Millright-CNC-Router

MillRight Mega V CNC Router

⚠️ NEVER LEAVE THE CNC UNATTENDED WHILE RUNNING ⚠️

⚠️ EYE PROTECTION REQUIRED WHEN MACHINE IS OPERATING ⚠️

⚠️ DUST COLLECTION MUST BE RUNNING BEFORE STARTING ANY JOB ⚠️

The MillRight Mega V is GRM's CNC router — a computer-controlled cutting and carving machine that uses a spinning router bit to remove material. It can cut, carve, pocket, profile, engrave, and create 3D relief work in wood, plastics, aluminum, and more. This page covers software, setup, settings, safety, and tips to help you get great results.

📄 Introduction to CNC Routing with the MillRight XL V2 — GRM's own getting started guide for this machine.
📄 Machine Operation Basics & Troubleshooting Guide — Official MillRight operating and troubleshooting manual.

---

Machine Specifications

Spec	Details
Model	MillRight Mega V (XL)
Cutting Area	35" x 35" x 6" (889mm x 889mm x 152mm)
Router	DeWalt DW618
Drive System	Steel rack and pinion (X and Y axes); lead screw (Z axis)
Controller	GRBL
Motors	NEMA 23 stepper motors
Resolution	~0.013mm on X/Y axes
Homing Switches	X, Y, and Z axis homing switches included
Compatible Software	VCarve Pro (Makerspace Edition), MillMage, Fusion 360, Universal G-Code Sender

---

Understanding CNC vs. Laser

If you're coming from the laser cutters, CNC routing works differently in a few important ways:

• The laser removes material with light — the CNC removes material physically with a spinning bit
• CNC produces chips and dust — dust collection is mandatory, not optional
• Tool selection matters — different bits are used for different materials and operations (unlike lasers which use the same beam for everything)
• Feed rate and depth of cut interact — too aggressive and you'll break bits or damage the machine
• Jobs take longer to set up but the machine can do things lasers can't — true 3D carving, joinery, cutting thick stock, aluminum machining

---

Software

CNC routing requires two types of software: a CAD/CAM program to design your part and generate toolpaths, and a sender program to stream the G-code to the machine.

CAD/CAM Software

Software	Cost	Best For	Notes
VCarve Pro (Makerspace Edition)	Included with GRM membership	2D cutting, profiling, pocketing, V-carving, sign making	Primary recommended software at GRM; installed on the CNC laptop; see VCarve section below for important notes on how the Makerspace Edition works
MillMage	Free 30-day trial; Core $99; Pro $199	Design + CAM + machine control in one program; great for LightBurn users	Made by the LightBurn team (launched Feb 2026); connects directly to GRBL machines; familiar interface if you already know LightBurn; perpetual license, no subscription; Get MillMage
Fusion 360	Free for personal/hobby use	Complex 3D parts, mechanical components, aluminum machining	Steeper learning curve; powerful for 3D work; use the GRBL post processor when saving toolpaths
Easel (Inventables)	Free (browser-based)	Simple 2D cuts; beginners	Easy to learn; limited compared to VCarve

Sender Software

Software	Cost	Notes
Universal G-Code Sender (UGS)	Free	Primary sender used at GRM; runs on the laptop connected to the machine; universalgcodesender.com — download from the MillRight Resources page
MillMage	See above	Includes built-in machine control — no separate sender needed if using MillMage end-to-end

VCarve Pro Makerspace Edition

GRM uses VCarve Pro Makerspace Edition, a special licensing model designed specifically for makerspaces. Here's what that means for members:

How It Works

• Design at home for free — Download the free VCarve Pro Makerspace

 Client Edition on your own computer and design your projects at home, 
 at no cost to you.

• Cut at GRM — Bring your file to GRM, load it on the licensed

 Makerspace master edition, generate your toolpaths, and cut on the CNC.

• Get access — A GRM administrator will invite you to join the

 Makerspace in VCarve via email or a shared link. Once joined, your 
 home client and the GRM machine will work together seamlessly.

This model means you can spend as much time as you want designing and refining at home, and only use CNC machine time when you're actually ready to cut.

Downloading the Free Client

[https://www.vectric.com/products/vcarve-makerspace-edition Download VCarve Pro Makerspace Client Edition] — free for all GRM members.

