Interface Overview

EasyTrace5000's interface is organized around a central canvas with sidebars for navigation and configuration. Understanding this layout will help you work efficiently.

Top Toolbar

The toolbar spans the top of the window. On the left, the Actions menu provides access to file loading, toolpath management, and SVG export. The center displaysthe workspace title. On the right, you'll find zoom controls (fit, in, out) and the theme toggle.

Left Sidebar: Operations Tree

The left sidebar organizes your loaded files into four operation categories:

Isolation Routing

Copper layer files (Gerber) for trace isolation

Drilling

Drill files (Excellon) for through-holes and vias

Copper Clearing

Gerber files for ground plane or keepout removal

Board Cutout

Outline files for the final board shape

Each category can be expanded or collapsed by clicking its header. Use the + button next to each category to add files specifically for that operation type. When you click on a loaded file, it becomes selected (highlighted), and its properties appear in the right sidebar.

Center Canvas

The main canvas displays your geometry. This is where you'll see source files, generated offsets, and toolpath previews.

Navigation

Pan: Click and drag anywhere on the canvas to move the view.
Zoom: Use the mouse scroll wheel, or the toolbar buttons (+, -, fit).
Fit to View: Press F or click the fit button to automatically zoom and center on all loaded geometry.

Coordinate Display

The bottom-left corner shows real-time cursor coordinates (X, Y) in millimeters, plus the current zoom level. This helps you verify positions and measure distances visually.

Right Sidebar: Properties & Settings

The right sidebar contains three collapsible sections:

Origin & Rotation

Controls where the machine's coordinate origin sits relative to your geometry, plus board rotation. The "Board Size" display shows the dimensions of all loaded geometry.

Machine Settings

Global parameters that affect G-code output: post-processor selection, start/end G-code blocks, units, PCB thickness, safe heights, and rapid feed rate.

Properties

Context-sensitive panel that shows parameters for the currently selected operation. Parameters are organized into three stages: Geometry (2D offsets), Strategy (depth/entry), and Machine (feeds/speeds). Action buttons trigger generation for each stage.

Footer: Status & Visualization

The footer bar at the bottom serves two purposes:

Visualization Panel

Click the eye icon to expand the visualization settings. Here you can toggle display elements (grid, rulers, wireframe), control layer visibility (traces, pads, drills, offsets, previews), and enable advanced debug features. See the Visualization Options section for details.

Status Bar

Shows status messages and progress for operations like file loading, offset generation, and export. Click the status bar to expand a log history showing recent messages—useful for troubleshooting.

The Workflow

EasyTrace5000 follows a non-destructive, staged workflow. Each stage builds on the previous one, and you can always go back to adjust parameters and regenerate. The stages are:

1. Load your source files (Gerber, Excellon, SVG)
2. Position your geometry (origin, rotation)
3. Configure machine settings (heights, speeds, post-processor)
4. Generate Offsets for each operation (2D geometry only)
5. Generate Previews with depth and strategy settings
6. Export G-code with feeds and speeds

Stage 1: Loading Files

There are several ways to load files into EasyTrace5000:

Using the Welcome Modal

When you first open the application (and haven't checked "Don't show this again"), you'll see the Welcome modal. From here you can load a built-in example project, click "Open Files" to access the file upload modal, or click "Start Empty" to begin with a blank workspace.

Using the File Upload Modal

Access this via Actions → Add Files, or the "Open Files" button in the Welcome modal. The modal shows four drop zones, one for each operation type. Drop files onto the appropriate zone, or click a zone to browse.

Drag and Drop

You can drag files directly onto the main application window. EasyTrace5000 will auto-detect the file type by extension and assign it to the appropriate operation category.

Category Add Buttons

In the left sidebar, each operation category has a small + button. Click it to open a file browser filtered for that operation's accepted file types.

Stage 2: Setting Up Coordinates

Verify that your coordinate origin is positioned correctly for your CNC setup.

Origin Offset

The Origin & Rotation panel in the right sidebar shows "Origin Offset" X and Y fields. These values shift where (0,0) sits relative to your geometry. By default, the origin is at the geometry's lower-left corner.

Two shortcut buttons are provided: Center places the origin at the geometry's center point, and Bottom-Left resets it to the lower-left corner.

Board Rotation

If your PCB needs to be rotated (perhaps to fit your stock material orientation), enter a rotation angle in degrees. Click Apply Rotation to rotate all geometry around its center. Reset Rotation returns to 0°.

