How to Set CNC Toolpath Properties in Mozaik – Phill Anton Consulting

To set CNC toolpath properties in Mozaik, open Toolpath Properties for the exact machine you run on, then work through each tab — ramping/lead-in, cut direction, small-part handling (skins or tabs), dado and pocket strategies, and per-tool fields like diameter, pass/plunge depth, stepover, and application. Because results vary by post and machine, treat the recommended values as starting points and test them on your own equipment.

This guide follows Mozaik's official walkthrough. Watch the original video on Mozaik's channel:

You can also reference Mozaik's official video directly. This walkthrough explains what each setting does and how to choose values; because behavior varies by machine and post, verify the recommended values on your own equipment.

First: confirm you are on the right machine

Toolpath properties are stored per machine, not globally. A common mistake is editing the default "CNC Router" when you actually run a copied or renamed machine — you set everything, run the job, and see no change because your edits landed on the wrong machine.

In Toolpath Properties, select the exact machine you run on, then make your changes.

How does ramping (lead-in) work?

Ramping controls how the tool enters the material instead of plunging straight down. Standard ramping drops the tool to the safe value above the material, then uses the plunge value to enter at an angle. The ramp distance is how far the tool travels horizontally while ramping in, so a longer distance makes a shallower angle and a shorter distance makes a steeper one.

Ramp distance — sets the travel for the ramp. In the session this was set to about 2 inches, and the same distance applies to ramp-out and helical ramping too.
Ramp off — turn ramping off and the tool plunges straight in. Some machines (described in the session as "home machines") will override ramping, so for those you set the distance to zero and turn ramping off.
Ramp out — for traditional posts, this ramps the tool out instead of pulling straight up out of the material.

What is helical ramping and when should I use it?

Helical ramping does the same angled motion but viewed from the top — it ramps off of the offcut/waste side rather than plunging into the part. It is most useful on laminate or melamine when running a compression tool: as the tool dulls, the initial lead-in can chip, and helical ramping moves that risk off the part itself.

Trade-off: you must increase part spacing. The session's rule of thumb was a 1/16" over tool diameter for standard ramping versus 1/8" over tool diameter for helical. There is also a helical ramp-out option that mirrors the standard ramp-out.

Linear vs zigzag ramp style

Zigzag is just a different ramp-in pattern — it ramps one way, ramps back, then carries on (described as roughly a one-inch ramp each way). The presenter has personally stuck with linear, but zigzag is available if you prefer it.

Which cut direction should I choose?

Conventional — counterclockwise. This is the presenter's default for most panel stock.
Climb — clockwise. There are benefits for a second pass on certain materials, but it is a deep topic (the session pointed to a forum video on conventional vs climb). Some materials like plywood are generally poor candidates for climb cutting due to deflection.

Important: cut direction only comes into play with full sheet skin. With a return skin or onion skin, the direction setting only applies to the skin pass — larger parts still run a conventional pass.

What does "Art Corners" do?

This setting shortens the amount of code the machine reads going around a corner, smoothing the operation so the machine does not nearly stop and change direction at each corner. It does not round your corners by design. However, it must be tested per machine — some machines do not process it properly and will actually round the parts, so it is often left off for those.

Per part vs stay down

Per part — the machine leads in and out for every single part on the table.
Stay down — leads in once, travels around the parts without cutting fully free at each one, and makes a full lap of the sheet in one pass.

Stay down saves time (no repeated lead-in/lead-out) and reduces chipping on melamine and laminate. It does not strictly require full sheet skin, but full sheet skin is recommended with it — it helps keep small parts on the table and helps a compression tool's second pass evacuate packed dust, leaving less mess.

How do I set up small-part handling (skins and tabs)?

Small-part handling decides whether parts get a skin or tabs left behind on the first pass. Options include None, tabs, full sheet tabs, and the skin modes below.

Skin thickness — material left behind on the first pass (going down to roughly a 32nd above the spoilboard).
Skin offset — oversizes the parts on the first pass so the second pass squares them to true size; this absorbs any tooling deflection that happens on the first pass. The presenter felt 1/16" is large and leaned toward about 0.015".
Tabs — when doing tabs, the thickness/length fields define the tab. Example used: a 1/32" thick, 2" long tab; everything else cuts through. Mozaik places tabs by its own algorithm — there is no manual control over placement.
Cut out manually — leaves the skin on the part so you can free it later with a razor knife (set skin offset to zero). Useful for sheets of small parts that would otherwise move. With tabs, the equivalent leaves the tabs in place to knock out or flush-cut later — good for low- or no-vacuum tables.
Feed rate reduction — a percentage reduction applied on the second/skinning pass. Example: a 20% reduction means the first pass runs 100% and the final skin pass runs 80%.

Onion skin vs return skin vs full skin

Onion skin — skins each small part, then immediately cuts that part all the way out.
Return skin — skins all small parts first, then returns to cut them out, which lets you control the small-part cutout sequence (e.g., sort smallest to largest by area).
Full sheet skin — the recommended pairing for stay-down nesting and for cut-direction control.

For stay-down nesting with full sheet skin, the presenter typically uses shortest movement for the cutout sequence so the spindle gets around the table quickest without backtracking.

What sizes count as a "small part"?

For tabs/small-part handling, the session described small parts as roughly 12" x 12" surface area, or anything with a minimum dimension around 5". Full sheet tabs apply to everything and override the small-part-only behavior.

Waste pocketing

This feature pockets out waste instead of cutting it free, and it only affects toe notches facing the inside of the sheet. The presenter associated it with integrated toe kick work. You set a surface area, and the machine pockets the waste so small loose parts do not come free and cause damage.

