Breaking End Mills

Rick Finsta · Jun 19, 2018

Alright, I had a job I took on as a subcontractor from my day job while we wait for some machine deliveries. I have a slot about 0.625" long, 0.120" wide, and 0.150" deep (all the way through the stock), so I have it running down about 0.015-0.025" below the part in a clearance slot in the soft jaw) in 1018. All I had to start with were 2-flute TiAlN carbides, 0.0625" tapered to 0.188" shank, 0.250" LOC. Running 8k RPM (everything I've got) I was running a constant engagement path at 8% stepover, 3.8IPM, full depth. It went though four pieces then broke a mill, and then I halved the chipload and the same thing happened. I'm running in an ER25 collet and best I can check (dial indicator) run out looks fine. I was running coolant to flush chips since I don't have air blast.

I've got some 4-flute on the way from Harvey and Niagara at 0.100-0.109" diameter and I don't want to break a bunch of those, too, since I'm basically doing this job for "free" to get some cash flow to the shop and help out a sister company at the same time.

Any starting point on feeds/speeds for this? I'm guessing that this slot was being made using another method by the last subcontractor. Sister company is just in dire straits to meet a deadline while they wait for a shipment from the normal sub.

Larry Dickman · Jun 19, 2018

Broken record time.

Look at Harvey's speed and feed charts. They are always a good starting point.

mhajicek · Jun 19, 2018

You may be running too slow and burnishing rather than milling. HSMAdvisor tells me .0031" (5%) stepover and 8.09 IPM for those conditions.

litlerob1 · Jun 19, 2018

Sorry, I'm not clear. Are you running full depth, .15" with a .0625 Endmill in 1018 CR?

plastikdreams · Jun 19, 2018

litlerob1 said:
Sorry, I'm not clear. Are you running full depth, .15" with a .0625 Endmill in 1018 CR?

That's what it sounds like...if so, some interpolation will go a long way.

mhajicek · Jun 19, 2018

Rick Finsta said:
I was running a constant engagement path at 8% stepover, 3.8IPM, full depth.

I assume this to be synonymous with "adaptive clearing" or "dynamic milling".

Matt@RFR · Jun 19, 2018

Rick, with HSM tool paths you want some clearance between the cutter and the work when possible. For your slot, I would stick with the 1/16" endmills. Here is a pocket we just got done with in 304 that worked perfectly. One tool roughed and finished 1,000 pockets, about 3/16" x 1/4" or so. Scale it however you like:

- .047" x .141" 3FL AlTiN
- .140" DOC
- 7% WOC
- 12,000 RPM (max) = 148 SFM
- 32.4 IPM = .0009 IPT

plastikdreams said:
That's what it sounds like...if so, some interpolation will go a long way.

Hmmm?

mhajicek · Jun 19, 2018

You might also try doing it in two depth passes of the same dynamic path. I'm doing a similar feature (.100" wide) in 17-4 H900 with a Harvey 967062-C6 (.062 x .186 3-flute flat TIALN) at 11650RPM, 7.69IPM, .0027 step, two passes of 0.093 depth.

zero_divide · Jun 19, 2018

I would use a 3mm 4fl stubby carbide endmill.

@10000 RPM 17ipm full slot at 0.045" deep

There is nothing hard about 1018.

litlerob1 · Jun 19, 2018

zero_divide said:
I would use a 3mm 4fl stubby carbide endmill.

@10000 RPM 17ipm full slot at 0.045" deep

There is nothing hard about 1018.

No, nothing "hard" but there is something gooey about it.

Which raises a question for the experts on HSM paths. The OP only has 8000 RPM, my question is; do you change anything for lack of RPM, or do you just scale the feeds down to make the right chipoad? High RPM gives you some chip clearing all by itself.

R

zero_divide · Jun 19, 2018

litlerob1 said:
No, nothing "hard" but there is something gooey about it.

Which raises a question for the experts on HSM paths. The OP only has 8000 RPM, my question is; do you change anything for lack of RPM, or do you just scale the feeds down to make the right chipoad? High RPM gives you some chip clearing all by itself.

R

Well at 8000RPM the feed would be 13.0ipm
The SFM is still low enough to use coolant or strong airblast.

Of course you could peel it off using any HSM style toolpath, but with 0.15" slot and 0.05" endmill it sucks.

Shawnrs · Jun 20, 2018

Spiral cut the slot with one of those larger endmills or drill a hole in the corner and plunge the center of the slot out and then finish mill the slot to size with the same endmill.

