Machining Operations

Adding Operations

Operations are created from selected geometry. The general workflow is:

1. Select one or more compatible features in the feature tree or on the canvas.
2. In the CAM panel, click Add to open the operation menu.
3. The menu is a vertical list of every operation type. Each row has an info chevron that expands an example card describing the cut. Click the row's add button to create the operation.
4. For operations that support rough and finish passes, choose Rough, Finish, or Rough + Finish.

If the selection is not compatible with the chosen operation type, a hint message explains what is needed. Fix the selection and try again. The hint row also offers a Select all button that selects every feature compatible with that operation in one click — handy when you want to, say, drill every circle or pocket every closed cutout at once.

From the Feature Context Menu

You can also create an operation directly from a feature. Right-click a feature in the feature tree (or on the canvas) and open the Create operation submenu. It lists only the operations that are valid for that feature — a closed subtract feature offers Pocket, Edge Route Inside, and V-Carve; a circle offers Drill; and so on — so you can add the right operation in one step without hunting through the full menu.

Which Operation Do I Need?

Start from what you want to cut. This table maps the common goals to the operation that does the job — click through to its description and parameters below.

Operation Types

Feature Requirements by Operation

Operation Parameters

Select an operation in the list to edit its parameters in the right panel. Selecting an operation also highlights its target features on the canvas and in the feature tree, so you can see at a glance exactly which geometry that operation will cut before you adjust anything.

Common Parameters

Pocket and Surface Clean Parameters

Offset-pattern passes simplify their internal polylines back into arcs and full circles where the geometry allows, with redundant points cleaned up via RDP simplification. The result is shorter, smoother G-code with fewer line segments — especially on circular and rounded-corner pockets.

3D Surface Parameters

3D Surface Rough, Finish, and Cleanup all target an imported model feature. Surrounding add features, subtract pockets, tabs, and clamps are protected automatically. Linking moves between cuts are optimized to reduce rapid travel, and Cut Direction is applied per-side so mixed outer / hole contours all cut in the requested direction.

Waterline Quality Controls

When 3D Surface Finish uses the Waterline pattern, an extra group of quality controls becomes available. These trade extra computation for cleaner steep-wall finishes. The planner now snaps each ring's entry to the matching point on the ring above and below — successive levels enter the cut at the same XY location, eliminating spiral seams down steep walls — and tip-cap paths over rounded apex regions are smoother.

Edge Route Parameters

V-Carve Parameters

Engrave Parameters

Drill Parameters

Booklet (PDF Setup Sheet)

Every operation's parameters include a Booklet field with an Export PDF button. It produces a printable setup sheet for that operation — tool, feeds and speeds, target features, toolpath stats, and a toolpath snapshot. See Operation Booklets for what the document contains.

Feed Reduction

Feed reduction lets a clearing operation slow the cutter only where it is working hardest. It does not change the toolpath geometry or raise the operation's programmed feed; it assigns a lower feed scale to the emitted cutting motion when the cutter is more heavily loaded. Use it to protect a tool through tight or full-width material while retaining the normal feed through easier stretches.

Choose a Mode

Read the Feed Colours

With feed colours enabled in the Sketch view, the toolpath and legend show the feed scales that the operation actually emitted. The legend is scoped to the selected operation and omits levels that do not occur in its toolpath, so the colours shown are the colours that will reach simulation, G-code export, and the operation booklet.

Where It Applies

Feed reduction is available on the clearing operations that expose it: Pocket, Surface Clean, 3D Surface Rough, and 3D Surface Cleanup. The control is grouped with the operation's speeds and feeds settings.

Seeded Circle Clearing

Choose Seeded circles as the Pattern for Pocket, Surface Clean, or 3D Surface Rough when you want the cutter to clear broad open areas with full circles before it finishes the remaining material with offset rings. Each open region at each depth level starts from its own largest clear circle, so the pattern is not tied to one arbitrary entry point or spiral centre.

The initial circles are full cutter paths, not clipped arcs. Once they reach the useful open area, the remaining clearing is planned as normal offset work around the material the circles already removed. This keeps the path covered while preserving the familiar ring finish near walls and islands.

Entry Moves — Helix & Ramp

By default a toolpath reaches each new depth by plunging straight down. That is hard on a cutter that isn't centre-cutting, and it is the loudest, most abrupt thing a router does. Pocket, Surface Clean and 3D Surface Rough can instead ease into the material along a helix or a zig-zag ramp. The controls live under Advanced → Entry in the operation's parameters.

