PDA

View Full Version : End Mill Busted-What did I do wrong ?



kNucKlbustr
11-01-2013, 10:17 PM
Using an 4-flute 1/8" end mill center cut, TIN coated.
At 1700 rpm. .050" DOC. Slotting 12"L.
The calculations say feedrate at 6.8 in/min.
It broke immediately. Did I calculate wrong ?

dp
11-01-2013, 10:27 PM
My experience with small 4-flute end mills is that they are 90% air and prone to breakage. If it was not dull then it was being shoved into the work faster than it was cutting. If it was dull it did what it should. Metallurgy of the cutter may also be a factor when the cutter is known to be sharp. That is to say, if it is a cheap Harbor Freight cutter like I'm inclined to buy it will likely snap off and assume candidacy for becoming another kind of tool.

firbikrhd1
11-01-2013, 10:39 PM
No expert here but possibilities include a defective end mill, poor quality import, chips binding in the slot for a start. A two flute end mill allows more clearance for chips when slotting. Coolant to wash the chip s away or a stream of compressed air can help. A 1/8" end mill isn't the stoutest thing going.
You didn't mention whether your end mill was carbide or HSS. I have zero experience with carbide end mills but I believe the may be more brittle than HSS and less forgiving of twisting or flexing if bound in the slot by chips.
Hopefully the really experienced machinists will give you their input. I am interested in seeing what they say as well.

Bob Fisher
11-01-2013, 10:46 PM
6 in per minute for a 1/8in two flute seems a bit much. What material? Aluminum at that feed with no coolant can build up on the tool and won't last long after that happens. If you ask me how I know that, I'll deny it! Bob.

kNucKlbustr
11-01-2013, 11:01 PM
6 in per minute for a 1/8in two flute seems a bit much. What material? Aluminum at that feed with no coolant can build up on the tool and won't last long after that happens. If you ask me how I know that, I'll deny it! Bob.

Sorry to leave that out. 6061 aluminum.

New Niagara SC406 TIN HSS. $16.

I used a 2 flute HSS double end mill at 5 in/min, mills ok. The edges of the slot are ruff, me thinks not sharp.

So that why i used a 4 flute, because faster feed ?

Running at 5in/min 12"L, 6 slots, takes forever. 1st pass .050", second pass another .050". Need 0.100" DOC.

lakeside53
11-01-2013, 11:04 PM
4 flute EM suck in Al... Are you sure the end didn't get blocked up before breaking?

I use 2 or 3 flute in AL, and really keep up on the kerosene lube.

dalee100
11-01-2013, 11:11 PM
Hi,

Yep. A 4 flute endmill in aluminum is asking for trouble. And for a tool that small, I would very seriously consider using a high helix endmill meant for aluminum if needed to mill that fast and deep in one pass.

Kersoine is a good cutting fluid for aluminum, but WD40 also works well for those who don't want kerosine.

dalee

David Powell
11-01-2013, 11:36 PM
Using an 4-flute 1/8" end mill center cut, TIN coated.
At 1700 rpm. .050" DOC. Slotting 12"L.
The calculations say feedrate at 6.8 in/min.
It broke immediately. Did I calculate wrong ?

Firstly I would prefer a 2 or maybe 3 flute end mill to cut a slot. Secondly, especially If I need a deep slot cut I do not use the power feed initially but I move the end mill vertically using the quill movement, as if drilling, then with the end mill out of the work move the table about a third of the diameter and repeat until I reach the end of the slot I need, then I engage the power feed and clean the slot up., then move sideways to get the width I need. Trying to cut a deep slot to width , with an endmill in one go with my light built Chinese made vertical mill is frustrating, produces poor results and I break end mills too often even using lots of cutting oil and compressed air. Hope this hint helps someone. David Powell.

kNucKlbustr
11-01-2013, 11:50 PM
I used a spray bottle w/ diluted TRIM.

So, unless the rpm increases, next pulley will go 2500 rpm, Ill need to be at approx 5ipm w/ a 2-3 flute.
2.5min per 12" run x 2 x 6= 30 mins. x,y,a running on Mach3, manual z axis.

