MapleCAM User Guide

MapleCAM is desktop CAM software for CNC routers and mills. It generates toolpaths and G-code from SVG and DXF designs.

What MapleCAM Does

1. Import vector designs (SVG or DXF files)
2. Create operations that describe how to cut each part (contour, pocket, engrave, V-carve, and more)
3. Generate toolpaths — the precise paths your cutting tool will follow
4. Validate toolpaths against your stock using 3D simulation
5. Export G-code for your CNC machine (GRBL or LinuxCNC)

Quick Start

If you're new to MapleCAM, start with Installation and then follow Your First Project for a guided walkthrough.

Documentation Sections

• Getting Started — Install, set up your machine, and complete your first project
• Workflow — How MapleCAM's design-to-G-code pipeline works
• Importing Designs — Bringing SVG and DXF files into MapleCAM
• Operations — Reference for all operation types (contour, pocket, V-carve, laser, etc.)
• Tools — Managing your tool library and presets
• Machines — Configuring machines and G-code dialects
• Visualization — 2D canvas, 3D view, and toolpath validation
• Exporting — Generating G-code and SVG output
• Reference — Keyboard shortcuts, project settings, defaults
• Troubleshooting — Common issues and FAQ

Installation

System Requirements

• Java 21 or later (free, from Adoptium)
• Operating System: Windows 10+, macOS 12+, or Linux (X11 or Wayland)
• Memory: 4 GB RAM minimum, 8 GB recommended
• Disk: ~100 MB for MapleCAM + Java runtime

Download

Download the latest release from the MapleCAM website.

Install Java

MapleCAM requires Java 21 or later. If you don't already have it:

1. Visit Adoptium
2. Download the installer for your platform
3. Run the installer with default settings

To verify your installation, open a terminal and run:

java -version

You should see output showing version 21 or later.

Running MapleCAM

Windows

Double-click the downloaded .jar file, or run from a terminal:

java -jar MapleCAM.jar

macOS

java -jar MapleCAM.jar

Linux

java -jar MapleCAM.jar

Initial Setup

When you first launch MapleCAM, the Initial Setup Wizard guides you through configuring your CNC machine.

The Setup Wizard

The wizard walks through:

1. Machine name — a label for your machine (e.g., "Shapeoko 4", "3018 Pro")
2. Work area — the X, Y, and Z travel dimensions of your machine, in millimeters
3. Capabilities — whether your machine has a spindle, a laser, or both
4. Spindle settings — minimum and maximum RPM (if applicable)
5. Safe Z height — the Z height for rapid moves above the stock (typically 5-10mm above your material)

After Setup

Your machine configuration is saved to your user profile and will be available in all future projects. You can modify it later via Tools > Machine Setup.

You can also configure additional machines if you have more than one CNC — each project selects which machine it targets.

Next Steps

Proceed to Your First Project for a guided walkthrough of the full workflow.

Your First Project

This walkthrough takes you from a blank project to exported G-code. We'll cut a simple shape using an outside contour operation.

1. Create a New Project

Launch MapleCAM. A new empty project opens automatically. If you already have a project open, use File > New Project (Ctrl+N).

2. Configure Stock

Open Tools > Project Settings and enter your stock dimensions:

• Width (X): the width of your material in mm
• Height (Y): the depth of your material in mm
• Thickness (Z): the thickness of your material in mm

The stock appears as a rectangle on the 2D canvas.

3. Import a Design

Drag and drop an SVG or DXF file onto the canvas, or use File > Import SVG / File > Import DXF.

Your design appears as paths on the canvas, positioned within the stock boundary.

4. Select Paths

Click on a path to select it. Hold Shift to select multiple paths. Selected paths highlight in the canvas and in the project tree on the left.

5. Create an Operation

With paths selected, create an operation in one of three ways:

• Right-click the selection and choose an operation type
• Toolbar — click the operation button in the toolbar
• Keyboard chord — press Ctrl+E, then C for a contour operation

For this walkthrough, create an outside contour to cut the shape out of your stock.

6. Assign a Tool

In the property panel on the right, click the tool dropdown and select an endmill from the built-in tool library. A 1/4" (6.35mm) flat endmill is a common starting point.

