454 Design: CAM reference

Every toolpath type, setting and check in 454 Design’s CAM, by topic. For a walkthrough from drawing to G-code, see the Design quick start.

CAM is in beta. Toolpaths are new and still being tested on real projects, which is still finding problems. Check every job before cutting material: open it in 454 Control and watch the preview all the way through, read the Checks tab, then run it in the air with Z zeroed well above the material. Every G-code file 454 Design saves starts with a note saying so. If something looks wrong, report it on GitHub (opens in a new tab), with the drawing if you can.

On this page: The basics · Profile · Pocket · Drill · Chamfer · V-carve · Inlay · Finishing, direction, leads, tabs, ramps · Tools and materials · Make toolpaths · Order, checking and saving · VCarve projects · How the toolpaths are checked

The basics

The Toolpaths panel sits on the right. Select shapes on the drawing, then press New toolpath (the + icon). The editor takes the panel’s place while it’s open, a little wider, so the drawing stays in view. It works nothing out while you change settings, as VCarve’s doesn’t: Create or Update works the toolpath out once, with a Working… panel. A V-carve’s depth, and warnings that need the toolpath worked out (a cutter too big for a pocket, say), show on its card after that. Its settings sit under headings (Tool, Depth, Passes, Entry and exit, Tabs), and only the ones that apply to the kind of cut are shown. Click or tab into any setting and the box above the buttons says what it does, with a small picture for stepover, ramp, lead in and tabs. Press Create to add the toolpath, or Cancel, and the list of toolpaths comes back. Each toolpath gets a card in the panel, where you can edit it, move it up or down, show or hide its preview, leave it out of the G-code, recalculate it, or delete it. Right-click a card for the same actions in a menu.

The row of icons under the panel’s name holds what you do with the whole job: Preview in wood, Preview in 454 Control and Job sheet, then Save template and Apply template. Rest the pointer on one to see its name; the ⓘ at the end of the row explains them. Save G-code… is the wide button under the list.

Naming a toolpath. Type a name in the editor’s Name box, or double-click the name on a card (or right-click it and choose Rename…), type, and press Enter. The name is shown on the card and the job sheet and written into the G-code, so 454 Control shows it too. Leave it empty and the toolpath is named after its kind of cut, such as “Outside profile”; the kind of cut is always shown on the line under the name.

Folding cards. The small arrow at the left of a card folds it to its title, so a long list fits on the screen; the arrow opens it again. The button with three lines in the panel’s header folds or opens every card at once. A folded card shows ⚠ beside its name when the toolpath has a warning, such as cutting past the material: hold the pointer over it to read why.

Recalculating rebuilds a toolpath from its shapes and the material as they are now, keeping its own settings (tool, depths, feeds). The Recalculate button (↻) on each card is highlighted when a toolpath is out of date, because its shapes or the material changed since it was made; Recalculate all in the panel’s header does every toolpath at once. A toolpath keeps its own copy of the tool’s feeds and speeds, so after changing a tool in the library, edit the toolpath to pick up the new values.

Nothing is guessed. A new toolpath starts with no tool and no depth, and Create stays disabled until you’ve chosen both. G-code can’t be saved while any toolpath has no tool. Z zero, the material’s thickness and where X0 Y0 sits all come from Job setup.

The hint under the editor’s settings says what the toolpath will do in plain words (depth, passes, rings, tabs, finishing), and starts with ⚠ when something is wrong. Read it before pressing Create.

Cutting past the material is always said. Every toolpath is checked against the material’s thickness (Job setup), from the deepest point it really cuts, whatever kind it is and however its depth was set. One that goes past the bottom says so with ⚠ in the editor’s hint and on its card: “goes 15.00 mm deep: through the 12.00 mm material and 3.00 mm into the spoilboard”. Save G-code and Preview in 454 Control stop and list them first, with Cancel or Save anyway (cutting into the spoilboard is sometimes meant). A change that puts a toolpath through, such as a thinner material or a parameter, names it straight away. A through cut’s own overcut is meant, so it isn’t flagged. If the material’s thickness isn’t set, depths can’t be checked, and Save G-code says so.

Two pockets in 12 mm material. The first takes its depth from the material, so it can't go through. The second was typed as 15 mm, and its card says what that means.

Save G-code stops first and names each toolpath that goes past the bottom. Cancel to fix it, or Save anyway if cutting into the spoilboard is what you want.

