Large insert drill recommendation for 6061

Looking for at least a 2.5" inserted drill with a 1.5" shank for a 40 taper machine. A 2x drill will work the only down side is I don't have TSC. Most of the time it will be used to 1.5" deep but do have some parts that will require 3" deep. Drill will be used in a production environment so I don't mind spending extra money for a high quality tool.

Okuma M560 so HP shouldn't be an issue.

What do you recommend?

Captdave said:

Looking for at least a 2.5" inserted drill with a 1.5" shank for a 40 taper machine. A 2x drill will work the only down side is I don't have TSC. Most of the time it will be used to 1.5" deep but do have some parts that will require 3" deep. Drill will be used in a production environment so I don't mind spending extra money for a high quality tool.

Okuma M560 so HP shouldn't be an issue.

What do you recommend?

Click to expand...

You need to consider tool weight. I run a 1.75" inserted drill and it is about the max weight for my tool changer.

We (and by "We" I mean Seco...) have our PerfoMax SD542 series drills that are available with 1.5" shank, and we could supply the correct inserts to break a chip, but it's still no small task - even in aluminum...

According to the recommended cutting data, for high-Si aluminum, that drill should be around 500sfm, which for 2.5" diameter, is 800 rpm. For low-Si aluminum, they recommend 1000sfm, which puts you at 1,600rpm. The recommended feed is nearly .0095"/rev, which equates to 7.6 in/min on the low end, and 15.2 in/min on the high end... Even in aluminum, my guess is you're going to be taxing the spindle at that low of RPM - granted, you could probably run faster to get closer into the torque curve, but then...

Consider that you're on a CAT40 machine - big-plus at best. The SD542 drill I mentioned above is basically a foot-long, so you're looking at a 13.5" gage-line tool minimum including the weldon/side-lock toolholder.

And then the fact that your machine doesn't have thru-spindle coolant... Not as big of a deal on the cooling side, but definitely desired for the chip-clearing. Perhaps if you slowed the feed enough, you could go for the long coil-like chips, in hopes that centrifugal force would "fling" the chips from the hole, instead of them breaking & packing in the hole - maybe?

But then I think about that 13-14" long tool in a CAT-40 - not to mention the weight like Sei2003 mentinoed - can you do a "heavy-tool" tool-change on that machine - so that you can slow the tool-arm down for big heavy tools?

---------------------

As a tooling sales guy, if you were my customer, I'd be strongly arguing against going this route, given the application you described... Personally, I'd be looking at a smaller drill, and interpolating the remaining stock to size... I'd suggest looking at a 40mm C5-Capto shank drill, on a short Capto-toolholder - giving you an 8.5" gage-length tool, that could drill as fast as 2,600 rpm & 28"/min or faster...

I'd then consider opening the holes with a high-helical indexable endmill - like our turbo mill, with polished inserts, and do a really agressive ramp-in helical interpolation to bring the holes to size...

---------------

This isn't really a ploy to sell you Seco stuff, or even sell you more tools. But you may have a tough time 1- finding a drill in that diameter, that's short enough to still be rigid, and 2- you can still push with your spindle. (Maybe more of a rigidity challenge than a horsepower challenge...) But, if you called me into your shop, this is probably what I'd recommend, despite not being exactly what you want to hear...

(Edit: Again - this is not an "ad" to sell my tools... I would not recommend using "our" big drill in your application, and if you chose to go the alternative route, "we" and others all have a good tool for the job...)

Sei2003 said:

You need to consider tool weight. I run a 1.75" inserted drill and it is about the max weight for my tool changer.

Click to expand...

??What machine? Did you get it at harbor freight? Note Dave is on an Okuma, weight isn't a problem.

Dave, I don't have a link but Sandvick builds the multi insert drills like 2 on each flute, but they have a lot of clearance for chip evac. And Iscars drills always kick ass run them dry often, not sure about size though.

Robert

Pretty sure you'd be much better off Interpolating those holes. A 1" endmill with flood coolant can do some serious aluminum removal even on a good 40 taper. I believe that size drill is jess a lil too big for ur mill esp since no TSC.

An indexed 1.25" Ripper(is that how those alum-specific ones are called?) mill will do a quick job of that hole. Helix-in. Rapid out. No need to wet you pants every time it rapids down to your part.

I vote for flooded helical plunging with about an inch or 1-1/4 endmill. An insert drill shines when you can force coolant thru it but without that it can become a blob.

Seeing the Seco ad reminds me of our early days using insert drills in a CNC turning center and somebody had sold me a Seco (then Carboloy). Got very frustrated trying to dope out what insert grade to use in 6061 and finally phoned their tech line. The punk at the other end said, and I am not making this up, "6061? What kind of steel is that?"

Oldwrench said:

The punk at the other end said, and I am not making this up, "6061? What kind of steel is that?"