7. Configure Settings

The property panel shows the operation settings. Key settings for a contour:

• Cut side: Outside (to cut around the shape)
• Depth: Set to your stock thickness (or slightly deeper) to cut through
• Tabs: Enable hold-down tabs to prevent the part from moving during the final pass

Feed rate, spindle speed, and depth per pass come from the tool preset — you can adjust them if needed.

8. Preview Toolpaths

Toolpaths generate automatically when you configure an operation. Switch to the 3D view (F5) to see the cutting paths visualized against your stock.

9. Validate

Run toolpath validation to check for errors. The validator simulates the cut using a 3D voxel model and reports any overcuts or issues.

10. Export G-code

Use File > Export G-code (or the toolbar button). Choose your G-code dialect:

• GRBL — for GRBL-based controllers (most hobby CNC machines)
• LinuxCNC — for LinuxCNC-based controllers

Save the .nc file and load it into your CNC controller software.

The CAM Pipeline

MapleCAM follows a four-stage pipeline from design to machined part:

Design → Operations → Toolpaths → G-code

1. Design (Import)

You start with a 2D vector design — an SVG or DXF file created in tools like Inkscape, Illustrator, LibreCAD, or AutoCAD. The design contains paths (lines, arcs, curves) that define the shapes you want to cut.

2. Operations

You assign operations to paths. An operation describes how to cut: contour around the outside, pocket out the interior, engrave along the line, V-carve with variable depth, etc. Each operation has settings like cut depth, feed rate, and tool selection.

3. Toolpaths

MapleCAM generates toolpaths from your operations. Toolpaths are the precise XYZ coordinates your cutting tool will follow, including:

• Tool offset (compensating for the tool's radius)
• Multi-pass depth stepping
• Lead-in and lead-out moves
• Rapid positioning between cuts
• Tab placement for hold-down tabs

Toolpath generation is automatic — it runs whenever you change an operation's settings.

4. G-code

Finally, you export G-code — the machine-readable instructions for your CNC controller. MapleCAM translates toolpaths into the G-code dialect your machine understands (GRBL, LinuxCNC, etc.), including spindle/laser control, feed rates, and safe movement heights.

Coordinate System

MapleCAM uses a right-handed coordinate system measured in millimeters:

• X — right (positive) / left (negative)
• Y — forward (positive) / backward (negative)
• Z — up (positive) / down (negative)

Z=0: The Stock Surface

The top surface of your stock is always at Z = 0. Cutting goes into negative Z values. For example, if your stock is 20mm thick, the bottom of the stock is at Z = -20.

This convention matches most CNC workflows where you zero the Z axis to the top of the material.

Safe Z and Clearance Height

Two Z heights control rapid (non-cutting) movement:

• Safe Z — the height for rapid moves between distant cuts (typically 5-10mm above stock). The tool lifts to Safe Z when moving between separate regions.
• Clearance height — a smaller lift for moves between nearby paths within the same operation (micro-lifts). This is faster than lifting all the way to Safe Z.

Both values are positive Z (above the stock surface) and are configured in Project Settings.

Projects and Files

Project Files (.mcp)

MapleCAM saves projects as .mcp files — compressed JSON containing your stock dimensions, imported parts, operations, tool assignments, and all settings. The design geometry is embedded in the project file, so you don't need to keep the original SVG/DXF alongside it.

Creating and Saving

• New Project — File > New Project (Ctrl+N)
• Save — File > Save (Ctrl+S)
• Save As — File > Save As (Ctrl+Shift+S)

Multi-Tab Editing

MapleCAM supports multiple projects open simultaneously in separate tabs. Each tab has its own undo/redo history, selection state, and dirty flag.

Recent Files

The File menu shows recently opened projects for quick access. Use File > Clear Recent Files to reset the list.

Project Settings

Each project stores:

• Stock dimensions — width (X), height (Y), thickness (Z)
• Material — selected from the material library (affects recommended feed rates)
• Machine — which machine configuration to target
• Safe Z — height for rapid positioning moves
• Clearance height — height for short repositioning moves

SVG Import

MapleCAM imports SVG (Scalable Vector Graphics) files — the most common format for 2D vector designs.

