Okay, I've just started using some 3/32" carbide, 4-flute, square end, plunge-cutting endmills that I had here - never used one of this size before...
Anyway, I don't know what's going on, but they start to plunge and either snap before the plunge is finished or after the plunge, when the cut starts to move laterally, they snap.
It's weird because I have the same end mills in 1/8" and can cut the same piece and pattern without trouble. I can also drop a 1/16", 2-flute without issue either.
Now the weird thing is that when I look at the hole, it looks like the mill just didn't cut - like it's dull, but they're brand-new. They feel sharp to the touch too.
More specs: Taig CNC; 6,700rpm; soft brass; 0.0625" plunge; 4ipm feed rate.

Any ideas? I've just killed two end mills and don't want to try another until somebody gives me some advice. Is 6,700rpm too fast??? Too slow?? Weird thing is that I was just cutting with a 1/16", 2-flute end mill and it was eating the metal like candy. The only other thing I can imagine is that 4-flutes is too much for a 3/32" cutter to clear the chips, but the chips are more like dust - something I haven't seen before. I slowed this down to 4ipm to let it have an easy time of it and that didn't help - I usually run at 8ipm or so with my other cutters. :confused:

Thanks,
Mark

I would suppose that there is just not enough clearance in the flutes for the chips to come up the flutes. A two flute can usually be made to do a decent job of 'drilling' a hole while plunging. Still the chips can occassionally weld into the flutes if lubrication is interrupted (in aluminum) and plug the tool. In deep slotting, it might be good practice to allow the tool to rapid up to clear itself before beginning the lateral movement.

The center cutting 4 flutes, IMO, are suitable for ramping in, not so good on the vertical plunge. A zigzag ramp, or a helical ramp or a boundary ramp are more desirable from a tool life point of view.

When we ran small endmills at our last shop, they programmed them to either spiral feed down into the stock or ramp feed, ramping is done when either x or y axis is moving durng the z-axis feed. Also, the RPM looked a little slow!
What grade of Carbide ar thos endmills, C2 C4 C6? C6 being the toughest grade!

Eric

I've used 4 flute cc minis in all 3 diameters, and one thing I've noted is that they have to be specified for aluminum in those itty bitty sizes. Every time I've gotten mixed up and used one with rake and relief angles ground for steel, they do exactly what you describe when cutting aluminum.

That "dust" chip description sure rang a bell ;)

Might be something else as your specific problem, but my own booboo history has always been wrong rake and relief angles when this sort of thing happens with the minis.



Tiger

When we ran small endmills at our last shop, they programmed them to either spiral feed down into the stock or ramp feed, ramping is done when either x or y axis is moving durng the z-axis feed. Also, the RPM looked a little slow!
What grade of Carbide ar thos endmills, C2 C4 C6? C6 being the toughest grade!

Eric


I don't know the grade - they are 30-degree helix made by Fastcarb Tool. I will try to ramp feed one tomorrow and see what happens. I was curious about this after I posted, so I put the same piece of stock back into the vise, installed a 2-flute, 1/16" end mill, reprogrammed SheetCam with the new diameter, but kept the feed and z plunge and everything else the same and ran it. The 1/16" did a fantastic job, even if it took over 75 minutes :-(

Oh well, maybe I need to try some 2-flute end mills in the 3/32"...

Thanks,
Mark

I've used 4 flute cc minis in all 3 diameters, and one thing I've noted is that they have to be specified for aluminum in those itty bitty sizes. Every time I've gotten mixed up and used one with rake and relief angles ground for steel, they do exactly what you describe when cutting aluminum.

That "dust" chip description sure rang a bell ;)

Might be something else as your specific problem, but my own booboo history has always been wrong rake and relief angles when this sort of thing happens with the minis.


They're 30-degree helix - not sure what that's intended to cut? Probably not soft brass? Shoot...

Mark

Sorry, I missed that you said the material was brass. A high helix is not likely to be the answer, because brass has a tendency to cause the tool to 'hog in', overload itself and wreck something.

For the best cut while drilling (plunging) the brass or bronze alloys, the tool flute should have no helix at all. If you have a tiny wheel on a Dremel, you can get the wheel inside the flute at the sharp edge at the cutting end, and grind it flat, with a flat face parallel to the axis of the tool. This flat does not need to be extremely wide, probably .020" wide would be sufficent. It should be accurately flat, and should not round over the edge. Even presented to the work at a 90 degree angle, an edge will still take a chip if it has clearance underneath.

Did you buy them on eBay
I bought some carbide endmills and they were snapping like popcorn
I believe that sometimes they unload the poor carbide on ebay.
when i used the same size cutter from MSC, it took the load no problem !
On 4 flute plunges, I never go deeper than 1/2 the cutter diameter.
A 2 flute will go 3 diameters, but those 4's cannot clear out the chips.
rich
I run down to 3/64 (.045 )too on carbide .