Depth and tabs from parameters. The Depth, tab Length and tab Thickness boxes take a parameter, or arithmetic with one: material / 2, dado_depth, tab_thk. The toolpath remembers it (its card shows 9.00 mm = material / 2) and is recalculated when the parameter or the material changes. A depth from a parameter needs the material’s thickness set, so it can always be checked. If a toolpath’s parameter can’t be worked out (it was deleted, or the thickness was cleared), its card says so and Save G-code refuses until it’s put right. Arithmetic without names (6 + 2) is just worked out, and a plain number unlinks the box.

Any closed shape can be cut: rectangles, circles, closed outlines, groups (such as a traced logo) and text. A group’s outlines, or a word’s letters, count as one shape.

Same as VCarve

Toolpaths are made from selected vectors, listed in the order they’ll run, and saved together as one G-code file with tool changes.

Groups

Groups keep toolpaths that belong together under one name, such as an inlay’s pocket and its clearing, or every cut on one part.

• Make one: click a toolpath card, then Ctrl+click the others, then right-click one of them and choose Group these toolpaths. Type the group’s name and press Enter. A single toolpath’s right-click menu also has Make a group of this toolpath, Add to each group on the sheet, and Take out of its group.
• The group’s header line folds the group to that one line (the arrow, or a click on the line), ticks all its toolpaths in or out of the G-code (the tick box shows a dash when only some are in), shows or hides them all on the drawing (the eye), and says how many it holds. Double-click its name to rename it. Folded, it shows ⚠ if any of its toolpaths has a warning; rest the pointer on it to see which.
• Right-click the header to recalculate the whole group, Save G-code for this group… (one file with just its ticked toolpaths, named after the group), move the group earlier or later, Ungroup (the toolpaths stay, in the same order), or delete the group and its toolpaths.
• In the cutting order a group’s toolpaths always stay together. The arrows on a toolpath in a group move it within the group; a toolpath outside a group steps past a whole group at once. Drag a group by the dots on its header to move it. Drag a card onto a card in a group to put it in that group, or onto a card outside any group to take it out.
• One sheet: a group’s toolpaths are all cut from the same piece of material, so a group holds toolpaths from one sheet only.

Profile

Cuts along an outline. Choose Profile, outside (the part keeps the outline’s size), Profile, inside (a hole keeps its size), or Profile, on the line (the cutter’s centre follows the line).

Profile, outside, cutting through, with four tabs. It's selected here, which is when its tabs are drawn.

Setting	What it does
Cut depth	How deep, from Z zero. Or tick through to cut the material’s full thickness.
Overcut	With through: how far past the bottom of the material to cut, so parts come free cleanly.
Per pass	The depth of each pass. Filled from the tool’s feeds and speeds for the chosen material.
Passes	How many passes the cut takes, with the depth each one reaches listed underneath (“1.50 · 3.00 · 4.50 · 6.00 · 6.35 mm”). It follows Cut depth and Per pass as you change them. Type a number and the depth is divided into that many even passes: Per pass changes to match. When the last pass would take much less than the others, the editor says so and offers Make them even.
Feed	Cutting speed. Also from the library; plunge rate and spindle speed come with it.

Profiles also take finishing, direction, leads, tabs and ramps.

Pocket

Pocket (clear the area) removes everything inside an outline to a depth. Islands are automatic: shapes inside the pocket’s outline (a letter’s hole, a boss) are left standing.

Offset rings: each pass follows the outline's shape, working outwards from the middle to the walls; the island is left standing.

Raster: straight passes back and forth, then one pass round the walls and the island.

Setting	What it does
Cut depth, Per pass	As for profiles.
Stepover	How far apart the clearing passes are, as a share of the cutter’s diameter. 40% is the default.
Clearing	Offset rings work outwards from the middle, following the pocket’s shape. Raster runs back and forth in straight lines at the angle you set (0° left to right, 90° front to back), then once round the walls. Raster is often quicker on long or rectangular pockets.

Pockets ramp into each depth by default (see Ramps), and link passes with short feed moves only where the cutter stays inside the pocket; otherwise it lifts, moves and ramps back in. Pockets also take finishing and direction.

If the cutter is too big for part of a pocket, that part is left and the hint says so. A narrow strip the cutter can’t reach needs a smaller tool.

