EasyTrace5000 CNC Milling Guide

Safety & Material

Interface Overview

A central canvas with a sidebar either side. The left holds your files, the right holds board placement, machine settings and the parameters for whatever you have selected. The footer carries status, the log and the display options.

Top Toolbar

On the left, the Actions menu covers file loading, toolpath management and SVG export. On the right, zoom controls, the 2D/3D toggle (F2) and the theme switch.

Left Sidebar: Operations Tree

Five operation categories, each holding the source files you assign to it:

Copper Isolation

Copper layer Gerbers, for separating traces and pads.

Drill

Excellon files, or SVGs whose circles and obrounds you want treated as holes.

Copper Clearing

Gerbers for pour or keep-out removal.

Board Cutout

Outline files for the final board shape.

Stencil

Soldermask or paste-layer Gerbers, for paste apertures.

Click a category header to open a file browser filtered to the types that operation accepts. Click a loaded file to select it; its parameters appear on the right. Everything you generate appears underneath the file, each with its own visibility toggle.

Center Canvas

Drag to pan, scroll to zoom, and use the zoom controls in the toolbar to fit the view. The bottom-left readout shows cursor position in millimetres and the current zoom.

2D and 3D

The canvas starts in 2D. When you reach the Toolpaths stage it switches to the 3D view by itself, because that is where a toolpath is worth looking at.

You are not stuck there. The view button on the right of the toolbar - or F2 - flips between 2D and 3D at any time, before or after generating anything.

Right Sidebar

Three collapsible sections. Origin & Rotation places the machine origin and rotates or mirrors the board. Machine Settings holds everything that affects every output file. Properties changes with your selection and shows the parameters for the step you are on.

Footer

Click the eye icon for the display options - what is drawn, and which layers are visible. Click the status bar to expand the log, which is the first place to look when something did not do what you expected.

Stages

Every operation is generated in stages. A stage is what the big generate button acts on: you set that stage's parameters, generate, and get a layer you can show, hide and redo on its own. Re-running a stage replaces its own layer and clears the ones after it, never the ones before - so changing your mind about depth never costs you the offsets you already generated.

Change something an earlier stage depends on - the tool diameter, the board rotation, a machine setting - and everything generated after it is invalidated and cleared. The message names the stage to go back to.

The Workflow

Seven steps. Steps 4 to 7 are the operation's four stages - the rest is setup you do once.

1. Loading Files

Four ways in, all equivalent:

• Welcome modal - load a built-in example, open the file modal, or start empty.
• File upload modal - Actions → Add Files. Drop zones for isolation, drill, clearing and cutout. Stencils are added from the tree instead.
• Drag and drop anywhere on the window. Files are matched to an operation by extension, so Gerber exported with Protel extensions lands in the right category by itself.
• Category headers in the operations tree, which open a browser filtered to that operation's types.

Each operation holds one file. Loading a second file into the same category creates a second operation of the same type.

2. Placing the Board

The origin you set here becomes (0,0) in your G-code. It has to match where you will zero the machine on the physical stock, so pick something you can find again: a board corner, or the board centre.

Origin Offset

Shifts where (0,0) sits relative to the geometry. By default it is the lower-left corner of everything loaded, and the Center and Bottom-Left buttons jump to those two. (From the canvas, C and B preview the same two positions and O commits one.)

Board Rotation

Rotates all geometry about its centre, in degrees - useful when your stock is a different orientation to your board.

Mirror

Flips horizontally or vertically, independently. Used for bottom-copper work. Cut direction is corrected automatically, so a mirrored board still climbs or conventionals the same way.

3. Machine Settings

Global settings that affect every output file - covered field by field in the Machine Settings Reference below. Set the post-processor first, because it decides which of the other options exist.

4. Generating Offsets

Select a source file and set the geometry parameters: tool and passes for isolation and clearing, cut side for cutout, hole handling for drilling, aperture settings for a stencil.

Click Generate Offsets. The result appears as an Offsets layer - thin centrelines showing where the tool will travel in X and Y. Curved geometry stays curved, so an offset pad exports as a real arc rather than a string of tiny line segments.

Nothing about depth exists yet. This stage is purely the shape of the path.

5. Generating the Preview

Select the Offsets layer and set the depth parameters: cut depth, multi-depth and depth per pass, entry type, plus tabs on a cutout or drill-cycle settings on a drill.

Click Generate Preview. The offset paths are redrawn at the real tool diameter, so you can see the copper that will actually be removed rather than the line the spindle centre follows.

The preview is a visual check - it is the last chance to catch a tool that is too wide for the gaps on your board.

6. Generating Toolpaths

Select the Preview layer and set the machine parameters: feed rate, plunge rate, spindle speed and dwell, the tool number, and whether to optimize.

Click Generate Toolpaths. The canvas switches to the 3D view so you can look over the result - depth passes, entry moves, retracts and rapids. The toolbar view button, or F2, takes you back to 2D.