Free CNC Project Files

Vectric maintains a library of over 100 free CNC-ready project files compatible with VCarve. These are a great way to get started or find inspiration:

Vectric Free CNC Projects

What You Can Do With VCarve Pro

• 2D routing and 2.5D machining (pockets, profiles, v-carving, inlays)
• Import SVG, DXF, and other vector formats
• Full drawing and layout tools to create designs from scratch
• Toolpath preview/simulation before cutting — catch mistakes before

 they happen

• Double-sided machining in a single session
• No project size limits (Pro Edition feature)
• True shape nesting to minimize material waste

Fusion 360 Post Processor

In Fusion 360, go to Actions → Post Process and select the Grbl / grbl post processor, then click Post. Do not use any other post processor — it will produce G-code the machine cannot read.

Fusion 360 Documentation | Fusion 360 YouTube

---

File Formats

Format	Use	Notes
SVG	2D vector design	Import into VCarve or MillMage for toolpath generation
DXF / DWG	2D vector (CAD)	Good for precise technical drawings; imports cleanly into VCarve
STL	3D model	Used for 3D relief carving in VCarve Pro or Fusion 360
.crv	VCarve project file	Native VCarve format; bring this to GRM to open on the CNC laptop
.nc / .gcode	G-code (toolpath output)	Generated by CAM software; sent to machine via UGS or MillMage

---

Connecting to Universal G-Code Sender (UGS)

1. Open UGS on the CNC laptop (go to ugsplatform → bin → ugsplatform). Mac users: select the version without the yellow square icon. Java must be installed — download from java.com if needed.
2. Plug the USB cable from the machine's electronics box into the laptop
3. In UGS, click the circular arrows (refresh) icon next to the Port dropdown to detect the correct COM port — it will usually find it automatically
4. Click the plug icon to connect — it should turn orange and machine settings will scroll across the console. If nothing appears, disconnect and try a different COM port.
5. Confirm the Controller State shows Idle (not Alarm) before proceeding

UGS Jog Controller Settings

Before jogging, set these values in the Jog Controller panel so movement is visible:

Setting	Recommended Value (mm)	Recommended Value (inches)
Step size XY	10 mm	0.394"
Step size Z	4 mm	0.157"
Feed rate	9,000 mm/min	354 in/min

---

Startup Procedure

1. Connect the CNC laptop to the machine via USB cable
2. Power on the machine controller (switch on the electronics enclosure)
3. Open UGS on the laptop and connect (see above)
4. Home the machine — click Home Machine in the Common Actions panel, or type $H in the console and press Enter. The machine will move to find all three axis home switches.
5. Secure your material to the bed using clamps, tape, or the spoilboard hold-down system
6. Set your Work Zero (X, Y, Z) — see zeroing section below

⚠️ Always home the machine at the start of every session. Without homing, the machine has no reference for where it is and jobs will not run in the correct location.

---

Setting Work Zero (X, Y, Z Origin)

Your CAD/CAM software will define the project origin — make sure your machine zero matches where your file expects it to be. Check the UGS visualizer to confirm.

X and Y Zero

Jog the machine to the correct starting corner or center of your material (matching what you set in VCarve). In the Common Actions panel, click Reset Work Coordinates to zero X and Y.

Z Zero (Paper Method)

1. Jog the bit over your material
2. Reduce step size to a small value (0.1mm or less) to avoid crashing into the stock
3. Slowly jog Z down until the bit just pinches a piece of paper between the bit and the material surface
4. In the UGS console, type one of the following and press Enter:
   • Inches mode: g92 x0 y0 z0.004
   • MM mode: g92 x0 y0 z0.01
5. This sets X and Y to zero and accounts for the paper thickness on Z
6. Jog Z up to a safe height — you are ready to run your program

Tip: The UGS visualizer shows where your job origin is set. A crosshair at lower-left means origin is front-left of stock; a crosshair at center means origin is center of stock. Make sure this matches your VCarve setup.

---

Clearing an Alarm

If UGS shows a red ALARM state:

1. In the Common Actions panel, click Turn Off Alarm Lock
2. If the alarm was caused by the machine hitting a homing switch, you will also need to jog off the switch after clearing the alarm — may need to be done twice depending on your step size
3. Once clear, re-home the machine before running any job

---

Running a Job

1. Load your G-code file in UGS: File → Open (or click the folder icon)
2. Check the visualizer — confirm the toolpath looks correct and the origin is in the right location
3. Turn on the DeWalt DW618 router — set the speed dial for your material (see table below)
4. Turn on dust collection
5. Click Start/Resume G-Code in the Common Actions panel
6. Stay by the machine — watch the first few passes carefully. If anything looks wrong, click Pause G-Code File or Soft Reset immediately.