What the Generator Guarantees

• Entries are placed where the tool fits. A helix or ramp is only synthesized inside an area the tool centre can legally occupy, with a margin kept off the wall so the entry groove doesn't score the surface a finish pass is meant to leave.
• It falls back rather than failing. If a helix doesn't fit, the operation tries a ramp; if that doesn't fit either, it plunges — and says so in the warnings list.
• Entries start close to the work. Each entry descends from one clearance above the previous level's floor rather than from global safe Z. On a deep pocket that is a large saving — a 20 mm deep pocket in testing dropped from 4228 mm of entry travel to 1132 mm.
• Existing projects are untouched. A project saved without entry settings generates exactly the same G-code it did before.

Trochoidal Cutting

A trochoidal path replaces one heavy full-width cut with a run of overlapping loops. The tool is only ever engaged over a small arc of its circumference, so radial load and heat drop sharply — you can usually run deeper and faster, and a small cutter survives material that would otherwise snap it. The trade-off is a longer path and a channel wider than the tool.

Trochoidal Edge Route

On a rough Edge Route Inside or Outside pass, set Strategy to Trochoidal. The pass leaves stock for a normal contour finish pass, which is what actually sets the final dimension. A finish pass is always a contour.

Trochoidal Engrave

Engrave was the last operation in the app that cut a full-width slot. Set Strategy to Trochoidal (slot) and it cuts a channel instead. This is a win for T-track, inlay, dado, and wire routing — anywhere the groove is meant to be wider than the cutter.

Trochoidal Parameters

Rest machining is not available for a trochoidal Edge Route: its swept channel can't yet be represented as a rest region.

Corner Relief

A round cutter cannot cut a square inside corner, so a square-cornered part never quite seats in a milled pocket. Corner Relief cuts a small extra excursion at each inside corner to make room for the corner of the mating part. It is available on Pocket and both Edge Route kinds, and is cut as a dedicated pass appended after the main path, at its own step-down levels.

The excursion is sized from the operation's own tool, and it ends where the cutter touches the corner rather than where its centre reaches it — so it removes about as little virgin material as the geometry allows.

When a Corner Is Skipped

The relief pass only descends at a corner when the operation demonstrably already cut there at or below the deepest relief level, so a relief move can never dive into untouched material. A corner is skipped, with an explanatory warning naming its coordinates, when:

• the adjacent edges are too short to hold the relief notch,
• the operation's toolpath doesn't actually turn that corner,
• the operation never reaches full depth there, or
• a tab covers the corner.

If the assigned tool has no stepdown set, the relief pass is skipped entirely rather than cutting to full depth in one go.

Helical Boring

Set a Drill operation's Drill Type to Helical and it bores the hole with a flat endmill instead of drilling it — a spiral down the wall, centre-locked, with no core left in the middle and a finishing revolution at the bottom. This is how you produce a hole larger than any drill in your rack.

• Requires a flat endmill. Any other tool type falls back to a simple plunge with a warning saying why.
• The hole must be larger than the cutter — strictly larger, not equal.
• And no more than twice the cutter diameter. Past that, use Edge Route Inside instead; the operation says so rather than generating something questionable.
• Descent rate comes from the same Ramp Angle (°) field the helix entries use — 5° by default.

V-Bit Countersinking

Set a Drill operation's Drill Type to Countersink, select a V-bit, and enter the Finished Mouth Diameter the fastener needs. PureCut CNC derives the plunge depth from that diameter and the tool's included angle, measured below each target hole's own top surface.

• Requires a V-bit and circular targets. The selected tool's angle and maximum cut depth must support the requested countersink.
• The mouth diameter is the design input. You specify the opening the screw needs rather than calculating a cone depth yourself.
• Invalid conditions stop safely. An unsupported tool, target, or depth produces a warning and no countersink motion for that target.

Rest Machining

When you add an Edge Route Inside or Edge Route Outside operation, PureCut CNC can automatically generate a rest region — a derived feature that represents the material left behind by the first tool that a smaller tool can clean up.

The rest region is created as a separate editable feature. The original operation targets are preserved unchanged. The rest operation targets the generated region with its tool reference cleared, so you can assign a different (typically smaller) tool to it independently.

Reassigning Operation Targets

To change which features an operation applies to, select the new features in the feature tree or on the canvas, then click Use current selection in the operation's properties panel. If the selection is not compatible, a message explains why.

You can include one or more Region features in any operation's target list to restrict where it cuts. Regions don't replace the machining target — they narrow it. With no regions selected, the operation cuts the full extent of its machining target. See Regions for how masked toolpaths are generated and what a region does and does not guarantee.

Reordering Operations

Operations are executed in the order they appear in the list. Drag operations in the list to reorder them. The order affects the G-code output — operations are exported in list order.