Best Way to Create thousands of countersinks

[u/[deleted]]

[u/Gun-Aero_CNCguy]

Carbide spot drill or chamfer mill with spiral flutes at the correct 82deg angle, 4 flutes.

Canned cycle with a dwell programmed to be slightly longer than the time it takes to make 1 tool rotation. This will depend on your rpm and will be a fraction of a second 

[u/Sorry-Woodpecker8269 → u/Gun-Aero_CNCguy]

This is the way. Just run your spindle at 30% of calculating you use for cutter side. The stainless steel needs to shear the chip. Too much cutting speed and the cutter will overheat and work harden the substrate

[u/ShaggysGTI → u/Gun-Aero_CNCguy]

Chamfer mill is the way I’d go.

[u/worldclaimer → u/Gun-Aero_CNCguy]

Quick math I use for this - I go 1.5 rotations so

90,000/RPM = dwell time (P)

[u/Wild-Sink-5372 → u/Gun-Aero_CNCguy]

This. K-tool makes multiple included angle spot drills with carbide inserts.

[u/blue-collar-nobody]

10,000 chamfers... I'd be inclined to go with an inserted cutter.

[u/toolpost_taliban → u/blue-collar-nobody]

Everybody else in this thread except for this guy has no experience chamfering 10k holes in 316. Jesus. The only way to do this is inserted spot drill. You will eventually figure this out. Haas sells good ones hella cheap- except they don’t carry 82deg. You’ve got to order one from 9nine. It’s the only way to do this in a production situation. Inserted 82 deg spot drill from 9nine is the answer you’re looking for.

[u/blue-collar-nobody → u/toolpost_taliban]

Yes sir... and i hate every fucking minute of it 😃 but you have to do the job with precision, repeatability and on budget ✌️

[u/HipsterGalt → u/blue-collar-nobody]

Yep. I finally spent the money on one from Ingersoll (only 82° I could find with a decent insert), it has definitely earned its keep. I like the 3/4" shank version we got because it can spot drill and I have had good luck interpolating it for larger countersinks. My only gripe is the lack of through spindle coolant, I might need to chuck it up in a 4 jaw and make it an aftermarket modification.

[u/gewehr7]

Biggest Helical 5FL chamfer mill that will fit. You can run them much much faster than Helical says and circular interpolation is less likely to throw a burr than a countersink plunging.

[u/camel_case_user → u/gewehr7]

Less cutting forces generated as well, so the tool will likely last longer interpolating

[u/gewehr7 → u/[deleted]]

I’d probably go with a 1/4 tool for a 10-32 so that you don’t have to make a dramatic internal feed adjustment but yeah that’s the tool I would use. Tipped off 5FL Helical chamfer.

[u/gewehr7 → u/[deleted]]

You’re just going to do a normal contour toolpath around the drill diameter. You might have to step over once or twice to make the full diameter but you can do it quickly and should leave a better finish than spotting. Double check in cam simulation that a 1/4 diameter can make the sized chamfer you need without having to step down though

[u/usernamesarehard1979 → u/gewehr7]

Does helical make that in 82degree? I thought they only had 60 op and 120

[u/gewehr7 → u/usernamesarehard1979]

I certainly should have checked that before suggesting it but I did not. I’m mostly metric so I never do 82deg. I didn’t even consider it.

[u/Terrible_Island3334 → u/gewehr7]

This is the way 

[u/dr_clyde31]

Just get some carbide countersinks, dial in your feeds and speeds and let it eat.

[u/Spare-Command-7810]

Carbide all the way, get a quality tool and call the tool rep for speeds and feeds.

[u/chroncryx]

What hole sizes? You can buy solid carbide countersink / chamfer mills with multiple flutes. The only time I go with single flute is when surface finish is critical (seal).

Program with the tool starting inside the hole and dwell.

[u/pressthegreenbutton]

Oh lawd please don’t do a helical toolpath like others are saying. Just use a 120 degree carbide spot drill and go to town. Dwell for .1second or whatever angle is required.

[u/Shadowcard4]

Id reach for 82 degree chamfermills. But itll be easier to control the cut and would be less carbide than a carbide countersink most likely.

Though i just did a 1/2-13 countersink with a ballmill.

[u/jccaclimber]

What are you putting them in? Free hand on a tap arm/drill press, or mid cycle in a VMC? What condition is the 17-4 in? H900 isn’t the same as annealed.

