Development goes fast, documentation may be outdated. Proceed with some caution.

EasyTrace5000 Parameter Guide

Every field, its range, its default, and what it changes

Reading This Page

Parameters are grouped by the step they appear in, then by the section heading they sit under in the panel. That is the order you meet them in the app: Source Geometry before you generate offsets, Z Strategy before the preview, Feeds & Toolpaths before the toolpaths.

Four columns are worth explaining:

Values: The range the field accepts, or the options in the dropdown. Out-of-range entries are rejected by the form rather than clamped silently.
Default: What a fresh operation starts with. Tool-derived fields have no default - they are seeded from the tool you pick.
Applies to: Which operations show the field. A field you cannot find is usually one that belongs to a different operation type.
Shown when: Several fields are conditional and only appear once another setting is on, or set to a particular value. If a parameter is documented here but missing from your panel, this is why.

The machine filters the form too

Some parameters only exist on one kind of machine. A field marked with a machine does not appear on the others - the laser fill settings never show up on a router operation, and depth and feed never show up on a laser one. Where nothing is marked, the field is a router one.

The same text is in the app

Every description below is the tooltip text for that field - hover the ? beside any label to get it in place. This page and the app read from the same string pack, so they cannot drift apart.

For what each operation does, see the Operation Guide. For how the stages fit together, see How a Job Works.

Machine settings are not on this page

Post-processor, safe and travel Z, rapid feed, units, PCB thickness, line numbers, tool length compensation and laser spot size are job-wide rather than per-operation. They are covered in the Machine Settings Reference.

Source Geometry

Tool Selection

Parameter	Values	Default	Applies to	What it does
Multi-Tool Drilling	on / off	off	Drill	When enabled, allows assigning different tools, tool numbers, and strategies to each hole diameter in the drill table.
Tool Shown when Multi-Tool Drilling is off	tool library	—	Copper Isolation, Copper Clearing, Board Cutout, Drill, Stencil	Select a tool from your library. The tool's diameter will be used for calculations.
Tool Number Shown when Multi-Tool Drilling is off	1 - 99	1	Copper Isolation, Copper Clearing, Board Cutout, Drill, Stencil	The magazine slot, carousel pocket or collet this operation's tool sits in - the T word your controller will receive. If your machine has no tool changer, leaving 1 on every operation is safe.
Tool Diameter	0.01 - 10 mm	—	Copper Isolation, Copper Clearing, Board Cutout, Drill, Stencil	The tool's cutting diameter - the widest circle it cuts. On copper isolation and engraving this is seeded with the V-bit's effective width at required depth, because that is what the offset has to use.

Offset Generation

Parameter	Values	Default	Applies to	What it does
Number of Passes	1 - 30	3	Copper Isolation	Number of offset passes to create. More passes clear more copper but take longer.
Step Over	10 - 99 %	50	Copper Isolation, Copper Clearing	Percentage of the tool diameter to overlap on each pass. 50% is a good default.
Combine Offset Paths	on / off	on	Copper Isolation	Merge all offset passes into a single geometry. Reduces G-code complexity but loses individual pass control.

Cutout Settings

Parameter	Values	Default	Applies to	What it does
Cut Side	Outside / Inside / On Line	Outside	Board Cutout	Where the tool sits relative to the polygon outline. Outside clears material around the shape. Inside clears within. On Path centers the tool on the line.

Peck Drill Parameters

Parameter	Values	Default	Applies to	What it does
Mill Holes Shown when Multi-Tool Drilling is off	on / off	on	Drill	If checked, generates circular milling paths inside any drill holes larger than the tool. If unchecked, generates a simple peck/drill at the center.
Step Over Shown when Multi-Tool Drilling is off and Mill Holes is on	10 - 90 %	50	Drill	Percentage of the tool diameter to overlap on each concentric milling ring inside oversize holes.

Laser Tool

Parameter	Values	Default	Applies to	What it does
Laser Spot Size Machine class: laser	0.01 - 1 mm	—	all operations	The effective cut width of your laser beam. Manufacturer should list it in the speceification sheet. Typical values: UV laser 0.02-0.08mm, Fiber laser 0.03-0.15mm.

Isolation

Parameter	Values	Default	Applies to	What it does
Isolation Width Machine class: laser	0.05 - 2.5 mm	0.3	Copper Isolation	Total width of copper to ablate around traces, measured from the trace edge outward. The number of laser passes is automatically calculated from this value, the spot size, and the step-over percentage.
Clearing Padding Machine class: laser	0 - 10 mm	1	Copper Clearing	Extra margin ablated around a copper region, beyond its own outline. Gives the beam room at the edges of a pour.

