• We want to encourage those of you who ENJOY our site and find it USEFUL to DONATE and UPGRADE your membership from active member to donating or premium membership. If you want to know the differences in membership benefits, please visit THIS PAGE:

    https://www.hobby-machinist.com/premium/

    Donating memberships start at just $10 per year. These memberships are in fact donations that help pay our costs, and keep our site running!
    Thank you for your donation, God Bless You
  • June Project of the Month (Click "x" at right to dismiss)
[4]

Getting ready to drill lots of holes - speeds/feeds check

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#1
I'm getting ready to drill approx 60 or so 1/4-20 tap holes in a 0.775" thick 6061 AL fixture plate. My sharpest 13/64 drill bit I have is from this set: https://www.amazon.com/gp/product/B001EYU5N8

I don't have a VFD so I really don't like changing speeds, so I almost always leave my belt config at 1800 RPM (good for AL or plastics which is all I machine). Using a few of the free speeds and feeds calculators I'm arriving at 5-7IPM. However, I also saw one calculator suggest that if the depth of the cut will be more than 3 times the diameter (which is true in this case) to reduce the speeds&feeds by 50%.

I don't mind how long it takes to drill, my goal is to not burn up the bit and break it in one of the holes. I have one of those cheap mister/coolers but I generally only use it for air, but I can use WD40 too.

Any thoughts, advice?
PS. I plan to do the tapping by hand since I don't have a spindle reverse or a tapping head.
 

Doubleeboy

Active User
Active Member
Joined
Dec 3, 2014
Messages
742
Likes
409
#2
probably want to countersink those holes after you drill them. Slow is better than too fast when drilling holes IMO. Knock the speed down and play it safe is what I would do. Kerosene, TapMagic or WD40 are your friend for aluminum. Number 7 drill is the preferred drill for 75% threads and in aluminum I go with that, for steel I go 60% threads usually. That said if 13/64 is all you have go with that.
 

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#3
Thanks, I'll dig through my drill stock to find a #7 drill but I doubt it'll be as sharp as the new set. I'm good with going slow as long as I don't go too slow for the RPM and burn up the drill bit from excessive friction.
 

cs900

maker of chips
H-M Supporter-Premium Member
Joined
Mar 21, 2016
Messages
217
Likes
215
#4
7IPM will be fine at 1800RPM. May even be on the slow side.

HSMadvisor is saying 13.5IPM and peck drill them at around .54" per peck.
 

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#5
Thanks cs900! I'll start at 7 to 9 and see how it goes...I think I generated the gcode for .4" chip breaking drilling so two pecks per hole. . Oh does HSM assume HSS drill bits because mine aren't HSS, they're cheaper metal with fancy coating.
 

Boswell

Hobby Machinist since 2010
H-M Supporter - Sustaining Member
Joined
Feb 27, 2014
Messages
575
Likes
239
#6
btw, GWizard for .2031 HSS at 1800 rpm recommends from 2 to 8.5 depending on the Conservative to Aggressive slider with no Peck. for Cobalt it is 1.8 to 7.7 ipm with a .2 peck.
 

cs900

maker of chips
H-M Supporter-Premium Member
Joined
Mar 21, 2016
Messages
217
Likes
215
#8
Thanks cs900! I'll start at 7 to 9 and see how it goes...I think I generated the gcode for .4" chip breaking drilling so two pecks per hole. . Oh does HSM assume HSS drill bits because mine aren't HSS, they're cheaper metal with fancy coating.
Sorry that was for carbide!!

1800 RPM @ 11IPM with a peck of .54" for coated HSS.
 

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#9
Thanks again guys! I got it done, the 7ipm @1800 rpm worked perfectly! After 60 holes the drill bit was luke warm and still sharp (I really like this set of drill bits btw). I mostly just used air for coolant and a random spritz of wd40 here and there. I'll post the details in my RF30 build thread but here's a quick pic:

 

Boswell

Hobby Machinist since 2010
H-M Supporter - Sustaining Member
Joined
Feb 27, 2014
Messages
575
Likes
239
#10
Looks Great! Did you use any PECK and if so, how deep for each peck?
 

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#11
Here're my settings from Fusion 360 for the "Chip breaking - partial retract" operation.

drilling.jpg
 

spumco

Active Member
Active Member
Joined
Jan 15, 2016
Messages
211
Likes
157
#12
FYI - Amazon has a pretty good deal on YG-1 parabolic stub length drills. I'm a big fan of parabolic flutes in aluminum as I can plow down with no pecks fairly deep. The flutes clear chips like mad, and you can up the feed rate. I'm running flood, but a squirt of kerosene or WD40 also works.

A quality, straight stub length drill means no spot-drill needed. One less operation & tool change.

