I seem to have lots of problems countersinking. I drill all my holes on a CNC mill and that works great. But the countersinks never quite seem to be right. They are generally not deep enough and that generally happens because the countersink slips in the chuck regardless of tight the chuck is. Then there is the problem that countersink manufacturers, such as MA Ford, blunt the point making figuring the required depth hard. I have tried six flute MA Ford and single flute Morse countersinks. The Morse is nice since it comes to a sharp point.

What has been your luck with countersinking on CNC mills or do you prefer to do countersinking as a second operation on a drill press? How do you ensure proper depth of cut if used on a CNC machine?

The following my latest tooling invention after a shotgun wedding of a countersink and a screw. The screw was being used to test depth and I got distracted while talking with someone near by. Screw sure started to glow fast and the two are pretty well welded together now.

http://www.cnczone.com/gallery/data/500/medium/IMG_4141.jpg

That is a technique Caterpillar use to weld pistons onto the end of piston rods for hydraulic cylinders; they probably leave out the distracting second person. :)

On a more serious tone do your countersinking first using a 90 degree spot dril and then drill the hole.

Ah, that's a slick idea, thanks! Is there something special about 90 degree or should 82 degree be used if countersinking for 82 degree screws? (I guess I assumed these screws were 82 degree screws...)

On a more serious tone do your countersinking first using a 90 degree spot dril and then drill the hole.

I don't think you will find an 82 degree spot drill. I have never bothered with the small angular difference; the mismatch between the angle on the head and the angle on the countersink is going to be very small.

Enco and MSC have a few but the selection is really small. Glad to hear the 90s work fine. Just out of curiosity, why would one choose a regular countersink if the spotting drill will work fine?

Sometimes the blueprint will specify the included angle, leaving you no choice.

Here's a small, free program I wrote a few years ago to calculate drill and countersink depths for various included angles and tip diameters.

http://mrainey.freeservers.com/Miscellaneous/depth.zip

I don't think anyone really answered your question, which I interpret as: How do you set the depth of the countersink when it doesn't have a sharp point?

My answer is:

1 -- Take a rough guess that isn't deep enough.

2 -- Insert a screw and measure how far the head protrudes.

3 -- Add that value to the depth setting to make it flush.

Ken

Enco and MSC have a few but the selection is really small. Glad to hear the 90s work fine. Just out of curiosity, why would one choose a regular countersink if the spotting drill will work fine?

As mrainey says you may have no choice. I keep forgetting I am the guy who designs, makes and sells our products so what I say goes (most times).

But don't use a spot drill to countersink after drilling unless everything is nicely clamped or it will chatter like crazy; countersinks are designed with very little clearance so they don't chatter easily.

There are countersinks available that are cnc qualified. They have a known flat ground on the nose that is usually +/-.001. Severance identifies their cnc countersinks with a flat ground towards the end of the shank.

If you don't know what the flat diameter is on your current c'snk you should still be able to measure the distance from the nose to full diameter of the tool and use some simple trig to figure how deep to go. For non cnc c'snks this is going to be different for each tool.

Thanks everyone. I countersunk several 1/4" flatheads today using a 1/2" spot drill. The ease of setup, consistency, quality of cut, sound, and speed were all significantly better than with a countersink. The chuck never really seemed to hold the countersinks well but has no problem with the spot drills.

Sometimes the blueprint will specify the included angle, leaving you no choice.

Here's a small, free program I wrote a few years ago to calculate drill and countersink depths for various included angles and tip diameters.

http://mrainey.freeservers.com/Miscellaneous/depth.zip

Michael, you should add this gizmo to ME Consultant Pro. Also need a depth chart for Flat Head Cap Screws in all the sizes.

Best,

Bob W.

You can buy 82 degree spot drills from MSC...but in my experience they are prone to chatter for spot drilling.

If I remember correctly, ISO/DIN flathead screws (DIN 7991, and whatever ISO equivalent) use a 90 degree countersink. American made flathead screws use 82 degree countersink. (can still be metric threads, but not conforming to ISO/DIN standard may have 82 degree countersinks)

The different angle is usually small enough to be negligible, unless you have two mating surfaces and the top surface is very thin. (countersink depth can get you in this case...I found this out the hard way)

I really like the 90 degree Minimaster tool/insert from Seco/Carboloy for spotting and countersinking. It is extremely stable and you can feed it at 0.007"/rev for spotting and coutersinking.

