What's new
What's new

Who can recommend an insert drill for stainless with only flood coolant?

Volitan

Hot Rolled
Joined
Sep 16, 2006
Location
Long Island, New York
We have about 1,000 holes 1.187 +/- .005 to put through 1/4" 304 stainless bars. Unfortunately no thru coolant here.
There's also another 1200 of these holes to go through 5/16" brass plate. These both get counterbored but I can do that with an endmill.
While we're at it there's a third thru hole that I need to keep around .662/.665 dia, years ago I tried smaller insert drills with no luck. Have things changed?

I have to work with: VF-1 with a gearbox, VF-2 with no gearbox and a claimed 20 hp dual vector drive, and a DT-1 with 15,000 rpm's and HSM enabled.

I'm thinking to use the low end torque on the gearbox machine with an insert drill for the stainless ones, but I hear they like thru coolant.

Any suggestions on insert drills for these?

Thanks
 
That shallow I don't think flood vs TSC will matter much.

The tolerances though ... my experience with insert drills is they don't make super clean holes. I would drill undersize and finish with an endmill, in one of your 40-taper machines. That way you can get right after it with the drill, and still have a neat on-size hole instead of trying to finesse the insert drill.

Regards.

Mike
 
I've never had good insert life when drilling holes in thin material. It seems once you get half way through the material wants to push away from the inserts and cause them to rub hurting their life.

Personally I would probably helix in with a 5/8" inserted high feed mill and then finish with an endmill.
 
I've never had good insert life when drilling holes in thin material. It seems once you get half way through the material wants to push away from the inserts and cause them to rub hurting their life.

Personally I would probably helix in with a 5/8" inserted high feed mill and then finish with an endmill.

I have no experience with high feed mills.
Looked one up quick, a Seco R217.21-00.625-0-LP06-2A (based on availability at MSC)

It says helical interpolation would be something like 3100 rpms, 103 ipm, .030 deep and cutting it dry for 304 stainless.
Sound about right?
 
I used to sell Seco - I wouldn't hesitate for a moment to recommend an SD522 drill for drilling short diameters, with flood coolant. Keep in mind, that the coolant's main fuction is to flush chips from the flutes - especially at deeper depths - while drilling. With short drilling depths, the chips will come out on their own without much issue.

IF chip evacuation becomes an issue, a macro with a short dwell - not a peck - to break the chips would help. I doubt there would be a need for this however.

On the 1.187 +/- .005" holes - My only concern would be holding that tolerance. Especially without the thru-coolant. I would expect poorer hole quality, as there will be more opportunity for scarring/galling/scratching of the hole from the dry/un-lubricated chips.

There are coolant-inducing tool-holders on the market, to induce coolant to the tool, for older machines. These add cost of course, but more importantly they add gage-length, which is going to be a big No-No for this style drill, on a 40-taper machine. So that's not really going to be an option.

Since you're going to be using an endmill to counterbore these anyway, my suggestion would be to use a 1.125" indexable drill, and then finish with an endmill. If you insist that the extra cycle-time will hurt, then buy the 1.187 drill on a guaranteed-performance basis. That way, if the drill won't hold size, you should be able to return the drill.

Also - Use a SHORT series weldon holder to hold the drill - This will offer 1" shorter gage-length, which will be very valuable on your 40-taper machine. (Edit: Actually, 2"... See below...)


1.125 Drill - SD522-1125-225-1250R7 | Secotools.com

1.187 Drill - SD522-1187-237-1250R7 | Secotools.com

Inner Inserts - SPGX0903-C1 T400D | Secotools.com

Outer Inserts, 1st choice - SCGX09T308-P1 DP3000 | Secotools.com

Outer Inserts, 2nd choice* - SCGX09T308-P1 T250D | Secotools.com
*This insert uses a PVD coating. It will not have the same wear resistance, but will offer a 'sharper' cutting edge, and may be necessary if you see built-up-edge problems with your gummy Stainless material, and no thru-coolant.

Short/Stubby Weldon Holder* - CAT40 1.1/4 End Mill Holder Stub Length
*You may have to cut the shank of the drill slightly to get the flange to bottom out on the face of the holder, but I would 100% do it. This holder will save you 2" of gage-length over a 'standard' length holder..."









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

Regarding your .662/.665 thru hole, indexable-insert drills are near worthless at this small diameter. Even replaceable-tip drills like Iscar's Cham-Drill are tough at these smaller diameters, when solid-carbide drills have come so far in terms of cost, and performance.

Here's a quick recommendation, although I'm not up to speed on Carbide Drills as I once was. Walter DC160. It may be worth a call to Walter for a better recommendation, as the DC160 may be a double-margin drill, which would be a No-No for drilling soft stainless with flood coolant.

Walter DC160 16.8mm Drill - https://gps.walter-tools.com/toucht...oQaDkn9I0hUvrA==#/trs/productInfo/productData


Another solid contender for drilling Stainless, is Mitsubishi's MVS lineup.
http://www.mitsubishicarbide.net/mmus/enus/drilling/20000192/20092269









Best of luck.
 
I have no experience with high feed mills.
Looked one up quick, a Seco R217.21-00.625-0-LP06-2A (based on availability at MSC)

It says helical interpolation would be something like 3100 rpms, 103 ipm, .030 deep and cutting it dry for 304 stainless.
Sound about right?

Sounds about right but I use coolant on SS. I cut mild and tool steel dry always but for some reason I've never played with doing SS dry.