Why Origin Matters

The origin you set here becomes (0,0) in your G-code output. Most CNC workflows involve homing the machine, then jogging to a known position on your stock and setting the work coordinate system origin there. Your origin setting in EasyTrace5000 should match that physical position—typically a corner or the center of the board.

Stage 3: Machine Settings

The Machine Settings panel contains global parameters that affect all G-code output.

Post-Processor

Select the G-code syntax your machine expects. GRBL is the default and most common for hobbyist CNC routers. Other options (GrblHAL, Marlin, LinuxCNC, Mach3, Roland RML) are experimental so they should be tested with caution.

Start/End G-code

These text areas contain commands that run at the very beginning and end of your program. Use these spaces if you for example you have commands to turn on/off dust collection, etc.

Heights

Safe Z: The height the tool moves to at program start/end and typicallyspindle is turned on/off.
Travel Z: The height for rapid moves between cutting operations. This can be lower than Safe Z for faster operation, but must still clear any clamps and high points.

Stage 4: Generating Offsets

With files loaded and coordinates set, you're ready to generate the toolpath geometry. This stage focuses purely on 2D offset paths—no depth or Z-axis settings yet.

Selecting an Operation

Click on a source file in the Operations Tree (left sidebar). The Properties panel (right sidebar) will collapse the origin and machine sections and show that operation's parameters.

Setting Parameters

The Properties panel shows parameters appropriate for the operation type:

Tool

Select from the tool library dropdown. The tool diameter auto-fills based on your selection.

Tool Diameter

The cutting diameter in mm. Determines the offset distance from source geometry.

Passes

Number of offset passes to generate. More passes = wider isolation zone.

Step Over

Percentage of tool diameter for spacing between passes. 50% = 50% overlap.

Combine Passes

When enabled, merges all passes into a single geometry group.

Operation-Specific Parameters

Mill Holes (Drilling only)

When enabled, undersized holes are milled with helical paths. When disabled, simple peck drilling is used.

Cut Side (Cutout only)

Determines offset direction: Outside (board matches outline), Inside (pocket), or On Line (centered on outline).

Generate Offsets

Click Generate Offsets (or Generate Drill Strategy for drill operations). The geometry engine processes your source geometry and creates 2D offset paths

When complete, new items appear under the file in the Operations Tree: "Pass 1", "Pass 2", etc. The canvas updates to show the offset geometry as thin colored lines representing tool centerlines.

Stage 5: Generating Preview

After generating offsets, you configure cutting strategy and depth settings, then create a preview that simulates what your tool will actually cut.

Depth & Strategy Parameters

When you select an offset pass in the tree, the Properties panel shows depth and strategy settings:

Cut Depth

Target Z depth below the surface. Enter as negative (e.g., -0.1mm) or positive—the system handles both.

Depth per Pass

When Multi-Depth is enabled, how much to cut per Z-level. Multiple passes reach the final depth incrementally.

Multi-Depth

Enable for materials requiring multiple passes to reach full depth. Disable for single-pass cuts.

Entry Type

How the tool enters the material: Plunge (straight down), Ramp (angled entry), or Helix (spiral entry).

Operation-Specific Strategy

Drilling: Canned Cycle

For peck drilling: None (G0+G1), G81 (simple), G82 (dwell), G83 (peck), G73 (stepped peck).

Drilling: Peck Depth / Dwell Time

Depth of each peck before retract, and pause time at hole bottom.

Cutout: Tabs

Number of holding tabs, plus tab width and height settings.

Preview vs. Offset

Offsets show the centerline path the tool will follow—where the spindle axis travels.
Previews show the full width of the tool's cutting envelope—what material will be removed.

Generating the Preview

After configuring depth settings, click Generate Toolpath Preview. A new "Preview" item appears under the file in the tree, and the canvas shows thick strokes representing the tool's cutting area. Offset layers are automatically hidden when preview exists.

Stage 6: Exporting G-code

With previews generated, configure machine parameters and export G-code.

Machine Parameters

When viewing a preview, the Properties panel shows feeds and speeds:

Feed Rate

XY cutting speed in mm/min. Lower = cleaner cuts but slower.

Plunge Rate

Z-axis speed for downward moves. Usually 25-50% of feed rate.

Spindle Speed

RPM for the tool. PCB routing typically uses 10,000-24,000 RPM.