Clearing with a larger bit, then a smaller one

A large bit clears a big pocket quickly but leaves its corners round and can’t get into narrow parts. A small bit reaches them but takes a long time over the whole pocket. Use both:

1. Make the pocket with the large bit, as usual.
2. Select the same shapes and make a second pocket with the small bit. Under Clean up after, choose the large bit’s pocket.

The small bit then cuts only where the large one couldn’t reach: the corners it left round, and any part too narrow for it. Typically that’s a quarter of the cutting a full pocket with the small bit would take, or less. The clean-up goes as deep as the large bit’s pocket, runs after it, and follows it if you change it.

Clean up after lists pockets on the same shapes with a larger bit. If that pocket is deleted, changed to other shapes, or unticked, the clean-up says so; if it’s deleted, the clean-up clears the whole pocket, so nothing is left uncut.

Same as VCarve

This does what VCarve’s larger clearance tool and rest machining do.

Drill

Drill at centres drills at the centre of each selected circle, taking a short way round them.

Drilling: a ring at each hole, and the dashed rapids show the order, a short way round them.

Setting	What it does
Cut depth or through	How deep each hole goes.
Peck	How far to drill before lifting to clear chips. 0 drills each hole in one plunge.

Different from VCarve’s post

GRBL has no drilling cycles (G81, G83), so drilling is written as plain moves. It runs the same way; the G-code is just longer.

Chamfer

Chamfer edges (V-bit) bevels an edge with a V-bit.

A chamfer is one pass along the edge: the V-bit's depth sets the bevel's width.

Setting	What it does
Bevel width	How wide the bevel is on the top face. The depth follows from the bit’s angle.
Bit	The V-bit’s included angle, filled from the library.
The line is	the part’s edge (tip on it): the bevel runs down to the line. the bevel’s top, going inside or going outside: the line is where the bevel starts, as VCarve’s “vectors at top”. Going inside countersinks a hole to its drawn size.

A bevel wider than the bit can cut is refused, with the reason in the hint.

V-carve

V-carve (V-bit) carves text, logos and artwork with a V-bit. The bit’s tip follows each shape’s centre-line, deeper where the shape is wide and rising to the surface at sharp points, so the carving’s edges land exactly on the outline and corners come out sharp. There’s no depth to set: the shape decides it.

V-carving “454”: the tip follows each stroke's centre-line, reaching out into the corners.

Setting	What it does
Bit	The bit’s included angle, from the library: a V-bit, or a tapered ball nose (its cone ends in a small ball; VCarve’s libraries store it as twice the angle on the bit’s name, so a “5.4°” bit is 10.8° here).
Max depth	Optional. Deeper than this, the carving gets a flat floor. A clearing pocket is added with it for the flat middles, runs first, and follows if you change the max depth; open it and choose its end mill.
Tip	The width of the bit’s flat tip, if it has one (engraving bits usually do). From the library. Lines narrower than the tip stay at the surface. For a tapered ball nose it reads Tip radius: the radius of its ball.

Warnings in the hint: the tool isn’t a V-bit; the carving is wider than the bit can make (set a max depth, or use a larger bit); or it would go deeper than the material.

Floor the clearing cutter can’t reach. An end mill is round, so it can’t get into the corners of the flat floor, or into any part of the floor narrower than itself. The V-bit goes back and flattens those places: straight down to the floor’s depth, then back and forth with its point, in passes 0.127 mm (0.005 in) apart. Its card says so: Floor: also flattens what “…” can’t reach. A pointed bit leaves fine ridges between its passes (about 0.1 mm high with a 60° bit, 0.25 mm with a 30° one), and a smaller clearing cutter leaves the V-bit less to do. This happens for a V-carve whose clearing pocket was added with it, and for an inlay made in this version or later. Change the clearing pocket’s cutter and the V-carve is worked out again.

Same as VCarve

Flat depth with a clearance tool works as VCarve’s does: clearing runs before the V-carve, and the V-bit flattens what the clearance tool couldn’t reach, going straight down to the floor’s depth there as VCarve’s does.

Inlay

The Inlay wizard makes both halves of a V-carve inlay from the same shapes, so they fit: the pocket in the base, and the plug, mirrored, in the inlay piece. Select the shapes, press + at the top of the Toolpaths panel (or the + key) for a new toolpath, and choose Inlay. Cut both halves with the same bit: a V-bit, or a tapered ball nose. The plug’s fit and the clearing allow for the bit’s real shape, ball tip included.

