What's new
What's new

Recommendations for countersinks with consistent dimensions

pMetal

Aluminum
Joined
Jul 14, 2014
Location
United States
I've gotten frustrated with the consistency of the countersinks that I have found available.

The problems I've encountered come in 2 varieties:
  1. The flutes come to a point, but the tip is blunted. This means that depth calculations based on the sharp point will be off.
  2. There is a flat at the bottom, but the flat's dimensions are not published and are not consistent. This means that depth calculations based on my estimate of the flat's dimensions will likely be off, since the flat is difficult to measure.
Either of these situations means that it requires that I make a trial piece to "dial in" the resulting countersink diameter to get it right within a few thousanths. And I have to repeat this when I replace the tool or move production to a different machine. This is an unnecessary problem to have in my opinion. The countersink manufacturers don't seem to understand that people use CNC these days and that we program the C-sink depth based on the expected tool dimensions.

I'm referring to the multi-flute type of countersinks (6 flutes for example), in small sizes (3/8", 1/2" or so)

Furthermore, why does almost every countersink manufacturer design their tools such that they have a reduced size shank? That's a terrible idea because it gives the toolholder/collet a weaker grip, it gives swarf a place to collect where it can't fall off on its own, and likely takes longer for the c-sink manufacturer to make as well. I understand why you may want a reduced size shank for a large c-sink (1" diameter or so), but for anything within range of ER collets, why would they want to reduce the shank?

Does anybody know of a countersink brand that does it right? Meaning either it should come to a sharp point, or come to a flat where the flat dimension is published and consistent? And ideally it would have a full-size shank too. The flat bottom design would be preferred since you don't have to worry about it getting dulled and then giving you different results when re-measured.
 
Seems you could handle this problem in tool setting; registering against a chamfer. That also handles the problems of re-grinding countersinks and chamfer tools; where you'd lose any initial reference.

I can see why a manufacturer wouldn't want to rely upon a sharp point as a reference surface -- and why you wouldn't want to either. The notion of a blunt tip makes more sense -- maybe someone does that as a reference? Still that begs the question of why not register tool length against a 82 etc. degree stop to begin with? Should get within a few thousands (and three or six or so lines of contact way better than a single sharp point).

Personally, I don't recall many, if any, countersinks slipping in a chuck or collet -- so the reduced shank seems to grip OK.

And I'd guess that for high production, many would use a combined drill countersink and that a whole lot of holes are still done manually with some sort of stop -- the small aerospace ones in micrometer stops. So, could be there isn't much of a market for countersinks made with more HSS/Cobalt/Carbide in them and precisely registered to a sharp or (better) blunt point?

Pretty sure, though, you could get someone locally to put an 82 degree point (or whatever) on most any diameter end mill you'd want; perhaps starting with a 90 degree point stock. And there are likely some here happy to make what you want from scratch.
 
I agree with Pete.

While I use SGS ( Now Kyocera ) countersinks and they are relatively consistent, I still either pick them up to a known diameter on the angle ( whatever angle they may be ), or just dial them in
as I go.
The pickup method gives consistent results quickly, while the dial-it-in is just as good albeit takes a bit more time.

As far as the reduced shanks, I never considered them to be a hindrance in CNC operations, but sure as hell preferred when same countersink ends up in a drillpress or a cordless drill for
off-hand countersinking.
 
Use a pre-setter. Besides being able to determine the theoretical sharp point dimension on countersinks and chamfer mills, there are other handy time saving/tool saving uses.
 
I use Harvey drill/mills for countersinking, but I interpolate the countersink instead of plunging and hoping it doesn't chatter. They have been very consistently ground, and they publish the geometry.

If you mean chamfering, then I use MA Ford carbide spotting drills. They have also been very consistent.

One thing I have seen though is you have to watch the tips for both of these types of tools as they are fragile. If you lose a bit off the tip, the tool will cut deeper than it is programmed to if you use a toolsetter to measure the tool length.

