Cutting ali on wood router - low rpms breaks bits. Why?

[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]

Originally Posted by lsteele ....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!!!) http://video.google.co.uk/videoplay?docid=6394744113356367969&ei=8Fo9Sb3GEJOQiQKh0vyqCQ&q=mister+cnc&hl=en

[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