SIM · Jun 20, 2018

If you have 1/4" LOC on your e/m I'd sink it in deeper for a final cut.

If you do not have a good HSM program to engage nicely I'd be taking in multiple cuts.

That said I'd try using a larger EM, mm or 3/32. 1/16 will work but its a lot of lil cuts.

Booze Daily · Jun 20, 2018

I would just stab it out with .010-.020 stepover and then profile it.

Rick Finsta · Jun 20, 2018

Thanks for all the feedback. I was thinking about the burnishing possibility. I've got more tools coming so I'll give this stuff a try and stop chickening out on what HSMAdvisor tells me!

Milland · Jun 20, 2018

It sounds like you sunk the part into soft jaws for location and clamping. If the jaws are set up so that it forms a closed bottom, then you're trapping chips that have to be flushed from the top.

Unless there's a really good reason, clearance or recut the pocket in the jaws such that you have a "free gap" that allows all chips to be flushed through and out of the vise. That's much more reliable from a chip clearing process than trying to flush from a closed bottom pocket.

I'm also confused about the first tool you used, a tapered endmill? That was just a desperation issue, as no other right-sized EM was available? Regardless, I think I'd want a lubricious coating on a 3-flute 3mm EM, then a light skim pass of a couple thou afterwards. Yes, unless you go a touch oversize there may be ridges left inside the slot, but surely cutting to .002" over on the slot width won't hurt, and that should do it if your spindle's not sloppy.

Max RPM, full depth, sink the endmill or use a stub, aim the coolant nozzles down and ensure good flow, ~.0008" tooth, Bob's your Aunt after the sex change operation.

Edit: Drill a clearance hole for endmill entry, a good .120 stub should do it.

litlerob1 · Jun 20, 2018

Milland said:
I'm also confused about the first tool you used, a tapered endmill? That was just a desperation issue, as no other right-sized EM was available.

I think he meant 1 diameter Endmill, that "tapered" to a bigger shank diameter.

Rick Finsta · Jun 20, 2018

Yup, exactly, sorry that wasn't clear. The first end mills were 0.0625" to the end of the flutes, and then tapered to the 0.188" shaft. I also realized I didn't specify that the slot is open on one end so I am flushing chips from the closed end out with the coolant stream.

One thing I'm seeing is a lot of recommendations for 3-flute mills. I will admit I have been guilty to now of using 3-flute for aluminum and 4-5 flute for steel, and I didn't really have anything on hand for this job, hence the 2-flute at first. I'll look into the 3-flute options as well.

Rick Finsta · Jun 24, 2018

Alright, Niagara d=0.109", 0.218" LOC, 0.125" shank 4-flute TiAlN coated. 8000RPM, 28.8IPM, 0.0009 IPT, 0.0076" (7%) stepover. The actual feed rate I'm seeing on the machine is 12-14IPM. So far I've got 100 pieces done and everything still looks great.

Thanks again for the help.

Funny looking back at the print I've got a +/- 0.030" on that slot so I could have just done it with an 1/8".

DMF_TomB · Jun 25, 2018

Rick Finsta said:
Alright, Niagara d=0.109", 0.218" LOC, 0.125" shank 4-flute TiAlN coated. 8000RPM, 28.8IPM, 0.0009 IPT, 0.0076" (7%) stepover. The actual feed rate I'm seeing on the machine is 12-14IPM. So far I've got 100 pieces done and everything still looks great.

Thanks again for the help.

Funny looking back at the print I've got a +/- 0.030" on that slot so I could have just done it with an 1/8".

.
got to be 1000's of slots done every hour by simple straight line motion. obviously the tool length to diameter ratio, the tool diameter to max milling cutting depth and feeds and speeds and coolant getting chips out of the way has to be figured out.
.
if nothing else usually using the biggest most rigid tool usually is faster. length to diameter tool ratio is very important and often unappreciated.
.
me i wouldnt care about a 200% feed increase if i was breaking tools and scrapping parts. i have often seen going slower with higher reliability was the faster in the long run. sometimes even a 2% sudden tool failure rate can be found to be slowing things down remaking parts and increasing tooling costs far more than the expected time savings trying to run tooling faster

Breaking End Mills

Stainless

Titanium

Diamond

Diamond

Diamond

Diamond

Titanium

Diamond

Stainless

Diamond

Stainless

Stainless

Titanium

Titanium

Stainless

Diamond

Diamond

Stainless

Stainless

Diamond

Similar threads