How long should an end mill bit last?

[MagTDK]

How long should an end mill bit last?

The bit I'm using is a 1/4 inch carbide 2 flute end mill. I've been cutting 3/4 inch MDF wood. I've only done like 10 cuts and the tip is now all burnt up (looks black). It also smells like somethings burning when cutting now, and the cuts are not as smooth anymore. Also the sound has a squealing pitch when cutting.

Do these bits not last long or am I doing something wrong? I'm cutting using a hitachi router set to max (24000) with my machine running at 30 inches per minute. And each depth pass is only .1875

Also can these bits be sharpened?

Thanks

[Madclicker]

I made the mistake of following the herd. I used carbide spirals because "everyone" said that was the bit to use. Big mistake I just recently figured out. I now use straight plunge carbides and the cuts are clean and crisp and the tools last much, much longer.

[drmosh]

30 ips is pretty slow, and 24k rpm is pretty darned fast. You're torching the bit. So yes, I can almost guarantee that you are doing something wrong, not the bit... but don't feel bad because finding the right "feeds and speeds" is as much of an art as a science.

There are LOTS of posts on cnc forums about this topic. Here's my advice and others can chime in:

1) everyone's machine is different - a setup for the same material on someone else's machine won't always be good for your's, but it's helpful to know what others are doing - the point here is take everyone else's numbers with a grain of salt
2) it's usually better to start of at the lower limit of rpm and feedrate then work your way up
3) you don't say if it's a spiral or straight flute bit, but if it was me I'd try the following setup: 60 ipm/10k RPM - see how that works and go from there. That feedrate is still probably too slow but it's a good place to start.
4) on mdf you won't get "chips" like you would in ply or hardwood, but it shouldnt be powdered or dust either. it should be kind of "downy" for lack of a better word.
5) YOU SHOULD NEVER SEE SMOKE/SMELL SMOKE/SMELL BURNING/SEE BURN MARKS/ETC - any of these are immediate indicators that your either moving too slow, spinning the bit too fast, or BOTH!
6) yes the bits can be resharpened

One final bit of advice - I learned on 1/2 bits because they are so much more forgiving, then worked down from there. Don't be suprised when you break a 1/4 bit (or 2, or 3...) as you're learning because they are the most delicate.

Hope it helps and good luck!

[MagTDK]

Thanks for the advice. By the way,the bit I was using was a spiral bit.

I noticed that if I go above 30 ipm on my machine it tends to round the corners somewhat so thats why I've been cutting at 30 ipm. I probably can get away with 40 ipm though. As for the bit, I'll try buying a straight flute bit if I can find one around here, otherwise I'll have to order it online. I'll also knock down the speed on my router to see if that helps because when I cut all I see is dust (I thought that was what I was suppose to see).

How deep of a cut do you normaly go for each pass? And how do you resharpen a bit?

[mxtras]

Originally Posted by MagTDK .....And how do you resharpen a bit?

You need specialized machinery to resharpen a cutter correctly. Not exactly for the DIY guy to pick up and learn quickly unless you have deep pockets.

Scott

[paulC]

Wood cutting builds up crap, be it sap or carbon.
You need to clean off any build up. There are proper cleaners but a lot of people simply soak in oven clearer.
And end mills are not for plunging.
Paul

[cutsall]

Been cutting MDF the last six years and have found the quality of the MDF has a lot to do with the longevity of tools. A double refined MDF such as Plum Creek or Ranger Board are not as abrasive as a cheaper brand. If you must run slower feed to control corner rounding and cannot reduce rpm accordingly then lighter depth cuts can be taken. If you take lighter cuts then you can end grind your end mill, grinding it back to the depth of cut you have been taking and not have to grind the o.d. I use spiral flute carbide end mills they have a better shear factor, the cutting edge does not hammer the cut the way a straight flute does and if you use a center cutting end mill you can plunge with them, have done so for twenty seven years in metal and wood. Each and every application is different and you must evaluate your limiting parameters, machine, material, tooling and adjust your approach accordingly. So we have all given you our opinions based on our experience and now it is up to you to experiment to find what works for you. Best of luck.

[ger21]

Are you using spiral router bits?, or end mills made for cutting metals? There's a big difference.

Heat kills router bits fast, and going too slow while spinning too fast adds up to too much heat.

For an Onsrud 1/4" 2 flute spiral cutting MDF, the recommended feedrate at 24000 rpm and 1/4" depth of cut would be 300-350ipm. That translates into ~125ipm at 10,000 rpm. If you have to go that slow, try a single flute bit, it will last longer.

As mentioned, keep your bits clean, and they'll last longer.

Squealing noise is very common with small diameter tools, not much you can do about it, but lower rpm's will help.

Getting any type of chips is difficult from MDF. We cut MDF with 1/2" bits, 15,000 rpm and 400ipm, and it leaves about 1/2 chips, 1/2 dust.

If you want to get them sharpened, you can send them to www.vortextool.com

[cutsall]

Originally Posted by ger21 Are you using spiral router bits?, or end mills made for cutting metals? There's a big difference. Heat kills router bits fast, and going too slow while spinning too fast adds up to too much heat.

Running 24000 rpm at 30 IPM will kill a carbide router bit or a metal cutting carbide end mill. I think the issue at hand is the accuracy he is trying to attain with a controller not capable of running at the feedrate needed to maintain the chip loading required. A vortec cold air gun or just a sufficient air blast to cool the tool might help but that is no guarantee because of the abrasive nature of the material. The slower the tool moves the more heat it builds and instead of the tool cutting the material the material is grinding away the tool. I doubt there is a solution that is tooling related but I agree the single flute upcut would be the way to go. North American Products has tooling that rivals Onsrud and is a bit easier on the pocket. If you are trying to cut a square corner with a machine that cannot achieve the accuracy at the feed rate required to preserve the integrity of your tool and are willing to sacrifice material program to cut a small circle with arc center past and (right or left) of your corner equal to the radius this will allow the cutter to make its transition from x to y or y to x and be back into perpindicular postion for a right angle cut the overrun will occur in the circular movement. It works. Your cutter runs staight past the corner the distance of the radius starts the circular movement cuts three quarters of a circle and continues straight back into your cut. Kinda primitive but it will work.

[MagTDK]

Thanks again for all the advice.

I did pick up a straight 2 flute bit earlier today and turned down my router to half the spindle speed. That helped tremendiously. I cut out like 6 pieces today and the bit still looks good (no burnt marks). I did try going lower but then the router sounded like it was struggling. Either way it's an improvement considering I only cut like 10 pieces with the other bit before I fried it. The cuts came out really smooth and straight too (no rounded corners). I'll have to try a single flute bit as well when I get a chance.

Fortunately I won't be cutting much MDF after this. Most of the material I will be cutting will be machinable wax.

[cutsall]

Great News. MDF is some messy stuff. Talcum Powder like dust gets everywhere.

[Madclicker]

Originally Posted by cutsall Great News. MDF is some messy stuff. Talcum Powder like dust gets everywhere.

Don't forget the dust collector....most important tool in the shop.