TGriffin
11-02-2013, 12:33 AM
Way too low an rpm plus the fact that you were using a four flute is what killed the end mill. A 1/8" end mill in aluminum should be run at around 8000rpm (4 X sfpm / Diameter = 4 X 250 /.125 = 8000), or as close as you can get with your mill. Use a two flute for chip clearance and be sure to use cutting oil because aluminum likes to stick to end mills. WD-40 works well on aluminum. 5 inches per minute should be fine for a .05" deep cut.

Tom

ahidley
11-02-2013, 12:48 AM
All good replys, exspecialy the last.... FAST RPM for the tiny 1/8 diameter, 2 flutes. Also use CLIMB MILLING on aluminum if your mill is capable and lots of coolant to prevent chip welding to the flutes.
If your machine is not capable of climb milling then perhaps you were climb milling and didnt know it and that is what broke it???

beanbag
11-02-2013, 06:53 AM
I bet if you look at the broken-off part of the end mill you will see a blob of aluminum stuck in the flutes. TiN is not a good coating for Aluminum anyway. What you want is either uncoated, ZrN, or TiCN. For this kind of cut, you need flood coolant blasting vigorously to clear out the chips. Otherwise, you will get built-up-edge, and break the end mill right away.

DR
11-02-2013, 07:27 AM
16 bucks, ouch.........

As beanbag says.

I've been in the business 30 years, even now sometimes I'm lazy. I use a four flute in aluminum because it's in the holder and I'm in a rush. Most times I end up with a broken cutter too. Occasionally you can get by with the four flute, but you must clear the chips. A mist coolant setup with high air pressure might work if no flood coolant available.

J Tiers
11-02-2013, 08:31 AM
lessee....

6.8 in/min, 1700 rpm. 6.8inper min/1700 revs per min = .004 movement per turn. Then advance per tooth should have been 0.001". Depth of cut at 0.05" isn't so much, and the usual issues of chip removal are not as important, they virtually fall over outside the cut.

On the surface of it, that speed and feed doesn't really seem totally out of line on a cut per tooth basis, although I would have preferred to use a 2 flute. That's even more likely since you went at 5" per min with 2 flute and no problem. At that rate you had actually a LARGER advance per tooth than with the 4 flute. (which could have helped)

maybe there is another issue.

If EM is not dead sharp. it will not TAKE a cut of 0.001", and so maybe a couple teeth pass by and the next one cuts 0.003". That can get to be an issue.

maybe it was skipping a bit as above AND recutting chips, so it took a much larger cut per tooth than you think. Rough edges may indicate re-cutting and re-welding of chips onto the walls. Or a dull cutter. Or buildup on the cutter.

Maybe it had some buildup due to gummy aluminum, and was acting dull, so it wouldn't cut correctly. You can cut hard aluminum alloys like 7075 much better than the soft gummy more pure alloys. The soft ones stick to and fill up the flutes, especially 4 flute cutters, and prevent cutting. You need to use lots of oily cutting fluid to "poison" the surfaces and prevent buildup.

If it really broke RIGHT AWAY, and it was a blind slot, plus the EM is not an end cutting type(4 flute tend not to be), then the process of dropping it into the slot was likely more "plowing" than "cutting", which may have instantly built up a blob that would flat refuse to cut at all.
If so, you were not cutting when you started the feed, you were still "plowing", and the EM failed by bending. Nearly every 2 flute is end cutting, so a 2 flute would have been fine.

kNucKlbustr
11-02-2013, 10:12 AM
Seems the consensus is lots of fluid. Ill have to rig up a drip bottle. The 4F EM CC snapped as it started. The bed moves L-R w/ a CCW spindle on the 1st pass, R-L on 2nd.
I finished one piece w/ an old 2F EM and the slot edges had this galled-like buildup that had to be scarp off hard w/ a blade.
The piece was off .007" DOC from end to end. The tailstock needs to be re-shimmed.
I still have another issue to deal w/ that was foreseen. The piece of rod is held between centers w/ a converted Ellis divider(A axis) and theres vibration towards the middle.
I havnt figured what type of screw jack to steady it, w/out it catching the milled slots as the divider turns, for the next slot.

