Hello Guest it is March 09, 2021, 02:53:47 AM

Author Topic: What kind of bit/end mill should I be using?  (Read 2661 times)

0 Members and 1 Guest are viewing this topic.

What kind of bit/end mill should I be using?
« on: August 09, 2018, 01:22:49 PM »
I have just finished the initial setup of a CNC router at my place of work, and being a novice when it comes to configuring everything, I am wondering what the best tool would be for aluminum/composite metal applications? Current setup and use is as follows:

CNC Router: Accu-Cut XPS 6F12F (http://computerizedcutters.com/our-products/accu-cut-xp)

Application: Cutting signage from 1/4" alum. 6061 sheets, and 1/4" composite metal paneling (Omega-lite)

I believe the current tool was a  3/16" Dia x 2" L x 5/8" Flute Carbide Single Flute bit, but I ended up accidentally breaking it.

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: What kind of bit/end mill should I be using?
« Reply #1 on: August 09, 2018, 03:21:06 PM »
A 1/4" bit would be stronger. I'd use a single  "O" flute bit.
Like an Amana 51401 or 51402.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: What kind of bit/end mill should I be using?
« Reply #2 on: August 10, 2018, 12:37:32 AM »
Hi,
the trick to cutting aluminium is to clear the chips as they are cut. If the chips get recut
they are very VERY likely to get stuck to the bit, sometimes called 'built up edge' or BUP.
Its a certainty it will bugger up your job, and make real hard work for your spindle.

Using air or even flood coolant gets rid of most of the chips, if you can do it.

If you cant then slower surface speeds (200 m/min) are appropriate but if you can clear the chips
surface speeds of 500 m/min are OK.

So with a 3/16 tool:

diameter (mm) = 3/16 X 25.4
                     =4.76mm
circumference=4.76 x PI
                   =14.95mm
surface speed =rpm x circumference (in m)
                    =21000 x 0.01495
                    =314 m/min
which is in the zone for aluminum.
Even a 1/4 tool will have a surface speed of 418 m/min, which would be fine IF you can clear the chips.

Craig
My wife left with my best friend...
     and I miss him!
Re: What kind of bit/end mill should I be using?
« Reply #3 on: August 10, 2018, 12:40:15 AM »
Hi,
just a thought, my previous post assumes carbide tools. You'd want to reduce surface speeds a lot for HSS.

Craig
My wife left with my best friend...
     and I miss him!
Re: What kind of bit/end mill should I be using?
« Reply #4 on: August 10, 2018, 05:16:38 AM »
Hi,
a couple of other ideas to think about.

You may have seen a lot of carbide tools with coatings like Titanium Nitride, Titanium Carbo Nitride and so on.
They are very good when cutting steels but not  with aluminium.

The coatings are very hard and aid lubricity so chips slide off and over the surface. Most of the coatings are variations of nitirides
which are trivalent. Aluminium is trivalent and the lubricity a coating might add for steel is actually 'sticky' for aluminium.

Consequently carbide tools sold for aluminium are often not coated at all. There are coatings that do work and work well including
C(hemical) V(apour)D(eposit) diamond (being essentially quad-valent) but are expensive and rare. Don't go there until you are 100% experienced and can get days
or even weeks without breaking a tool before you consider these exotics. There is one coating that is not common but not that expensive,
Titanium Diboride, and its just the bees knees for aluminium.

I use small, I mean very small endmills for making circuit boards, 0.4mm and 0.5mm (16-20 thou) and you only have to look cross-eyed at
them and they break. You are likely to have quite a few accidents before you get good at it. Cheap tools are OK when starting out but once you get
good enough to not break too many you should be using branded tools, they are more expensive, lots more expensive in cases but often are that much superior.

Harvey Tools have a vast range and all good. I tried some Raptor endmills from Destiny Tools and while expensive, in stainless and tough steels like 4340, just the best
I've ever used. I haven't tried their Viper DVH tools but are meant to be good for aluminium, 45 degree variable helix, with and without coatings.

I know a lot of sources say don't bother with coolant with carbide tools, I find though I get a huge performance lift when using flood coolant, I suspect more because
of flushing the chips out of the cut zone. When flood cooling works it will improve tool life by a factor of ten or better!

Craig
My wife left with my best friend...
     and I miss him!
Re: What kind of bit/end mill should I be using?
« Reply #5 on: August 10, 2018, 07:08:46 AM »
^ very interesting about the coating valency and its relevance to materials cutting. I'll bear that in mind.
I've had some pretty good carbide tools from AliExpress, the Chinese suppliers seem good at making these. Their HSS tools are a bit 3rd world but their carbide ones are well worth it and certainly a lot less intimidating cost-wise for a new guy.
Re: What kind of bit/end mill should I be using?
« Reply #6 on: August 10, 2018, 11:59:44 AM »
Thanks for the information! It is saving me many hours of times/headaches since I am attempting to to set up our table from scratch with no manual or anything. I really appreciate it.

I have one more question regarding bit type, downcut vs upcut, which would be better suited for my application? I'm assuming downcut leaves a better finished edge (a lot of the sign work would require this), and upcut is better at removing and clear material, is this correct?
« Last Edit: August 10, 2018, 12:05:24 PM by mikel92 »

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: What kind of bit/end mill should I be using?
« Reply #7 on: August 10, 2018, 12:13:20 PM »
You should get similar edge finish with either one. I'd use an upcut with aluminum, because the chips have nowhere to go with a downcut.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: What kind of bit/end mill should I be using?
« Reply #8 on: August 10, 2018, 02:14:34 PM »
Hi,
downcut is useful if the materials really soft and you want to prevent the tool from lifting the cut edge. If the cut is not right
through the chips have nowhere to go and can't be used. As a consequence the vast majority of tools are regular upcut.

Quote
I've had some pretty good carbide tools from AliExpress, the Chinese suppliers seem good at making these

I used to think so.....until I started using Harvey Tools, Destiny Tools, Kyocera Tycom, Kennametal and Iscar.

Craig
My wife left with my best friend...
     and I miss him!
Re: What kind of bit/end mill should I be using?
« Reply #9 on: August 15, 2018, 04:22:17 PM »
I just ran a cut, and did a mix of inside cuts and outside cuts. the tool went clockwise, but counterclockwise on the out side. Is going counterclockwise worse for the bit?