View source for 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.

📄 '''[https://docs.google.com/document/d/1ps4U4pA57WeHdFLsr8Kg67PdEkbcAdCeBgEzXij422k/edit?usp=sharing Introduction to CNC Routing with the MillRight XL V2]''' — GRM's own getting started guide for this machine.<br>
📄 '''[https://drive.google.com/file/d/11xfBGAzft6EYSblhZbTTBced2QuHm9ZQ/view?usp=sharing Machine Operation Basics & Troubleshooting Guide]''' — Official MillRight operating and troubleshooting manual.

----

== Machine Specifications ==

{| class="wikitable" style="width:100%;"
|-
! 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 ===

{| class="wikitable" style="width:100%;"
|-
! 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; [https://lightburnsoftware.com/products/millmage-core 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 ===

{| class="wikitable" style="width:100%;"
|-
! Software !! Cost !! Notes
|-
| '''Universal G-Code Sender (UGS)''' || Free || Primary sender used at GRM; runs on the laptop connected to the machine; [https://universalgcodesender.com universalgcodesender.com] — download from the [https://millrightcnc.com/resources/ 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 ===

📄 [https://docs.google.com/document/d/1GRmUllWCRU5CWijUJGNBciV7FUCqNSrgM06p7rCUkOI/edit?usp=sharing VCarve Pro Makerspace Edition Instructions]

VCarve Pro Makerspace Edition works slightly differently than a standard VCarve license:

* The full software is installed on the '''GRM CNC laptop''' — you can design and cut here
* At home, download the '''free VCarve trial''' to design your files — save as a VCarve project (.crv)
* Bring your .crv file to GRM on a USB drive, open it on the GRM laptop to generate toolpaths and cut
* You cannot generate toolpaths or save G-code from the trial version at home — only at the GRM machine

'''Post Processor (critical):''' When saving toolpaths in VCarve, you must select the correct post processor:
* Standard cutting: '''Grbl (mm)''' or '''Grbl (inch)'''
* 4th axis rotary work: '''G-Code WrapY2A (mm)''' or '''G-Code WrapY2A (inch)'''

In VCarve v11+, go to Toolpath commands (arrow at top left) → '''Save Toolpath''' → select the correct post processor from the dropdown.

[https://www.vectric.com/support/tutorials/vcarve-desktop Download VCarve Trial] | [https://www.youtube.com/channel/UCqkhkxqPPLdtYy8ybykTlzQ Vectric YouTube Tutorials] | [https://www.vectric.com/support/tutorials/vcarve-desktop Vectric Tutorial Videos]

=== 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.

[https://help.autodesk.com/view/fusion360/ENU/ Fusion 360 Documentation] | [https://www.youtube.com/c/AutodeskFusion360/featured Fusion 360 YouTube]

----

== File Formats ==

{| class="wikitable" style="width:100%;"
|-
! 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) ==

# 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.''
# Plug the USB cable from the machine's electronics box into the laptop
# 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
# 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.
# 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:

{| class="wikitable" style="width:100%;"
|-
! 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 ==

# Connect the CNC laptop to the machine via USB cable
# Power on the machine controller (switch on the electronics enclosure)
# Open UGS on the laptop and connect (see above)
# '''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.
# Secure your material to the bed using clamps, tape, or the spoilboard hold-down system
# 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) ===
# Jog the bit over your material
# Reduce step size to a small value (0.1mm or less) to avoid crashing into the stock
# Slowly jog Z down until the bit just '''pinches a piece of paper''' between the bit and the material surface
# In the UGS console, type one of the following and press Enter:
#* '''Inches mode:''' <code>g92 x0 y0 z0.004</code>
#* '''MM mode:''' <code>g92 x0 y0 z0.01</code>
# This sets X and Y to zero and accounts for the paper thickness on Z
# 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:

# In the '''Common Actions''' panel, click '''Turn Off Alarm Lock'''
# 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
# Once clear, re-home the machine before running any job