How to Import

• Drag and drop an SVG file onto the canvas
• File > Import SVG (menu)

Supported SVG Elements

MapleCAM supports standard SVG path elements including lines, arcs, cubic and quadratic Bezier curves, and basic shapes (rect, circle, ellipse, polygon, polyline). Transforms (translate, rotate, scale, matrix) are applied during import.

Tips for Preparing SVGs

• Convert text to paths — MapleCAM imports geometry, not fonts. In Inkscape: select text, then Path > Object to Path.
• Flatten transforms — while MapleCAM handles transforms, flattening them in your editor can avoid surprises.
• Remove clipping masks and filters — MapleCAM ignores raster effects, gradients, and clipping paths.
• Use mm units — MapleCAM interprets SVG coordinates in millimeters. Set your document units to mm for accurate sizing.
• Check path direction — for contour operations, path direction (CW vs CCW) can affect which side is "inside" vs "outside."

DXF Import

MapleCAM imports DXF (Drawing Exchange Format) files — the standard interchange format for CAD software.

How to Import

• Drag and drop a DXF file onto the canvas
• File > Import DXF (menu)

Supported DXF Entities

MapleCAM supports common DXF entities including LINE, ARC, CIRCLE, ELLIPSE, LWPOLYLINE, POLYLINE, and SPLINE.

Tips for Preparing DXFs

• Use mm units — ensure your DXF is drawn in millimeters for accurate sizing.
• Join open paths — disconnected line segments may not form closed contours. Use your CAD software's "join" or "pedit" command to create closed polylines.
• Flatten to 2D — MapleCAM imports 2D geometry. If your DXF contains 3D elements, flatten them before importing.
• Remove construction geometry — layers containing reference lines, dimensions, or annotations should be removed or hidden before export.

Working with Parts

When you import a design, it becomes a part in your project. A project can contain multiple parts, each imported from a separate file.

Selecting Parts

Click on a part in the 2D canvas or in the project tree to select it. Hold Shift to select multiple parts or paths.

Positioning

Drag a selected part on the 2D canvas to reposition it within your stock area. Parts must fit within the stock dimensions to generate valid toolpaths.

Parts in the Project Tree

The project tree (left panel) shows all parts and their paths. Expand a part to see individual paths, and expand paths to see the operations assigned to them.

Operations Overview

An operation tells MapleCAM how to cut a path or set of paths. Each operation type produces different toolpaths suited to different tasks.

Operation Types

Spindle Operations

Laser Operations

Creating Operations

There are three ways to create an operation:

1. Right-click selected paths and choose from the context menu
2. Toolbar buttons for common operation types
3. Keyboard chords — press Ctrl+E then a key for spindle operations, or Ctrl+L then a key for laser operations (see Keyboard Shortcuts)

The Property Panel

When an operation is selected, the property panel on the right shows all configurable settings. Changes take effect immediately and toolpaths regenerate automatically.

Property Cascade

Operation settings are resolved through a cascade:

1. Operation — settings you've explicitly set on this operation
2. Operation Group — inherited from the group (display grouping only)
3. Tool Preset — defaults from the assigned tool's preset
4. Built-in Default — hardcoded fallback values

This means you only need to override the settings that differ from your tool preset.

Contour

A contour operation cuts along a path, offsetting the tool to one side so the finished edge is exactly on the design line.

Cut Side

• Outside — tool cuts outside the path (for cutting a shape out of stock)
• Inside — tool cuts inside the path (for cutting a hole or recess)
• On-line — tool center follows the path exactly (no offset)

Key Settings

Tabs

Hold-down tabs are small bridges of uncut material that keep the part attached to the stock during the final passes. Without tabs, a part cut all the way through may shift or be thrown by the cutting tool.

Tab settings:

• Tab count — number of tabs around the contour
• Tab width — width of each tab (mm)
• Tab height — height of uncut material (mm)

Multi-Pass Depth

If the total depth exceeds the depth-per-pass setting, MapleCAM generates multiple passes at increasing depths. The final pass cuts to the exact target depth.

