Drilling Aluminum - full or partial retract

[SGoldthwaite]

I have about 60 0.204" holes and another 60 27/64 inch holes to drill for a fixture plate I'm making.  I'm through drilling 6061 aluminum 1" thick with mist cooling on a Tormach PCNC 1100 with HSS twist drills.  In Fusion 360 CAM if I choose peck drilling with full retract it takes a long time to finish everything.  Just a chip breaking partial retract is a lot faster.  I haven't done much CNC yet, so I'm looking for some advise.  Can I get away with partial retract for both these holes? 

For the 0.204 holes, my setting are:
4700 RPM
plunge feedrate: 25 IPM
This gives me a surface speed of 250 ft/min and chip load of about 0.0027"

For the 27/64 drill, the setting I'm planning are:
2250 RPM
plunge feedrate 18 IPM
That gives surface speed of almost 250 and chip load of 0.004"

I'd appreciate any feedback.

BTW - The 0.204 hole will be tapped 1/4-20 and the 27/64 holes will be 1/2-13.

[Steinwerks]

I run 2% of drill diameter per revolution for feed. Usually quite safe in aluminum and mild steels. Feed harder in plastics. No experience with the mister, but with flood I will chip break peck (high speed peck, whatever you want to call it) through about an inch without thinking about it if my drill is over .200". I don't see why you wouldn't get away with it though. If you're worried, try it on a piece of scrap first.

My default is 200SFM for HSS uncoated drills, so for your .204" I would run 3745 RPM @ 15.28 IPM.

Your chipload appears to be .0027/flute. Should work but nearing 3% drill diameter that I run as a maximum.

[Laurens-3DTechDraw]

N. Stein wrote:

I run 2% of drill diameter per revolution for feed. Usually quite safe in aluminum and mild steels. Feed harder in plastics. No experience with the mister, but with flood I will chip break peck (high speed peck, whatever you want to call it) through about an inch without thinking about it if my drill is over .200". I don't see why you wouldn't get away with it though. If you're worried, try it on a piece of scrap first. My default is 200SFM for HSS uncoated drills, so for your .204" I would run 3745 RPM @ 15.28 IPM. Your chipload appears to be .0027/flute. Should work but nearing 3% drill diameter that I run as a maximum.

Sounds like he has got only mist cooling and no flood. But that might be wrong.
About feed and speed totally depends on your tool. I've got HSS drills where a 10mm drill can feed 0.35mm/rev and ones that can only handle 0.16 mm/rev so not really something one can judge if it's optimal.

[fredsi]

Would agree with N. Stein that the feed(s) might be  a bit too fast for the rpm...

But to answer your question - how bad will you feel if/when you have completed 60-90 holes of so and a drill packs with chips? This is a one off (fixture plate) and not production, right?  I consider 6061 to be 'gummy' when compared with the alloys I like to cut (2024/7075, and the like). As such, I don't like taking chances with it and that's with flood coolant. So, I'd vote for full retract so the tool has the best opportunity to clear chips.

Fred

[SGoldthwaite]

Thanks for the info.  This is a one-time part, not production. I only have mist cooling.

[lenny_1962]

another trick instead of mist squirt WD40 as it goes along drilling the holes works great.

[Anonymous]

Even in aluminum, with HSS I would think that SFM is way high. I might stress on that even with Carbide haha.

[tacticalkeychains]

No matter what you are doing, Full is always better. It gets the chips out, and coolant in (mist too)

Your feeds are pretty good, always double check here - http://zero-divide.net/index.php?page=fswizard.

I run as fast as I can for 6061 Alum.  WD-40 is excellent for Aluminum, but if you are already using Kool Mist, I would up the volume of liquid for drilling.Are you running about 5psi? 

Since you have a Tormach you have probably seen some of my videos?  I don't drill much with the Tormach, usually just interpolate the hole so I can use the same endmill for making the part, this saves LOTS of time due to Tormach's slow tool change. Stick with 3 Flute ZRN Endmills (Accupro and Helical come to mind) and just push as fast as you can.

[Anonymous]

Try Guhring drill series 549 get the drill from Guhring for trial, if it does not work return for refund

SFM = 260
Feed = .010/rev

no peck do it in one shot
be sure you have good mist at the tool

[SGoldthwaite]

Kurt Schütz wrote:
Try Guhring drill series 549 get the drill from Guhring for trial, if it does not work return for refund SFM = 260 Feed = .010/rev no peck do it in one shot be sure you have good mist at the tool

I finished the job, but the parabolic drill seems interesting, I'll have to pick one up and give it a try. <br>

[SGoldthwaite]

I drilled all my holes.  It went okay, but I did have some squealing with the 0.204" holes.  I had mist coolant running, but if I also gave the drill a squirt of WD-40, it was much quieter, but I only used it on a few holes as a test.  The drill ejected the chips pretty well, they weren't sticking to the bit. The bit didn't squeal the whole time, mostly near the end. The 27/64" was quieter, a bit of squealing, but not much.  The mist coolant is Kool Mist #78 mixed 1:25

I drilled a few test holes playing around with the feed and speed. Here's the CAM I ended up with:

• 0.204": 2-flute HSS jobbers drill, 2880 RPM, 11 ipm plunge, full-retract peck, peck depth 0.10", pecking depth reduction 0.010", min peck depth 0.025"


• 27/64": 2-flute HSS jobbers drill, 1550 RPM, 10 ipm plunge, full-retract peck, peck depth 0.12", pecking depth reduction 0.015", min peck depth 0.025"

[Anonymous]

Those feeds and speeds sound much more realistic without full flood coolant! Much softer than the first post. I think with carbide, or even Cobalt, things would have been less squealy.