Dado options

These apply to dado tools only:

Run past — runs past the part by half the tool diameter to ensure parts fit together. This is the fastest, most efficient dado method and what most customers use.
T-bone and dog bone — available alternatives; harder to hide and cannot be hidden with blind dados, but offered for those who need them.

Note: dado tools are called automatically in Mozaik, which tries to fit the largest tool that fits in the groove. Example: with 1/4", 3/8", and 1/2" down-shears in your set, a 3/4" dado pulls the 1/2" down-shear because it is the largest that fits. The same idea of dedicating a tool to a specific cut shows up when you cut V-grooves on shiplap panels.

Pocket options

Pocketing strategies apply when a tool is set as a pocket tool. There are three strategy options; the session favored raster, which cleans out the pocket fast and leaves a clean surface. There is also a radius option that radiuses the points to reduce witness marks where the machine changes direction.

Radius corners are not supported on a couple of machines (e.g., certain BSE-type machines were kept off), while others handle it fine. The recommendation is to run a test door with it on and off and compare. This setting is what helps clean up MDF/shaker-style doors, and it benefits from a well-trammed machine.

How do I set individual tool properties?

Mozaik works off center-line machining: it looks at your part size and offsets the toolpath by half the tool diameter. Key per-tool fields:

Diameter — critical. If you sharpen a tool, update the diameter before generating G-code, or the offset will be wrong. These per-tool fields feed the same optimizer pass that drives your part labels.
Pass depth / plunge depth — the depth a tool cuts in a single pass; never more than the tool's cut length. Rule of thumb on smaller tools: about half the diameter. Setting these to zero means unlimited depth (it will try to go through in one pass), which the presenter avoids — for example setting around 7/8" so it can clear 3/4" material. Pass depth and plunge depth are typically kept the same value (plunge was set to 1" in the session).
Stepover — applies to dado and pocketing tools; it measures the amount of material already machined. Counterintuitively, a smaller stepover removes a larger amount of material on the next pass. Rule of thumb: never more than half the tool diameter.
Pocket ramp — the horizontal distance the tool travels when ramping into a pocket. This value only applies when the tool is used as a pocket tool (it does not apply to cutout tools), and it exists because some tools cannot plunge straight into a pocket.
Add for through cut — extra distance pushed through the material into the spoilboard for cutout tools. It varies by machine setup and zeroing, so it is trial and error; adjust if cutting too deep or not deep enough.
Add for blind bore — accounts for the spur length of a drill bit in the spindle, to fine-tune hole depth for hinges, guides, and shelf pins. This depth fine-tuning matters when you choose between line bore and custom bore and when you set up drawer guides.

Speeds and feeds

Mozaik ships safe starting values (e.g., 18,000 RPM was called standard for a cutout tool). Feed rate is what you tune — get a chip load from your tooling rep or a feed calculator, and aim for a fine chip, not dust. Not every machine can run optimal feed rates, so get as close as you can and learn your machine's behavior. Plunge rate should be at least half the feed rate, if not slower; slowing it can fix issues like the spindle over-traveling a corner on MDF doors when there is play in the Z-axis.

Application: telling Mozaik what each tool is for

The application setting controls when a tool is called:

Roughing — only used on the first pass when skins are on.
Cutout — final pass / cutout for all parts.
Drill — drilling operations.
Dado — dado tools (called automatically, largest-fits-the-groove).
Pocket — pocket tools with their own strategy. You can choose "use pocket tool" so Mozaik grabs whatever it sees as a pocket tool instead of naming a specific one.
Dovetail — keeps the tool out of automatic operations so it is only used for dovetail drawers.
Sharp corners — hardcoded to run at the tool's included angle for corner cleanout (e.g., 90, 60, 45, 30); the path runs at half the tool's included angle.
CNC door — any tool that has a drawn tool shape. This drives the 3D visual of a profiled edge for the customer; it does not auto-select the tool — you must add it to the panel tool group. The more accurately the tool shape is drawn, the easier panel tool group setup becomes.

Other notes

Priority number — ignore it; it no longer applies in Mozaik.
T-mapping number — only for specific machines that need an actual mapped tool number.

Related guides

Get it done-for-you

You can set this up yourself using the steps above. If you'd rather skip the setup, PAC's Mozaik training and done-for-you setup can help — phillanton.com.

Full disclosure: this guide is published by Phill Anton Consulting.

FAQ

Why do my toolpath property changes do nothing when I run a job?

Toolpath properties are stored per machine. You likely edited the default "CNC Router" while running a different (copied or renamed) machine. Reopen Toolpath Properties, select the exact machine you run on, and reapply your settings.

Does a smaller stepover mean a smaller cut?

No — it is the opposite. Stepover measures the material already machined, so a smaller stepover value removes a larger amount of material on the next pass. Keep stepover no more than half the tool diameter.

Should pass depth and plunge depth be the same?

The presenter keeps them at the same value as a rule of thumb (plunge was set to 1" in the session). Never set either deeper than the tool's cut length, and avoid leaving them at zero, which lets the tool attempt the full thickness in a single pass.

When is helical ramping worth the extra part spacing?

Use it on laminate or melamine with a compression tool, where a dulling tool can chip on the initial lead-in — helical ramping moves that risk off the part. Budget the extra spacing: about 1/8" over tool diameter for helical versus 1/16" for standard ramping.

Do I need full sheet skin for stay-down to work?

No, stay down does not strictly require full sheet skin, but it is recommended. It improves the odds of keeping small parts on the table and helps a compression tool's second pass clear packed dust for a cleaner shop floor.