PDA

View Full Version : Snaped a chinese cutter. My fault?



Black_Moons
10-23-2010, 10:18 PM
Hi, I recently tryed puting some notchs in some 1/8" thick hot rolled (1018?) using a 1/4" 2 flute ball nose endmill at 300rpm (slow I know..)

It worked fine as long as I took passes about 0.1" deep, but I tryed one slot at 0.5" deep and it basicly snaped before getting half way in. The entire time it was cutting (even the shallow passes) it made a 'snaping' noise. I only fed at about 4 to 6IPM, Snaped about half way up the flutes. (1 1/2" flute length or so..)

Was this my fault for feeding too deep? Too fast feed for the RPM? (Aka too high of chip load per tooth) Or just a bad chinese cutter improperly ground/heat treated or somesuch?

When I finished the job with my 5/16 (that turns out the 1/4" was too narrow anyway!), it did'nt make that 'snaping' noise while cutting normaly at same RPM and same 0.1" DOC, Did not try doing any more one pass 0.5" DOC's. made a much better cutting noise like my standard endmills.

Ken_Shea
10-23-2010, 10:22 PM
BlacMoons,
As you mentioned, way too slow and too fast a feed, and .5 DOC is pretty much out of the question.

Live and lean, who hasn't done the same.

I am not even going to mention further on the Chinese EM, you'll discover the truth fast enough. ;)

gwilson
10-23-2010, 10:23 PM
I suppose you should have backed off on depth of cut,or feed rate if you heard a snapping noise. That might have been the result of the cutter actually flexing some,and snapping back straight just as it finished each cut.

Regardless, I generally have found that Asian HSS is on the more brittle side . Another problem with them seems to be inconsistent sharpness. Some will be quite sharp,while others just do not have that keen edge.

Maybe you should check the edge before using an end mill,and hone it a bit if necessary.

bborr01
10-23-2010, 10:28 PM
If you need a radius at the bottom of the slot, cut it with a regular end mill and then put the ball nose in.

That should eliminate the snapping noise.

Also, 1/2 inch DOC is pretty deep with a 1/4 inch end mill in steel.

And way too slow, try around 7-800.

Coolant?

Brian

Evan
10-23-2010, 11:17 PM
A ball nose end mill cannot be fed anywhere near as fast as a regular end mill. The problem is that the cutting edges have a variable SFM which approaches zero as the edge nears the tip of the ball. Any attempt to use it like a regular end mill is inviting trouble as you found out.

J Tiers
10-23-2010, 11:33 PM
Hi, I recently tryed puting some notchs in some 1/8" thick hot rolled (1018?) using a 1/4" 2 flute ball nose endmill at 300rpm (slow I know..)

It worked fine as long as I took passes about 0.1" deep, but I tryed one slot at 0.5" deep and it basicly snaped before getting half way in. The entire time it was cutting (even the shallow passes) it made a 'snaping' noise. I only fed at about 4 to 6IPM, Snaped about half way up the flutes. (1 1/2" flute length or so..)



Does NOBODY ELSE see a BIG PROBLEM with the above?

He has 1/8" thick 1018.... HOW DID HE GET 0.5" DEEP CUTS?

He had to be going in and cutting through the thickness of the material from the 'face" of it. Dunno about you folks, but no way would I do that..... I would cut in from the 1/8" face if the notches were on the edge, as it seems they must be.

The snapping noise he mentions is probably the material as the tooth leaves it and the thin material snaps back as the cutting force is released....

Me, I would have bagged the ball end cutter and depended on the radius of the cutter to create the rounded bottom of the notch, if I "see" this correctly. Coming in from teh edge of the material it should work great.

The 1/8" thick material should cut like butter.

As for 1/2" deep, I have done that with a 3/8" roughing cutter, in 1018, and was able to feed about as fast as I could crank the mill..... and I only have 1/4 HP. The cutter was chinese , too. I was cutting the adjustment slot in a replacement steady rest jaw.

