[cygnus x-1]

I just killed an end mill and I'm not sure why. Looking for some feedback. Here are the specifics:

Haas TM-1
1/4" carbide 4 flute, standard SGS endmill, ~3/4" flute length
Speed: 4300RPM
Feed: 17IPM
Doing a helical plunge (clockwise) into 1020 steel
Plunge angle is 3deg, helix radius was 0.125"

It didn't sound very good going in and within 10 seconds the end was completely busted up. The above parameters seem pretty conservative (too much so maybe?) so I'm a bit confused as to why the tool died so quickly. Any ideas?


C|

[txcncman]

Your IPM sounds a little aggressive to me. I know technically you are not plunging, but I usually error on the side of caution and put this type of move at 2-5 IPM for almost any tool size. 3 degrees ramp is probably ok. Anything less than 1.5 D on the helix will not really give the chips any place to go. What was the total depth you were reaching for?

[cygnus x-1]

Pocket depth was 0.2" and there was hardly any time for chip buildup. I was watching it the whole time and it didn't even get to the bottom of the pocket before it crunched.

Should I maybe have used a 2 flute?

C|

[txcncman]

No. 4 flute is the way to go for steel. I just think you were too aggressive on your feed rate.

[Shane1234]

i like to go slow on full axial cuts, whether thats slotting or helical ramping. once you get back to side cutting, bump that feed back up.....

[Geof]

Your feed rate was equivalent to about 0.001" per tooth which is high for that diameter cutter. Especially since most machines run the centerline of the cutter at the programmed feed rate which means the outer edge is running at a higher effective feed rate.

[cadcam]

what size was the slot I think the issue is with the 3deg plunge as that can be aggressive in a small contained area in steel. So clockwise being a conventional cut why, instead of a climb less stress on the tool. please more info.

[dertsap]

I think the issue is with the 3deg plunge .

that was the first thing that came to my mind , I'd knock it in half

[DMF_TomB]

i think 2 flutes work better on plunging, yes they have 4 flutes that cut to center but still think there is more room for chips with 2 flutes on plunging.
.
chip clogging can cause unforeseen forces especially when center of mill is covering your line of sight and you cannot really see whats going on
.
a carbide 2 flute end mill should be able to take a 0.002" chip load. i am guessing you can run at the same feed with the 2 flute end mill and it should not break.
.
also i would use cutting fluid. you did not mention it. it helps chips to flow out of flutes too. i have seen carbide end mills overheat and melt where a little cutting oil which usually boils and turns to mist by the time end mill is close helps. even hot oil mist seems to works for me. i do not apply cold cutting oil to red hot carbide. i apply to metal so metal is covered in oil. never apply cold cutting oil to hot carbide unless it is high volume flood that was on cutter from the beginning.

[dertsap]

i have seen carbide end mills overheat and melt where a little cutting oil which usually boils and turns to mist by the time end mill is close helps. even hot oil mist seems to works for me. i do not apply cold cutting oil to red hot carbide

i don't think that carbides are meant to be red hot while cutting , and enough heat to turn coolant to steam probably isn't too good either

[txcncman]

@TomB - You are sooo right. 2 flutes work better for plunging. They call them drills. In a perfect world, a real machinist with plenty of time and tools and tool holders on his hands would drill a pilot hole before plunging an flat end mill into a piece of material, steel or otherwise. But, humans tend to be both lazy and greedy creatures. Because of this, we try to take short cuts. And the short cut here is to not pre-drill a pilot hole for the end mill to slip into.

[extanker59]

@TomB - You are sooo right. 2 flutes work better for plunging. They call them drills. In a perfect world, a real machinist with plenty of time and tools and tool holders on his hands would drill a pilot hole before plunging an flat end mill into a piece of material, steel or otherwise. But, humans tend to be both lazy and greedy creatures. Because of this, we try to take short cuts. And the short cut here is to not pre-drill a pilot hole for the end mill to slip into.

Was there really any need to belittle others? Just somebody looking for help. Arrogance isn't helpfull and if you didn't intend it to be helpfull, why spend any time writing here?

[txcncman]

@tanker - I was not belittling anyone. I was glad TomB introduced the opportunity to discuss the "best" way to insert an end mill into a cut and why most people will choose not to use the "best" way. I see my comments as a way of interjecting some humor into a serious discussion. I am sorry if your sense of humor does not match my own.

How do your comments help anyone? If you are sure I am being arrogant and belittling others, maybe a private message would do more to get me to change. A public message just invites a public response and more of what already seems to offend you. Actually, that is a rhetorical question. I know why people use this tactic while trying to communicate in such forums. The idea is that if you can get other people to dislike me more, then it will seem that they like you better. I am not here to win a popularity contest. I am here to educate and give out the best information possible based on my knowledge and experience to make my chosen industry a better place. I am in this industry because it suits my mental abilities well and gives me an opportunity to support myself and my family in a comfortable lifestyle. If I can even educate 1 person per year into better machining practices, that is a plus in my book. And if I can turn up the pressure on someone that is not trying to reach higher standards so they they get out of the industry, that is a plus also.