Justin

1. Try holding the C/S in a collett or grind a flat on the shank and hold it in an endmill holder.
My guess is that your drill chuck is shot and you are not getting it tight enough.

2. Use the correct angle spot drill or C/S ( 82 deg. ).
Don't start substituting tolerances or tools to make your job easier.

3. As far as total depth guesstimate and then adjust.
If you can get the the C/S to stop slipping ( see #1 ) you will only need to do this once.

4. You may also want to slow your feed down, maybe you are pushing it to hard.

PS
Don't make junk or ruin machinery and tooling, unless you are the one funding this whole project.

We all make mistakes, but C/Sing a hole with a bolt in it ?? Come on !!

If C/sinking in a mill I like the 6 flute. The rigid setup in a collet keeps them from chattering and they cut really quickly. The same countersink will chatter like squirrel in a lose vise on a drill press. (Chatterless my ASS - MA Ford).
I ONLY allow single flute to be used on the drill presses.
If you are doing large CSinks - interpolating works really well (I do this with the 6 flute CSinker).

Just like others have said - I guess on the depth and adjust accordingly. Once you have done this a few times you will know (write it down) what dia the tool will cut when zeroed on the flat.

I have to agree with premier_industr here.

Do the job right and make sure the angle of the counter sink is matched to he screw. The reality is that the proper countersink does have an impact on the screws ability to retain itself in position. Beyond that you want your product to reflect positively on you if it is torn apart in the field.

Now about that part and its improper countersink reflection on your product, I work in industrial maintenance where the vast majority of the equipment is custom made. Mechanical workmanship is always of a concern and things that don't stay together are complained about loudly. So unless you have a technical reason that will get by the plant mechanics, don't go about delivering products that show you don't have the least concern about workmanship. Little things add up.

As to the countersink slipping in the drill there are a number of possibilities. The first thing that comes to mind is that the chuck is junk. The second is that you need to put some meat into the tightening procedure. The third is that you are feeding way to fast. The fourth would be a lack of lubricant. In any event I'd go with some of the other suggestions and put the thing into a collet.

I'd also go so far as to say don't make junk even if you are funding the whole procedure. One thing that we on the floor have to deal with is the wanton manager coming to the shop trying to push through a piece of machinery based on the idea that it is only a prototype or experimental device. You would be surprised how often those so called temporary things have to be maintained. Same thing with the guys making something for the home hobby shop. You can do it right the first time or spend untold number of years maintaining what you built. It isn't often a question of money either it is simply a willingness to do the job right. Even when money is a concern a little thought about the project can often make for positive economics and good workmanship.

Dave


1. Try holding the C/S in a collett or grind a flat on the shank and hold it in an endmill holder.
My guess is that your drill chuck is shot and you are not getting it tight enough.

2. Use the correct angle spot drill or C/S ( 82 deg. ).
Don't start substituting tolerances or tools to make your job easier.

3. As far as total depth guesstimate and then adjust.
If you can get the the C/S to stop slipping ( see #1 ) you will only need to do this once.

4. You may also want to slow your feed down, maybe you are pushing it to hard.

PS
Don't make junk or ruin machinery and tooling, unless you are the one funding this whole project.

We all make mistakes, but C/Sing a hole with a bolt in it ?? Come on !!

Humor turned into a bit of chastising here. Gosh, good thing I don't share the big mess ups :)

Anyway, I'll pick up some 82 degree spotters and all will be good.

Don't make junk or ruin machinery and tooling, unless you are the one funding this whole project.

We all make mistakes, but C/Sing a hole with a bolt in it ?? Come on !!

I really like Geof's idea to use the spot drill. If you want to locate the hole with any precision, you ought to spot drill it anyway. On the CNC machine, or even manual, why load up and run 3 tools on the hole when 2 will do?