----

== Running a Job ==

# Load your G-code file in UGS: '''File → Open''' (or click the folder icon)
# Check the visualizer — confirm the toolpath looks correct and the origin is in the right location
# Turn on the '''DeWalt DW618 router''' — set the speed dial for your material (see table below)
# Turn on '''dust collection'''
# Click '''Start/Resume G-Code''' in the Common Actions panel
# 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 ===

{| class="wikitable" style="width:100%;"
|-
! 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 ===

{| class="wikitable" style="width:100%;"
|-
! 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:'''

{| class="wikitable" style="width:100%;"
|-
! 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 ===

{| class="wikitable" style="width:100%;"
|-
! 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 ===

{| class="wikitable" style="width:100%;"
|-
! style="background:#ffe4e4;" | Material !! style="background:#ffe4e4;" | 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 [[Laser_cutting_and_etching#Emergency_Procedures|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 ==

{| class="wikitable" style="width:100%;"
|-
! 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 [mailto:support@millrightcnc.com 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: [mailto:support@millrightcnc.com support@millrightcnc.com] or the [https://millrightcnc.proboards.com/ MillRight CNC Forum]. Also join the '''MillRight CNC User Group''' or '''MillRight CNC Mega V Group''' on Facebook.

----

== Resources & Tutorials ==

{| class="wikitable" style="width:100%;"
|-
! Resource !! Description !! Link
|-
| '''GRM Introduction to CNC Routing''' || GRM's own getting started guide for the MillRight XL V2 || [https://docs.google.com/document/d/1ps4U4pA57WeHdFLsr8Kg67PdEkbcAdCeBgEzXij422k/edit?usp=sharing 📄 Open Guide]
|-
| '''VCarve Makerspace Edition Instructions''' || How the Makerspace Edition license works at GRM || [https://docs.google.com/document/d/1GRmUllWCRU5CWijUJGNBciV7FUCqNSrgM06p7rCUkOI/edit?usp=sharing 📄 Open Guide]
|-
| '''Machine Operation & Troubleshooting Guide''' || Official MillRight operating manual || [https://drive.google.com/file/d/11xfBGAzft6EYSblhZbTTBced2QuHm9ZQ/view?usp=sharing 📄 Open Guide]
|-
| '''MillRight CNC Tutorial Videos''' || Official MillRight YouTube tutorial playlist || [https://youtube.com/playlist?list=PLfrJs0EaebcWigKYo0-bBn4SR2TizWSWz 📺 Watch Playlist]
|-
| '''MillRight Resources Page''' || UGS download, additional docs and videos || [https://millrightcnc.com/resources/ millrightcnc.com/resources]
|-
| '''Homing Switches & Coordinate Systems''' || MillRight video on homing and coordinates || [https://www.youtube.com/watch?v=61FNml8M3i0 📺 Watch]
|-
| '''Basic Fusion 360 CAD/CAM''' || MillRight video on Fusion 360 for CNC || [https://www.youtube.com/watch?v=oSYyz21TcJU&t=57s 📺 Watch]
|-
| '''MillMage Documentation''' || Official docs for MillMage setup and use || [https://docs.millmagesoftware.com docs.millmagesoftware.com]
|-
| '''Vectric Tutorial Videos''' || Official VCarve tutorials from beginner to advanced || [https://www.vectric.com/support/tutorials/vcarve-desktop vectric.com/tutorials] \| [https://www.youtube.com/channel/UCqkhkxqPPLdtYy8ybykTlzQ Vectric YouTube]
|-
| '''Fusion 360 Documentation''' || Official Autodesk Fusion 360 docs || [https://help.autodesk.com/view/fusion360/ENU/ Autodesk Help] \| [https://www.youtube.com/c/AutodeskFusion360/featured Fusion YouTube]
|-
| '''MillRight Community Forum''' || Ask questions, get help from other users || [https://millrightcnc.proboards.com/ millrightcnc.proboards.com]
|-
| '''GRM Discord / Volunteers''' || Ask for help with settings, file prep, or troubleshooting || Ask at the space or in Discord
|}