Clearing Strategy

Parameter	Values	Default	Applies to	What it does
Clearing Strategy Machine class: laser	Offset Paths - Concentric, streak-proof / Filled Polygon - Laser software controls fill / Hatch Fill - Directional line coverage	Offset Paths - Concentric, streak-proof	Copper Isolation, Copper Clearing	How the laser fills areas that need copper removal. • Filled Polygon: Exports solid shapes - your laser software handles the fill pattern. SVG only. • Offset Paths: Concentric paths shrinking inward. Most reliable for streak prevention. • Parallel Hatch: Straight lines at a fixed angle. Fast but single-direction. • Hatch: Perpendicular sets of lines. More passes shift the angle between each other.
Pass Spacing Mode Shown when Clearing Strategy is Offset Paths - Concentric, streak-proof or Hatch Fill - Directional line coverage Machine class: laser	Step Over % / Lines per cm / Lines per inch	Step Over %	Copper Isolation, Copper Clearing	Choose how to define the distance between consecutive laser passes. Step Over uses a percentage of spot size. Lines/cm and LPI set the density directly.
Step Over Shown when Clearing Strategy is Offset Paths - Concentric, streak-proof or Hatch Fill - Directional line coverage and Pass Spacing Mode is Step Over % Machine class: laser	10 - 99 %	50	Copper Isolation, Copper Clearing	Percentage of the spot diameter that adjacent paths overlap. Lower values (more overlap) give better copper removal but increase processing time. 50% is a good starting point; reduce to 30% if streaks appear.
Lines per cm Shown when Clearing Strategy is Offset Paths - Concentric, streak-proof or Hatch Fill - Directional line coverage and Pass Spacing Mode is Lines per cm Machine class: laser	1 - 1000 lines/cm	200	Copper Isolation, Copper Clearing	Number of laser passes per centimetre. Higher values produce denser coverage.
Lines per Inch Shown when Clearing Strategy is Offset Paths - Concentric, streak-proof or Hatch Fill - Directional line coverage and Pass Spacing Mode is Lines per inch Machine class: laser	5 - 2540 lines/inch	508	Copper Isolation, Copper Clearing	Number of laser passes per inches. Higher values produce denser coverageance.
Hatch Passes Shown when Clearing Strategy is Hatch Fill - Directional line coverage Machine class: laser	1 - 8	2	Copper Isolation, Copper Clearing	How many hatch passes to run. Each additional pass is rotated from the base angle, so coverage evens out instead of streaking along one direction.
Hatch Angle Shown when Clearing Strategy is Hatch Fill - Directional line coverage Machine class: laser	0 - 180 °	45	Copper Isolation, Copper Clearing	Angle of the hatch lines in degrees. For parallel hatch, lines run at this angle. For cross-hatch, the second set runs perpendicular (angle + 90°). 45° is a good default - it crosses both horizontal and vertical traces.

Cut Settings

Parameter	Values	Default	Applies to	What it does
Cut Side Machine class: laser	Outside / Inside / On Line	Outside	Board Cutout, Drill	Where the laser kerf falls relative to the board outline. • Outside: Laser cuts outside the line (board stays full size). • Inside: Laser cuts inside the line (board shrinks by kerf). • On Line: Laser follows the exact line (board shrinks by half the kerf on each side).

Stencil Settings

Parameter	Values	Default	Applies to	What it does
Stencil Output Machine class: router, knife	CNC Milling (G-code) / Vinyl / CO2 Laser (SVG)	CNC Milling (G-code)	Stencil	What the stencil is cut on. Router mills the apertures and exports G-code; Knife cuts on the line with a cutter offset and exports a vector file. Changing this changes which parameters and stages the operation has.
Aperture Offset Machine class: router, laser, knife	-1 - 1 mm	-0.05	Stencil	Shrinks (negative) or expands (positive) the stencil apertures. -0.05mm is a common default to prevent solder bridging.
Ignore Regions Machine class: router, laser, knife	on / off	on	Stencil	If checked, ignores large copper pours and traces, only generating apertures for actual component pads (flashes).
Exclude Drill Pads Machine class: router, laser, knife	on / off	on	Stencil	Automatically removes stencil apertures that sit directly over through-holes to prevent solder paste from falling into the holes.
Registration Holes Machine class: router, laser, knife	on / off	off	Stencil	Generates 4 circular alignment holes outside the board boundaries to help pin the stencil in place during manual application.
Registration Hole Diameter Shown when Registration Holes is on Machine class: router, laser, knife	0.5 - 10 mm	3	Stencil	The physical diameter of the registration pins/dowels you plan to use.
Registration Margin Shown when Registration Holes is on Machine class: router, laser, knife	1 - 25 mm	5	Stencil	How far outside the calculated board boundary to place the registration holes.
Aperture Corner Radius Machine class: knife	0 - 2 mm	0	Stencil	Rounds each aperture corner so a drag knife or vinyl cutter can follow it. A radius smaller than the cutter compensation comes out square, because a round cutter cannot cut a corner tighter than itself.

