Countersinking

[wildcat]

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.

[Geof]

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.

[wildcat]

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...)

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

[Geof]

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.

[wildcat]

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?

[mrainey]

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

[lerman]

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

[Geof]

Originally Posted by wildcat 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.

[cadman]

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.

[wildcat]

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.

[BobWarfield]

Originally Posted by mrainey 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.

[fpworks]

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