1. Quick Start — your first part#

We are going to make a coaster: a 100 mm disc with a shallow recess in the face, cut from 12 mm stock and held in by tabs so it doesn't fly off the table on the last pass.

It is a small job, but it uses every part of the app you will use on every job after it — stock setup, the tool library, two operations, the simulator, and export. Allow about twenty minutes.

What you need: a browser. Nothing to install, no account. Work is saved to your own computer as a .fkam file when you ask for it.

The finished project is 01-circles.fkam — download it and use the toolbar's Open button if you get stuck, or to compare against what you built. Build it yourself first, though: the point of this chapter is the doing.

The app at a glance#

Open the app and this is what you get — an empty project on a default piece of stock.

Five regions, and everything in this guide happens in one of them:

The Draw tab is the menu for everything#

The sidebar's Draw tab holds three groups, and every job is a matter of picking something from one of them:

• Draw — Pen for freehand paths, Text for lettering, and a shape button. The shape button shows whichever shape you used last (Circle in the picture); click it to arm that shape, or click the chevron beneath it to open the shape picker.
• CAM Operations — the nine ways of cutting: Profile, Trochoidal, Pocket, Drill, Surface, V-Carve, Photo V-Carve, Inlay, 3D Profile. Select geometry first, then click one.
• Path Tools — the six ways of changing geometry rather than cutting it: Boolean, Offset, Pattern, Nest, Tabs, Corners.

Clicking any of these replaces the menu with that tool's form. Fill it in, press the button at its foot, and close it with the × in its header to come back to the menu. That one gesture — select something, click a tool, fill in the form, close it — is the whole app. The rest of this chapter does it four times.

Nothing is offered that can't work: an operation only lists tools from your library that can actually make the cut, and one needing a closed shape says so rather than failing later.

The shape picker#

The chevron under the shape button swaps the sidebar for the picker:

Eighteen shapes and the clock designer, in three families:

Click one and the picker closes, that shape is armed, its parameters appear under the Draw menu, and a banner across the canvas tells you what the next click will do — "Drawing Circle — click to place, drag to size from the centre, Esc to cancel." The status bar bottom-left changes from Mode: Select to Mode: Circle so you always know what a click is about to do. Esc puts you back to selecting.

The button then remembers that shape, so drawing another takes one click, not two.

Gear, Escapement, Pendulum and Track ignore drag-sizing. They are placed at the size their own parameters give them — a gear's size comes from its module and tooth count, a pendulum's from the beat you want, a track piece's from what it has to connect to. Dragging cannot make a gear that meshes wrong.

1. Set up the stock#

Before anything else, tell the app what is on your table. The stock is the reference everything else is measured from — cut depths, the origin, the simulation, and the warnings you get at export.

Click Setup in the sidebar tab bar (next to Draw and Paths). The sidebar fills with the setup panel, and the 2D view keeps showing the stock so you can see your edits land as you make them.

Set:

Under Work Origin, pick where X0 Y0 sits on the stock. The bottom-left corner is the default and is what most hobby machines are jogged to. Leave Z Origin on Top of stock — Z0 at the surface, cuts going negative, which is what you get when you zero the bit on the workpiece with a touch plate or a piece of paper.

Under Material, choose the wood you are actually cutting. It is not cosmetic: the material's hardness feeds the automatic feeds and speeds, and it drives the chip-load warnings later.

Close the setup panel with the ×.

Stock, origin and material — everything else in the project is measured from these.

Working in inches? Click the units button in the toolbar and type inches instead. It changes what you see and type, never what is stored, so you can flip back and forth at any time and share the file with someone working in mm.

2. Draw the coaster#

Go to the Draw tab.

1. Click the shape button under DRAW. If it isn't already showing Circle, click the chevron beneath it and pick Circle from the picker.
2. Set Radius to 50 in the parameters that appear below.
3. Click once in the middle of the stock on the canvas.

The circle is placed at the size you typed, centred on where you clicked. (You could also have dragged to size it by eye — click places at the typed size, drag sizes interactively.)

Now the recess:

1. With the Circle tool still active, change Radius to 40.
2. Click again on the same point. Because a click always centres the shape on the cursor, the two circles come out concentric.

You now have two paths. Press Escape to leave the shape tool and return to select.

From centre is about dragging, not clicking. Tick it and a drag grows the shape outward from where it started instead of running corner to corner — drag repeatedly from one point and you get concentric shapes without measuring. It also makes the shape resize about its middle afterwards. It rides with each object, so you can change it later from that object's properties.

Both circles are still shapes, not frozen outlines — each chip in the Objects strip reopens the editor that made it.

Click either circle and the Properties panel gives you back Radius, not a frozen outline — that stays true for the life of the project.

3. Check your tool#

Click the Tool Library tab above the canvas. The library ships with a starter set of cutters and is saved both with the project and in your browser between sessions.

Find a 6 mm end mill, or add one with +. What matters for this job:

An operation only lists the tool types that can do its job. Pocket offers end mills and ball noses; V-Carve offers V-bits and tapers; Drill offers drills. So if a cutter you expected isn't in the list, it is the wrong type for that operation — not the wrong size. Max Z never hides a tool; it warns you in the depth field instead.

Return to the 2D View tab.

4. Pocket the recess#

Select the inner (80 mm) circle on the canvas.

In the Draw tab, the lower half of the sidebar is the operation menu. Under CAM Operations, click Pocket.

Set:

Click Generate Toolpath.

The toolpath appears on the canvas, and a chip for it appears in the Ops strip along the bottom.

The auto strategy rasters the open ground and contours the boundary.