A.K. Boomer
11-02-2013, 10:24 AM
I like the triple flutes for aluminum and my machine is limited on RPM's so I just cut back on the feed rate but one thing for sure - whatever means your using for cutting fluid throw allot of it at it...

I have a mister and I just blast the cutter to help clear out chips, generally works pretty well...

the smaller the bit the higher the RPM's but if your machine don't go there then cut back on the feed and depth, I should be rapping out at triple the RPM's that I have for a 1/8" cutter but I just make due and make adjustments...

Rosco-P
11-02-2013, 11:26 AM
If you're doing lots of slotting, maybe a horizontal mill is in your future. Lots of small mills around, Burke #3 or 4, B&S #0, etc., small footprint, selling cheap, cheap cutters, deep cuts, etc.

Jaakko Fagerlund
11-02-2013, 12:48 PM
I havnt figured what type of screw jack to steady it, w/out it catching the milled slots as the divider turns, for the next slot.
V-block that you shim to the correct height.

outback
11-02-2013, 01:52 PM
Your cutting speed was way to low. At 200 feet/minute (low for aluminum) I figure 6400 RPM which is more RPM than most machines can run. Feed rates for small endmills is more of a ratio of depth of cut and feed rate. With tiny endmills I have my best success with a .010" depth of cut and multiple passes. That gets the job done while rarely breaking the endmill.

Coolant or cutting oil is important particularly with aluminum and particularly with small endmills. Anything oily works well in aluminum and is better than nothing.

CNC is really the answer for tiny endmills. Those tiny endmill have absolutely no feed back on our crank handles. A little to much feed and the end mill is a goner and does it with no warning. With CNC the feed rate is preset in the program and that is exactly how fast the tool feeds. CNC does not do cutting feedback like a manual machine. I run 1/16 and 1/32 end mills in my CNC mill and rarely break off a tool. Set the RPM high and the feed rate low like 2 to 3 IPM and sit back and relax.
Jim

kNucKlbustr
11-02-2013, 09:12 PM
My book says for aluminum alloy. 1/8 EM, .050" DOC, feed per tooth is .001

If, I get the courage to run this old beast at 2500, is it safe to say, feed rate at .025" DOC is 10 ipm ?
2500 * .002 * 2

Zero_Divide
11-02-2013, 10:03 PM
My calc says at 1700 rpm you got to feed 5.1 ipm
Its all about flute lenghth.
Also coolant is mandatory

J Tiers
11-02-2013, 11:07 PM
What was the machine?

Was the slot blind on both ends? so you had to drop it into the material?

If so, the problem may have been with the entry to the material, which could also happen with starting the slot on the end of the piece.

The cutter is more "free" as it starts. If it was dropping into the work on a blind slot, it may have wandered excessively due to an aggressive feed down, and the wander might have broken it. EMs don't like that and accept far less of it than drills do.

if it was starting into the end of the part, same thing applies, you may need to "baby" it into the work to avoid it catching and bending sideways, resulting again in a break.

outback
11-04-2013, 08:17 AM
My book says for aluminum alloy. 1/8 EM, .050" DOC, feed per tooth is .001

If, I get the courage to run this old beast at 2500, is it safe to say, feed rate at .025" DOC is 10 ipm ?
2500 * .002 * 2

Your formula is 2500 X .002 X 2 What is the "2" for?? If you use a 2 lip endmill and the feed is .001 per tooth the endmill must advance .002 per revolution. Take the .002/rev X 2500 RPM and I got 5"/min feed rate. A 4 flute endmill would be
10"/min. I break plenty of 1/8 endmills using much less feed rate than that.

Okay, I see it now. Since the depth of cut is .025 instead of .050 you are going to double the feed rate, right?
Jim