If you find yourself drilling lots of 1/4-20 holes, especially in aluminum, you might consider switching to form taps. No chips, no backing it out every turn or two. Nicer threads. Just buy a 15/64 or "C" drill and have at it.

I've also switched from buying/using drill indexes to individual drills. There are about 5-10 drill sizes I use constantly and I've found that buying a few nice drills in just those sizes means they cut better and I'm not up the creek if I wreck one. I sitll have an index for those odd-ball sizes, but mostly use the 'good'' drills in the most-frequently needed sizes.

Just a suggestion, but if you buy 5-packs of individual drills they can get pretty inexpensive. As I mentioned, I'm big fan of the YG-1 stuff. They aren't top of the line, but they're way, way cheaper than OSG, Guhring, or Nachi and they are light-years ahead of 'cheap' drills. Widia is another lower-cost but quite good quality brand.
 

Boswell

Hobby Machinist since 2010
H-M Supporter - Sustaining Member
Joined
Feb 27, 2014
Messages
575
Likes
239
#13
I also switch to sub length and also only buy the sizes I need. By that I mean that I keep at least one of all standard sizes but have 4 or 5 of the sizes that I use most often. I resharpen the larger bits and just replace the smaller ones when needed.
 

stioc

Active Member
Active Member
Joined
Feb 22, 2017
Messages
172
Likes
356
#14
FYI - Amazon has a pretty good deal on YG-1 parabolic stub length drills. I'm a big fan of parabolic flutes in aluminum as I can plow down with no pecks fairly deep. The flutes clear chips like mad, and you can up the feed rate. I'm running flood, but a squirt of kerosene or WD40 also works.

A quality, straight stub length drill means no spot-drill needed. One less operation & tool change.

If you find yourself drilling lots of 1/4-20 holes, especially in aluminum, you might consider switching to form taps. No chips, no backing it out every turn or two. Nicer threads. Just buy a 15/64 or "C" drill and have at it.

I've also switched from buying/using drill indexes to individual drills. There are about 5-10 drill sizes I use constantly and I've found that buying a few nice drills in just those sizes means they cut better and I'm not up the creek if I wreck one. I sitll have an index for those odd-ball sizes, but mostly use the 'good'' drills in the most-frequently needed sizes.

Just a suggestion, but if you buy 5-packs of individual drills they can get pretty inexpensive. As I mentioned, I'm big fan of the YG-1 stuff. They aren't top of the line, but they're way, way cheaper than OSG, Guhring, or Nachi and they are light-years ahead of 'cheap' drills. Widia is another lower-cost but quite good quality brand.
Wow, thanks for the tip! I had no idea there was such a thing as a parabolic drill, sounds fancy and sounds like it works well too. So parabolic drills clear chips better hence no need for pecking?

Is this the one you're talking about? https://www.amazon.com/YG-1-Machine-Straight-Parabolic-Diameter/dp/B014J2E76W/

BTW the Dewalt drill I used is also a 130 (or 135?) deg drill so when I drilled from the other side after flipping the piece over I didn't spot drill (I actually forgot lol) but supposedly the 130/135 deg drills don't walk like the 118 deg ones do - worked for me!
 

spumco

Active Member
Active Member
Joined
Jan 15, 2016
Messages
211
Likes
157
#15
Yes, that's the bunny. Pokes holes like mad. I just drilled about 4" deep in some brass with a 31/64" YG-1 parabolic in one shot on my manual lathe. No pre-drill - just a spot to get it started concentric. I was ready to pull it out to clear things but the chips kept flowing out instead of packing in the flutes.

[By the way, that 15/64 is for a 1/4-28 form tap, not 1/4-20. Be sure to check the tap mfgr's recommended pre-tap hole size and don't take my word for it]

As far as speeds go - if you buy name-brand (not Dewalt!) cutting tools the manufacturer usually has feeds & speed recommendations, as well as tech data about pecking depths. In the case of the 15/64" YG-1 drill, they recommend 3200RPM and .003IPR in aluminum. That works out to 9.6IPM feed.

And because of the parabolic flute, you should be able to do that .750 deep hole in one shot - no pecks. I'd have the squirt gun at the ready, however, and keep it lubed and blow the chips off when it retracts.

Using your settings, Fusion reports 10:45 to drill all the holes (not including spotting). Using the YG-1 settings, it's 7:23.

Depends on how fast you can change belts/gears to the higher ratio, I guess.

Finally, the tip angle of 118 vs 130 isn't what lets you get away without spotting the hole. It's the short length drill and a split point that does it. I'm pretty sure that the 130 tips are designed for harder material. I happen to favor them for everything (except plastic) since my drills are used in all materials.
 
[6]
[5] [7]
Top