[lsteele]

Hello,

I've been experimenting with cutting ali on my mdf router and have broken quite a few bits when cutting at lower rpm, and I don't understand why.

I have a kress 1050, which has a lowest rpm of 10,000 (upto around 20K I think). I'm using a mix of 1/8" bits, mostly 2 flute. I've got an aquarium air pump blowing air at the cutter and am squirting generous doses of wd40 at the tip every 30 seconds or so. Now, using this set up I've had reasonable success when I have the Kress at the middle of it's rpm range (indicated on the dial as 1-6 - it doesn't say the rpm but I guess it's linear). But everything I've read about cutting ali seems to suggest that lower rpm is better, so I've been experimenting with turning the rpm down to the lowest setting. Everything seems to run ok at first, then (after some minutes) the cutting noise will change and a few seconds later the bit snaps. I'm guessing the ali is melting on the tip blunting it. But what I don't get is why I'm getting better results with higher rpm. Can anyone enlighten me?

When cutting on a mill (as opposed to router) the rpms are much lower, so is it the flood cooling on a mill which prevents this problem?

Thanks in advance. Incidentally I posted this here as I'm using a cnc router more geared up to wood - hope this is the right place.

-Luke

[mactec54]

Hi Isteele
You need a little more information what is your feed rate if your feed rate is to high or to slow you can get the problem you are having also some material is better than others
to cut so spindle RPM plus feed rate plus material plus cutting fluid all of these things have to be correct to make it work

I hope that you are not using bits as bits are for cutting wood & endmills or milling cutters are for metal

[Freff]

I think it's a matter of finding the right balance between the RPM, feed rate and the coolant/lubricant.

I have found during recent tests that a decrease in rpm resulted in a faster feed rate.

I have never found WD40 much use as it's a releasing agent rather than a lubricant. Having said that it works great on drilling or boring larger holes in aluminium.

I would suggest using an agent specifically for use with aluminum. Sorry I can't be more helpful.

Tony

[lsteele]

Ok, my depth of cut is 0.3mm and my feedrate is 450-600mm per minute. (That's 0.012" and ~24ipm, I think.)

I've kept everything constant except the rpm. And of course the cutters, since I'm getting through those pretty quickly.

The cutters are all carbide.

I've been using wd40 since I've seen it mentioned repeatedly in regard to cutting ali. What else should I use? Bear in mind this machine is made out of mdf, so I need something I can apply in small quantities.

As I said (and I'm happy to be told I'm wrong) it seems like the cutters are melting the ali which sticks to them and so blunts them. As a rule of thumb does reducing the rpm mean more heat or less? (I would have thought less but since each flute's cutting more metal maybe more?)

Thanks again.

[Geof]

....As I said (and I'm happy to be told I'm wrong) it seems like the cutters are melting the ali which sticks to them and so blunts them. As a rule of thumb does reducing the rpm mean more heat or less? (I would have thought less but since each flute's cutting more metal maybe more?)

Thanks again.

What tends to happen especially if the feed rate is too high and coolant/lubrication is inadequate is that chips get packed into the flutes then you get a mess because they rub, melt and the cutter breaks.

Always use two flute if possible to get better chip clearance. Keep the chipload below 0.0005" per tooth (0.01mm). With carbide you should be able to go at full rpm because the surface feet per minute is just over 600; carbide can cut aluminum at 3 times that. At 20000rpm your feed will be not more than 400mm/min.

But really the most important thing is adequate lubrication. You could try automatic transmission fluid (ATF) it works very well. Brush it on ahead of where the cut will be. Kerosene works well but is more of a fire hazard. Or see if your local Shell petrol station has ever heard of Shell Dromus B. This is a cutting fluid made by Shell for the last 80 or a 100 years ro so. It is mixed with water normally but works very well just brushed on neat.

[Freff]

I think your depth of cut maybe slightly to much for such a small bit. If it was a 4 flute end mill, maybe. I also think your feed may be a bit fast. I'll go down to the workshop later and get you the name of the lub I use.