The pocket in the base (left), and the plug (right), which Design makes on a mirrored copy with its boundary, on an “Inlay plug” layer beside the design.

Setting	What it does
Carving bit	Choose… the V-bit or tapered ball nose from the tool library. Its angle, tip, and feeds and speeds for the material you’ve chosen come with it.
Clearing end mill	Choose… the end mill that clears the flat floor. A smaller one leaves the V-bit less to finish.
Pocket depth	How deep the pocket’s flat floor is. 5 mm to start.
Plug start depth	How deep the plug’s walls begin. The plug seats this deep in the pocket. 2.5 mm to start.
Plug depth	How deep the plug is carved. More than the start depth, so it stands proud. 5 mm to start.
The plug on a sheet of its own	Ticked to start: the plug’s mirrored copy and its boundary go on a new sheet, Inlay plug, its own piece of material with its own G-code file. Untick it to put the plug beside the design instead.

Under the depths, the wizard says how it fits, and anything that stops it (no bit chosen, a plug depth less than its start depth, deeper than the material). It remembers what you chose for next time.

Create makes two groups of two toolpaths each: Inlay pocket (its clearing pocket, then its V-carve) and Inlay plug (the same, on the mirrored copy inside its boundary). All of it is one step to undo.

The V-bit finishes the floor. Where the clearing cutter can’t get into corners or narrow parts, the V-carve flattens them, so the plug seats. An inlay made before version 0.6.2-beta.44 doesn’t have this: make it again.

How it fits: flipped into the pocket, the plug wedges on its walls at the start depth, leaves pocket depth − start depth underneath for glue, and stands plug depth − start depth above the surface to plane off. The hint states all three.

Trim the inlay piece to the boundary before gluing. Stock left outside it hits the base and stops the plug seating.

Finishing, direction, leads, tabs, ramps

These settings appear in the editor for the toolpath types they apply to. Here, a profile’s editor with tabs and arc leads switched on:

Finishing

Profiles (inside and outside) and pockets: Finishing — leave an amount on the walls during the roughing passes, then, with then finish it ticked, take it off in one pass at full depth. The cutter is barely loaded on that pass, so walls come out cleaner and truer. Untick it to leave the material for another toolpath or tool.

Direction

Profiles, pockets and chamfers: Climb (the default) usually leaves the better finish on a rigid machine; Conventional can suit flexible setups or brittle material.

Lead in/out

Inside and outside profiles: Arc (a quarter circle that meets the line tangentially) or Line (at 45°), sized by the box beside it (the cutter’s diameter by default). The cutter sweeps onto the line from the waste side and off it again, so no pass starts or stops on the finished wall, and the path starts mid-way along the longest straight edge.

• Passes that ramp in get only the lead-out: the ramp is already a gentle way in. Passes that plunge (Ramp in set to Plunge), and a finishing pass, which drops straight into the roughed slot, get both.
• In a tight hole the lead shrinks to fit, and is left out if even a small one would touch the wall.

Start point

Profiles (outside, inside and on the line): Start says where each shape’s cut begins. Automatic starts at a corner of the path, or with leads in the middle of the longest edge. To choose, press Set start and click the outline where you want it: on an edge that’s cleaned up anyway, at the grain end, or away from a detail, so the small mark where each pass begins lands somewhere harmless. One start per shape: click again to move it. Press Done when finished, or Automatic to go back. The start shows on the drawing as a ring with a dot. Lead-ins, ramps and tabs work from the chosen start, and a start on a tab never cuts into it.

A chosen start: the ring with a dot, on the top edge. Each pass of this profile begins there.

Tabs

Profiles: tick Add tabs, then either click Edit tabs and click the outline to add a tab (click a tab to remove it), or type how many and press Add to space them evenly round each shape. Clear removes them all. Set their Length and Thickness. Both are the wood a tab leaves holding the part: the length along the middle of the cut, whatever the size of the bit (the bit stays up for the tab’s length and its own width, so its round ends don’t eat into the tab), and the thickness measured up from the bottom of the material, so a cut through with an overcut still leaves the full thickness. Choose their Shape:

• Flat (the default): the cutter steps straight up at one end of the tab, runs level across it, and steps straight down at the other end, leaving a small flat-topped bridge.
• 3D (tapered): the cutter ramps up from the cut’s floor to the tab’s full thickness at its middle, and back down to the floor, leaving a triangular bridge as long as the tab’s length. 3D tabs are easier to cut through when freeing the part, and leave a smaller mark to clean up.

