User manual · Chapter 3 of 9

Setup

The machine, the piece of stock, the cutters and the materials. Everything later in a job is measured from what is entered here, so it comes first.

Why setup comes first

Two things decide whether a correct drawing turns into a correct part. The machine decides how far the tool can travel, how fast it may move, and what form the G-code file takes. The job decides where zero is: every depth is measured from its Z zero and every position from its XY datum. Get either of them wrong and a perfect toolpath cuts in the wrong place, to the wrong depth, or not at all.

You can change the setup later. Toolpaths made before the change are then flagged as out of date, and Manufacture ▸ Operations ▸ Recalculate All rebuilds them.

Job Setup

Job Setup describes the material you are cutting, not the drawing. It is the Setup tab in the left-hand column, and it is shown whenever you choose the Setup stage. Fill in each card and press Apply. The application then moves you on to the Design stage.

A new job has no stock, and its width, height and thickness boxes are empty. Nothing can be drawn until the job has been applied with a size.

Machine: The machine this job will be cut on. Built-in machines are marked "(built-in)". It sets the travel the job is checked against, the feed limits, and the post-processor that writes the G-code.
Job Type: Single sided cuts from the top only. Double sided adds a second face, cut after the stock is turned over. See Double-sided jobs below.
Job Size: Width (X), Height (Y) and Thickness (Z) of the stock, and Units (mm or inches). X and Y are the sheet as it lies on the bed, seen from above.
Z Zero Position: Material surface or Machine bed. This is where you will touch the tool off, and every cut depth is measured from it.
XY Datum Position: Which corner, or the centre, is X0 Y0. It is the point you jog the machine to before pressing start. Use offset moves the origin away from that point by the X and Y you type.
Modeling Resolution: How fine the grid behind 3D models and the simulation is, from Draft (fastest) through Normal, High (3× slower) and Very High (7× slower) to Maximum (15× slower). It affects 3D work and the preview only. 2D vector cutting is exact at any setting.
Material: What the stock is (MDF, plywood, oak, maple, walnut, pine, acrylic, aluminium, brass or steel) and the Colour it is drawn in. The material is the starting point for feeds and speeds.

Measure the stock before typing its thickness. Sheet goods are rarely their nominal size, and a profile cut to 18 mm through a sheet that is really 17.5 mm leaves no skin while one cut to 18 through a sheet of 18.4 leaves the parts attached.

Front-left is the usual datum because it is the corner you can see and reach. Centre suits round or symmetrical work. Whatever you choose here has to match what you do at the machine.

Material surface is the common choice for Z zero. It copes with a sheet that is not quite its nominal thickness, because depths are measured from the face you actually touched off. Choose Machine bed when the thickness left under a pocket matters more than the depth from the top.

Changing the size later

You can reopen Job Setup at any time, change the size and press Apply again. The Job ▸ Job Setup… window also has Scale existing drawing to fit the new job size. Leave it off when the drawing is a real object at its true size, and turn it on when the drawing is artwork that should fill whatever stock you have.

The Job Setup Wizard

Job ▸ Job Setup Wizard… asks the same questions over four pages, one subject at a time. It produces the same result as the form.

Machines

A machine in Carvect Pro holds what the application needs to know about the real one: its travel on each axis, the post-processor that writes its files, and the limits of its spindle and feed. A few generic machines are built in. Setting up your own takes a few minutes and pays for itself on the first job.

Open Setup ▸ Machine ▸ Machine Library… (also in the Machine menu, and the Change machine button on Home).

Select the built-in machine closest to yours and press Duplicate. Built-in machines cannot be edited or deleted, so you always work on a copy.
Give it a Name.
Under Travel min and Travel max, enter the travel on X, Y and Z. These are what the envelope check compares every job against.
Choose its Post processor. See Post-processors below.
Under Spindle & feed, enter Max RPM, Min RPM, Max feed and the machine's Rigidity. A value of 0 uses the default for that kind of machine. Automatic feeds never exceed these limits.
Tick Automatic tool changer only if the machine changes bits by itself. Without it, a job that uses more than one bit is exported as one file per bit.
Optionally choose a Machine model (STL) so the 3D view shows your machine.
Press Save, then Set as active.

The Machine Builder — verify by jogging panel moves a marker inside the machine's travel in the 3D view. Jog each axis in the + direction; if the marker moves the opposite way to your machine, flip that axis's Direction in the table. Export… and Import… move a machine between computers as a small file. Reset Defaults removes all your own machines and restores the built-in set, so use it with care.