Edit:
If others say a drill can be made to work I wouldn't discount that. I just never perused it since I have oodles of feed mills and inserts and they work well for me
 
As mentioned the Seco Drills have worked very well for me. Although I did not try any others as they just worked so well.

We had two plates needing holes.
One was 1/8" x 2 x 3" with a 1-1/8" hole, the other 1/8 x 2 x 2 needing a 1" hole.

Two vices, two parts with a few second cycle time, flood coolant allowing guy to pick out next pair of plates.


How many? I ran releases in lots of 2000 plates each size, indexing the inserts every few orders. Sizes held +/-.001 and I adjusted shimming inserts with paper...yeah I know not recommended, but it worked. FYI- my +/-.001 was based on size hole the drill made, not to nominal, then adjusted to that size and made mating pieces to fit that size hole. We pressed in bronze bushings.

Job ran for several years.
 
just drill it with a standard size drill bit and bore to size. set up multiple offsets and parts to complete a bunch at once with one cycle. easy.

Sure, if he doesn't want to make any money on the job then he can use a HSS "drill bit" and chip away at it.
But this isn't 1950, and he has 1000 holes to do.
 
Sandvik insert tip (Corodrill 870 series I think?) or Sumitomo SMD series with the cast iron geometry (corner chamfer to help insert life).

No spot drill necessary and you can run them pretty hard. Insert tips are not cheap but we got good life in 304 and 17-4 at the old shop. Both left good wall finish. We used the Sandvik in lathes and the Sumitomos in VMCs. No real reason other than I got Sandvik tooling packages with the lathe and Swiss I bought there.
 
Sandvik insert tip (Corodrill 870 series I think?) or Sumitomo SMD series with the cast iron geometry (corner chamfer to help insert life).

No spot drill necessary and you can run them pretty hard. Insert tips are not cheap but we got good life in 304 and 17-4 at the old shop. Both left good wall finish. We used the Sandvik in lathes and the Sumitomos in VMCs. No real reason other than I got Sandvik tooling packages with the lathe and Swiss I bought there.

I love the 870 drills, but was hesitant to recommend those since it's thin stock so I went with the 880 drills. I could be wrong though, the 870 might hold up better?
 
Great info, I'm going to look into all of these options. Thanks!


just drill it with a standard size drill bit and bore to size. set up multiple offsets and parts to complete a bunch at once with one cycle. easy.

That's how we are doing it now. I usually get order of 50-200. In this case it's 5x that and it's a bit of a rush so I need to save some time where I can. Whatever tools I buy for this I can use again, this one repeats pretty often.
 
Sandvik insert tip (Corodrill 870 series I think?) or Sumitomo SMD series with the cast iron geometry (corner chamfer to help insert life).

No spot drill necessary and you can run them pretty hard. Insert tips are not cheap but we got good life in 304 and 17-4 at the old shop. Both left good wall finish. We used the Sandvik in lathes and the Sumitomos in VMCs. No real reason other than I got Sandvik tooling packages with the lathe and Swiss I bought there.
We recently switched to Sumitomo for one job at 7/8 in aluminum and were highly impressed with it's performance. Made Iscar look like someone else's red headed step child. I'd ask for a demo drill to try and have them observe. We bought all the samples they brought in at 50% of list.
 
One word of caution with replaceable-tip drills, is that the generate more thrust than indexable-insert drills, since they two-effective flutes, and thus usually operate at high feedrates. This may be a problem on thinner parts.

Somewhere around 7/8" diameter is a fair tipping point between replaceable-tip vs. indexable-insert drills. One of the bigger factors would be drilling diameter.

I will say however, that the will absolutely produce a better hole quality & size tolerance. No question there.




If it made sense to go that route, Allied Genesys line of replaceable-tip drills are really affordable. (Last time I checked into it anyway - It's been a few years.)
 
Thin material blows. You can make lots of "thin" stuff into thick stuff though. Stack them up 6x=1.5" and Drill them with whatever indexable drill you want
A tiny bit more than the diameter of the drill won't matter that much.

R
 
Stack them up 6x=1.5" and Drill them with whatever indexable drill you want

This is usually a "no no" with indexable drills. Since these drills produce a coin, they can lodge, jam, & blow up the drills.

I could maybe see it if you had a solid support under the bottom layer of material so that there's no flex or deflection, and then toe-clamped down tight as to avoid any gaps between the laminate.

What's your trick & experience with these?




For the record, this all revolves around the coin getting lodged between layers of stacked material, where there is a slight air-gap, and which semi-traps the coin. The coin is allowed to move laterally, but is not held securely so as to be cut by the drill. The machine keeps pushing, and soon, the inserts are crushed, the drill body is wiped out, and the hole is damaged...



I've seen this done semi-successfully once, with a Sandvik 880 drill, but it was risky, and the drill didn't like it. Judging by the spike in spindle-load & Z-axis thrust/load as the drill broke through the first layer & into the second - there was some kind of temporary interference going on with the coin. I suspect it was just one minor escalation away from a ruined $700 drill body...

That being said, some of the big players are now playing with modified insert pocket geometry/positioning, to eliminate the coin produced, and thus, allow them to drill stacked materials, with air-gaps, as is common with laminated weldments.
 
@Jashley, mostly you're right. The slug, coin whatever is or would be a problem. I guess we'd need to know how big these 1/4" pieces were. If they're 3x3 it's probably fine, but bigger, I agree it could be perilous.

R
 








 
Back
Top