Tony

[Kipper]

The Kress goes to 30.000 RPM btw.

I think you might be better to try compressed air or be brave and use a fine mist to clear the chips (very fine for MDF!!!) [ame=http://video.google.co.uk/videoplay?docid=6394744113356367969&ei=8Fo9Sb3GEJOQiQKh0vyqCQ&q=mister+cnc&hl=en]A very wet mister [/ame]

[martinw]

Dear Isteele,

Trend do router cutters specially for aluminium. They also do a paste wax that is really good as a cutting compound.

http://www.trend-uk.com/en/UK/

Best wishes,

Martin

[lsteele]

Thanks for all the comments.

Geof, I think you've described exactly what was happening - there's lots of chips collecting around the cutter, and in fact the wd40 seems to be causing it to cling together rather than moving away from the cut. Also at the moment my air pipe isn't terminated with any kind of nozzle, so perhaps putting one on would increase it's efficacy at blowing the chips out the way. I'll do that before considering compressed air.

Also I tried using the formulas I found here

http://astro.umsystem.edu/atm/ARCHIV.../msg00755.html

and calculated a similar ipm figure to you. But where did you get that figure for chipload?

And one more question - on videos I've seen of bona fide milling machines the end mill seems to go through ali like butter. Is this possible because flood coolant allows higher chiploads?

Thanks again. Off to buy some automatic transmission fluid now.

-Luke

[Kipper]

Take a look in Mach3 it's pretty good at chiploads and feedrates.

[mactec54]

Hi isteele

The numbers that Geof is giving you are for ideal conditions in a normal CNC machine not a MDF build machine you will most likely have to cut every thing in half or less to make it work well on your machine & WD40 is way better than the transmission fluid just brush it on The air blast coolant mix will work the best in your case set the air blast about 8/10 psi just a small jet of air to clear the chips away from the cutting area

[Freff]

Luke, go to your local Machine Mart and get a card of Mig welding nozzles. 0.5mm - 1.5mm. They have a small thread that will screw into a piece of tube and give you a more concentrated direct blast of air on your work.

Tony

[martinw]

Dear Isteele,

Whatever route you go, water based coolants are not going to be a good idea anywhere near an MDF router. Sorry, you probably know that...

Best wishes,

Martin

[lsteele]

I though I'd post a progress report.

First of all I bought some proper coolant hose from ebay - some of the plastic pipe made out of interlocking segments. It came with several nozzles, and I put the narrowest on, with a ~1mm tip. This has made a big difference to the air flow. Previously the pipe from my aquarium pump had nothing on the end. Now there's a really fast directed stream of air pointing straight at the cutting tip.

Second, I made the Z carriage on my machine slightly taller, with the end result that I can fit the 1/8" cutters in the collet right up to the base of the flutes. Previously I had to have them sitting further out from the collet than I would have liked in order to be able to reach the bottom of the aluminium stock. I also made some adjustments to my x-axis to eliminate a bit more backlash.

Finally I bought some new cutters from sgstool.com. These are marketed as being specifically for aluminium. They were considerably more expensive than previous cutters I've bought. I'm not sure whether this is because I bought them in the UK (they have a distribution centre a couple of miles from me), or whether it's because they're higher quality.

Anyway, after all these changes I'm now seeing a significant increase in the quality of the cuts I'm making. The air hose blows all the swarf away from the cutter, and the whole thing makes a satisfying cutting noise, rather than a distressing grinding, on the verge of breaking kind of noise it had previously emitted.

I think the improvments to the swarf removal (thanks to the nozzles on the air hose) followed by the new cutters are the most significant factors.

I've been trying different lubrication methods but I haven't arrived at a favourite. ATF, white spirit and WD40 all seem to work. If I decide one's significantly better than the others I'll let you know.

Incidentally I'm keeping the Kress close to the middle of it's rev range, ~18k rpm I'd guess.