When to Use Contour

• Cutting shapes out of stock (outside contour + tabs)
• Cutting holes or slots (inside contour)
• Profiling edges to final dimension

Pocket

A pocket operation clears material from an enclosed area, cutting the interior down to a specified depth.

Clearing Strategies

MapleCAM offers three clearing strategies:

Offset

Concentric passes moving inward from the boundary. Produces a clean finish on the pocket walls. Best for finish quality.

Raster

Back-and-forth parallel lines across the pocket area. Fast material removal but may leave small scallops on walls. Best for roughing or when wall finish doesn't matter.

Spiral

A continuous spiral path from outside in. Maintains constant tool engagement for consistent cutting forces. Good balance of speed and finish.

Key Settings

Islands

If a pocket path contains inner paths (holes or shapes inside the boundary), MapleCAM treats them as islands — raised areas that are not cleared. This allows cutting pockets with complex internal geometry.

When to Use Pocket

• Recesses and cavities
• Clearing areas for inlays
• Removing large volumes of material
• Any enclosed area that needs to be lowered

Facing

A facing operation surfaces the top of your stock flat. It's a specialized pocket that covers the entire stock area (or a margin within it).

When to Use Facing

• Flattening warped or uneven material
• Bringing stock to an exact thickness
• Creating a smooth reference surface before other operations

Key Settings

Facing vs Pocket

Facing is essentially a pocket operation that covers the entire stock area. Use facing when you want to surface the whole top; use a pocket when you want to clear a specific enclosed region.

Engrave

An engrave operation follows paths at a fixed shallow depth. The tool center travels exactly along the design path with no offset.

Key Settings

Engrave vs Contour (On-Line)

Both engrave and on-line contour follow the path centerline. The difference:

• Engrave is designed for shallow, single-pass marking
• Contour (on-line) supports multi-pass depth, tabs, and lead-in/out

For simple shallow marking, engrave is simpler. For deeper cuts along a line, use an on-line contour.

When to Use Engrave

• Text and lettering (with text converted to paths)
• Fine detail lines
• Serial numbers or labels
• Decorative line work

V-Carve

A V-carve operation uses a V-shaped bit to carve paths at variable depth. Narrow areas are cut shallowly, wide areas are cut deeply. This produces the classic "carved sign" look where the bottom of each groove forms a V profile.

How V-Carving Works

MapleCAM computes the medial axis (centerline skeleton) of each enclosed region. The V-bit follows this centerline, plunging deeper where the region is wider and shallower where it's narrow. The result is a groove whose edges precisely follow the design outline.

Key Settings

Flat-Bottom V-Carving

For designs with wide areas, the V-bit alone may not reach the full width without cutting excessively deep. Flat-bottom V-carving uses a flat endmill to clear the wide areas first, then the V-bit finishes the edges. This limits the maximum depth while still producing clean V-shaped edges.

When to Use V-Carve

• Wooden signs and lettering
• Decorative carving
• Any design where you want a classic hand-carved appearance
• Works best with enclosed shapes (closed paths)

Chamfer

A chamfer operation cuts an angled edge along a path using a V-bit. Unlike V-carve (which fills enclosed areas), chamfer follows the path edge to create a beveled edge.

Key Settings

When to Use Chamfer

• Decorative edge bevels on cut parts
• Deburring edges after contour cuts
• Creating angled edges for visual or functional purposes

Helical Contour

A helical contour is a contour operation that enters the material using a helical (spiral) ramp rather than a straight plunge. This is gentler on the tool and produces a better surface finish, especially for deep cuts.

How It Works

Instead of plunging straight down to each depth level, the tool spirals downward along the contour path, gradually reaching the target depth. This distributes the cutting force and avoids the shock of a straight plunge.

Key Settings

Same as Contour, with the addition of helical entry behavior. All contour settings (cut side, depth, tabs, etc.) apply.

When to Use Helical Contour

• Deep contour cuts where straight plunging would stress the tool
• Hard materials where gradual engagement is important
• When surface finish on the contour wall matters

Decorative Patterns

MapleCAM includes 92 built-in decorative patterns across 8 categories. Patterns fill an enclosed region with geometric designs, which are then cut using standard toolpath generation.

