CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > Tips & Techniques > Router Bits

Thread Tools Display Modes
Old 08-11-2018, 08:04 PM
rcrawford rcrawford is offline
Cobra Owner
Join Date: Dec 2011
Location: Alberta
Posts: 2,291

I've always had good luck running a single o-flute aluminum bit at 18000rpm and 120ipm.
Russell Crawford
Cobra 408 ATC with recoil
Alberta, Canada
Reply With Quote
Old 08-15-2018, 04:19 PM
TinKnocker TinKnocker is offline
CAMaster owner
Join Date: Jun 2014
Location: MD
Posts: 297

Yeah I usually run .020 per pass even with a 1/4" bit. The 5005 alloy is probably fairly soft. I've found the harder the aluminum the better it cuts for me, it seems counter intuitive but the I think the softer stuff gums the bits. I don't have too much experience with the various alloys though, I'm usually cutting 6061-T6 or 2024-T3 and occasionally 7075-T6.

V-Carve Pro V8
1.7kw Spindle, FTC and counter balance and T-rails
Recoil Ready
Reply With Quote
Old 08-16-2018, 10:07 AM
kjoiner kjoiner is offline
CAMaster Owner
Join Date: Sep 2016
Location: Work - Duluth, GA, Home - Roswell, GA
Posts: 101

I agree with the others regarding depth of cut. For a 1/8" bit, I'm usually at .020 per pass. I run around 10-13K RPM at 30 IPM and have pretty good success. I also shoot some WD40 on the material to help prevent the chips from welding onto the cutter. I also have an air nozzle pointed at the bit.
As far as materials, if it's flat, I'll cut it from 6061. If I need to bend it, I used 5052 because 6061 tends to crack with tight radii.

Kyle Joiner
Duluth, GA
CAMaster Stinger 1 23
FTC, Laser Cross Hair
Vectric V Carve Pro
Remote Handheld Keypad
Solid Edge ST10
Reply With Quote
Old 08-16-2018, 12:54 PM
BradyWatson BradyWatson is offline
CAMhead Legend
Join Date: Oct 2014
Location: 1 hour South of Philly
Posts: 310

Originally Posted by jjwdawg View Post
I have a large aluminum-cutting job coming this week, and I'm trying to get my process dialed in ahead of time. The material will be 1/8" thick 5005 with a black anodized finish. My only aluminum-cutting experience has been polymetal and really thin (.040", I think) sheet.

I don't have the material on hand to test with, so I'm using the only thick aluminum I had - an old road sign, about 0.100 thick. I've no idea what type of aluminum it is, whether it would be classified as hard or soft, etc.; and I suspect that's the main cause of my frustration :-)

I'm using a Southeast Tools SOU302 1/8" O-flute bit with a .055" pass depth. I'm misting enough to keep things cool, I think.

I was advised to try 60IPM & 12k RPM, but, having already broken a few bits on my own earlier, I decided to start slower, 15IPM & 8k RPM. I did a test job of various shapes totaling about 30-40 inches of cut. This seemed to work well and leave a good finish, but it's painfully slow.

Next, I jumped to 60IPM/12K - it got about 5 inches into the job before snapping the bit.

So, my question is: should I keep testing to see how much chipload/feed I can get out of this type bit? Or, should I assume that my material is just wonky, and I should wait until I get the real stuff in hand?

Anyone with production experience with this type of material who could share some feed/speed/bit suggestions? This job has the potential to turn into steady, long-term business, so I want to get it right!
"Cousin James",
Anodized black 5005 is a bit of what I would call a 'poo sandwich' - The anodized skin is very hard, but the actual AL in the middle can get soft and smear - so dialing in speeds can be a little tricky, but certainly not impossible.

I think it is important to reiterate the 'laws' that govern routing aluminum:

#1 - Never, ever...not even once, plunge straight down into aluminum. All tool entries need to be ramped into the material.

#2 - Spindle RPM should be within routing speeds, not milling speeds...and NO your Camaster is NOT a 'mill'. All spindles sold on these machines are rated at full torque @ about 1/2 max Hz. This means 12k RPM.

#3 - ALL alloys of aluminum benefit from coolant - not necessarily lubricant. For most AL parts under about 1/4" thick, the air moving over the bit from the dust collector is adequate. Otherwise, 20 psi from a 'football inflator' blowing on the bit, cold gun ($$$) or even a fogger with H20 & alky will keep things cool. Gooey smear is no good...hard chips are what you want.

