10. Simulating and exporting#

Everything up to here has been about making toolpaths. This chapter is about the last stretch: checking they do what you meant, translating them into your controller's dialect, and getting the file onto the machine.

The simulator#

Press Simulate G-code in the toolbar — the green button, grey until there is a toolpath to simulate. The program is built from every visible operation, in program order (Paths → Toolpaths), and loaded into the player. While it's open the button turns into a red Stop, which closes the simulator just as the player's × does — useful when you've hidden the player in the 3D view.

It opens on the finished part, not on bare stock. That's deliberate — the question you opened the simulator to answer is usually what does this come out like, and showing you the answer immediately beats making you watch four minutes of cutting first. Press Play and it winds back to bare stock and animates from there.

On a job of several sheets it plays one of them — the one picked in the toolbar's ◀ Sheet N of M ▶ picker. Step the picker and the simulation rebuilds for that sheet.

The player under the stock: the position and progress bar above the controls, the spindle and chip load bar below them, and the program's messages above both.

The readouts#

Two bars sit under the stock, and they are the reason to run a simulation rather than just look at the toolpath.

Position and progress — the current line number, the tool's Z, the feed (or rapid), and elapsed against total cycle time. That total is worth reading before you commit an evening to a job.

Spindle and chip load — the RPM with its router dial equivalent, and the chip load as actual / target with a verdict: 🔴 rubbing · too hot, 🟢 sweet spot, 🔵 chips too large. See chapter 3 for the bands. On manual feeds it also suggests the feed that would bring you back into the band.

2D and 3D#

2D View plays the program flat, with a trail behind the tool. It's the quicker read for travel moves, ordering and retracts.

The same moment in 2D. The trail is coloured by chip load against the aim — the legend under the player gives the bands — so a stretch cut too light or too heavy shows where it happened.

3D View removes real material from a solid block. This is the one that tells you what the part will look like — scallops, flat spots, an over-deep pocket. The toggles top-right turn Axes, Toolpaths, Stock, Tool, Shapes and Follow Tool on and off.

It keeps itself up to date#

Leave the simulator open, change an operation, and it rebuilds and reloads by itself once the operations settle. You don't have to press Simulate again. An imported .gcode file is the exception — that program is not something the app generated, so it is left alone.

What a simulation proves and what it doesn't. It proves the toolpaths do what you meant — the right shapes, the right depths, in the right order. It knows nothing about whether your machine is trammed, your stock is where you think it is, your workholding will hold, or your bit is sharp. The export review says this too, and it is right to.

The post-processor#

Controllers disagree about the details of G-code. A post-processor profile is the set of rules for turning toolpaths into the dialect yours speaks.

Nine profiles are built in — FluidNC (mm), FluidNC (inches), Grbl (mm), Grbl (inches), grblHAL, LinuxCNC, Mach3, UCCNC and a Generic one. FluidNC (mm) is the default; it and the Grbl profiles cover most hobby machines.

The buttons across the top act on the profile selected in the list: Duplicate copies it, Export saves it as a .fkset file to share, and Delete removes it (the last one can't go). Add Profile starts a new one, Import brings profiles in from a .fkset — always added beside yours, never over them — and Restore Built-ins puts every built-in back to factory and brings back any you deleted, leaving your own alone.

Any of them can be edited, and 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.

What's in a profile#

Unit mode is the only thing that decides whether the file is in inches or millimetres. The toolbar's mm/in toggle is a display setting and has no effect on the exported file.

Keep the placeholders on their own axes — X{x} Y{y}, I{i} J{j}. If your machine's axes run the other way round, set Setup → Machine Axes (Machine axes) rather than swapping them here: a swap mirrors the part and runs every arc backwards, and the move and arc fields say so in amber if a template does it.

Compact G-code leaves out of each move whatever the controller already holds. G0/G1, the axes and the feed are all modal — they stay in force until changed — so after G1 X10 Y5 Z-1 F800, a move to X12 is written as just X12. The file comes out much smaller and the controller runs it exactly the same; the simulator and Resume read it either way. Every built-in profile is for a controller that works this way. Turn it off only for firmware that needs every word on every line (Marlin, unless it was built with motion modes).

Turn off Output arc moves if your controller's arc handling is unreliable — everything comes out as short straight moves instead. Bigger file, no arcs to misinterpret.

The tool change block is worth setting up properly. The default M5 / M0 stops the spindle and pauses so you can change the bit and re-zero. If your controller handles tool changes differently, this is where to say so.

Sharing a profile#

The Import and Export buttons at the top of the profile list (the same icons as the toolbar's) share a profile with someone else: Export saves the selected profile as a .fkset file, and Import brings profiles in from one. An imported profile is always added — if you already have one with the same name but different contents, it comes in as "Name (imported)" beside yours, and an identical one is skipped. Nothing you have is changed. A check shows what's about to come in, with OK and Cancel, before anything does.