Pattern Categories

Applying a Pattern

1. Select an enclosed path
2. Create a Pattern operation (Ctrl+E, A)
3. Choose a pattern category and design from the dropdown
4. Adjust scale and rotation as needed

Pattern Settings

When to Use Patterns

• Decorative panels and wall art
• Coasters and trivets
• Custom signage backgrounds
• Anywhere you want a geometric fill instead of a plain surface

Laser Operations

Laser operations are available when your machine has a laser capability enabled. They use laser power and travel speed instead of spindle speed and feed rate.

Laser vs Spindle Operations

Laser Operation Types

• Laser Contour — vector cutting along paths
• Laser Engrave — raster engraving of filled areas
• Laser Hatch — line-fill patterns inside regions
• Laser Pattern — decorative patterns via laser

Creating Laser Operations

Use the keyboard chord Ctrl+L followed by:

Laser operations only appear when the current machine has laser capability enabled.

Laser Contour

A laser contour operation cuts or marks along paths using the laser. The laser follows the design paths, burning through or marking the material.

Key Settings

When to Use

• Cutting thin materials (plywood, acrylic, cardboard)
• Marking or scoring lines on surfaces

Laser Engrave

A laser engrave operation fills enclosed areas with raster scanning, burning the surface to create an engraved image or filled region.

Key Settings

When to Use

• Engraving images or photos onto material
• Filling enclosed shapes with a burned surface
• Creating solid dark areas

Laser Hatch

A laser hatch operation fills enclosed areas with parallel lines at a specified angle, creating a hatched or shaded appearance.

Key Settings

When to Use

• Shading or texturing areas
• Creating crosshatch patterns (multiple hatch operations at different angles)
• Area marking without full raster fill

Laser Pattern

A laser pattern operation fills an enclosed area with a decorative pattern, cut using the laser. This is the laser equivalent of the Decorative Patterns spindle operation.

Key Settings

When to Use

• Decorative laser-cut panels
• Intricate pattern work on thin material
• Ornamental designs that would be difficult with a spindle

Tool Library

MapleCAM maintains a tool library — a persistent collection of cutting tools with their dimensions and default cutting parameters. The library is shared across all projects and stored in your user profile (~/.maplecam/tools.json).

Built-in Tools

MapleCAM ships with a set of common tools pre-configured. These cover typical endmill sizes, V-bits, and other common cutters.

Managing Tools

Open the tool library via Tools > Tool Library.

From the library dialog you can:

• Add a new tool with custom dimensions
• Edit an existing tool's properties
• Delete tools you don't use
• Duplicate a tool as a starting point for a similar one

Assigning Tools to Operations

When you create or select an operation, the property panel shows a tool dropdown. Only tools compatible with the operation type are shown:

• Flat and ball endmills — contour, pocket, facing, engrave
• V-bits — V-carve, chamfer, engrave
• Any tool — engrave operations accept all tool types

Tool Properties

Tool Types

MapleCAM supports the following cutting tool types:

Flat Endmill

A cylindrical cutter with a flat bottom. The most common CNC tool. Produces flat-bottomed pockets and square-cornered profiles.

Best for: Pockets, contours, facing, engrave

Ball Endmill

A cutter with a hemispherical tip. Produces a rounded bottom in cuts. Used for 3D surface finishing and smooth contours.

Best for: 3D surface finishing, smooth pocket floors, contours where rounded bottoms are acceptable

V-Bit

A conical cutter with a pointed tip. The cutting width depends on depth — deeper cuts are wider. Characterized by the included angle (e.g., 60, 90 degrees).

Best for: V-carving, chamfering, fine engraving

Tapered Endmill

An endmill with tapered sides. Produces angled walls in pockets and contours. Stronger than a straight endmill for deep cuts.

Best for: Mold making, deep pockets with draft angles

Surfacing Bit

A large-diameter cutter designed for flattening stock surfaces. Often called a spoilboard surfacing bit or fly cutter.

Best for: Facing operations, spoilboard surfacing

Presets and the Property Cascade

What Are Presets?