Opening the Operations Manager

Click Operations & G-Code in the Properties panel, or go to Actions menu → Manage Toolpaths.

Selecting and Ordering Operations

Each operation with a generated preview appears as a checkbox item. Check the operations you want to include. Drag items to reorder them. Typical order: Isolation → Drilling → Clearing → Cutout (cutout last so the board stays attached).

Output Options

Export as single file

Combines all selected operations into one G-code file.

Include operation comments

Adds descriptive comments identifying each operation.

Optimize toolpaths (Experimental)

Applies path optimization to reduce travel moves and group nearby cuts.

Output Filename

The filename for the downloaded G-code file.

Calculate and Export

Click Calculate Toolpaths to process. The preview area shows generated G-code with statistics: line count, operation count, estimated time, and total travel distance. Click Export G-code to download.

Operation Types

Each operation type has specific parameters organized across three stages: Geometry (2D offsets), Strategy (depth/entry), and Machine (feeds/speeds).

Isolation Routing

Isolation routing cuts trenches around your PCB traces, electrically separating them from the surrounding copper. The tool follows paths offset outward from the trace edges.

Geometry Stage Parameters

Tool / Tool Diameter

Smaller tools (0.1-0.2mm) allow tighter trace spacing but are fragile.

Passes

Number of concentric offset paths. More passes = wider isolation zone.

Step Over (%)

Distance between passes as percentage of tool diameter. 50% gives good overlap.

Strategy Stage Parameters

Cut Depth

For standard 35µm (1oz) copper on FR4, 0.1-0.15mm is typical.

Multi-Depth / Depth per Pass

Enable for deeper cuts requiring multiple Z passes.

Entry Type

Plunge (default), Ramp, or Helix entry into material.

Machine Stage Parameters

Feed Rate

XY cutting speed. 100-400 mm/min typical for PCB isolation.

Plunge Rate

Z-axis cutting speed. Usually 25-50% of feed rate.

Spindle Speed

10,000-24,000 RPM typical for PCB work.

Drilling

Drilling operations process Excellon files containing hole and slot definitions. EasyTrace5000 analyzes each feature against your tool diameter and selects an appropriate strategy.

Strategy Selection

The system compares each hole/slot diameter to your tool diameter:

Exact Fit (green)

Hole diameter equals tool diameter. Uses peck/plunge drilling.

Undersized Tool (yellow)

Tool is smaller than hole. If "Mill Holes" is enabled, uses helical milling.

Oversized Tool (red)

Tool is larger than hole. Will peck at center (hole will be oversize).

Geometry Stage Parameters

Tool / Tool Diameter

Select a drill bit or end mill matching your hole sizes.

Mill Holes

Enable to use helical milling for undersized holes instead of simple drilling.

Strategy Stage Parameters

Cut Depth

Total drilling depth (typically PCB thickness + clearance).

Entry Type

Plunge (standard drilling) or Helix (spiral entry for milled holes).

Canned Cycle

For peck drilling: None, G81, G82 (dwell), G83 (peck), G73 (stepped).

Peck Depth

Depth of each peck before retracting. 0 = single plunge.

Dwell Time

Pause at hole bottom (seconds). Helps clear chips.

Copper Clearing

Copper clearing removes large areas of unwanted copper. Unlike isolation (outward offsets), clearing offsets inward to pocket out the interior.

Geometry Stage Parameters

Tool / Tool Diameter

Larger tools clear faster.

Number of inward offset passes.

Step Over (%)

50% provides good material removal and tool engagement.

Strategy Stage Parameters

Cut Depth / Multi-Depth

Same as isolation—configure depth per pass for thick copper.

Entry Type

Ramp or Helix recommended for pocket entry.

Board Cutout

Cutout operations generate the path to separate your finished PCB from stock material.

Geometry Stage Parameters

Tool / Tool Diameter

Wider, stronger cutting tools can be used for faster cutting and a lower risk of breaking.

It's common to try and re-use the same tool as used for drilling.

Cut Side

Outside: Physical board will match outline file.
Inside: If geometry is oversized.
On: Tool center follows the polygon perimeter line.

Strategy Stage Parameters

Cut Depth / Multi-Depth

Full PCB thickness. Multi-depth required for thick material.

Number of Tabs

Holding tabs around perimeter. 4-6 typical for small boards.