Z Strategy

Depth Settings

Parameter	Values	Default	Applies to	What it does
Cut Depth	-10 - 0 mm	-0.1	Copper Isolation, Copper Clearing, Board Cutout, Drill, Stencil	Final target depth for all cuts, relative to the material surface (Z=0). Should be a negative value (e.g., -0.05mm).
Multi-depth Cutting	on / off	on	Copper Isolation, Copper Clearing, Board Cutout, Stencil	Enable multiple passes at different depths for deep cuts. Reduces tool stress.
Depth per Pass Shown when Multi-depth Cutting is on	0.001 - 5 mm	0.1	Copper Isolation, Copper Clearing, Board Cutout, Stencil	Incremental depth of each pass when using multi-depth cutting. Smaller = gentler on tool.
Multi-depth Milling Shown when Mill Holes is on	on / off	on	Drill	Mill oversize holes in several Z levels instead of one full-depth pass. Easier on small cutters.
Depth per Pass Shown when Mill Holes is on and Multi-depth Milling is on	0.01 - 10 mm	0.5	Drill	Material removed per Z level while milling an oversize hole.
Entry Method Shown when Mill Holes is on	Plunge / Helix	Helix	Drill	How the cutter enters an oversize hole. Helix spirals down and loads the tool gently; Plunge drops straight in and needs a centre-cutting bit.

Cutting Strategy

Parameter	Values	Default	Applies to	What it does
Entry Type	Plunge	Plunge	Copper Isolation, Copper Clearing, Board Cutout, Stencil	How the tool enters the material. Plunge: straight down. Ramp: diagonal. Helix: spiral down.

Peck Drill Parameters

Parameter	Values	Default	Applies to	What it does
Peck Depth	0 - 5 mm	0	Drill	Depth to drill before retracting when using peck drilling. Smaller = more retracts = cleaner holes.
Dwell Time	0 - 10 s	0	Drill	Pause duration at bottom of hole (seconds). Allows chips to clear and reduces burrs.
Retract Height	0 - 10 mm	0.5	Drill	Height to retract to between holes. Should clear board but minimize travel time.
Canned Cycle	None (G0 + G1) / G81 - Simple Drill / G82 - Dwell / G83 - Peck / G73 - Peck (Stepped)	None (G0 + G1)	Drill	Pre-programmed drill cycle. G83 (peck drilling) retracts periodically to clear chips.

Cutout Settings

Parameter	Values	Default	Applies to	What it does
Number of Tabs	0 - 12	0	Board Cutout	Number of small tabs to leave uncut, holding the board in place.
Tab Width	0.1 - 10 mm	0.5	Board Cutout	The length of each holding tab in mm.
Tab Height	0.1 - 5 mm	0.5	Board Cutout	The thickness of the tab. A value of -0.5mm on a -1.8mm cut will leave a 0.5mm thick tab.

Feeds & Toolpaths

Feeds & Speeds

Parameter	Values	Default	Applies to	What it does
Feed Rate	1 - 5000 mm/min	—	all operations	Speed at which the tool moves while cutting (mm/min or in/min).
Plunge Rate	1 - 2000 mm/min	—	all operations	Speed at which the tool descends into material (mm/min or in/min). Usually slower than feed rate.
Spindle Speed	100 - 30000 RPM	10000	all operations	Rotation speed of the spindle (RPM). Higher speeds for smaller tools.
Spindle Dwell	0 - 60 s	1	all operations	Time in seconds to wait. Essential for high inertia spindles that need extra time to come up to speed.

Toolpath Options

Parameter	Values	Default	Applies to	What it does
Optimize Toolpaths Machine class: router	on / off	on	all operations	Reorder and simplify the finished toolpath to cut travel time. Turn it off to keep the paths in exactly the order they were generated.