Restore built-ins (the list icon beside them) resets every built-in profile to factory and brings back any you deleted. Your own profiles are kept as they are. It lists exactly which built-ins lose your edits and which come back before anything changes.

The export review#

Export G-code runs a preflight check first and shows you a G-code review before writing anything.

The summary#

Read the top block against reality, because this is the last point at which a mistake is free:

• Post-processor and output units — is this the file your controller wants?
• Work origin (XY) and Z origin — do these match how you actually zeroed the machine? The Z line spells it out: "Top of stock — set Z0 at the top surface."
• Safe height, max feed, spindle range — your machine's limits as the app understands them.
• Operations, estimated run time, deepest cut — is the deepest cut deeper than your stock, and is the run time what you expected?
• Tools — every cutter the program calls for, with its speed.

The warnings#

Warnings don't block the export; the button just changes to Export anyway. Read them anyway. They cover:

• Operations that failed, or that are stale because their geometry changed after the toolpath was generated
• Toolpath that runs outside the stock, or past your machine's table travel or Z travel
• Tool changes and spindle commands your controller may not act on
• Chip load outside a safe band, and spindles that can't run slow enough for the material's surface speed
• For inlays, a male plug that doesn't match its female socket

More than one sheet#

When the parts are spread over several sheets of stock (see More than one sheet), the review says so above the button — "The parts are on 3 sheets: one file per sheet with toolpaths (3), each cut from the sheet's own corner" — and the button becomes Export 3 sheets.

Each sheet is its own program, named <project>_sheet2 and so on, with its toolpaths moved so that sheet's corner is the work origin. The checks — on the stock, table travel, deepest cut — judge every operation against its own sheet, not against sheet 1. A sheet whose parts have no toolpaths yet gets no file.

Simulate G-code and the Machine tab work on one sheet at a time: the one picked in the toolbar's ◀ Sheet 1 of 3 ▶ picker.

A tiled job works the same way with tiles instead of sheets — Export 4 tiles, files named <project>_tile2 and so on, each checked at its own origin. See 14. Double-sided and tiled jobs.

Splitting by tool#

If the job uses more than one tool, a Split into one file per tool option appears, along with a File prefix box. The button becomes Export N files.

This is usually the right choice. One file per cutter means you load a bit, run its file, and stop cleanly — rather than trusting your controller to do something sensible at a tool change. A single-tool job doesn't offer either option.

Getting it to the machine#

The .gcode file lands in your downloads. Copy it to your controller however you normally do.

On a FluidNC controller you can skip the file altogether: the Machine tab sends the design straight to the controller's SD card and runs it from there, with a map to check the job against the stock first. See 12. Running the machine.

Before you press cycle start, the things the app told you but cannot check:

1. Zero X, Y and Z where the review said they were.
2. Check the first move. Bring the tool to Z-safe and step through the opening lines in your sender before letting it plunge.
3. Confirm the bit matches the one the review named.

Then cut it.

Restarting a job that stopped#

A broken bit, a power cut, a job you had to cancel half way: the program can be restarted from where it stopped instead of from the top. A bare "start from line N" in a sender is not a restart — line N then runs in whatever state the machine happens to be in, while the program's state at that line was built up by everything before it. FreazyKam writes a new file that puts that state back first.

1. Simulate the job and open the G-code viewer (the document icon on the player).
2. Find the line where it stopped — scrub the simulator to where the cutting stopped, or click the line in the viewer. The simulator shows the stock as it stands at that line.
3. Press Resume from line N at the top of the viewer. (It is hidden while playing — pause first.)
4. Choose where to restart. Picking one moves the simulator to its line, so you can see where it begins; Cancel puts it back.

The panel shows the tool in force, where the tool comes in and how — up to safe Z, across, then down at the plunge feed — and any warnings. Tick Pause after the spindle command when your router is switched by hand: the file stops (M0) once the spindle should be running, so you can check it before anything moves. Then Download resume file and run it like any other.

Zero must be exactly where it was for the original run. If the machine lost power, alarmed, or the stock moved, find X, Y and Z again first — the resume file goes back to the coordinates the job was using, and has no way to know they have moved.

The file is the original program's own text from the restart line on, with only the entry move added, so it works for any controller and for G-code from any CAM program, not only FreazyKam's. A few states cannot be resumed from a line of G-code alone, and the panel says so rather than guessing: relative or inverse-time moves, cutter compensation, inside a canned cycle, after the coordinate system was changed (G92/G10), rotary axes, or before the program has set X, Y and Z.

Next#

• 11. When something goes wrong — failures, refusals, and what they mean
• 12. Running the machine — driving a FluidNC controller from FreazyKam