Tab Width

Width of each tab in mm. 2-3mm usually sufficient.

Tab Height

Material left in tab. 0.3-0.5mm—enough to hold but easy to remove.

Machine Settings Reference

This section provides detailed information about each machine setting and typical values.

Post-Processor

Height Settings

Safe Z (typical: 5-15mm)

Maximum clearance height. Used at program start/end. Should clear all clamps, fixtures, and the highest point of your workpiece.

Travel Z (typical: 2-5mm)

Height for rapid moves between cutting operations. Lower than Safe Z for faster operation, but must still clear the workpiece surface and any chips/debris.

Speed Settings

Rapid Feed (typical: 1000-3000 mm/min)

Speed for G0 positioning moves. Some controllers ignore this (moving at max speed), while others respect it.

Feed Rate (per-operation, typical: 100-400 mm/min for PCB work)

Cutting speed during milling. Lower = cleaner cuts but slower. Higher = faster but risks tool breakage or poor cut quality.

Plunge Rate (per-operation, typical: 30-100 mm/min)

Speed for downward (Z-axis) cutting moves. Usually much slower than XY feed rate because plunging loads the tool differently.

Spindle Speed (per-operation, typical: 10000-24000 RPM)

Rotation speed of the spindle/tool. PCB routing typically uses high speeds with low feed rates.

Visualization Options

The Visualization panel (footer, left side—click the eye icon) controls what appears on the canvas. Most are development leftovers but fun to use.

Display Options

Grid

Shows a reference grid on the canvas. Grid spacing adapts to zoom level.

Wireframe

Renders all geometry as paths only (no fill). Useful for debugging file geometry.

Board Bounds

Shows a rectangle indicating the overall bounds of all loaded geometry.

Rulers

Displays measurement rulers along the canvas edges with tick marks in mm.

Layer Visibility

Regions

Filled areas (copper pours, pads) from source geometry.

Traces

Line/stroke elements (traces, routes) from source geometry.

Pads

Individual pad flashes from source geometry.

Drills

Drill holes and slots from source geometry.

Cutouts

Board outline geometry.

Offsets

Generated offset geometry (thin lines showing toolpath centerlines).

Previews

Generated preview geometry (thick strokes showing tool cutting area).

Advanced Options

Fusion Mode

Enables boolean fusion of overlapping geometry. When multiple shapes overlap, they're merged into unified polygons.

Preprocessed

Show source geometry already polygonized, pre-boolean.

Arc Reconstruction

Attempts to recover true circular arcs from polygonized geometry post boolean operations. Allows arc commands instead of many small line segments.

Debug Points / Debug Arcs

Shows diagnostic overlays for geometry debugging. (Can highlight previous visualization options.)

B&W Mode

Renders geometry in black and white only.

Verbose Debug

At the bottom of the Visualization panel is a "Verbose Debug" toggle. When enabled, detailed logging information appears in the browser's developer console and in the status log history. Useful for troubleshooting issues.

Tips & Troubleshooting

Best Practices

Start with an Example

Before processing your own files, load the built-in example and walk through the complete workflow. This helps you understand what to expect at each stage.

Verify Origin Before Export

Always double-check your origin setting before generating final G-code. The origin in EasyTrace5000 must match where you'll set your work coordinate origin on the machine.

Process Operations in Order

When exporting G-code, consider the logical order of operations:

1. Isolation routing (creates the trace boundaries)
2. Copper clearing (removes unwanted copper)
3. Drilling (a lot of times can use the cutout tool, or vice versa)
4. Cutout (last, so the board stays attached during other operations)

Common Issues

Always Blank/black canvas

Cause: Browsers can be weird, especially laptops with multiple GPUs.
Solution: Closing and restarting the browser should load the canvas viewport correctly.

Files Won't Load

Cause: Unlikely silent parsing error
Solution: Try reviewing file contents or testing in another operation/extension.

Geometry Appears Rotated or Mirrored

Cause: Your EDA software may use different coordinate conventions.
Solution: Use the Rotation setting to correct orientation. For mirroring, flip the design in your EDA before export.

Drill Holes Wrong Size

Cause: Tool doesn't match hole diameter and milling is disabled.
Solution: Enable "Mill Holes" for undersized tools, or use a drill bit matching your hole sizes.

Offset Generation Takes Long

Boolean operations on complex geometry are computationally intensive. More passes takes longer to calculate.