A preset stores default cutting parameters for a tool. When you assign a tool to an operation, the preset's values become the starting point for that operation's settings.

Preset parameters include:

The Property Cascade

When MapleCAM needs a value for an operation setting, it looks through a cascade of sources:

1. Operation — if you've explicitly set the value on this operation, that value is used
2. Operation Group — if the operation is part of a group, group-level settings apply
3. Tool Preset — the assigned tool's preset provides defaults
4. Built-in Default — hardcoded fallback values

This means:

• You only need to override settings that differ from your tool preset
• Changing a tool preset updates all operations using that tool (unless they have explicit overrides)
• Operation-level overrides always take priority

Material-Specific Presets

Different materials require different cutting parameters. The material selected in Project Settings can influence recommended preset values.

Default Presets

See Default Tool Presets for a table of the built-in preset values.

Machine Configuration

A machine in MapleCAM describes your CNC hardware — its physical dimensions, capabilities, and the G-code dialect it speaks.

Machine Properties

Creating a Machine

Use Tools > Machine Setup wizard, or open Tools > Manage Machines for direct editing.

The Machine Setup wizard walks you through each setting step by step. Direct editing gives you access to all fields at once.

Multiple Machines

You can configure multiple machines. Each project selects which machine it targets. The machine selection affects:

• Available operation types (spindle vs laser)
• G-code dialect for export
• Work area validation (parts must fit within the machine's travel)
• Spindle speed range validation

Machine Storage

Machine configurations are saved in your user profile (~/.maplecam/machines.json) and are available across all projects.

G-code Dialects

MapleCAM supports multiple G-code dialects to match different CNC controllers.

Supported Dialects

GRBL

The most common controller for hobby CNC machines. Used by Shapeoko, X-Carve, OpenBuilds, 3018 machines, and many others.

Key characteristics:

• Spindle control via M3 S{speed} / M5
• Feed rate set with F{rate} on motion commands
• Arc commands G2/G3 with I/J offsets
• No subroutines or canned cycles

LinuxCNC

An open-source CNC controller running on Linux PCs. Common in more advanced hobby and semi-professional setups.

Key characteristics:

• Full G-code implementation including canned cycles
• Spindle control via M3 S{speed} / M5
• Supports tool change (M6 T{n})
• Comment syntax: ; comment or ( comment )

Dialect Differences

Choosing a Dialect

Select the dialect in your machine configuration. If you're unsure, GRBL is the safe default — it works with the majority of hobby CNC controllers.

The dialect is used during G-code export. You can change it at any time without regenerating toolpaths.

2D Canvas

The 2D canvas is MapleCAM's primary design view. It shows your stock, imported parts, and toolpath previews from above.

Navigation

Canvas Elements

• Grid — reference grid (toggleable)
• Rulers — millimeter rulers along top and left edges
• Stock outline — rectangle showing your material dimensions
• Parts — imported design geometry (paths and shapes)
• Toolpaths — cutting paths overlaid on the design (when generated)
• Selection highlight — selected paths and operations are highlighted

Selecting

• Click a path to select it
• Shift+click to add to selection
• Click empty space to deselect all

Dragging Parts

Click and drag a selected part to reposition it within the stock area.

3D View

The 3D view shows a three-dimensional visualization of your stock, toolpaths, and simulated cutting results. Toggle it with F5 or View > 3D View.

Camera Controls

Visualization Layers

The 3D view displays multiple layers that can be toggled individually:

Layer Visibility

Toggle layer visibility using the controls in the 3D view toolbar. Hiding layers like rapids or cutting volumes can make complex toolpaths easier to read.

Toolpath Validation

MapleCAM includes a 3D voxel-based toolpath validator that simulates your operations against the stock and detects errors before you run your machine.

What Validation Checks

The validator builds a 3D voxel model of your stock, then simulates each toolpath cutting through it. It detects:

• Overcuts — the tool removing material outside the intended operation region
• Plunge errors — the tool entering material at an unsafe rate or location
• Boundary violations — cutting outside the stock dimensions

Running Validation

Validation runs automatically after toolpath generation. Progress is shown in the status bar. You can also manually trigger it via Operations > Recalculate Toolpaths.