Regards.

Mike
 
All good logic Pmetal

Guess it would/might be logical to have a chart gong from point or snub to standard dimensions so one might quickly program a bevel/chamfer..
knowing the cutter angle it would not long to trig out a chart.
 
It's a valid complaint IMO. But there are solutions to it.

But really everything has a blunt, Drills, Taps, Spots, Inserts, nothing is actually sharp--it would be too fragile.

I use a Ring to set Chamfer tools, but I also run them high. Unless it's an hour of Chamfering.

R
 
Talk to any of the manufacturers who make countersinks... Ask them to quote you a run of customs with a known diameter flat, with tolerances... Chances are, if you model it on one of their standard tools, and just add a dimension/tolerance that you're happy with, they won't cost you more than a buck or two more than the off the shelf tool, and the lead time will be the same. I can name at least 5 companies off the top of my head who would happily make you a solid carbide coated countersink to whatever dimension and tolerance you like. I can name at least 2 or 3 who would have them in your hands in under 5 days.
 
By and large I have given up on using counter bore tools unless it is a very long running job. I just surface them with an endmill. That way I am precisely the same as the modeled geometry. Usually I have a suitable tool loaded in the machine, so there is no tool change. You have to run the CS tool so slow, that I don't think it is all that much slower. I have a standard routine of helically boring the screw clearance, that helixing up from the bottom to get the CS. I've never thrown a stopwatch on it, but compared to the way I used to do it (spot, drill, countersink), it doesn't feel slower... especially since I don't need to go find and load three tools. I'm doing short run production, when I was doing high volume, I would just get a tool ground that did all three steps in one shot.
 
By and large I have given up on using counter bore tools unless it is a very long running job. I just surface them with an endmill. That way I am precisely the same as the modeled geometry. Usually I have a suitable tool loaded in the machine, so there is no tool change. You have to run the CS tool so slow, that I don't think it is all that much slower. I have a standard routine of helically boring the screw clearance, that helixing up from the bottom to get the CS. I've never thrown a stopwatch on it, but compared to the way I used to do it (spot, drill, countersink), it doesn't feel slower... especially since I don't need to go find and load three tools. I'm doing short run production, when I was doing high volume, I would just get a tool ground that did all three steps in one shot.

I think you are mixing up counterbores with countersinks. OP was asking about countersinks. Sort of a PITA to interpolate a countersink with a square endmill ;).

Regards.

Mike
 
Yep that flat situation will bite especially if you work in a shop (most shops?) where they wish to do all the programming and then you fix it to run. Anyway for countersinks the programmer most always programs using the model of a pointed CS so if you do not have that loaded and have one with a flat nose then the CS will be deep. Evernote if they program and you also load a CS with a point you always do well to back off the CS as always if you do not it will bite you bad right on the A**.:mad5:
 
I think you are mixing up counterbores with countersinks. OP was asking about countersinks. Sort of a PITA to interpolate a countersink with a square endmill ;).

Regards.

Mike

Yep, I was typing faster than I could think. I meant countersinks. I regularly surface them with a square or bull nose endmills. They are surprisingly quick to do. Combined helix bore and surfaced counterbore is about 10 seconds with an acceptable surface finish. Don't get me wrong, I still use countersink tools for long running production, but for short run I bore in and surface out. I am virtually guaranteed of an accurate part. When it comes to countersinks, I greatly prefer to surface them rather than dick around with nebulous countersink tools.
 
For any countersink or chamfer that needed to be sized, I stopped using actual countersinks and moved to stub length end mills with a 45 ground on them. I found the quality and consistency was much better, and it gave me a bit more flexibility. We also had a couple of sizes of screw on carbide tip 45 degree toolholders that worked wonders for the very small features, and were fairly repeatable.
ISCAR Cutting Tools - Metal Working Tools - MM ECF
 








 
Back
Top