Either way, only the passes below a tab’s top go over it, and tabs are kept on finishing passes too.

A new toolpath starts with the tabs you used last: their number, length, thickness and shape. The first time, that’s 4 tabs, 4 mm long and 1.5 mm thick, flat. Thin tabs can let a part break free while the cutter is still going round it, so check the thickness suits the wood before you cut. Preview in wood shows tabs in amber.

Ramps

Profiles and pockets: Ramp in sets how each pass goes down into the material.

• Ramp (the default): the cutter slopes down along the cut over the length in the box beside it, as fast as the cutting feed allows with the bit coming down no faster than the plunge rate. On a long, gentle ramp that’s the cutting feed; on a short, steep one it’s slower. Leave the box empty for four cutter diameters (at least 4 mm), which follows the cutter if you change it; type a length to set your own. On a profile the passes run into each other without stopping: each lap ends back at the start and the cutter carries straight on, ramping down to the next depth as it goes. After the last pass it carries on past the start and cuts the ramped stretch again at full depth, so a through-cut never leaves a sloping web holding the part. Pockets ramp along their rings, or back and forth along a line when rastering. Converted VCarve toolpaths keep VCarve’s ramp length.
• Ramp, slowly: the same ramp, at the plunge rate all the way down, as before Design 0.152.0. For a cutter or wood that needs it gentler.
• Plunge: the cutter goes straight down at the plunge rate, then cuts. Use it with a cutter that can plunge (a centre-cutting end mill), and a plunge rate to suit.

Ramping is easier on the cutter and the machine than plunging, especially in hardwood and with small cutters. On a profile, a ramp is different from a lead: a ramp comes down along the line; a lead comes onto the line from the side, at depth. The toolpath’s card and the job sheet show which it does (Entry), and the hint under the settings says how far it ramps.

Any cut that slopes down, such as down the side of a 3D tab, comes down no faster than the plunge rate either.

Tools and materials

Choosing a tool opens the tool library. Pick the machine and material in its bar; the toolpath takes that tool’s feeds and speeds for that material. Recently used at the top holds your last six.

• Edit a tool: name, type, units, diameter, angle and flat tip for V-bits, flutes, notes, and its tool number on the chosen machine.
• Feeds and speeds are per material: with a material chosen, Edit shows that tool’s feed, plunge, spindle speed, pass depth and stepover for it. A material with none yet offers Add feeds, started from another material’s (a note says which, and in which units).
• + Tool, Duplicate, Delete, + Material, and Import VCarve library… (reads VCarve’s tools.vtdb). No VCarve? Start an empty library.

Toolpaths keep their own feeds. Editing the library doesn’t change toolpaths already made, so a job you’ve checked can’t change under you. Choose the tool again in a toolpath to take the new values. The library lives in this browser and is shared with 454 Control.

Make toolpaths

The wand button at the top of the Toolpaths panel looks at the drawing and proposes toolpaths for it. Nothing is added until you’ve read the summary and pressed Add.

• Holes, slots and cut-outs (a closed shape inside a part) are cut through, round the inside.
• Round holes the size of a bit in your tool library are drilled with that bit, a toolpath for each size. Deep ones (more than three times the bit’s width) are pecked.
• Parts (a closed shape inside nothing, or inside a hole) are cut out through, round the outside, with the tabs you used last.
• The bit is the one you used last, with its feeds and speeds from the tool library. Choose another in Cut with, and the summary is worked out again for it.
• Each one is worked out before it’s offered, with its depth and a time estimate, and anything worth knowing: deeper than the bit can cut, or feeds the library didn’t have (and what was used instead).
• Left out, and said why: text (V-carve or profile it yourself), open shapes, shapes a toolpath already cuts, holes narrower than the bit, copies stacked on another shape, outlines that cross or double back on themselves, and outlines drawn round a part closer than the bit is wide (an offset copy). Construction lines and hidden layers are left out quietly. With no material thickness set, nothing is made: every cut goes through it.
• Untick any you don’t want, then Add. They go in the usual cutting order, as one step that Undo takes back. Check them in Preview in wood, and air-cut the first job.

Order, checking and saving

Order

A new toolpath slots into the usual cutting order: holes, chamfers, pockets, V-carves, inside profiles, on-the-line profiles, outside profiles, so the part is held until the end. Reorder with the arrows on each card; an order you’ve arranged is kept, and editing never moves a toolpath. A toolpath that would run after the outside profile has cut the part free gets a warning.

