Spot Drilling and Countersinking

Hey guys,

I am newer to the field so as always, sorry if this is a stupid question.

What is the difference between using a spot drill versus a countersink? Could I just spot drill deep enough to spot and CS in one quick operation? Or are there reasons (geometry of the drill or whatever) that you want to spot, drill, then use specifically a countersink cutter?

Also, they advertise using countersinks for chamfering as well. Any pros/cons using a countersink to chamfer versus a standard chamfer bit?

Thanks in advance guys.

MRudisill said:

Hey guys,

I am newer to the field so as always, sorry if this is a stupid question.

What is the difference between using a spot drill versus a countersink? Could I just spot drill deep enough to spot and CS in one quick operation? Or are there reasons (geometry of the drill or whatever) that you want to spot, drill, then use specifically a countersink cutter?

Also, they advertise using countersinks for chamfering as well. Any pros/cons using a countersink to chamfer versus a standard chamfer bit?

Thanks in advance guys.

Click to expand...

Lots of variables.. Spot drill or center drill? A 90deg spot works well for spotting and c'sinking for threaded holes, and/or clearance holes, but only for hss/cobalt, you need to match the drill point (or less, but not sure) angle for solid carbide (if a spot is needed, depending on length of drill). A FHCS has an 82deg angle so need a countersink for that, metric fhcs are 90 deg so you could use a spot and use for c'sinking if the spot drill is big enough. Also, different kinds of spots. Don't know the name, but they make ones that have like a chisel point, not really flutes. We use a 90 deg drill/mill, like this -

https://www.mscdirect.com/product/details/06298731

BUT we only cut aluminum and brass. Not sure how well it would work for anything harder. A plus, it can spot, light chamfering, and limited profiling if your parts are thin'ish.

I've heard a lot of guys say "the customer won't notice the 3deg difference" for countersinks and they just use a 90deg spotting drill for them.

Personally? I 45deg chamfer with the 90deg spotting drill where possible (make the spot larger than the finished hole) especially for tapped holes. I use a single flute countersink for any holes that call for a specific angle or make it clear they are for a screw head clearance on the print.

There are also adjustable options like Harvey Tool's inserted chamfer/countersink cutter. I think I've seen a dozen or so companies that make something similar and over all it is cheaper than having a draw full of countersinks of different angles and sizes.

Rick Finsta said:

I've heard a lot of guys say "the customer won't notice the 3deg difference" for countersinks and they just use a 90deg spotting drill for them.

Personally? I 45deg chamfer with the 90deg spotting drill where possible (make the spot larger than the finished hole) especially for tapped holes. I use a single flute countersink for any holes that call for a specific angle or make it clear they are for a screw head clearance on the print.

There are also adjustable options like Harvey Tool's inserted chamfer/countersink cutter. I think I've seen a dozen or so companies that make something similar and over all it is cheaper than having a draw full of countersinks of different angles and sizes.

Click to expand...

I don't recall the details, but had a print once (aero or medical) that had a reall oddball angle, like 101 or 102 degrees. I was like "oh a 100 will be fine" Nope, had to have quotes for custom countersinks to "make it to print".

Mike1974 said:

I don't recall the details, but had a print once (aero or medical) that had a reall oddball angle, like 101 or 102 degrees. I was like "oh a 100 will be fine" Nope, had to have quotes for custom countersinks to "make it to print".

Click to expand...

I've had a few of those. Just 3D contour it with a ball or bull mill.

Also had a part one time, OLD print, that called out a shallow 3" drilled hole, with a 118 degree point on the end, had to 3d contour the 118 degree point in.

As for spotting, I don't do it anymore, at least with a traditional spotter. I only use split points, so if I'm running a stubby drill, I'll drill in .050 or so at a light feed, and then pile drive it. Jobber length, I'll spot with a shorty, or if its aluminum, you can get away with using the jobber to spot for itself, just feed it light, then punch it.

As for counter sinking, chamfer tool, hit it at the end, or before tapping.

You can also buy spot drills with an 82 degree angle if you want to drill and countersink in one operation, just don't mix them up with your 90 degree spot drills.

Bobw said:

I've had a few of those. Just 3D contour it with a ball or bull mill.

Also had a part one time, OLD print, that called out a shallow 3" drilled hole, with a 118 degree point on the end, had to 3d contour the 118 degree point in.

As for spotting, I don't do it anymore, at least with a traditional spotter. I only use split points, so if I'm running a stubby drill, I'll drill in .050 or so at a light feed, and then pile drive it. Jobber length, I'll spot with a shorty, or if its aluminum, you can get away with using the jobber to spot for itself, just feed it light, then punch it.

As for counter sinking, chamfer tool, hit it at the end, or before tapping.

Click to expand...

I worked with a guy who used to lightly spot for drill & tap, drill, then come back with the c'sink and set his R plane so the tip dropped into the hole and only fed in as far as needed. Not sure it really saved time on an old ass Hurco with a umbrella changer calling the tool twice.

kenton said:

You can also buy spot drills with an 82 degree angle if you want to drill and countersink in one operation, just don't mix them up with your 90 degree countersinks.

Click to expand...

I did not know that. Thanks for the heads up.

I have never understood why the use of 90 degree spotting tools when most drills are 118 and greater tip angle.

I usually spot shallow first (spot diameter smaller than the drill diameter), then drill, then chamfer with the spot drill or countersink last.

I use a 90 degree spot drill. Spotting shallower then the Od of the drill makes the angle difference (90 vs 118 or 135) irrelevant, If anything it provides a slight ramping in of the drill while still letting it find center. I get fantastic tool life using this method. Because most of my work is 1 off stuff, tool life is more important than shaving a few minutes off a cycle.

Many people don't like using a 90 spot for a 118 drill. IMO they have problems because they spot bigger then the drill. This puts lots of stress on the outside corners of the drill when you plunge in, causing them to dull or even break quickly. Spotting shallow solves this because the initial stress is now placed closer to the midpoint of the flute/working edge. Because the angle is different, the chip starts out small and "ramps" up to the full cut.

TheBigLebowski said:

I use a 90 degree spot drill. Spotting shallower then the Od of the drill makes the angle difference (90 vs 118 or 135) irrelevant, If anything it provides a slight ramping in of the drill while still letting it find center.

Click to expand...

This method helps alleviate the contact between the "corner" of the drill or the intersection between the angle and the OD of the drill but it does not alleviate the initial contact of the work and the angle of the drill. does that make sense?

I believe the angle is relevant because the goal is for the tip of the centered hole and the tip of the drill to make initial contact first. what causes a drill to initially not drill centered is runout and that tiny little web or flat spot at the tip that can cause "walking", that is why split point tip drills don't require a center.

You always want to spot shallower than the diameter of the drill regardless of angle.

Hasn't this topic been beaten to death over the years here already?