the tones, so the light parts of the picture are cut deepest.

Sketch Carving

Carves a drawing or scan as fine lines, like an engraved plate. Import the picture first.

Line thickness: How heavily lines are cut, from 0 to 100. On a V-bit heavier means deeper and wider.
Trace light lines on dark: For a chalk-on-blackboard image. Off follows dark lines on a light background.
Use flat depth / Flat depth, Carving pass step: As for a V-carve.

Prism

Raises a shape as a faceted roof: a cone from a circle, a pyramid from a square, a ridge from anything longer than it is wide. It is a V-carve turned inside out: the surface rises from the edge at the bit's flank angle to the shape's centre line.

Cut depth: 0 gives exactly the depth that brings the apex to the surface. Less, and the roof levels off into a flat top; more, and it stops short.
Pass pitch: How far each pass steps in. 0 uses the bit's own engagement.

3D roughing

Three strategies take the bulk of the material off a 3D model, leaving a little for finishing. Use the biggest bit that reaches.

3D Adaptive Clearing: Holds a constant load on the bit, as 2D adaptive does. Optimal load 0.1 to 0.2 is normal; each level can be deep.
3D Pocket Clearing: Works level by level, clearing each level like a pocket.
3D Parallel Clearing: Works level by level in parallel raster lines.

Their shared settings:

Model depth: How deep to go. 0 takes the depth from the model, which is what you normally want.
Rough depth per level: How far down each level steps. 0 lets the operation choose.
Machining limit boundary: Model boundary, Material boundary or Selected vector(s), with a Boundary offset to grow or shrink it.
Machining allowance: Material left on every surface for the finishing pass (0.5 mm to start). Leave some: it gives the finish something even to cut.
Stepover: For pocket and parallel clearing, the fraction of the bit's diameter between passes.
Profile pass, Order: Pocket clearing only. A final loop round each level, and whether to work Level by level or Region by region.
Raster angle, Avoid re-cutting cleared areas: Parallel clearing only.
Entry: Ramp or plunge.

The forms warn you when the model is deeper than the machine can reach.

3D finishing

Four strategies make the finished surface with fine, closely spaced passes. The stepover here is what you will feel with your hand: halving it roughly doubles the time. The finish pass normally uses a ball-nose bit.

3D Parallel Finishing: Parallel passes across the model at a Raster angle. This is the one with extra options: Zig-zag to cut both ways, Space the passes along the surface (constant cusp) to crowd passes together on slopes so the ridges stay even, and Waterline the steep walls to finish anything steeper than the Steep angle (45°) with level contours instead.
3D Scallop Finishing: Passes spaced to leave an even scallop height all over.
3D Contour Finishing: Passes that follow offsets of the outline.
3D Pencil Finishing: Traces the inside corners and creases a larger bit could not reach. Run it after another finish.

Their shared settings are the Model depth, the Machining limit boundary (with an offset of 0.1 mm to start, so the finish runs just past the edge), the Stepover (0.08 of the bit's diameter to start), the Cut direction, and a Stepover retract that lifts the bit slightly between passes so it does not drag chips across the surface.

The strategy is fixed by the command you chose, and the form's heading names it. To use a different finish, add that operation.

The Toolpaths list

The Toolpaths tab on the right lists every operation in cutting order, with its tool and depth. The bar at the top chooses whether you see This sheet, the Selected sheets or All sheets.

The eye on each row shows or hides it. Hidden toolpaths are left out of Simulate Visible Toolpaths.
▲ and ▼ move the selected operation earlier or later.
Double-click a row to edit it. Right-click for Rename…, Edit… and Delete.
A row marked ⚠ recalc is out of date: the shapes it was made from have changed since. Double-click it and press OK, or use Recalculate Selected, before you cut.
A locked operation carries a locked badge.

The buttons under the list repeat the common commands: previews, checks, export, delete and clear.

Operations

On the ribbon under Manufacture ▸ Operations:

Recalculate Selected: Rebuild the chosen operations from their bit and settings. Use it after editing the shapes they were made from.
Recalculate All: Rebuild every operation, for instance after changing Job Setup.
Lock / Unlock: Freeze an operation that is right. A locked operation keeps its moves: it is never recalculated, flagged out of date or deleted, and the shapes it was made from can no longer be selected, so nothing can move them out from under it.
Merge Toolpaths: Reorder so that operations using the same bit run together, for fewer tool changes. The order within each group is kept.
Optimize Order: Reorder to reduce travel between operations. It changes the sequence only, never what is cut.
Clear Toolpaths: Delete every toolpath in the job. The drawing is left alone.

Every toolpath is saved in the .cvc file with the drawing, so reopening a job brings back its toolpaths exactly as they were.