DeWalt DW618 Speed Settings

Dial Setting	RPM (approx.)	Best For
1	~8,000 RPM	Aluminum, soft metals (single flute bit)
2	~10,000 RPM	Hardwoods, dense materials
3–4	~12,000–16,000 RPM	General wood routing, plywood, MDF
5–6	~18,000–24,000 RPM	Plastics, light engraving, V-carving

---

Bits & Tooling

Common Bit Types

Bit Type	Best For	Notes
Upcut Spiral (End Mill)	General cutting, profiling, pocketing in wood and plastic	Pulls chips up and out; clean bottom edge; most common for general work
Downcut Spiral	Clean top surface finish on plywood	Pushes chips down; can pack into deep pockets
Compression Bit	Finished plywood and sheet goods	Clean top and bottom edges; best for cabinet/panel work
V-Bit (60°, 90°)	V-carving, lettering, decorative engraving	Used with VCarve's V-carving toolpath
Ball Nose	3D relief carving, curved surfaces	Used for finishing passes on 3D work
Straight Flute	Plastics, acrylic	Reduces heat buildup; prevents melting
Single Flute	Aluminum, soft metals	Clears chips efficiently; slower feed rates required

Bit Shank Sizes

The DeWalt DW618 uses a standard router collet:

• 1/4" shank — most common; fits the standard collet
• 1/2" shank — larger bits; requires collet swap — ask a staff member

---

Feed Rate & Depth of Cut

General starting points for 1/4" upcut spiral bit:

Material	Feed Rate	Depth Per Pass	Router Speed
Softwood (pine, cedar)	1500–2500 mm/min	4–6mm	Dial 3–4
Hardwood (oak, maple)	1000–2000 mm/min	3–4mm	Dial 3–4
Plywood (birch, cabinet)	1500–2500 mm/min	4–6mm	Dial 3–4
MDF	2000–3000 mm/min	4–6mm	Dial 3–4
Acrylic / Plastics	1000–2000 mm/min	1–2mm	Dial 5–6
Aluminum (6061)	500–1000 mm/min	0.5–1mm	Dial 1–2

⚠️ When in doubt, go slower and shallower. Multiple passes at conservative depth are almost always better than one aggressive pass.

---

Workholding

• Clamps — most common; ensure clamps don't interfere with the toolpath
• Double-sided tape — good for thin stock or when clamps would be in the way; use carpet tape or machinist tape
• Screws into spoilboard — for larger sheet goods; screw through sacrificial areas into the spoilboard
• Tabs — add small holding tabs in VCarve to keep cut pieces attached until the job finishes; snap or cut off afterward

Always confirm clamps and fasteners are clear of the toolpath in the UGS visualizer before running.

---

Spoilboard

The spoilboard is the sacrificial MDF surface the machine cuts into. It protects the machine bed and allows cutting all the way through material.

• Cutting into the spoilboard is normal and expected
• The spoilboard needs to be surfaced (flattened) periodically — ask a staff member if it looks uneven or heavily damaged
• Do not cut into the aluminum bed beneath the spoilboard

---

Materials Reference

✅ Approved Materials

Material	Cut	Carve/Engrave	Notes
Softwood (pine, cedar, poplar)	Yes	Yes	Easy to machine; watch for tearout with wrong bit direction
Hardwood (oak, maple, walnut)	Yes	Yes	Slower feed rates; sharp bits essential
Plywood (birch, cabinet grade)	Yes	Yes	Use compression or downcut bit for clean edges
MDF	Yes	Yes	Heavy dust — dust collection essential; dulls bits faster than solid wood
Acrylic (cast)	Yes	Yes	Single or straight flute bit; prevent melting with correct speeds
HDPE / Plastics	Yes	Yes	Single flute bit; good chip clearance needed
Aluminum (6061)	Yes	Yes	Single flute bit; slow feed; shallow passes; cutting fluid recommended
Foam (tooling foam, rigid)	Yes	Yes	Very easy to machine; watch for static buildup with chips
Carbon fiber / Fiberglass	Caution	Caution	Extremely hazardous dust — full respiratory protection required; consult staff before attempting

❌ Do Not Cut These Materials

Material	Why
PVC / Vinyl	Toxic fumes when machined
Polycarbonate	Melts and chips unpredictably; poor results and fumes
Steel / Hardened metals	Machine is not rated for ferrous metals
Any material of unknown composition	Always verify material before cutting