[SGoldthwaite]

I'm just learning this stuff.  I think I'll do some testing with some different drill bits and try various feeds and speeds. The parabolic bit looks interesting.

[Anonymous]

SGoldthwaite wrote:
I'm just learning this stuff.  I think I'll do some testing with some different drill bits and try various feeds and speeds. The parabolic bit looks interesting.

I work with a lot of 17-4 stainless, drilling 5xd or more often up to 3/4". My concept lately is that SFM calculation and drilling don't really go hand in hand, unless you are drilling a pilot hole first. Most of my bit failures are happening and the VERY tip/split point, and you reference SFM off the OD?? A .25" drill and a .75" drill are doing the same work right at the tip, so I'm now spinning my smaller drills only a slight bit faster than the big ones.

I also bought a good drill bit sharpener so I can create a high end split point myself. Seems like a lot of bits I get have terrible finish grinding, so the point of the drill has to rub itself into the material. A high end precise split point goes a long way with how happy the drill is.

[Anonymous]

SGoldthwaite wrote:

I drilled all my holes.  It went okay, but I did have some squealing with the 0.204" holes.  I had mist coolant running, but if I also gave the drill a squirt of WD-40, it was much quieter, but I only used it on a few holes as a test.  The drill ejected the chips pretty well, they weren't sticking to the bit. The bit didn't squeal the whole time, mostly near the end. The 27/64" was quieter, a bit of squealing, but not much.  The mist coolant is Kool Mist #78 mixed 1:25 I drilled a few test holes playing around with the feed and speed. Here's the CAM I ended up with: 0.204": 2-flute HSS jobbers drill, 2880 RPM, 11 ipm plunge, full-retract peck, peck depth 0.10", pecking depth reduction 0.010", min peck depth 0.025" 27/64": 2-flute HSS jobbers drill, 1550 RPM, 10 ipm plunge, full-retract peck, peck depth 0.12", pecking depth reduction 0.015", min peck depth 0.025"

Holy slow batman!  When in doubt with 6061 you should peck a lot though, so this is very safe.  If you need to run production you will just have to find the sweet spot with feeds and speeds and pecking depth.  For comparison, I run a 17/64 parabolic HSS drill from Mcmaster Carr ($15 or so) with low pressure flood coolant at 4000 rpm, 60 IPM plunge, 0.850" deep in 6061 (no pecking).  Thousands and thousands of times.

[SGoldthwaite]

hoser1 wrote:

Holy slow batman!  When in doubt with 6061 you should peck a lot though, so this is very safe.  If you need to run production you will just have to find the sweet spot with feeds and speeds and pecking depth.  For comparison, I run a 17/64 parabolic HSS drill from Mcmaster Carr ($15 or so) with low pressure flood coolant at 4000 rpm, 60 IPM plunge, 0.850" deep in 6061 (no pecking).  Thousands and thousands of times.

At first I did a few test cuts pecking without full retract and the chips were getting stuck in the flute.  I don't have flood cooling on my Tormach, only mist.  I want to try one of those parabolic bits, I'm gonna order one from McMaster and do a few tests.  I attached a picture of the fixture plate with the holes drilled.  I still need to tap them.  I'm gonna do that on the Haas TM2 (circa 2005) with rigid tapping. The reason I did all the holes on my Tormach is I want to learn about using the Tormach (I just got it).  Although, when I need to make another fixture plate I may do the whole thing on the Haas. It's has flood cooling and a tool changer.  I could set the whole thing up and just let it run.

Another little issue I had was my fixture plate takes up most of my Y-axis travel. I had enough room to get a 7/16 end mill to do the long sides of the plate, but not enough for a larger diameter end mill.  So there was some chattering. For the short sides I had plenty of room and used a 3/4" end mill - it did much better.

Here's links to some pics of the surface finish
7/16" mill: https://goo.gl/photos/cFT6qeyp3WbXb4KR7
3/4" mill: https://goo.gl/photos/4LShJRiKmQiGJ1hq5

Here's a link to a short video clip of cutting the side with the 7/16" mill: https://goo.gl/photos/vQHsBPCU9toUYhfQA
0.05" Doc, 3815 RPM, 30 IPM.  I tried both climb and conventional milling on the side cut, they both performed about the same.

I'm just getting started with CNC machining, so every time I make something, I'm learning something new:) 

[Laurens-3DTechDraw]

Tapping in a different machine then where the holes were drilled is tricky one. Make sure you really measure it out well. If the tap is just a little off the holes centre you might be breaking them like matchsticks.

[SGoldthwaite]

Laurens-3DTechDraw wrote:
Tapping in a different machine then where the holes were drilled is tricky one. Make sure you really measure it out well. If the tap is just a little off the holes centre you might be breaking them like matchsticks.

The Haas has a nice electronic probe, so I should be able to get the fixture plate positioned accurately. 

[Laurens-3DTechDraw]

SGoldthwaite wrote:
Laurens-3DTechDraw wrote: Tapping in a different machine then where the holes were drilled is tricky one. Make sure you really measure it out well. If the tap is just a little off the holes centre you might be breaking them like matchsticks. The Haas has a nice electronic probe, so I should be able to get the fixture plate positioned accurately.

I would check 1 or two holes to be sure.

[Anonymous]

🙂