Click to expand...

The soft kind.

I highly recommend Sumitomo WDX drills. They have 2D up to 68mm dia.
I'm using their "DL1500" DLC coated inserts, and they chip break beautifully in 6061.
Tried a few other brands before, but these perform significantly better.

I run a 32mm at 2800rpm, about 28ipm feed but have run it over 35ipm no problem.

http://www.sumicarbide.com/pdf/drill/Drills_WDX.pdf

IF you decide to not go with a drill, I would recommend a 1-1/2" cutter from Mitsubishi and do ramp cuts. Nothing that I've tried comes close to their aluminum specific inserted cutters.
You could rough out that hole or holes pretty darn fast on that Genos. Obviously not as fast as drilling but I don't know your quantities.

Mtndew said:

Obviously not as fast as drilling but I don't know your quantities.

Click to expand...

Thank you Dew, OP didn't ask about process recommendations, he asked about a drill, because a drill IS the single most effective tool for material removal.

R

Revolution drill by allied will do that all year long. And you think you have horsepower until you start using these in the range they are to be used in.

Captdave said:

Okuma M560 so HP shouldn't be an issue.

Click to expand...

2.5" will be an issue. No way you could run it at mfg'r feeds n speeds.

Buy a drill the you can "plunge mill". Basically punch in a starter hole and then start plowin out material by steppin over and drilling until you have your rough 2.5" Ø hole. Finish as needed.

At about 1:30 watch the drillin'.

litlerob1 said:

Thank you Dew, OP didn't ask about process recommendations, he asked about a drill, because a drill IS the single most effective tool for material removal.

R

Click to expand...

He has what? 30 HP?
I am pretty sure he can use all 30 of them in a helical cut. His RPM will be in a higher HP curve spot.
With a 2.5" drill even in alum he will be out of torque very fast.

Plus he got no TCS to flush the chips.

Pretty sure in HIS situation he can be more productive with a proper ramping mill.
Just IMO.

After looking more closely at the toque required for a drill that size coupled with no TSC I put together a couple of "test" models in the CAM and it looks like the 1.5" ripper mill based in the parameters Curtis gave me makes it look a whole lot more appealing the a single use/purpose ~$1,000 drill with inserts. Basically 11 seconds more per hole then drilling and interpolating with a 3/4" end mill. That is with conservative numbers so will see what it will really do.

I will say that a 1" indexable drill does pretty well without TSC, but flow at the tip would be nice. After drilling, used a 3/4 3FLT aluminum specific end mill 10K 150IPM 10% step over to a 3.3" finish size is good after the initial high engagement at the start of the cut (Spikes to 110%) then relaxed to about 60% load. Bore is 2.2" deep.

Should have the ripper in on Wednesday so will update after some proper testing.

Thanks for every ones input!

I should also ad that with 10 parts on the table you can't even find the parts as their buried under all the chips! I do think a ramp mill will help with the chip control as well.

litlerob1 said:

because a drill IS the single most effective tool for material removal.

Click to expand...

Maybe if all you have is a drill press.

david n said:

2.5" will be an issue. No way you could run it at mfg'r feeds n speeds.

Buy a drill the you can "plunge mill". Basically punch in a starter hole and then start plowin out material by steppin over and drilling until you have your rough 2.5" Ø hole. Finish as needed.

At about 1:30 watch the drillin'.

Click to expand...

Just a thought on that - If you're going to plunge-mill with a drill like that, especially when doing a slot, it's better to "skip" steps, and drill full-diameter holes at full feedrate, then come back and plunge out the webs between all the holes. Not only will you get better productivity from the drill on the full-holes, but you'll get better stability when drilling/plunging the webs too, since now the center insert will be engaged in the cut. Better stability turns into more feed/productivity here too. Programming becomes a little trickier here, but I'm sure you CAM-pro's can work that part out.

The 1.5" ripper works 1000x better than the 2 flute. You can get it in a facemill style and with 3 flutes is a hell of a lot quieter than the 2 flute screamer. I haven't used my 2 flute one in a few years.

For the record, water jetting a 2.4" through hole in 1.5" thick 6061 at ~45ksi would be about 2 minutes. Dunno if it would make sense to pre cut these that way but it's a thought.

rcoope said:

For the record, water jetting a 2.4" through hole in 1.5" thick 6061 at ~45ksi would be about 2 minutes. Dunno if it would make sense to pre cut these that way but it's a thought.

Click to expand...

Maybe I'm just cheap but even if the hole were oddly shaped like an infinity symbol or something it's hard to imagine applying all that overhead to an operation you could do with a HSS endmill. I'd think 2 minutes not an unreasonable time to get that metal roughed out of there. Sure a big insert drill would beat that handily but without TSC it's a big risk of wiping out a very high-cost tool.

Any machine operation comes down to a calculated risk; his decision is, is it worth it?