Any reason not to run smaller drills at high RPM's?

Hi guys,

I have 16K RPM spindle. I have a high-quantity production job which has .125", .140", and .238" holes. I've noticed in some folks's programs that they don't run smaller drills at top speed. Just wondering if that's SOP, or just being cautious, or no reason at all? I have 10k parts to run, so am looking to squeeze every second out of the runtime. Right now I'm using Guhring 659's for the smaller holes, and OSG EX-Gold for the bigger hole.

Thanks, and regards.

Mike

There's no reason not to run them at the recommended surface speed...Often with the usual 12k (or 16k for you now) we end up running at well below what they can be run at.

Finegrain said:

Hi guys,

I have 16K RPM spindle. I have a high-quantity production job which has .125", .140", and .238" holes. I've noticed in some folks's programs that they don't run smaller drills at top speed. Just wondering if that's SOP, or just being cautious, or no reason at all? I have 10k parts to run, so am looking to squeeze every second out of the runtime. Right now I'm using Guhring 659's for the smaller holes, and OSG EX-Gold for the bigger hole.

Thanks, and regards.

Mike

Click to expand...

.
from experience small drills are run at lower sfpm and feed as they have a higher chance of sudden tool failure even if just 2% sudden failure at the recommend max sfpm and feed.
.
i count tool breakage, part damage and rework or remaking scrapped parts. when the average time is included of scrapped parts being remade or reworked plus labor to replace tools it is often vastly massively faster to go slower than recommended max sfpm and feed.
.
i have seen where the sudden tool failure was adding 40 minutes to part average of hundreds of parts on a carbide drill that was only being used for 5 minutes on each part. it was easily shown if drill took 7 minutes instead of 5 minutes it was much faster as it eliminated the 40 minutes used to rework replace damaged parts from sudden tool failures

Sorry, forgot to state material -- 6061, so 16K would only be ~600 SFM with the smaller drills.

Regards.

Mike

Finegrain said:

Sorry, forgot to state material -- 6061, so 16K would only be ~600 SFM with the smaller drills.

Regards.

Mike

Click to expand...

.
.
i have seen plenty of tools where coolant not reaching tip and aluminum stuck to flutes causing sudden tool failure.
.
i track results of hundreds if not thousands of parts. most times even a 2% scrapping part or reworking part in addition to replacing broken tool adds up at the end of the year.
.
i have seen carbide drills breaking and causing so much scrap and rework costs they did not save anything over using hss drills if anything they cost more to use in time and money over hss drills. sometimes a carbide drill instead of going 10x faster if it only goes 2x faster is the much better answer to lowering total cost to produce parts
.
if you go 100mph in your car and roll it over doing a 40mph max curve at high speed you are not saving any time on the trip, if anything it will take you longer to get there

I don't have a lot of experience really pushing the small drills to their limit, but like DMF_TomB says, the one thing that you cannot improve on is the cooling. You can ramp up the rpm and the feed, but you cannot force the coolant to cool it faster. You might even prevent coolant from getting anywhere near the cutting zone, so it is basically dry machining under water. So if you've got a good dry machining techique (proper pecking), then push that.

I have been running 1/4" 3" long parabolic drills in alu at 10k no bproblem.
With a 1/8 you can max out without any problem.
Just remember to peck accordingly.

I run 3.0 mm / 3.5 mm carbide drills at 16k (with through coolant) in aluminum without issue, I would run anything up to 1/4" that way IMHO. Thing you have to watch is stick-out. Want it short. The longer it is the more likely whip will be induced and it'll break not even touching the part. HSS will be more prone to this than carbide.

I'm running the drills at 10K and 12K. Realized it saves like 1/2 a second to go to 16K.

Regards.

Mike

Aluminums not so bad, try it in some of the softer more melt-able plastics and you soon find speed can have to go down as diameter does bellow a certain size!

Finegrain said:

Hi guys,

I have 16K RPM spindle. I have a high-quantity production job which has .125", .140", and .238" holes. I've noticed in some folks's programs that they don't run smaller drills at top speed. Just wondering if that's SOP, or just being cautious, or no reason at all? I have 10k parts to run, so am looking to squeeze every second out of the runtime. Right now I'm using Guhring 659's for the smaller holes, and OSG EX-Gold for the bigger hole.

