CNC Router Bits - Newbie question

regional

#1

For those of you that have a CNC router and cut aluminum, what router bits/brands do you find the most useful?
I have spent a couple of hours looking over the CNC router threads on this forum, I am not seeing it in any one place. Since we are wrapping up build season, and we just picked up a Velox 50-50 yesterday, I wanted to get some recommendations since I know bits break… :stuck_out_tongue:


#2

We have been using 4mm huhao endmills recently, and we like them a lot better than the 1/8” onsruds we were using before that. I know a lot of other people have similar experiences. We also use various drill bits from lakeshore carbide to drill holes and those have never broken, though they do dull after a few hundred holes (which doesn’t matter too much except for the sound).

EDIT: we use an Omio X8


#3

We just got our router this summer, but so far we found that we use single-flute 4mm and 6mm endmills most often. The 6mm are good for faster cuts, while the 4mm are better for finer cuts. We also use some single-flute 2mm endmills for sharp interior corners, and 8mm 2-flute endmills for cutting plywood for prototypes.

We placed a large order from Alibaba before the season. IIRC the endmills were only ~$2/piece and took less than a month to arrive from China. Unlike most tools in the shop we think of endmills as disposable, so we buy them cheap and expect to break a good number of them throughout the season. It’s a lot easier than finding expensive endmills and having to take good care of them


#4

We’ve had excellent results with Viper DES-V20805S endmills. They provide much better chip evacuation than the Onsrud 65-012 endmills we used before.

Our machine is a 96" x 48" ShopBot PRSAlpha with a variable speed spindle (4,100-18,000 RPM). We use compressed air blast while cutting aluminum to keep things cool and remove chips. A very small amount of WD-40 also helps – usually a spritz on the surface of the aluminum before the beginning of the toolpath.

We’ve only cut 6061 and 6063.

Below are our settings for each tool. Note that the Vipers enable us to cut much faster without sacrificing quality.

Viper DES-V20805S

  • 84IPM
  • 10,500 RPM
  • 0.010" depth per pass

Onsrud 65-012

  • 30IPM
  • 6,000 RPM
  • 0.010" depth per pass

#5

You’re taking 25 passes to go through 1/4" material? I think your DOC numbers might be an order of magnitude off…


#6

No, those numbers are correct. It is an extremely flimsy machine and I do not recommend purchasing one for FRC. However, it is the hand we were dealt by the school.

It’s part of why we now send parts out to be waterjetted whenever possible. When we need to do something in-house, we avoid 1/4".


#7

Those feeds seem insanely fast. The Velox VR-5050, which are pretty common in FRC, cut at 100 ipm max. Our router cuts at 250 ipm. I imagine if you slowed down your feed to a more reasonable number you will be able to use a larger DoC.


#8

Vipers require high feedrates to load up the flutes, otherwise they get dulled really fast.
That being said, .01 DOC is laughable. Onsrud bits will easily run at 30 IPM and .06" or more DOC (I know 115 runs them at 0.125" DOC regularly).
I am an advocate of these guys though: https://www.aliexpress.com/store/product/2pcs-lot-4mm-Single-Flute-Spiral-Cutter-router-bit-CNC-end-mill-For-Acrylic-carbide-milling/2947084_32802213140.html?spm=2114.search0104.3.50.73ba7e2bBkZpY5&ws_ab_test=searchweb0_0,searchweb201602_1_10065_10068_10130_10547_10546_10059_10548_10545_10696_100031_10084_10083_10103_451_452_10618_10307,searchweb201603_1,ppcSwitch_2&algo_expid=bd8f1d84-55db-4249-8ee0-d583b8ad9861-7&algo_pvid=bd8f1d84-55db-4249-8ee0-d583b8ad9861&transAbTest=ae803_1&priceBeautifyAB=0
Many teams now use these with great success. wcproducts.net sells 4mm endmills for $15 each that are also quite good, but it’s better to just use those in the short term before switching to Huhaos.
4mm x 12mm for regular plates, and 4mm x 17mm for cutting 1/2" through 2x1 and 1x1 tubes. They won’t provide as clean of an edge as Onsrud bits do, but they are still very, very good. I recommend starting at 18k RPM, 42 IPM at 0.04" DOC for slots. WD-40 does a good job of lubrication as well.


#9

We use Vortex 5609a and 5625a bits for aluminum at AndyMark. Our router can hit 18,000 RPM, so we usually run the 1/4” bit at 108ipm and .060” DoC and 54ipm for the 1/8” bit at a .030” DoC. Could we go deeper, faster? Probably. But for us it’s about getting tool life and speed and finding the balance.


#10

@asid61

You’re correct about feedrate and spindle speed – an important limiting factor in both the Viper and Onsrud 65- endmills is the rated chip load, which is in the range of 0.003-0.006" per flute. Outside of that range, they heat up and clog up, or just break.

@AriMB

It’s not the endmills that complain about deeper cuts, it’s the machine – it’s too flimsy to deal with the cutting forces. I double checked some tests tonight from a few years ago at 0.025" and even 0.015" DOC. Both produced terrible chatter and waviness at both high and low spindle speeds. I’m sure you could run a more rigid machine at a greater DoC, as most of these endmills assume 1D passes.

Both of you are free to argue with the machine if you don’t believe me.


#11

We’re using the Onsrud 63-600 series.

1xD DOC, 80% radial stepover in Aluminum,.

24,000 RPM, 90+ IPM on 1/4", slightly less on 3/16"

22,000 RPM, 130 IPM on 3/8"


#12

Given the radial stepover, I am guessing you are just running adaptives (or traditional pocketing?) for all of the pockets rather than contours? Or is there some other magic going on?


#13

We run those feed rates or similar when slotting as well. But yes unless it’s a very large cutout we will pocket it rather than contour it.


#14

How do you combat heat build up and chip clearing with such high feed rates? Fogbuster or something similar?


#15

We mostly use the 1/8" Onsrud 63-600 bits. I’ve found chip evacuation to be a major problem so I slowed the speeds down from 18k down to 15k. I have gone full DOC in .25" aluminum with .05 stepover at 30 ipm however I would recommend going at a much lower DOC and increasing the ipm.
In polycarb you can go way faster. I’ve gone full DOC in .25" poly at .07 stepover and 60 ipm and it still sounded completely fine.


#16

I would consider at minimum an air blast to be essential to clear chips. We have a mister.