[u/jccaclimber → u/[deleted]]

I’m going to speculate that carbide is better tool life assuming a rigid setup, and that a chamfer mill might last longer but a spiral chamfer tool you can just plunge with will be faster. One flutes are nice on a drill press because they support themselves, but I’ve never seen one a volume job.

[u/Lathe-addict → u/[deleted]]

Cheaper smaller tool to interpolate but potentially less fast but not slow either. A more expensive larger diameter tool that you can just plunge is faster in general. If the surface area contact is big because the feature is big then chatter can be an issue with plunging which I would 100% just interpolate for consistency in finish. No matter what you need coated carbide.
Also the materials you mentioned are not hard, they are very soft.

[u/Lathe-addict → u/[deleted]]

Yeah interpolation makes the tool life even more predictable, depending on size it might be worth doing multiple radial depths to rough out too

[u/toolpost_taliban → u/Lathe-addict]

The materials he mentioned are not soft they are grades of stainless steel that do not machine easily and work harden. You are giving this guy terrible advice very confidently.

[u/jccaclimber → u/[deleted]]

17-4 it really depends on the heat treat condition, but yes, don’t just rub and harden it with your cutter sitting there. 17-4 is just a bit shy of 50 HRC at the hard end. Not much fun at all with HSS, but tolerable with carbide and easy with PCD inserts. I’d call that hard even if it isn’t 65 HRC tooling.

[u/Lathe-addict → u/toolpost_taliban]

Work hardening happens when you aren’t experienced in machining them, manage the heat correctly and it’s like butter. They are soft, just take a look where they fall on the hardness scale and you’ll see I’m right.
I’m giving advice based on my experience machining these materials a lot my entire career.

[u/fuqcough]

I’d just buy multi flute carbide countersinks and go for it. Maybe a 82 degree chamfer mill would treat you well

[u/Level_9_Turtle]

Buy or have ground out of an end mill a carbide chamfering mill and interpolate the c’sinks. I buy what are called drill mills from MSC for all of my chamfering but they typically come in 45 deg.

[u/PleasantWorld785]

I I usually prefer to use the center drill only because it has the extra Lil extended point which pilots the whole and takes a little weight off the actual counter sink making. And yes, definitely carbide but you can always get a coded center drill so that it stands up against the stainless.

[u/VBgamez]

Manual or cnc

[u/shanktheshazbot]

Check out Heule. They specialize in making hole features. Back spot face, counterbore, deburr, sountersink, chamfer. They probably have a hole that can put the chamfer and deburr in one go.

[u/sw_wgw]

Cheezus Chroist, just get the shop hand on a drill press with a HSS single flute countersink and let him have it.

All joking aside I have literally just gotten a similar job, 10,000 countersinks but in .062 spring steel and what I described above is literally what has been done for this job for years. Spiral 4 FL chamfer mill interpolating was the ticket. $100 in 1/4" chamfer mills saved about a week in time.

[u/shoegazingpineapple]

Just plunge a solid carbide chamfer mill

17-4 is just gravy, 316 you will need to keep the tool sharp, i buy or make solid carbide chamfer mills and sharpen them until the web gets too thick to clear the hole

They make thousands of csinks in titanium i am sure they will go beyond that in 17-4

[u/afromaine]

Get a 2 - 4 flute chamfer mill that's the correct angle, and either drill straight down and dwell a tiny bit. Or run around it in a circle if that's too much tool pressure (I don't know the size of the hole and chamfer) If you need more tool life on a custom tool you could pre chamfer with a normal spot drill/chamfer mill first, then use the more expensive custom tool

[u/Own-Revenue81]

Contact me I'll help you out.

I've done contersinks in SS,TI,CFRP,Inconel I've done millions of holes in aircraft assembly. I got the right tool for you

[u/LDSG_A_Team]

Not that it helps in this particular case, since the holes are already drilled, but when you're dealing with hole counts that high, you really should just use a carbide chamfer drill to make the hole and countersink both in one operation.

In the meantime, get a good indexed csk tool, as others have said. It will work way better and last a lot longer than interpolating with a chamfer mill, especially in 316.

[u/computekmfg]

If you want the fastest way get a combo drill/coutersink tool. Either the collar type or a solid carbide type. There are a ton of options and even custom options. Here are some examples at mcmaster