Thanks, and regards.

Mike

Click to expand...

The Guhring 5514 is great in 6061 Aluminum. It's funny that Guhring doesn't list it in their drills for Aluminum recommendations but if you look at the feeds and speeds page for the 5514 it recommends 805 SFM, .016"/Rev for .25" Dia.. I think feed per Rev is somewhere around .010" for .125" Dia.. I know a shop that drills about a million holes a year in 6061, .200" Dia., .600" deep, no pecking, no coolant thru, 14000 rpm, 175 IPM. The holes are really nice and the drill makes tiny chips you can hear hitting the sheetmetal.

I have a couple of rules whe ln it comes to drills.. I don't run high production to often... So take my opinion with a grain of pepper...

Rule 1: it should say guhring on the side of the drill... Ive literally drilled practically every type of steel (hard, annealed, and superalloy) and non ferrous material using a guhring drill and they havent let me down yet. I rarely even look at other companies drills anymore.

Rule 2: run it like they tell you to. If you are running 10k parts, then start with a couple extra and figure out what the drill will do. ( do you have a delivery varience?) if you run 4000 holes and the first drill breaks, then you run 4034 and the second drill breaks... Then it's pretty safe to say that drill is good for 3900 holes. Now you know for the next order...log this data for future use. (actually the more accurate way is to calculate how many inches it drilled)

Guhring did a test run of 10, 000 holes with a single drill in cast iron. And saved like 500 hours of machine time.. The drill companies know what hey are talking about. Listen to them. (correction - guhring did that test with a reamer. Still impressive )

While i agree with most of what tom b says.. I think it depends more on the job. If there is room to scrap a part then do it and run as fast as you can. 30 seconds per part on 10k parts is somewhere between $6,250 and $22,000 of billable machine time (depending on the machine.) That's money you can be making doing something else, and in my mind is worth breaking a drill or two, and scrapping a part or two, to acheive. Again.. Depends on the job.

That's my nickels worth of opinion.. For what it's worth

Tonytn36 said:

I run 3.0 mm / 3.5 mm carbide drills at 16k (with through coolant) in aluminum without issue, I would run anything up to 1/4" that way IMHO. Thing you have to watch is stick-out. Want it short. The longer it is the more likely whip will be induced and it'll break not even touching the part. HSS will be more prone to this than carbide.

Click to expand...

Run these in shrink fit tools and your runout is pretty much nil. We have moved all of our production drilling to Guhring carbide drills with TSC, somewhere between 200-1,000 psi depending on machine and application. The drill shanks are always a standard available shrink holder size so that part becomes easy, and as short as possible on both holder and tool. We are not running excessively high sfm as drilling is not usually a long portion of the cycle time, and it would be a bad gig if we loose a $1,000 pallet load because we wanted to shave a few seconds on the drill cycles. The other thing, most of our pallet cycles are 3-6 hours, so unless we can save enough time to get another pallet load in for the day, it really doesn't make too much of a difference.

Steve

I'm currently testing some Walter TSC (400 psi TSC) Carbide drills aluminum. I'm very impressed by these drills. 130,000+ inches each so far, testing on 3 separate machines.

BTW: These weren't "test tools" supplied by the tool vendor, we just decided to try them and ordered them off the shelf from normal supply chain. Gotta watch "test tools" as we've had many instances over the years where vendor supplied test tools performed extremely well during testing only to go to crap once the switch was made and you started getting "production tools".

Another vote for Walter Titex in Carbide.

If you take the drill diameter and multiply by .03 or(3% of the diameter,) and use it as your CHIP LOAD per revolution, you can then feed the drill at any revolution. However, you will need the used surface speed of the material being used.

The old men, (I being one of them) say the first peck is good up to 3 diameters, the rest .5 diameter for pecking the rest.

Drill Size .020).060).100).250) .500)
Chip load .0006.0018 .003 .0075 .015 PER/RPM (2500)

Feed Rate 1.5" 4.5" 7.5" 18.75" 37.5"

I think it's correct, the formula is.

Regards,

Stanley Dornfeld