Interpreting Results

After validation completes, the project tree shows status indicators on each operation:

• Pass — no issues detected
• Warning — potential issues that may be acceptable
• Error — definite problems that should be fixed before cutting

The 3D view's Remaining Material layer shows the voxel simulation result — you can visually inspect what material remains after all operations.

Validation Resolution

The validator uses a default voxel resolution of 0.2mm. This means the simulation has approximately 0.2mm precision — features smaller than this may not be accurately represented.

Always Validate Before Cutting

Validation is your last check before sending G-code to your machine. While it can't catch every possible issue (e.g., workholding, tool breakage), it catches the most common CAM errors that could damage your work or machine.

G-code Export

Exporting G-code is the final step — it translates your toolpaths into machine-readable instructions.

How to Export

1. File > Export G-code or use the toolbar export button
2. Choose a file location and name (.nc extension)
3. The G-code is written using the dialect configured in your machine settings

What the G-code Contains

The exported file includes:

• Header — initialization commands, units (G21 for mm), coordinate mode
• Spindle start — M3 S{rpm} to start the spindle
• Toolpaths — G0 (rapid) and G1 (linear) / G2/G3 (arc) moves
• Safe Z retracts — G0 Z{safe} between operations
• Spindle stop — M5 at the end
• Footer — return to safe position, program end (M2 or M30)

Pre-Export Checklist

Before exporting, verify:

1. All operations have valid toolpaths (no errors in the tree)
2. Toolpath validation passes (no overcuts)
3. Stock dimensions match your actual material
4. Tool assignments are correct
5. Feed rates and speeds are appropriate for your material

G-code Dialects

The export format is determined by your machine's G-code dialect. See G-code Dialects for details on supported dialects and their differences.

SVG Export

MapleCAM can export your toolpaths as an SVG file. This is useful for documentation, review, or further processing in vector graphics software.

How to Export

File > Export SVG — saves the current toolpaths as vector paths in an SVG file.

What's Included

The exported SVG contains the toolpath geometry — the actual paths the tool follows. This includes cutting moves but typically not the stock outline or rapid moves.

When to Use SVG Export

• Creating documentation of your cutting plan
• Reviewing toolpaths in a vector editor
• Sharing toolpath previews without sharing the full project file

Keyboard Shortcuts

Standard Shortcuts

Key Chords — Spindle Operations (Ctrl+E)

Press Ctrl+E to enter endmill operation mode, then press the second key within 2 seconds. Available operations appear in the status bar. Press Escape to cancel.

Spindle operation chords are only available when the current machine has spindle capability.

Key Chords — Laser Operations (Ctrl+L)

Press Ctrl+L to enter laser operation mode, then press the second key.

Laser operation chords are only available when the current machine has laser capability.

Canvas Navigation

3D View Navigation

Project Settings

Access via Tools > Project Settings.

Stock

Heights

Material

Select the material from the material library. Material selection affects recommended cutting parameters.

Machine

Select which machine configuration this project targets. This determines available operation types and G-code dialect for export.

Default Tool Presets

MapleCAM ships with a library of pre-configured tools and presets. These are based on tested speeds and feeds for hobby CNC machines.

Tool Categories

• V-Bits — 30, 60, 90 degree V-bits in various sizes
• Ball Nose — ball endmills for 3D finishing
• Tapered Ball — tapered ball endmills for detailed carving
• Flat Endmills — standard flat endmills from 1mm to 1/2 inch
• Compression — compression spiral endmills for clean edges on sheet goods
• Surfacing — large diameter surfacing/spoilboard bits

Preset Values

Preset values vary by tool size and type. Key parameters:

Customizing Presets

Open the Tool Library (Tools > Tool Library) to view, edit, or create tool presets. Changes are saved to your user profile and persist across projects.

Default Materials

MapleCAM's material library includes common CNC materials organized by category.

Material Categories

How Material Affects Operations

The selected material influences recommended cutting parameters through tool presets. Harder materials generally require:

• Lower feed rates
• Lower depth per pass
• Potentially lower spindle speeds (especially metals)

Customizing Materials

Materials are stored in your user profile (~/.maplecam/materials.json).