#4 - Since drilling violates rule #1, all holes should be done with an inside profile cut, using a tool smaller than the hole. Spiral ramping should be used. ALL of the 'holes' or inside profile cuts should be ganged up into a single toolpath and run separately from the outside profile or pocket toolpaths. This is because a speed of say 75 IPM might be perfectly fine for profile cutting, but a 1/4" hole cut with a 3/16" bit, will be a VERY quick - tool snapping - "NERNT". You really want to think about the circumference (unroll the hole circle to linear so you can understand the speeds) of the holes, then pull those feeds down to something reasonable.

#5 - A CNC router is lightweight & provisions need to be made for it. Despite what most think, these machines are flimsy compared to a cast iron milling machine. Thought should be put into the fact that machine deflection, and NOT tool deflection, is the culprit when cut quality suffers or you break tools. Avoid SHOCK LOADS as much as you can.

#6 - Choose the right geometry & LARGEST dia tool for the material at hand. ER-series collets are available in 1/16" increments & metric. My go-to bit for most AL things I cut is an Onsrud 3/16" single flute spiral-O. This lets me cut 1/4" holes on up and with something like a 7/8" LOC, I can confidently profile up to about 3/8" thick (even 1/2") without too much trouble. If you do the math, a 3/16" dia bit has TWICE the volume of material than a 1/8" dia bit - and that means it's twice as stiff, with only a 1/16" kerf width penalty. Furthermore - if you are having trouble holding the material down because the bit is an upcut spiral, switch to a STRAIGHT spiral-O geometry made for cutting non-ferrous. Onsrud has them & others.

#7 - Stepdown/Pass Depths - For most AL projects out of bar or sheet, restrict your pass depth to somewhere in the .02-04" range. Smaller depths, for smaller cutters. AND keep in mind that SMALL CUTTERS LIKE/NEED HIGH RPM! (to get the SFM right) - I don't like discussing chipload because it is NOT ideal cutting settings for quality. It is the suggested speeds for maximum tool life. My customers only care about quality. Shoot for that.

#8 - Hold down - Avoid screws! They bend/distort the metal and cause problems like spring-back during cutting. You really need to hold metal down with either vacuum or clamps. If it moves even a little bit while cutting, you run the risk of jambing the bit (and breaking it) - but to me, more importantly, you kill the edge quality/smoothness.

I wasn't expecting there to be so many 'rules'...but there you have it. Probably the most important ones for your situation are getting the right RPM, coolant, adequate hold down and pass depth. KEEP THE TOOL MOVING! - You can't make any money running 15 IPM...My advice would be to start at 13 to 15k RPM, 72 XY, 30 Z IPM, .025" Pass depth using a single flute spiral O, 3/16" dia or larger, depending on your design constraints.

Good luck!
IBILD Solutions - High Definition 3D Laser Scanning Services - Advanced CNC Training and Consultation - Vectric Custom Video Training
Reply With Quote
Old 08-16-2018, 10:17 PM
Hallex Hallex is offline
Camaster owner
Join Date: Oct 2014
Location: Al
Posts: 121

Thanks Brady
That was truly awesome and informative 😀
Camhead FAN
Reply With Quote
Old 08-17-2018, 09:30 AM
BradyWatson BradyWatson is offline
CAMhead Legend
Join Date: Oct 2014
Location: 1 hour South of Philly
Posts: 310

You're welcome ~ I broke my share of bits early on...and had some pretty challenging jobs where I had to get it right.

1/2" Naval Brass floor inlay @ Christopher Newport University...pretty much the practical limit of routing non-ferrous...
Attached Images
File Type: jpg LibraryRotunda1.jpg (50.4 KB, 22 views)
IBILD Solutions - High Definition 3D Laser Scanning Services - Advanced CNC Training and Consultation - Vectric Custom Video Training
Reply With Quote
Old 08-17-2018, 09:47 AM
Jim Becker Jim Becker is offline
CAMaster Owner
Join Date: Jan 2018
Location: SE PA
Posts: 1,051

That was very informative, Brady! Thanks for posting it!
Jim Becker

SR-44 (2018), 1.7kw spindle, Performance Premium, USB, Keypad, T-Slot table (y-axis configuration), WinCNC, VCarve Pro upgraded to Aspire

Non CNC stuff...

SCM/Minimax - slider/JP/BS
Festool "a good collection"
Stubby - lathe
Oneida Cyclone

Retired from full time work in the telecom industry 9/2017
Commission work for equestrian tack storage and other custom furniture and cabinetry
Located Bucks County PA
Reply With Quote

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is On

Forum Jump

All times are GMT -4. The time now is 08:28 AM.

Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2019, Jelsoft Enterprises Ltd.