Countersinking in production

dallack · Apr 8, 2011

We're running a repeat job where we need to countersink a lot of holes in steel.
We drill the hole 6,9mm, then countersink to a 14,5mm (90°).

Currently we are using a solid carbide TiAlN coated countersink, and get about 5000 holes before the cutting edges are too chipped to use.
Machine is a HAAS VF2-SS, I think with a more stable machine we would see longer tool life, but it's the best we've got.

Is there a good tool that uses some kind of replaceble tips?
I found something in Iscars catalouge for their system with replaceble cutting tips, it only had 2 cutting edges, I wonder if it would chatter or not.

scojen · Apr 8, 2011

dallack said:
and get about 5000 holes before the cutting edges are too chipped to use.

5000 holes and you have a complaint, don't you have a way to sharpen the countersink. While an insert style counter sink will probably work you are not goint to get any life out of an inset than you are getting now invest in more counter sinks and keep at least two in stock and have the used ones resharpened.

Scott

beege · Apr 8, 2011

You might get better results circularly interpolating (maybe a finish pass?) with a 90 degree mill.

I have seen an insert tool, but don't remember who makes it. It also serves as a spot
drill, and chamfer mill.

jelrod1 · Apr 8, 2011

Allied makes drill bodies and inserts and they have one that is 90 deg and works well. It is a single insert just like the drill insert but for chamferring.

gorrilla · Apr 8, 2011

beege said:
You might get better results circularly interpolating (maybe a finish pass?) with a 90 degree mill.

I have seen an insert tool, but don't remember who makes it. It also serves as a spot
drill, and chamfer mill.

I've used those inserted tools to chamfer and spot drill. They work nice, but they are fragile as hell. And when the insert blows, it generally takes the pocket with it.
We do fairly short run production work, almost exclusively. We've found better luck with the level of experience we're able to get in our area with solid tools rather than inserted everything. Inserts start to wear or hit an inclusion in our castings, and if your not right on top of it, with your hand on the E stop, your gonna blow up an expensive cutter in a flash. Maybe even if you ARE right there. Also, as I mentioned, with the level of experience we're privvy to, an insert can start wearing, and if the operator isn't experienced enough to recognize that change in pitch or finish, then again, it can get expensive in a hurry.
We were using small carbide tipped spade drills for a while. When they were cutting right, you could blast through the parts fast. But let an insert wear a bit, or worse, encounter an inclusion in a piece of cast, and you just spent $350 to $400 in a flash. When your down out of sight in a hole, those inclusions are landmines. We went back to solid carbide in most cases. They'll still break, but they seem to be a lot tougher than the inserted drills. In some cases of low production volume for a particular size hole, we still use HSS. It's a question of how much backup is affordable, and how often you drill that sized hole.
If I could just get the boss to let me put a tool sharpener in the shop, I could cut down on the amount of backup needed. It's all a question of ROI, as is everything I suppose.

dallack · Apr 10, 2011

I'm not complaining, I'm just interested in making things go faster, or better.

The supplier of these countersinks offers resharping, but with the cost of sharpening and recoating it's not much cheaper than buying a new one.

wrustle · Apr 10, 2011

Let's figure a solid carb .750" dia. 90 degree c'sink runs you roughly $60.

At 5,000 holes that's only a fraction over a penny per hole. $.012 per hole.

Using an inserted 90 degree c'sink (tool life untested) let's for the sake of arguement base our comparison on one completely used insert to do the 5,000 holes.

The tooling cost would be $85.00 for the cutter (a "hopefully" one time purchase) with the insert costing you approx. $9.00/ea. leaving you with an estimated per cost hole of $.0018 per hole using one insert.

Sounds to me like it may be worth a try.

McMaster-Carr

Best Regards,
Russ

viper · Apr 10, 2011

If you are chipping your CS, that tells me you have an unstable machining condition and probably can be rectified with a different CS geom or change in feeds and speeds. In our experience, high spindle speeds with a CS will create problems because you engage a large are of the cutter at the same time. Slower speed with higher feed seemed to work better for us.

What cutter are you using? We have also had to have some custom ground for us because most off the shelf CSs seem to be junk or are too pricey.

I also assume you are choked up on that cutter as much as possible? Rigidity is paramount. I will tell you we ran about 4000 CSs in 17-4 H900 and the CS is still running to this day. I don't know if we have actually worn one out but obviously a more aggressive CS operation would change that.

Mud · Apr 10, 2011

Are you using a single flute or multiple flute tool, and what speed and feed are you using?

PixMan · Apr 10, 2011

Love to know what spindle speed you can throw at the problem, because if you were to use one of the insert type countersinks that Wrustle posted and add a full-edge PCD insert in place of carbide, you may never need another tool.