Supported SVG Elements

This page lists the SVG elements and attributes that MapleCAM can import.

Supported Elements

Supported Attributes

Not Supported

• Text elements (convert to paths in your editor first)
• Raster images (<image>)
• Gradients and patterns (fill/stroke styling)
• Clipping paths and masks
• CSS styling (inline style attribute is partially supported)
• Filters and effects
• <use> / <defs> references (may have partial support)

Supported DXF Entities

This page lists the DXF entities that MapleCAM can import.

Supported Entities

Not Supported

• 3D entities (3DFACE, 3DSOLID, MESH)
• Dimension entities
• Text and MTEXT
• Hatching
• Blocks and INSERT references (may have partial support)
• External references (XREF)

Common Issues

No toolpaths generated

Symptom: You created an operation but no toolpaths appear.

Possible causes:

• No paths are assigned to the operation — select paths first, then create the operation
• The tool is too large for the geometry — try a smaller diameter tool
• Depth is set to zero — check the depth setting in the property panel
• The operation has an error — check the project tree for error indicators

"No compatible tools" when creating an operation

Symptom: The tool dropdown is empty or shows no options.

Possible cause: The tool library has no tools compatible with the selected operation type. For example, V-carve operations require V-bits.

Fix: Open Tools > Tool Library and add a compatible tool, or use one of the built-in tools.

Export produces empty or very small G-code file

Symptom: The exported G-code file contains only header/footer but no cutting moves.

Possible causes:

• No operations have generated toolpaths
• All operations have errors
• Stock dimensions are zero

Validation shows overcuts

Symptom: Toolpath validation reports overcut errors.

Possible causes:

• Tool diameter is too large for tight corners in the geometry
• Contour cut side is wrong (inside vs outside)
• Operations overlap in ways that remove unintended material

Fix: Review the operation settings, consider a smaller tool, or adjust the geometry.

Imported design is wrong size

Symptom: The imported SVG or DXF is much larger or smaller than expected.

Possible causes:

• SVG units are not set to millimeters — MapleCAM interprets SVG coordinates in mm
• DXF was drawn in inches — convert to mm in your CAD software before exporting
• ViewBox scaling mismatch in SVG

Fix: Check your design software's export settings and ensure units are millimeters.

Application won't start

Symptom: Double-clicking the JAR file does nothing, or a command-line error appears.

Possible causes:

• Java is not installed or is an older version
• Java installation is not on the system PATH

Fix: Install Java 21 or later from Adoptium. Verify with java -version.

FAQ

What file formats can MapleCAM import?

SVG (Scalable Vector Graphics) and DXF (Drawing Exchange Format). Both are 2D vector formats. See SVG Import and DXF Import for details on supported elements.

What CNC controllers does MapleCAM support?

MapleCAM exports G-code for GRBL and LinuxCNC controllers. GRBL covers the majority of hobby CNC machines (Shapeoko, X-Carve, OpenBuilds, 3018, etc.). See G-code Dialects.

Can MapleCAM do 3D carving?

MapleCAM is a 2.5D CAM application — it works with 2D designs and controls depth (Z), but does not support full 3D surface machining from STL or 3D models. V-carving provides variable-depth cutting within 2D shapes.

What units does MapleCAM use?

All dimensions are in millimeters. If your design is in inches, convert before importing.

Where are my settings stored?

User data (tools, machines, materials, preferences) is stored in ~/.maplecam/ on Linux/macOS and %USERPROFILE%\.maplecam\ on Windows.

Can I use MapleCAM with a laser?

Yes. If your machine has a laser module, enable laser capability in the machine configuration. This unlocks laser operations (contour, engrave, hatch, pattern) with power and speed controls instead of spindle/feed settings.

How do I update MapleCAM?

Download the latest release from the Downloads page and replace your existing JAR file. Your settings and tool library are stored separately and will be preserved.

What is the .mcp file format?

MapleCAM project files (.mcp) are gzip-compressed JSON. They contain the full project state including imported geometry, operations, settings, and tool assignments. The original SVG/DXF files are not needed after import — the geometry is embedded in the project.