5. Add holding tabs#

If we cut the outline now, the coaster comes free on the last pass and gets thrown by the cutter. Tabs are small bridges of uncut material that hold the part in place until you cut them with a chisel.

Select the outer (100 mm) circle. Under Path Tools, click Tabs.

Click Apply Tabs. Four tabs appear on the circle, evenly spaced. Drag any of them along the path to move it — put them where you would rather have the cleanup work.

Tabs are attached to the path, not to an operation, and they get their own chip in the Objects strip. Any profile cut on this path will honour them.

6. Cut the outline#

With the outer circle still selected, click Profile under CAM Operations.

Cut side is the field to get right. Outside leaves the part at the size you drew. Inside is for holes — the drawn line is the finished wall of the hole. Centerline runs the tool's axis down the line, which is what you want for a groove, and takes half the tool width off each side of your geometry.

Click Generate Toolpath.

The four breaks in the outer path are the tabs — the material that holds the coaster in the sheet until you cut it out by hand.

7. Check the order#

Look at the strip under the canvas. It has two tabs, and they are not the same thing:

• Objects is your document — one chip per thing in the project. The two circles, the tabs, the pocket, the profile. Click a chip to select the thing and reopen the editor that made it.
• Ops is your program — one chip per toolpath, in the order the machine runs them, which is the order they are written to G-code.

Switch to Ops. You should see Pocket then Profile. That order matters: cut the recess while the coaster is still solidly attached to the sheet, and cut it free last. If they are the other way round, drag the Pocket chip in front of the Profile chip.

Operations that share a tool are drawn as one coloured band with a marker at each tool change, so you can see at a glance how many times you will be at the machine swapping bits.

8. Simulate it#

Click Simulate G-code in the toolbar.

The 2D view plays the program with a cut trail behind the tool. Click the 3D View tab to watch the same run remove material from a solid block — this is the view that shows you what the part will actually look like.

The player controls sit along the bottom:

• Play / Pause — or the spacebar
• Reset — back to the start
• The seek slider — scrub anywhere in the program
• 1× 2× 4×… — playback speed
• The document icon — opens the G-code viewer, which follows along line by line

The stats bar above shows the current line number, the tool's Z, and the current feed — with the elapsed and total cycle time on the right. That time estimate is worth a look before you commit an hour of spindle time.

In the 3D view, the buttons top-right toggle Axes, Toolpaths, Stock, Tool, Shapes and Follow Tool.

Paused at 2:33 of 3:55. The recess is cut and the cutter is part way round the outline, so you can see exactly how much of the job is left. The readout under the stock gives the line number, Z, feed, and the chip load — green here, which is where you want it.

What the simulation proves is that the toolpaths do what you meant. It does not know whether your machine is trammed, whether the stock is where you think it is, or whether the bit is sharp. Close it with the × on the player.

9. Export the G-code#

Click the Post-Processor tab and check the active profile is right for your controller. Grbl (mm) is the default and covers most hobby machines; Grbl (inches), grblHAL, LinuxCNC, Mach3, UCCNC and a Generic profile are built in too. Any profile, built-in included, can be edited — a built-in carries a Reset button that puts it back to factory defaults, so you can experiment without losing the original. To keep both, duplicate a profile and edit the copy.

Back in the toolbar, click Export G-code. Before writing anything, the app runs a preflight check and shows you the result as a G-code review:

• Operations that failed, or that were edited after their toolpath was generated and are now stale
• Toolpath that runs outside the stock, or past your machine's table travel
• Tool changes and spindle-speed commands your controller may not act on
• Feeds and speeds that put chip load outside a safe band for the material

Warnings do not block you — the button reads Export anyway — but read them. They are the last thing standing between a mistake and a broken cutter.

The review also summarises the job before you commit to it: the post-processor and output units, where X0 Y0 and Z0 are, the stock, the number of operations, the estimated run time, the deepest cut, and every tool the program calls for. Read the origin lines against how you actually zeroed the machine — that is the mistake this panel exists to catch.

If the job uses more than one tool, a Split into one file per tool option appears. Tick it and a File prefix box appears with it, and the button changes to Export N files — one per cutter, so you load a bit, run its file, and stop cleanly rather than trusting your controller's tool-change handling. Our coaster uses a single tool, so neither option is offered.

Click Export. The .gcode file lands in your downloads.

The last check before the file leaves the app. A clean pass still shows you the whole job — read the origin lines against how you zeroed the machine. Warnings, when there are any, don't block the export; they tell you what to look at first.

10. Save the project#

Click Save Project As… (Ctrl+S) and give it a name. You get a .fkam file — the whole project: geometry, tools, stock, operations and all.

.fkam keeps the objects, not just their outlines. Reopen this file and the coaster is still two circles with editable diameters, the tabs are still tabs, and the pocket still knows it is 3 mm deep. Exported SVG and G-code are one-way; the .fkam is the one to keep.

If the browser closes on you before you save, the app offers to restore unsaved work next time it opens.

Open 01-circles.fkam alongside yours if you want to check your work — same stock, same two circles, same tabs, same two operations.

What you just learned#

Every job in this app is the same five moves:

1. Set the stock — dimensions, origin, material
2. Draw or import the geometry
3. Pick geometry, pick an operation, generate — repeat per feature
4. Order the operations in the Ops strip, and simulate
5. Preflight and export

Everything else — v-carving, inlay, 3D surfacing, gears, nesting — plugs into step 3.

Next#

• 2. The canvas — draw and edit geometry with more control
• 3. Stock, origin and tools — feeds, speeds and the tool library in depth
• 5. Profiles and pockets — the five pocket strategies and when each wins