Thanks for all the suggestions. If there are any more developments I'll post here!

Luke

[harryn]

I have had some luck with 0w-20 synthetic motor oil as a lubricant for metal cutting - but I am just a weekend hack - not a metal cutting pro at all.

[tahustvedt]

I mill a lot of aluminium with my Kress FME1050 and CNC router and find it works best if I run shallow pass depth and very high feed rates and high rpm. I made a spreadsheet to help me calculate the rates. With a 1/8" two flute carbide tool I would run at 25000 rpm (between 4 and 5 on the dial) and a feed rate of 49 mm/second (116 IPS) with a 0.13 mm pass depth. It ploughs through aluminium very quickly and produces a nice finish. I lubricate with either WD40 or red spirit.

Normally I use a 4 mm four flute carbide end mill and run 100 mm/second, 0,17 deep and 20000 rpm. It takes no time at all to cut aluminium at these speeds.

I measured the rpm of my Kress FME1050 and found that it is not linear. This is what I got:
1 = 10000
2 = 15000
3 = 20000
4 = 22000
5 = 27000
6 = 29000

[Geof]

Thanks for all the comments.

Geof, ....and calculated a similar ipm figure to you. But where did you get that figure for chipload?...
-Luke

I had not looked at this thread for a while.

As mactec54 points out my numbers are based on a full size CNC but I had already halved the chipload (more or less).

Yes big CNCs do go through aluminum alloys like butter, and emphatically YES it is the flood coolant especially when taking a full width deep cut. As an example we run a cut in 6061 T655 using a 5/8" two flute cutter full width 0.4" deep at 11,000rpm and 110ipm at which point the machine runs out of torque. Is has happened that the coolant pump did not turn on and the result was a short stub of cutter embedded in a block of mushed up aluminum with the matching stub still in the toolholder.

[lsteele]

Hi tahustvedt,

That's interesting. Could you post a copy of that spreadsheet? Unfortunately I can't get feed rates that high on my current router, but maybe the next one...

Thanks,

-Luke

[tahustvedt]

Ok, here it is, I made an english version. It's in Open Office and Excel 97 format. I can't guarantee that it works well for everyone but it works wel on my machine.

The way it works is that you first fill in the diameter and number of flutes of the tool. Then you select an RPM that puts the SFM within the recommended maximum and it calculates appropriate feed rate and depth. If you find that the machine can't move fast enough you can lower the RPM or increase the depth override factor.

I have never changed the depth override factor myself as my machine is pretty fast. Also, I haven't tested the steel calculations yet either. I'm changing it as I find the need for it. Hehe

[lsteele]

Hello,

Since I started this thread I've been cutting up quite a bit of ali, with increasing success. Thanks to ironing out some backlash in my machine and refining my techniques following the advice given the results seem to be getting better.

The one thing that's still causing me difficulty is profiling through thicker pieces of ali (i.e. 1/2"/12.7mm). While trying to do this I've recently broken a 1/8" and 1/4" bit, both quite expensive ones at that! What I think is happening here is that what vibration and backlash there is in the machine cause a slight wobble in the cutter, and on subsequent passes the groove that's left from the previous pass forces the cutter to move in the same pattern. My guess is this puts stress on the cutter causing it to snap. Does this sound like a credible explanation? On all the parts I cut there's a clear pattern of oscillations (don't know how else to describe it) along the sides, which have become less prominent as I've adjusted the machine. Both times the cutter broke it'd got about 8-10mm through the material (and was seemed quite content) before suddenly snapping.

In my cam program's profiling section there's a 'clear offset' option, whereby the a pass is performed at an offset from the profile, before making a second pass at zero offset, then going to the next step down. If my theory's right it sounds like this would eliminate the stress a straight forward profile's causing. Or is there another strategy that might achieve the desired effect?

Anyway, before I try I try again I wanted to get some feedback 'cause I can't afford to work my way through any more cutters. Any comments gratefully received!

Luke