Did you buy them on eBay
I bought some carbide endmills and they were snapping like popcorn
I believe that sometimes they unload the poor carbide on ebay.
when i used the same size cutter from MSC, it took the load no problem !
On 4 flute plunges, I never go deeper than 1/2 the cutter diameter.
A 2 flute will go 3 diameters, but those 4's cannot clear out the chips.
rich
I run down to 3/64 (.045 )too on carbide .


Yeah, they're Ebay, but supposedly made in USA. The Chinese imports I have from Ebay seem to work okay too. I don't know, it just seems like maybe this entire lot is bad? I wrote the seller and am waiting to see what he says. I may try another one today and only plunge 1/2 of the diamter and see what happens, but there's just something else going on here because of the "squeal" these make when they touch and start to plunge - just doesn't sound right. I have some ball nose ones from another vendor that I may try, just to see if they work and sound differently.

Mark

Sorry, I missed that you said the material was brass. A high helix is not likely to be the answer, because brass has a tendency to cause the tool to 'hog in', overload itself and wreck something.

For the best cut while drilling (plunging) the brass or bronze alloys, the tool flute should have no helix at all. If you have a tiny wheel on a Dremel, you can get the wheel inside the flute at the sharp edge at the cutting end, and grind it flat, with a flat face parallel to the axis of the tool. This flat does not need to be extremely wide, probably .020" wide would be sufficent. It should be accurately flat, and should not round over the edge. Even presented to the work at a 90 degree angle, an edge will still take a chip if it has clearance underneath.


Does the helix refer to the number of spirals/turns per unit length, or are they referring to the faces of the spirals themselves? I guess I don't understand this all very well :confused:

The helix is the angle of the flutes relative to the axis of the cutter. On a high helix end mill, the flutes have to go around the cutter more revolutions than a standard end mill. High helix is analogous to a finer pitch screw thread. The advantage of the high helix is usually better surface finish. The disadvantage is that the chips have to travel farther up the flutes to be ejected from the cutting zone. So high helix are not good at deep slotting in aluminum but leave a lovely finish when profiling steel.

I agree that the 4 flute is probably loading up and cannot clear the chips.

Hi. Didn't read every post here so I might be missing something. How's your runout? Are you using the same collet for that particular tool? For that small of a tool, I'd spin it as fast as I can and make shallow cuts.

JR

So high helix are not good at deep slotting in aluminum but leave a lovely finish when profiling steel.

I agree that the 4 flute is probably loading up and cannot clear the chips.

they make high helix for alumininum , i've cut production cycle times nearly in half using high helix , because you can hog out a lot more material with them , while a normal carbide endmill is recommended to cut at 1/2 the dia , high helix is up to full dia

10,000 RPM [or max] and .0005" feed per tooth with coolant, go full depth and if you need to, slow the feed down. I did "Bowtie" slots in 316 stainless 1/16" dia. x .100" deep and went thru a few of these [.0625 dia.] endmills before I figured it out. Once I established the approach, it was smoothe sailing for me then!

!!Whoo-hooo!!

10,000 RPM [or max] and .0005" feed per tooth with coolant, go full depth and if you need to, slow the feed down. I did "Bowtie" slots in 316 stainless 1/16" dia. x .100" deep and went thru a few of these [.0625 dia.] endmills before I figured it out. Once I established the approach, it was smoothe sailing for me then!

!!Whoo-hooo!!

I don't understand the ".0005" feed per tooth" - there have to be more factors that play into that - I'm missing something? :rolleyes:

I've found a nice speed/feed for what I'm doing now. I'm cutting brass with a 1/16" 2-flute carbide. I've found that I get a pretty nice finish at 6,700rpm, two passes of .0625" at 4-5ipm feed rate. That's not very fast, but finish is nice and I have gotten probably 15" hours cutting time on my latest end mill. I don't use liquid coolant. I have a thin stream of air directed right at the cutting tip. That seems to cool it pretty well (I've stopped it and touched it and it was room temp) and keeps the chips completely away from being churned back into the flutes.

I'm still experimenting a little, but that seems to be what works best for me.

Mark

Mark,
Lets review feed in relation to milling, ie:
chipload per tooth.
rpm X (feed per tooth X number of flutes) = feed in IMP
6,700 X (.0005" X 2) = 6.7 inches per min.
It doesn't sound logical but Iv'e been doing it like this for a while.
Your feed is a bit slow fer me, but if you enjoy the results, great!
What ever it takes to get it done R I G H T !
[and looking good for the Ladies doesn't hurt!]

