[Vincent82]

the company where i'm working is making since a while contracts that are implicating thin stainless steel 304 sheets cutting (0.016’’-0.024’’). unfortunately, the actual machinery has only been designed to cut non ferrous material (multicam 5000 series).

our objective would to be able to cut thin ss 304 sheets laminated on plywood with our multicam 5000 series milling machine. the milling needs to be done preferably dry (cannot be made with the traditional flood of coolant), with a ¼’’ mill bit.

at this moment, we have try with ma ford tuffcut xr series (altin coated carbide) with compressed air and mineral oil at feed and speeds advised by them on their web site. it works well, but unfortunately the bit last about 10 minutes (cutting 295'' total).

anyone can help me about the increasing of the tool life:

what is causing this early tool wear abrasion, heat build up or both?

how long would a bit normally last for dry milling with air stream and mineral oil with ep?

should i get better bit life (less tool wear) by using a mist of water base coolant ( between 5 and 10 for 1) with a device like spraymaster http://www.tricocorp.com/products/product.aspx?c=5&p=22
?

please if anyone can help me it would be appreciated

[JROM]

First "bits" are used in a wood shop, endmills are used for cutting metal.
Heat is your enemy. If you can't use flood coolent try a cold air gun. Also you might try painting the parts with Moly-Dee. Its a cutting fluid made for high pressure cuts.

[Vincent82]

yes endmill is the right english term to use... For the tests I have made with coated carbide tools, I was using 6 cfm (air gun flow) of compresses air as coolant and mineral oil as a lubricant and tool was lasting 10 minutes only...

If stainless is condidered as an high pressure cut, I will try painting of moly-dee the cutting zone and using compressed air to see what would be the impact on tool life.

So if I'm right moly-dee will reduce abrasion.

[mark c]

What is the RPM and feedrate you're using? 10 minutes is WAY too short to last. I'm thinking you should use a smaller end mill. I program our stainless about that thickness using a 1/16 end mill using mist coolant. SFM should be 250 or so and about .001 per tooth chip load. It's possible you're going too slow and work hardening the material.
HTH

[johnmckeown]

i agree with marc heat is your problem with 304,slower rpm and higher feeds will help.if you can get away with 303 you will be better off as it will not work harden as easy,good luck and keep it kool
john

[davereagan]

Since you are only cutting .016-.024" thick stainless, how about varying the depth every 5 minutes with whatever extra cutting length you have to work with? Even if you only have .250" to play with, that's 8 different z depths and edges to use on the stainless.

[Vincent82]

The only kind of steel accepted is mainly the 304... the most difficult to mill.

Concerning the RPM I'm using, I try several... MA Ford as we can see on their tool infos http://www.maford.com/pdf/XR%20speedsfeeds.pdf
they are advising for .0013 - .0020 per tooth as chip load for .25'' endmill
I try several combinaison such as
30 ipm @ 4500 rpm
30 ipm @ 5000 rpm
30 ipm @ 5500 rpm
40 ipm @ 4500 rpm
40 ipm @ 5000 rpm
40 ipm @ 5500 rpm

For 40 ipm @ 4500 rpm (tool is wear and some tooth broken) & 30 ipm @ 5500 rpm (tool is wear), I try for all tool life with ONLY compress air flow and mineral oil... and I get the tool less damages with 30 @ 5500 (tooths not damaged)

Do a mist of water soluble coolant (which kind are you using mark c) my tool life?
Should I changed my speed/feed?

Thanks for your help guys!

[roninB4]

If your feeds and speeds are correct (I didn't check) and if you have a problem with chipping of teeth then it may be something else. Do the thickness of your material you may be having problems with vibration. Carbide is great for high speed but is so brittle that it doesn't stand up to shock or vibration very well. You could be experiencing micro chipping of the cutting edges and once this occurs your cutter will not last long. Take a single pass with your current set up and inspect the cutter with an eye loupe of 5x or 10x very carefull. A carbide cutter should exhibit NO ragged cutting edges, the only thing you should ever see after cutting is wear. Chipping will always be a sign of excess shock or vibration, provided it has normal tool life and correct speed/feeds. Carbide also doesn't work very well for interrupted cuts as this is also a form of shock during the initial cut load. Beyond the cooling others have correctly suggested I can't think of another area to look at besides your material clamping methods. It's thin material, it's going to vibrate unless you put the clamp down to it.

[Vincent82]

Thanks for your answer. The anchor method we are using is a vacuum table and the sheet is not moving. When tooth were broking, it was more because of incorrect feed/speeds. The problem is more concerning the wear of the tool after 8-10 min. We were only using mineral oil and compressed air stream.

So next try when we will have received the Spraymaster, I will use Trim Mist on cutting area and compressed air stream to flush chips by hoping this time it will work

[roninB4]

Re-cutting of chips is a problem that does need to be corrected and can very well be contributing to the problem. The material sheet may not be moving from the position but if it's vibrating I would still contend that this is part of your problem. The 8-10 minutes running time is simply not acceptable for carbide. If you place your finger on the sheet near where the cut is being performed (do be careful please) you may very well detect vibration that cannot be discerned by eye. Thin sheets are well known for localized movement and clamping near the cut path is quite critical to avoid this. I'll agree that the flushing of chips will help greatly but I don't think you can rule out localized vibration unless you've tested it. It makes a big difference. Good luck.