To change the machine for the job in hand, use the Machine card in Job Setup or Setup ▸ Machine ▸ Set Active Machine…. The status bar shows the active machine at all times.

The envelope check

Whenever the stock is larger than the machine's X or Y travel, the machine name in the status bar turns red and gives the axis and the numbers. When you export, the toolpaths themselves are checked against the travel on all three axes and you are warned about anything outside it. Both checks use the active machine, so they are only as good as the travel you entered.

Post-processors

The same toolpath has to be written differently for different controllers. A post-processor is the set of rules that does that. Each machine names the post it uses, and Setup ▸ Machine ▸ Post Library… is where the posts live. Four are built in.

As with machines, duplicate a built-in post to change it. The settings are:

Name, Key, Description: How the post is listed, the short id it is saved under, and a note about what it is for. Changing the key of a saved post breaks jobs that refer to it.
Units: Whether the file is written in millimetres or inches. This is what the machine expects, and it is independent of the units the job was drawn in.
Arcs (G2/G3): Write curves as arc moves. Off, every curve is broken into short straight moves, which works on any controller.
Arc IJK absolute: Whether arc centres are given from the origin or from the start of the arc. If arcs come out as wild loops on a machine that otherwise runs fine, this is the setting to look at.
Line numbers: Number each line, with the start, step and wrap-around value (N start and the maximum).
XYZ dp: Decimal places for coordinates. Three is normal in millimetres, four in inches.
Comments: Whether operation and tool names are written into the file, and in which bracket style.
File ext: The extension exported files get.
Line ending: Windows (CRLF) or Unix (LF).
Modal motion: Leave out a motion word when it has not changed from the line before. Smaller files; turn it off if a file misbehaves part-way through.
Header, Footer, Tool change: The blocks written at the start, the end, and at each tool change. Header 1st toolchange says the header already loads and starts the first tool, so no separate tool change is written for it.

Preview… shows a sample program written with the settings as they stand. Set as default makes a post the one new machines use.

Before cutting anything with a new or edited post, export a short job and compare it with a file you know runs on that machine. The units line and the arc settings are the two that cause most trouble.

The Tool Database

Every toolpath is cut with a bit from the tool database. Open it with Setup ▸ Tool Database.

The bits are listed in a tree: Milling (end mills, ball nose, bull nose, V-bits, engraving, tapered mills, tapered ball, round-over and cove, surfacing), Hole Making (drills, centre drills, spot drills, reamers, counterbores, countersinks) and Other. A picture of the selected bit is drawn from its dimensions, and the dimension you are editing lights up on it.

Each bit has these groups of fields:

Identity: Name, Tool Type and Notes. The type decides which toolpaths accept the bit and how the simulation draws it.
Geometry: Diameter (D), Shank Ø, Flute length, and where they apply the Included angle and Tip Ø of a V-bit or tapered bit, and the Corner (sharp, rounded or hollow) with its Corner radius.
Cutting Parameters: Pass depth (the most this bit should cut in one pass) and Stepover, as a percentage with the length worked out beside it.
Feeds and Speeds: Spindle speed, Feed rate and Plunge rate, with the resulting Chip load shown so you can check it against the maker's figures. The Material and Machine boxes above decide which set of numbers you are looking at, because the same bit runs at different speeds in MDF and in aluminium.
Tool Number & Vendor: The Tool number, Vendor and Part number, kept with the bit for your records and for reordering.

Use Add, Duplicate and Delete to manage the list and Apply to save your changes to a bit. Measure your bits. A cutter sold as 6 mm is often 5.95 mm, and on a fitted joint that difference shows.

To start with a full library, choose Manufacture ▸ Tools ▸ Load Default Bits (Metric) or Load Default Bits (Imperial). The shipped sets hold 63 metric and 57 imperial bits covering the common shapes and sizes. The Tools tab in the right-hand column has Export… and Import… buttons for moving a library between computers. Importing asks whether to Merge the file into your library or Replace it.

The Material Database

A bit has general-purpose numbers. What it should actually run at depends on what it is cutting, and that belongs to the material. Setup ▸ Material Database holds the materials.

A material has a Name, a Kind, the usual Thickness, Width and Length of the stock you buy, a Colour and Notes. Below those is a grid, Cutting defaults, per tool type: for each type of bit, and for a given bit diameter, the Feed, Plunge, Spindle speed, Stepdown and Stepover.