Within a toolpath, the shapes are cut in a short way round them, starting from X0 Y0, not in the order you picked them. A shape inside another (a hole in a part, with both in one profile) is cut first, so the part isn’t freed before its holes are cut. This goes for drilling, chamfers and profiles. Between them, the bit lifts 6 mm, or less inside a part if you set Lift inside a part in Job setup.

Check

Check looks over the drawing before cutting: open shapes, shapes in pieces, doubled shapes, crossings, and shapes no toolpath cuts. It lists what needs a look, selects those shapes on the drawing, and offers to fix the ones it can.

Preview in wood

Preview in wood, the first icon in the row at the top of the Toolpaths panel, shows the material as it will look after the ticked toolpaths, as a block of wood in 3D: pockets with their floors and rounded corners, V-carving with its slopes, tabs holding the parts, and through-cuts showing the spoilboard underneath.

Drag to turn it and look from any side, right-drag (or Shift+drag) to move it, and scroll to zoom. The cube in the corner turns with the block: click a face (Top, Front, Right…), an edge or a corner to look from there. Reset view puts it back as it opened. On a computer that can’t show 3D, it shows the same thing from above, shaded.

Watch it cut. Under the picture, Play starts from uncut wood and cuts the toolpaths in order, with the bit shown at its real size and shape, lifting and plunging as it will. Turn the block, zoom, or click the cube while it plays, to watch from any side. Pause holds it, and the slider goes to any moment of the job, back or forward. This shows what the finished piece can’t: the order things are cut in, and where the bit travels between cuts. Speed starts at whatever plays the whole job in about 45 seconds; choose Real time to see it as the machine would do it. The clock is the job sheet’s estimate, so a real job runs somewhat longer. (Where 3D can’t be shown, it plays from above, with a ring for the cutter: blue while it’s in the wood.)

It’s worked out from the toolpaths’ own moves, in order, each cut by its bit’s real shape: a flat end mill, a ball-nose (from the tool library), or a V-bit at its angle and tip, on a grid about 0.1 mm fine for a small job. So a wrong depth, a pocket that leaves an island, or a part with no tabs shows here before any wood is cut. It also says the deepest cut, and warns in red if a rapid move would cut wood.

Use it as well as, not instead of, the preview and air run in 454 Control, which check the G-code itself with the machine’s own limits.

Saving G-code

Save G-code… writes every included toolpath to one file, in order, with a tool change wherever the tool changes, numbered from your library, and each toolpath’s name so 454 Control can show which one is running. It refuses while any toolpath has no tool chosen.

One file per bit: when a job uses more than one bit, Save G-code asks whether to save One file (454 Control stops at each bit change and says which bit to fit) or One file per bit. Per bit, you pick a folder and it saves a file for each stretch of the job cut with one bit, in cutting order, named so they sort in order: Sign - 1 of 3 - T1 6.35 mm cutter.nc, Sign - 2 of 3 - T2 60° V-bit.nc, and so on. A bit used again later gets another file rather than moving its cuts earlier, so nothing is cut out of order (a profile that frees a part never comes before the carving on it). Each file says at the top which file it is. Run them in order, and keep Z zero and XY zero the same between them. It asks before replacing files already in the folder.

Templates: for jobs you make again and again (signs, boxes, cutting boards), Save template (the fourth icon in the row at the top of the Toolpaths panel) saves the toolpaths’ settings to a file: bits, depths, passes, feeds, tabs, ramps, finishing and their order, but not the shapes. Apply template (the fifth icon) makes them again in another drawing. Each toolpath finds its shapes by the name of the layer they were on, so draw the parts of the job on layers named for what happens to them (say “Carve” and “Cut out”), and use the same names next time.

Before making anything, it lists each toolpath with the shapes it found, and any it can’t make (no layer of that name, or nothing on it). They’re added after any toolpaths already there, with tabs spaced evenly, and Undo takes them all back. Depths that cut through use the new drawing’s material thickness, so set that first, and check each toolpath before cutting.