7. Exporting G-code

Open the Export Manager from any operation's Output node, or from Actions → Manage Toolpaths. Only operations that have been through Generate Toolpaths appear.

1. Select and order. Check the operations you want and drag them into the order you want to run them - typically isolation, clearing, drilling, and cutout last so the board stays attached. (The list also reorders from the keyboard: Space to grab, arrows to move, Space to drop.)
2. Set the output options (below).
3. Review the G-code preview, with line count, operation count, estimated time and total travel.
4. Export to download. The file extension comes from the post-processor.

Output Options

Export as single file

Combines every selected operation into one program. Required if you want tool changes handled across operations.

Include operation comments

Adds comments identifying each operation in the output.

Optimize toolpaths

Reorders and simplifies the paths to cut travel time. On by default.

Insert tool changes

Emits a tool change whenever the tool number changes, with a retract and spindle stop around it. Greyed out on posts that do not support tool changes.

Group by tool

Reorders operations so each tool is used once. This overrides the order you dragged, so it is never applied unless you ask for it.

Split drill files by hole diameter

Multi-file mode only. Writes one program per hole size, so each file loads exactly one cutter.

Output filename

Base name only - the extension follows the post-processor.

Operation Settings

What to set for each operation and why. Full ranges and defaults are on the Parameter Guide; what each operation is for is on the Operation Guide.

Copper Isolation

Cuts a clearance channel around copper so traces and pads end up electrically separated. Passes run outward from the copper edge; each extra pass widens the cleared band.

Geometry: tool and tool diameter - smaller tools (0.1-0.2 mm) allow tighter trace spacing but break easily; number of passes; step-over; combine passes.

Depth: 0.1 to 0.15 mm is typical for 35 µm copper, plus multi-depth and depth per pass for thicker copper.

Machine: feed 100-400 mm/min, plunge 25-50% of feed, spindle 10,000-24,000 RPM.

For a V-bit, the width it cuts depends on how deep it goes, so the offsets are calculated from the width it will actually produce at your cut depth rather than the number on the packet.

Drill

Handles holes from Excellon files and from SVG circles and obrounds. Each hole is measured against the tool and given a strategy automatically.

Milling holes and slots

Turn on Mill Holes and any hole wider than the tool is cut out rather than drilled: the tool drops inside the hole and walks a circle inset by its own radius, taking as many passes as the step-over needs to clear the middle. It is how you get a 3 mm hole out of a 1 mm bit, and it is slower than drilling - which is why it is a choice rather than the default.

Obround slots work the same way, along a line instead of a circle. The tool runs the slot's centreline and stops one radius short of each end, so the finished slot matches the width and length you drew.

Multi-tool drilling. Turn on Multi-Tool Drilling to open a table with a row per hole size. Each row gets its own strategy (peck, mill or skip), its own cutter diameter and its own tool number. Auto-match Tool Library fills strategy and cutter for you. Copy Excellon T numbers pulls the numbers out of the file header - those are the file's own indices, not your machine's slots, so check them before you cut. A row left without a tool number falls back to the operation's number.

On export, a single-file job puts the tool changes inline. In multi-file mode, Split drill files by hole diameter writes one program per size, which is how you run a multi-tool drill job on a machine without a changer.

Key parameters: mill holes and mill step-over; drill cycle (G81/G82/G83/G73), peck depth, dwell time, retract height; entry type and multi-depth for milled holes.

Copper Clearing

Removes large copper areas - ground pours, fills - rather than just isolating them. Passes work inward until the area is gone. Islands inside a pour are recognised and left alone.

Running out of material to remove is the intended end state here, so a message saying the geometry collapsed at some pass is this operation finishing normally, not failing.

Key parameters: tool diameter and step-over, then the same depth settings as isolation. Larger tools clear much faster and are the right call unless the area has fine detail.

Board Cutout

Cuts the board free from the stock along its outline, with holding tabs so it does not shift on the last pass.

If your outline has small gaps where segments do not quite meet, you get a prompt offering to close them rather than an open path that would produce a nonsense toolpath. Multiple boards in one file are handled as separate outlines.

Key parameters: cut side - outside gives a board matching the outline, inside makes a window, on-line centres the tool on the line; number of tabs (4-6 for a small board), tab width (the bridge length along the outline) and tab height. 2-3 mm wide and 0.3-0.5 mm tall is a good starting point.

Depth: the full stock thickness, with multi-depth on. Cut the board out last.

Stencil

Generates solder-paste apertures from your pad geometry, ready to cut. On the CNC route you choose what cuts it.

Stencil Output picks between Router, which mills the apertures out of thin stencil stock and exports G-code, and Knife, which produces a vector file with the cutter offset applied, for a drag knife or vinyl cutter. Choosing one changes the rest of the form, since a milled stencil needs depth and feeds and a cut one does not.