Load shipped materials adds a set of 21 woods, sheet goods, plastics and soft metals, with starting numbers for each. Edit them to suit your machine as you learn what it likes.

Automatic feeds and speeds

With Machine ▸ Auto Feeds & Speeds on (it is on by default, and the same switch is in Preferences), choosing a bit in a toolpath fills its feed, plunge and spindle speed from the job's material and that bit, and holds them within the active machine's limits. The numbers come from published chip-load figures. They are a starting point. Your machine's stiffness and the sharpness of the bit are not in the calculation, so listen to the cut and adjust.

A second setting, Keep the plunge rate within what the bit can take, lowers the plunge rate for small bits in hard material. It never raises anything.

Templates

A template saves the setup you use most: the stock you buy, the machine you own, the tools you reach for and the operations you always run. Starting a job from one skips the setup.

File ▸ New from Template… starts a job from a template. Setup ▸ Machine ▸ Template Library… manages them. Two are built in, a sign-making setup in MDF (mm) and a plywood cut-out setup in 3/4 inch sheet (inches).

To make your own, set a job up the way you like it and press New from Current Job in the Template Library. A template holds a Name, Notes, the Machine and Post, the Job setup, a list of Default tools and Pre-staged operations. Set as default marks the template you use most, and the library opens on it. Apply to New Job starts a job from it straight from the library.

Pre-staged operations wait under Toolpaths ▸ Staged Operations until you have drawn something for them to cut. Select the shapes and apply them from there, or clear the list if you do not need them this time.

Sheets

A job can hold more than one sheet: the two faces of a double-sided job, the boards of a sliced 3D model, or several boards in one layout. Each sheet has its own stock, its own drawing and its own toolpaths.

The Sheets tab in the left-hand column lists them. + adds a sheet, − removes the selected one, and Rename names it. Click a sheet to make it the active one. Show all sheets in view (also View ▸ Show All Sheets) draws every sheet at once so you can see how they relate.

Double-sided jobs

Some parts need cutting from both faces: a sign with a pocket on the back, a tray with feet, a carving finished on both sides. Choose Double sided under Job Type in Job Setup. Two more settings appear:

Flip Direction Between Sides: How you will turn the stock over: Flip left ↔ right (about the Y axis) or Flip top ↔ bottom (about the X axis).
Zero off same side: Keep one Z zero for both sides, set on the same physical face. When it is on, you do not re-zero after the flip.

The bar above the views now shows Side 1 (Front) and Side 2 (Back). Click one to work on that face. Each face has its own drawing and toolpaths. You draw Side 2 as you will see it once the stock is turned over, and Show other side draws the opposite face faintly, mirrored, so you can line features up through the board.

Export handles the mirroring. See Exporting a double-sided job in the Output chapter.

Changing a double-sided job back to single sided asks which side to keep, and deletes the other side's drawing and toolpaths.

Nesting

Nesting packs parts onto the sheet to waste as little as possible. Select the parts and choose Arrange ▸ Nest Parts… or Manufacture ▸ Output ▸ Nest Parts…. The Nesting tab in the right-hand column holds the same settings.

Tool Dia. (D): The bit the parts will be cut out with. Parts are kept at least this far apart so the cutter fits between them. Set it to the largest bit any profile uses.
Clearance (C): Extra space between parts on top of the tool diameter.
Border Gap: How far parts stay from the edge of the sheet. Leave room for clamps.
Rotate parts to find best fit: Allow parts to be turned, in steps of the Rotation step angle. Turn it off for material with a grain or a printed face.
Mirror parts to find best fit: Allow parts to be flipped over. Only safe when the two faces of the part are the same.
Allow parts inside other parts: Let small parts sit in the holes of larger ones.
Nest two-sided parts: Keep a double-sided part's two faces aligned when it is moved.
Remove original parts: Delete the parts from their old places once they are nested. Leave it off on a first try so you can compare.
Sheet Options: The corner packing starts from, and whether rows fill Along X or Along Y.
Use bounds layer: Nest inside a shape you have drawn on a layer instead of the whole sheet, to avoid a damaged area, a knot or a clamp.
Copies: How many of each part to place.

Press Preview to see the layout and the utilisation figure, and Reset Preview to try again. Nesting packs by each part's bounding box. Toolpaths already made from the parts need recalculating after they move.