Mark,
Lets review feed in relation to milling, ie:
chipload per tooth.
rpm X (feed per tooth X number of flutes) = feed in IMP
6,700 X (.0005" X 2) = 6.7 inches per min.
It doesn't sound logical but Iv'e been doing it like this for a while.
Your feed is a bit slow fer me, but if you enjoy the results, great!
What ever it takes to get it done R I G H T !
[and looking good for the Ladies doesn't hurt!]


I have turned up the speed a bit, but the noises scare me :rolleyes:
But the result is nice - that's why I'm thinking that another Taig, running nice and slow, would double my production and not mess up what I think is a good configuration for me? :cheers:

Don't be afraid of the noise, that's machining.
if you are pleased with your results then go for it.
I only wish to enlighten you on how "We do it in the BIG shops" !!

10K rpm at .0005 per tooth is .002 per rev times 10 k is 20 ipm
Jim

?

10K rpm at .0005 per tooth is .002 per rev times 10 k is 20 ipm
Jim

What he is trying to say, is that at 10,000 RPM each tooth of the cutter will advance .0005" with each revolution of the cutter, in the machining industry, this is called "Chip Load" !

Eric

Chip load per tooth
the amount of material being removed by each flute per revolution
see the formula:
10,000 rpm x .0015 [this is calculated by .0005" per flute x 3 (number of flutes)]
feed in ipm = 15 ipm

That's not very fast, but finish is nice and I have gotten probably 15" hours cutting time on my latest end mill.

I'm still experimenting a little, but that seems to be what works best for me.

Mark


15 hours, WOW, if I was getting 15 hours of tool life, I would pick it up quite a bit. Thats a sure sign that your going WAY TOO SLOW. Are you trying to make money or are you just playing around and having a good time. I guess it is brass and RPM is limited, but cutting tools are called consumables for a reason. There is a line somewhere that maximizes profit between tool life and time, and for me 15hrs is just eating up $65/hr time to save a few dollars on endmill. I guess it varies based on your overhead and how fast you need that job off of the machine.

As for being afraid of the noise, you'll learn whats a good noise and whats a bad noise in time. It can get VERY loud sometimes, but as you become more expierienced, you'll be able to hear the slightest variations and you'll know what each change in tone means, (shes getting a bit dull, 2 more parts max/ lost a corner / chipped the edge / cut that part a little long on the bandsaw etc...)

The chipload thing, that goes back to the basic of basics. Purge your mind of RPMs and IPM, they are simply functions of the two things that should be stuck in your head, Surface Speed and Chip Load. If you asked me how fast I was running a cutter, I'll tell you 400sfm, .0025 per tooth, I'd have to take the 15seconds to calculate the RPMs and IPM.

A good chip load is music to my ears!

If she's not singin to me, she's not happy. If I can get her singin as apposed to moaning, then I'm happy. Once in awhile, a good moan is cool but......Oh, wait a minute we're talking about machining.

most of the problem is the inferior cutter ,its rediculous to have to run so slow ,you can be sure that if someone puts those cutters on ebay , they bought them for next to nothing , sold them to you for a little more than next to nothing , how many hands have these tools been thru ? they were probably made for pennies in china , products are concidered made in america if they are assembled here , like putting tools in a box for example , bottom line is you get what you pay for ,if you pay 2 or 3 dollars more for a decent tool ,you will see the difference
its the equivelant from spam to tenderloin , sure spams cheaper but it tastes like crap
brass cuts very easily , but running it at .0005 your only going to dull your tool because brass is very abrassive , at 6700 rpm you should be running at roughly 15 ipm with a four flute minimum, if your plunging you would be better off with a slot drill ,because these are made for it , an endmill is not designed to plunge , even though we may do it at times

the noise and the burred looking hole get me
is there clearance on the front of the tool?
is the tool resonating ?(flexing spirally)
are the cutting edges equal size and angle?
sounds like junk cutters
like most things you get what you pay for
mike

the noise and the burred looking hole get me
is there clearance on the front of the tool?
is the tool resonating ?(flexing spirally)
are the cutting edges equal size and angle?
sounds like junk cutters
like most things you get what you pay for
mike


I'm pretty sure it's the cutter. I can run any other size or number of flutes without trouble. For the most part, I pay around $4 each for these little cutters and this batch was just bad. But overall, I can't complain. I've got twenty hours now on the 1/16" that I said I had fifteen on a couple of days ago - and it's still going strong. I just can't bring myself to pay tons of money when a little bargain basment shopping and an occasional bum cutter is the only price I pay :cool:

dude for those little cutters you'll be surprised the difference in price between good ones and not so good of ones , not much , and things go far smoother , if you break two cheap cutters so what , but you could have bought one good one and if its run properly it won t break , its all about saving the grief

someday i should follow my own advice , i ve got two of everything in my workshop ,one good one and one broken cheap piece of crap