Preview in 454 Control, the second icon in that row, loads exactly the G-code Save G-code would write into 454 Control, for its 3D preview and playback, its time estimate (with your machine’s acceleration) and its checks, with no file to save or open. Nothing is sent to the machine. If Control is already open, the job goes to it, without reloading it or disconnecting the machine; in the desktop app its window comes forward, and on the website the job is waiting in your Control tab. If Control isn’t open, it opens with the job. While a job is running on the machine, Control keeps its loaded file and says so.

Same as Carbide Motion

The G-code is plain GRBL: tool changes are M6 with a T number, which 454 Control and Carbide Motion both handle with their tool-change routine.

Job sheet

Job sheet, the third icon in that row, puts everything about the job on one printable page, to keep at the machine: the material and its thickness, a picture of the job to scale with each toolpath numbered where it starts, a setup checklist (where to zero X, Y and Z, the first tool, how far the cutting reaches so clamps stay clear), the tools, every toolpath in cutting order with its tool, feeds, depths and estimated time, and anything that needs attention. Click the job name or Notes to edit them before printing; Print… prints it, or saves it as a PDF.

The top of a job sheet. The tools, the toolpaths in cutting order, and notes follow.

The tool numbers (T1, T2…) are the ones in the G-code, and the sheet describes exactly what Save G-code will write: toolpaths left out of the G-code are left out of the sheet too, and any that are out of date are recalculated first. In a multi-sheet project, it covers the chosen sheet.

Note

The times are estimates at the programmed feeds, without acceleration, so real jobs run somewhat longer. 454 Control’s estimate, which uses your machine’s own settings, is closer.

VCarve projects

Opening a VCarve .crv brings in its drawing, material and zero, and its toolpaths as previews. Make these editable converts them into 454 toolpaths, keeping VCarve’s tools, depths, passes, feeds, order and settings:

• Profiles, with tabs, ramps, allowance and direction
• Pockets, including raster clearing and its angle
• Drilling, and chamfers in both of VCarve’s modes
• V-carves, with the bit’s angle and tip, the start depth and the flat depth
• V-carve inlays cut with a second tool for the floor: the V-carve, and its clearing pocket, as a pair

Depths, feeds and the cutter’s size are the project’s own, whether it’s in inches or millimetres. If 454 can’t read a toolpath’s depth it doesn’t convert that toolpath, and says which: it never makes one up.

Inlays come across as a pair: the V-carve and its clearing pocket, linked, so the V-bit flattens the floor the clearing tool is too wide to reach, in passes as far apart as the project’s V-bit says, as VCarve’s does. Check it in Preview in wood before cutting.

How shapes are found: each toolpath in a VCarve project records what it cuts, by VCarve’s own IDs: a shape, a block of text, or a group, and 454 reads that record. It doesn’t depend on where anything is, so it works even if parts were moved after VCarve last calculated. For a project without that record, 454 falls back to matching VCarve’s saved toolpath previews to the shapes; if nothing matches, the toolpath comes across with no shapes: open it with Edit and pick them. (On a big project that matching isn’t tried: it would take minutes.) A toolpath whose shapes have been deleted from the project since it was calculated comes across without them too.

Text: VCarve keeps text as text, and 454 puts each letter where VCarve does, as outlines: straight text in lines, set left or centred, fitted to a box or not, and text on a curve. Text set to the right, or on a curve with unusual settings (off the curve, or not filling it), is left out, and 454 says which. To bring that in, select the text in VCarve, use Convert Text to Curves, save a copy, and open the copy.

Lines, arcs and open shapes: a single line or arc comes across as one, and an open shape stays open.

Material and zero: the material’s size and thickness come from the project, with XY zero where the project has it: a corner or the centre.

Multi-sheet projects: each sheet comes in as a sheet, named as in VCarve, with one shown at a time. Choose the sheet at the top of the Toolpaths panel: it shows that sheet, lists its toolpaths, and Save G-code saves that sheet only, named for it. Each sheet is its own job, cut from its own material, so a toolpath can’t mix shapes from different sheets. See Sheets for adding your own.

Check converted jobs

Conversion is careful, but read each toolpath’s hint and run Check before cutting, as you would with any new job.

How the toolpaths are checked

Every toolpath type is tested the same way before release: every point along every move is checked to keep the full cutter radius from every wall and island, and every reachable point is checked to be cut. V-carves and inlays are checked against exact answers (a V-carved 10 mm bar comes out 8.662 mm deep against an exact 8.660), and an inlay’s fit is proved by simulating both halves and pushing the plug in. Converted toolpaths are compared with VCarve’s own paths.