Corner radius exists because a round cutter cannot turn a corner tighter than itself. On a drag knife/vinyl cutter a square aperture corner means the blade can overshoot or distort the opening; rounding it gives the blade something it can track easier.

Aperture offset shrinks or grows every aperture. A small negative value such as -0.05 mm is the usual starting point; it stops paste bridging between close pads.

Registration holes are optional alignment holes outside the board, for pinning the stencil over the PCB. They ignore the aperture offset and the corner radius - they have to match your dowels, not your paste.

Lasering a stencil instead? That lives in the Laser Guide.

Machine Settings Reference

These apply to every operation in the job.

Post-Processor

The G-code dialect your controller expects. Set it first: it decides which other settings appear, including tool changes, tool length compensation, rotary routes and any extra fields that post needs.

Start / End G-code

Free-text blocks emitted at the very start and end of the program. Use them for dust collection, coolant, a homing sequence, anything your machine needs around the job.

Units

Millimetres or inches. Selecting inches scales the output; it does not change how you enter parameters.

PCB Thickness

Used for depth checks and for the cutout's full-depth guidance.

Safe Z (typical 5-15 mm)

Maximum clearance height, used at program start and end. Must clear every clamp, fixture and high point.

Travel Z (typical 2-5 mm)

Lower retract for moves between nearby cuts. Faster than going to Safe Z every time, but it must still clear the workpiece and any debris.

Rapid Feed (typical 1000-3000 mm/min)

Speed for positioning moves. Some controllers ignore it and move at maximum; others respect it.

Line Numbers

Any program can carry N line numbers, with a step you choose. Each post has its own default, but the choice is yours - some controllers and file senders want them, most do not care.

Tool Length Compensation

Only shown for posts that support it. Table tells the control which offset to use after each swap. Table (implicit) lets the control take the offset from the tool number itself. Probe leaves it alone, because the machine measures the tool during the change. Pick whichever your controller is set up for.

Rotary Route

Only shown for posts with a rotary axis. Not used by EasyTrace5000 - it is here because the setting is shared with EasyShape5000.

Extra post fields

Some posts need settings no other post does - the Roland profiles are the largest example. They appear here when that post is selected.

Post-Processors

Ten dialects ship with the suite, shared with EasyShape5000:

GRBL · grblHAL · UCCNC · Mach3 · LinuxCNC · Fanuc · WinPC-NC · Makera (Carvera) · Marlin · Roland RML

Each sets its own file extension, arc format and tool-change dialect.

Visualization Options

Open with the eye icon in the footer. Some of it exists for debugging, but several toggles are useful day to day.

Display

Grid

Reference grid, spacing adapts to zoom.

Wireframe

Paths only, no fill. The fastest way to see what a file actually contains.

Board Bounds

Rectangle around all loaded geometry.

Rulers

Millimetre rulers along the canvas edges.

Layer Visibility

Source geometry splits into regions, traces, pads, drills and cutouts; what you generate splits into offsets, previews and toolpaths. Each is toggled independently, and the setting sticks per operation rather than resetting when you regenerate.

Advanced

The rest are diagnostic overlays - fusion mode, preprocessed geometry, debug points and arcs, black-and-white rendering. They exist for working out why a file looks wrong, and they are safe to leave off. Verbose Debug is the one worth knowing: it writes detailed logging to the browser console and the status log, and attaching that output to a bug report makes it far more likely to get fixed.

Tips & Troubleshooting

Best Practices

Start with an example

Load a built-in example and run it all the way through before processing your own board. It is the fastest way to learn what each step should look like.

Verify the origin before exporting

Your origin has to match where you will zero the machine on the stock. Check it once more before the final export - it is the single most common cause of a scrapped board.

Order operations for the job

Isolation, then clearing, then drilling, then cutout last so the board stays attached while everything else happens. Drilling and cutout often share a tool, which is worth planning for if your post has no tool change.

Common Issues

Canvas is blank or black

Cause: browser graphics compositing, common on laptops with two GPUs. Fix: restart the browser; it renders correctly on reload.

Files will not load

Cause: an extension the operation does not accept, or a file variant that will not parse. Fix: check the log in the status bar - errors are reported there with a line number. Re-export from your EDA tool with Protel extensions if drag-and-drop puts files in the wrong category.

Geometry appears rotated or mirrored

Cause: board rotation or mirror left set from earlier. Fix: reset both in Origin & Rotation, then regenerate anything you had already generated.

Drill holes come out the wrong size

Cause: the tool is larger than the hole, so it pecks at the centre and the hole opens up to the tool. Fix: use a smaller bit, or turn on Mill Holes and let it mill the hole to size.

Offset generation takes a long time

Cause: a lot of geometry. Isolation on a dense board is the usual suspect. Fix: fewer passes, a larger step-over, or clear the pour with a Clearing operation instead of widening isolation.

An operation is invalidated

Cause: a machine setting, a board transform, or a parameter an earlier stage depends on was changed. Fix: regenerate from the stage named in the message. Only the layers after your change are cleared.