---

Safety Rules

• Always wear eye protection — chips and dust fly unpredictably
• Hearing protection recommended for long jobs — the router is loud
• Never reach into the cutting area while the machine is running
• Keep hands away from the bit at all times — the DeWalt DW618 spins at up to 24,000 RPM
• Always stay by the machine while it's running — never leave a running job unattended
• If something looks or sounds wrong: click Pause G-Code File in UGS to pause, or Soft Reset to stop immediately
• Turn off the router before making any adjustments to workholding or bit height
• Dust collection must be running before starting any job — wood and MDF dust is a fire and health hazard

See Emergency Procedures on the main laser page for emergency contact and first aid kit location.

---

Helpful Tips

Always Air Cut First

Before cutting your actual material, raise Z by 10–20mm and run the job — watch the toolpath trace out and confirm it matches your expectations. This catches origin errors before they cost you material.

Tabs

For profile (cutout) operations, always add tabs in VCarve to keep parts from flying loose when the last pass finishes. Set tabs to at least 3mm high and 6–8mm wide for most work.

Climb vs. Conventional Milling

• Conventional milling (default) — safer for wood; less chance of grabbing
• Climb milling — better finish on some materials; can grab on less rigid setups — use with caution

VCarve defaults to conventional milling, which is correct for the Mega V.

Save Your Settings

• Save VCarve files with descriptive names (e.g., oak-box-lid-2025.crv)
• Store files in Google Drive or on a USB drive
• Note your bit, feed rate, DOC, and router speed alongside your project

---

Troubleshooting

Problem	Solution
UGS won't connect	Click the refresh (circular arrows) icon to re-scan ports; try a different COM port; check USB cable is seated in the electronics box
Controller State shows ALARM	Click Turn Off Alarm Lock in Common Actions; if caused by a homing switch, also jog off the switch afterward; re-home before running
Machine won't home	Check USB connection; confirm controller is powered on; check that homing switches are not physically obstructed
Lost connection mid-job	Disable laptop sleep/screensaver before running long jobs; check USB cable
Binding on X or Y axis	Loosen the rack; move gantry to front/right of machine; check pinion gear engagement with rack; tighten front screw; move to next rack screw and repeat until reaching back/left of machine. Contact support@millrightcnc.com if binding continues.
Bit breaking	Feed rate or DOC too aggressive; wrong bit for material; bit not secured properly in collet; material shifting during cut
Chatter / vibration	Feed rate too fast; bit too long; workholding loose; reduce DOC and feed rate
Rough surface finish	Bit dull; feed rate too fast; step over too large; try a finishing pass at higher speed and shallower DOC
Job running in wrong location	Work zero not set correctly — confirm VCarve origin matches where you zeroed on the machine; check the UGS visualizer origin marker
Wrong post processor used	Re-save toolpaths from VCarve using Grbl (mm) or Grbl (inch); from Fusion 360 use Grbl / grbl under Actions → Post Process

For additional help: support@millrightcnc.com or the MillRight CNC Forum. Also join the MillRight CNC User Group or MillRight CNC Mega V Group on Facebook.

---

Resources & Tutorials

Resource	Description	Link
GRM Introduction to CNC Routing	GRM's own getting started guide for the MillRight XL V2	📄 Open Guide
VCarve Makerspace Edition Instructions	How the Makerspace Edition license works at GRM	📄 Open Guide
Machine Operation & Troubleshooting Guide	Official MillRight operating manual	📄 Open Guide
MillRight CNC Tutorial Videos	Official MillRight YouTube tutorial playlist	📺 Watch Playlist
MillRight Resources Page	UGS download, additional docs and videos	millrightcnc.com/resources
Homing Switches & Coordinate Systems	MillRight video on homing and coordinates	📺 Watch
Basic Fusion 360 CAD/CAM	MillRight video on Fusion 360 for CNC	📺 Watch
MillMage Documentation	Official docs for MillMage setup and use	docs.millmagesoftware.com
Vectric Tutorial Videos	Official VCarve tutorials from beginner to advanced	Vectric YouTube
Fusion 360 Documentation	Official Autodesk Fusion 360 docs	Fusion YouTube
MillRight Community Forum	Ask questions, get help from other users	millrightcnc.proboards.com
GRM Discord / Volunteers	Ask for help with settings, file prep, or troubleshooting	Ask at the space or in Discord