Limy Sami · Apr 10, 2011

PixMan said:
add a full-edge PCD insert in place of carbide, you may never need another tool.

PCD in steel?............... I thought diamond and steel didn't mix, something new out there?

SteveinAZ · Apr 10, 2011

We use inserted countersinks from Everede and they seem to hold up pretty well...we have a set from 5/8" to 1" and all use the same insert. They were pretty reasonable IIRC, and you can run them waaaay faster than you would think. The only downside is they have an odd tone when cutting, which takes a long time to get used to. We have used them primarily in soft, low carbon steel, but also have run them in T316 and 6061, so they are pretty versitile. The high spindle speed also throws the chip off well.

Steve

PixMan · Apr 10, 2011

Limy Sami said:
PCD in steel?............... I thought diamond and steel didn't mix, something new out there?

WHOOPS! My bad!

I had it in my head that it was aluminum. Must've been that 5000 holes per tool thing.

Honestly, if it were really hard steel or A286 or smthing, maybe CBN, but PCD is absolutely wrong. My mistake!

Century Tool of CT and Vermont Indexable both make some really nice insert countersink/centerdrill tools.

SeymourDumore · Apr 10, 2011

Dumb thinkin' out loud here.....
While 5000 holes are nothing to sneeze at for a tool life, I would try to do my countersinking BEFORE the hole with the center drill.
I know I know... the tip angle isn't the same but! This is only steel we're talking about and the drill edges should hold up pretty well. ( I'm still surprized that the drill lasts that long for 5000 pieces. )

gregormarwick · Apr 10, 2011

I normally do countersinks with helical using carbide or inserted chamfer mills. High speed/feed, small helical lead. Really easy on the cutter, nice finish, excellent chip control, pretty quick.

Eg. I make a part that has some c/sinks for a M12 c/sink cap screw in 316L, predrilled 12.5mm. Two flute indexable chamfer mill with TCMT1604 inserts, 4000rpm, 3800mm/m, 1mm lead. Takes about 4 seconds per hole.

J&L/MSC over here sells TiALN coated solid chamfer mills for about £20 for a 12mm. We treat them as disposable. Also, I'd be pretty bloody happy with 5000 holes per cutter!

ewlsey · Apr 10, 2011

Get a solid carbide 16mm (or so) drill ground with a 6.9mm step to make the chamfer. Then you can drill the hole and chamfer at the same time.

Won't work with multiple hole depths though.

dallack · Apr 11, 2011

Wow, thanks for all the suggestions!
These parts are laser cut 8mm steel that we drill and countersink holes in.
As viper suggested stability isn't perfect, on some parts I can put the CS al the way in a short milling chuck, put on some parts there's clamps in the way, so it has to stick out a little bit too long.

Spindle speed is about 1300rpm, feed 110-120 mm/min (don't have the program here to check exactly)
Plunging straight down into the drilled hole, no peck.
We're in the low range of the recommended feed/rev, with higher feed the whole machine makes a shake at the bottom of the hole.

I've been thinking about a 90° spot drill as well, maybe a carbide one would be fast enough.

gregormarwick, that's some serious speed! Does it work with a solid CS as well?

gregormarwick · Apr 11, 2011

dallack said:
gregormarwick, that's some serious speed! Does it work with a solid CS as well?

Yes, it works, we do a few 316L parts with 8mm c/sunk holes the same way using a 12mm solid carbide, but I don't think you'd be impressed with tool life. But I don't think I've ever tried it in steel so I can't say for sure if it'd work in your situation.

Limy Sami · Apr 11, 2011

What about a piloted CSK,........... makes all the difference to chatter etc etc.

stroker · Apr 11, 2011

Countersinking

dallack said:
We're running a repeat job where we need to countersink a lot of holes in steel.
We drill the hole 6,9mm, then countersink to a 14,5mm (90°).

Currently we are using a solid carbide TiAlN coated countersink, and get about 5000 holes before the cutting edges are too chipped to use.
Machine is a HAAS VF2-SS, I think with a more stable machine we would see longer tool life, but it's the best we've got.

Is there a good tool that uses some kind of replaceble tips?
I found something in Iscars catalouge for their system with replaceble cutting tips, it only had 2 cutting edges, I wonder if it would chatter or not.

Hi
We use these Nine9 Nine-9 Exporter Importer of Tools and System for Manufacturing Technilogy.
Regards
Mike

Countersinking in production

Aluminum

Stainless

Stainless

Aluminum

Stainless

Aluminum

Titanium

Titanium

Diamond

Diamond

Diamond

Stainless

Diamond

Diamond

Diamond

Diamond

Aluminum

Diamond

Diamond

Hot Rolled

Similar threads