Finally, I am just me. I doubt I will ever change to please you. That is not my goal, as stated above. If you feel my suggestions are in error, you are welcome to rebutt them or make counter suggestions. I have been "corrected" in many venues, this one and others. Usually those "corrections" do not address any facts as I know them in my experiences and reality. Usually those "corrections" address a personality and communication conflict. I have also been lauded in those same venues by others. My supporters always seem to outnumber the detractors though. So, again, I see no reason to change my communication style to suit a few when it seems the many get benefit from it.

In the future, I will make this concession: I will attempt to not make public comment on any thread that you have already posted to. If I feel a need to communicate some information on such a thread, I will take the time and effort to contact the other parties with a private message. I hope that will satisfy your sensibilities.

Good day.

[osphoto]

Thanks for the reminder of the pilot hole!

I don't use four flutes (any more) but I recall them being a major pain for my novice experience. (Still novice experience.)

I appreciate the question that started this forum and I appreciate the humor. The humor will help remind me why I may have destroyed a bit and my work.

To be Human is to Error. And I've not yet graduated from "school of hard knocks".

To Txcncman, please keep posting! Some folks just can't handle the truth, no matter how much sugar coating you do.

[cygnus x-1]

And we're back with an update. Tried again with a plunge angle of 1 deg, changed direction to CCW, and reduced feed rate of 12IPM. That did the trick! So looks like it was just overloaded. Which is a surprise because I'm usually too conservative.


Regarding myself being lazy: I would comment on that but I just can't be bothered.


Why did I helix in CW instead of CCW? Umm... well... yeah... I guess because that was the default setting? And I figured it would work? :wee:


I usually try to drill pilot holes to avoid plunging but the pocket is only 0.2" deep and I figured it wouldn't be worth the bother of loading up another tool.

And in steel I always try to cut dry (with carbide) and use full axial depth cuts with low stepover to use more of the side flutes. Most of the time my parts are small and the operations short so I can stand by with the air gun to blow away chips if they build up. For longer ops I'll use a continuous air blast rigged up from an old air brush compressor. Some day I should probably wire up an aux relay from the control so I can program the air blast instead of doing in manually. But I don't cut much steel so it hasn't been a pressing concern.


Anyway, mission accomplished, thanks to you guys!


C|

[DMF_TomB]

i use 2 flute carbide end mills always with oil on Stainless and low carbon steel.
.
i find 4 flute end mill work better in larger diameters
.
with 2 flute end mills i can go straight down in Z or travel outline of part which is essentially a long slot. in stainless, carbide can go red then yellow and melt when cutting dry very easily. with a little oil my end mills easily last 10x longer
.
i cut out parts from a large sheet using plunging and slot milling easily and reliably. only problem i ever has is when part is 99% cut i usually have to hold it down with a wood stick to keep flopping around or use double sided tape sticking part to thin plywood so cut out parts do not flop around

[ger21]

Was there really any need to belittle others? Just somebody looking for help. Arrogance isn't helpfull and if you didn't intend it to be helpfull, why spend any time writing here?

I didn't see any belittling or arrogance in his post at all. Another case of someone reading something into a post tha wasn't there at all.

[DMF_TomB]

I just killed an end mill and I'm not sure why. Looking for some feedback. Here are the specifics:
Haas TM-1
1/4" carbide 4 flute, standard SGS endmill, ~3/4" flute length
Speed: 4300RPM
Feed: 17IPM
Doing a helical plunge (clockwise) into 1020 steel
Plunge angle is 3deg, helix radius was 0.125"
It didn't sound very good going in and within 10 seconds the end was completely busted up. The above parameters seem pretty conservative (too much so maybe?) so I'm a bit confused as to why the tool died so quickly. Any ideas?
C|

you solved your problem. for next time you mention 3/4" flute length.
.
thats not the same as amount sticking out of collet
at stickout of 1" or more feed and depth of cut and plunge angle need reducing.
.
often settings need a reduction in 1/2 from having an end mill stick out an extra 1/4"
.
i find increasing my metal removal rate by using shorter stub length end mills is easy to do. often a regular or long length end mill is used but most do not realize how much this extra length reduces their metal removal rate

[cygnus x-1]

you solved your problem. for next time you mention 3/4" flute length.
.
thats not the same as amount sticking out of collet
at stickout of 1" or more feed and depth of cut and plunge angle need reducing.

Oh, I know all about tool stickout. I use the fantastic feed/speed calculator Gwizard to determine machining parameters. It tells you how much tool deflection to expect based on tool stickout and a bunch of other parameters. It usually comes up with pretty good values for feed/speed/DOC/stepover, but I haven't figured out how to use it for plunging angles yet.

Anyway I always put cutting bits into collets right up to the flutes, unless I need more reach for depth.


C|