You can work out a table of depths to drill and errors versus a true 82 degree countersink pretty easily. Specs on the flat head cap screw head diameter are found here:

http://www.fairburyfastener.com/xdims_shcs_flat.htm

From that and a little trig and geometry, I get the following table:

http://www.thewarfields.com/cnccookbook/img/CNCCookbook/CounterSinkDepths.jpg

First column is bolt size, second is diameter of head, third is depth to drill (1/2 the diameter, since we have a right triangle and the cone of the head is the hypoteneuse), fourth is the error of the 90 degree spot drill versus the 82 degree true angle of the head.

These numbers will sit the head flush with the theoretical max diameter. According to the web site given, the heads will typically be a tad smaller in diameter (the edge is not sharp) and so the bolt will sit a little less than flush.

I've no idea what the tolerances are on these bolts anyway to know how these errors compare to expected errors anyway. This not to mention how accurately will the 82 degree countersink finish the hole either? We can go on about what's the runout on 3 separate cutters to spot drill, drill, and then countersink, yada, yada, yada.

As I say, I like Geof's method. I think it will save some time and effort!

Best,

BW

I counter sink on my haas,Im using er 40 collets to hold my drill and counter sinks,and if i have a problem with that then i grind a flat on the counter sink and drive it home.
Also those ma ford 6 flute suk!!
I use the o em zero counter sinks,has 1 hole thru it.I never have trouble with counter sinking with those.
Another thing i did was take and draw out a 80 deg counter sink,on cad.
And then drew some lines in 1/8th increments in the vertical direction,then i took and measured the distance across at those incraments.I usualy add .01 and im good.gl

this may have been said already, but if your csink is slipping up in the chuck why not just push it all the way up to begin with?.

all my drills, reams, c'sinks etc, get put as far up as they can go. it cant slip if its bottomed out in the chuck. if the shank on your c'sink is to short to reach the bottom of the chuck then press it againt the jaws or put a spacer behind it

I've had good luck with GARR Carbide Spot drills...They make both 90 and 82 deg. The 90's are a 1 to 1 relationship so if you need a 1/4 inch diameter, program .125 dp........When touching tool off raise up for your flat....about .002 for 3/16, .004 for .25, .008 for 3/8, .016 for 1/2".....You see the pattern? The web thickness about doubles for each fractional size increased.

The very best countersinking tool in the world. (imho)

I've had it over a year and never changed the carbide bit thru 100's of countersinks, 1" in dia. in hot roll 1/4" mild steel. This thread reminded me to order another blade for a spare just in case. Many thanks to you guys, and here's a sample of the tool, bit, hole and a quarter for size. Really easy to set up the depth since it stops cutting on it's own if you use your quill stop. I usually set it high, hit the hole wide open no mercy, insert the bolt, measure the difference, then add it on the knee dial, repeat to confirm consistant result.

http://www.stealthdumptrucks.com/counterbit.JPG

It's called "Counter-Bit", ade by Vernon Devices, Inc. Link below:
http://www.vernondevices.com/counterbit.htm

eBay store: http://stores.ebay.com/Vernon-Devices-Specialty-Tools

Did some experimenting today and found that for 1/2" 90 and 118 degree Keo HSS spotting drills held in a chuck that the calculated 1833 rpm and 7.3 ipm worked great - no slipping, consistent depth, nice cutting - all was fine. However, the only 82 degree spotting drills I could find are Melin NC cobalt. These are _much_ longer than the Keos. In a chuck the 1/2" would start chattering before reaching full depth. However, when stuck way up in a collet all worked fine at the same speed and feed. The countersinks are going to be just for the drill press from now on. Thanks for the suggestions.

I use a home-made aid for setting c-sink tools in a CNC.

It's simply a piece of round stock that has a hole drilled thru it, and a c-sink at one end. The aid will allow you to set/reset your tool reliably. The tool length will be off by a certain amount every time, depending on the length of your setting aid. But you just need figure that number out once fo that particular settig aid. I try to make mine so that number is an even 1.000". So, if you put a c-sink with a pefect point on it into my aid, the point comes 1.000" short of the bottom of the aid.

By setting my tool in this thing, I am setting to the cutting edge instead of the tip.

I easily attain +-.005 depth on my c-sinks this way (on the first hole).