Ken_Shea
10-23-2010, 11:37 PM
Ha-Ha, good call JT, I did not see that :D

There was just too much wrong for that operation to have a good outcome.

Liger Zero
10-23-2010, 11:42 PM
Ha-Ha, good call JT, I did not see that :D


Not only did you break a cutter but you broke the laws of TIME AND SPACE! :eek:

Black_Moons
10-24-2010, 12:45 AM
Hah, In retro spect it was more like 0.3" DOC, but the 1/8" thick peice was mounted verticaly in the vise, ie I was trying to put a rounded nose in it, Like you would if you side milled a sheet of steel with a normal endmill, but I wanted to facemill it because well, It was harder to mount that thing on its side and not crush the internal threads..

I was making one of these: http://motorbicycling.com/attachments/f4/2636d1222043500-made-new-clutch-flower-nut-retaining-screwin.jpg

RB211
10-24-2010, 12:55 AM
Sounds like your workpiece was flexing while being mounted in the vise. This will break endmills as well.

Ken_Shea
10-24-2010, 01:06 AM
Not only did you break a cutter but you broke the laws of TIME AND SPACE! :eek:

Wasn't me that broke that cutter, but I've done my share over the years, almost always due to lack of attention, unnecessary expense is a great teacher.

MuellerNick
10-24-2010, 05:48 AM
Why guess? Every manufacturer (except the Chinese) has extensive material of cutting recommendations. Surface speed, DOC, feed per tooth, lubrication. Consult it, consume less mills.

A ball nose cutter cuts much better when you tilt it (or the work) so that the center line of the cutter is not in contact with the material.
Say you tilt the mill's head by 30 and and feed such way the tip of the cutter points away from the feeding direction (drag, like with a pen), you no longer have the zero-speed-problem on the tip.


Nick

airsmith282
10-24-2010, 08:28 AM
300 rpm is a bit slow and if the feed was to fast then yup you broke,it , in steel i always mill at 400 to 450 max and slow feed and even i can take 30 thou or more and not think twice about it with chiness cutters, 300 rpm you would have to take extreamly slow on the feed,even at 30 thou or more might fall alsleep to ,

but its all cool, took me a bit to learn my mill and its limints and a few broken cutters alonge the way and i snaped a few really costly ones man it hurt but it happens,

RKW
10-24-2010, 09:29 AM
I think you are still off. You must mean 0.03" or 0.003" but not 0.300" since 1/8" = 0.125".



Hah, In retro spect it was more like 0.3" DOC, but the 1/8" thick peice was mounted verticaly in the vise, ie I was trying to put a rounded nose in it, Like you would if you side milled a sheet of steel with a normal endmill, but I wanted to facemill it because well, It was harder to mount that thing on its side and not crush the internal threads..

I was making one of these: http://motorbicycling.com/attachments/f4/2636d1222043500-made-new-clutch-flower-nut-retaining-screwin.jpg

bborr01
10-24-2010, 09:52 AM
One other thing that I don't see mentioned.

1 1/2 inch flute length on a 1/4 inch end mill is way longer than standard length.

I wouldn't use an extra long end mill unless I had a need to reach extra deep into a slot.

Brian

gwilson
10-24-2010, 10:02 AM
Gad! I missed all of those details last night. Must have been tired. Having the info that the 1/8" was mounted vertical helps a lot. So does the 1 1/2" length of flute. Always use as sort a cutter as you can. As said,a round nose is not a very efficient cutter. I had thought about that,but missed commenting. You really should mill out as much as possible with a regular end mill,and mill the radius separately.

John Stevenson
10-24-2010, 10:07 AM
Drill a slightly undersized hole where you want the slot to finish, rough out with a 6mm end mill [ 0.236" ] then swap to your ball nose for the final pass which will only remove a gnats cock and save the cutter.

The drill and the 6mm cutter will do all the heavy work, the ball nose is only for the clean up pass.

.