What's new
What's new

What is the most efficient way to cut a counterbore?

F35Machinist

Cast Iron
Joined
Nov 3, 2021
Location
California
As the title suggests, I'm curious what people's opinions are on this subject. I bore almost all counterbores by helical interpolation with an endmill after drilling the hole. Is this the fastest way or perhaps one of these other options:

1. drill thru hole, drill counterbore, finish with endmill
2. drill thru hole, drill counterbore, flat bottom drill to finish
3. same as above, but drill counterbore before thru hole
4. drill thru hole, use counterbore tool
5. Custom drill/counterbore combo
6. something else?

Which is the fastest option? Second fastest? Material is 6061 aluminum. Does the answer change if the material is 316 stainless? Assume a 2.5 second chip to chip.
 
C'mon, you know the math is gonna be different depending on how many per part and how many parts. I think drilling is the cheapest metal removal method by volume so lots of options that you've outlined.

If you were doing a million holes a year, a custom form drill with the drill, counterbore and maybe even a chamfer at the top, would make perfect sense. One tool, stab the holes as fast as you can push the material out of the way.

After that, maybe an old school counterbore cutter so you're not wasting cycle time interpolating. Drill the primary holes. Chase with the counterbore.

If it's normal 50-100 parts, obviously do what you're doing.

If it's fewer parts, I sometimes even use a 1/4" drill to stab a pilot hole and then 1/4" 3-flute to circle-interpolate both the counterbore and "drill holes". Using that method, you can do multiple sizes of finished holes but, only change tools twice (once for the drill, once for the 1/4" 3-flute).
 
C'mon, you know the math is gonna be different depending on how many per part and how many parts. I think drilling is the cheapest metal removal method by volume so lots of options that you've outlined.

If you were doing a million holes a year, a custom form drill with the drill, counterbore and maybe even a chamfer at the top, would make perfect sense. One tool, stab the holes as fast as you can push the material out of the way.

After that, maybe an old school counterbore cutter so you're not wasting cycle time interpolating. Drill the primary holes. Chase with the counterbore.

If it's normal 50-100 parts, obviously do what you're doing.

If it's fewer parts, I sometimes even use a 1/4" drill to stab a pilot hole and then 1/4" 3-flute to circle-interpolate both the counterbore and "drill holes". Using that method, you can do multiple sizes of finished holes but, only change tools twice (once for the drill, once for the 1/4" 3-flute).
We can assume for the purpose of the exercise that the quantities are infinite. I was mostly curious if there is some fast way to make counterbores that I haven't tried. In real life, most of my quantities are small so I will keep doing what I'm doing but I've never tried a step drill for instance and I'm sure many others haven't either. The question is not a "real world" problem.
 
I don't think you can beat a single tool for efficiency. You could get a drill/counterbore combo and do it in one shot. With off the shelf tooling, would be drill and flat bottom drill or endmill plunge with the correct size. That being said, I do the same as you, drill and then interpolate with an endmill. Drill hole first gives room for coolant and chips. I could be wrong, but I think actual counterbore tools are holdovers from old tech and I don't think I've ever really seen shops use them anymore. It was an easy way to position clearance features that isn't really needed anymore. I'm sure there's exceptions, like maybe certain shops or how things are done, but for general machining, I don't know anyone that uses them.
 
For a production part a step tool often makes best sense.
Even a homemade one with spinning a drill on a surface grinder and clearances by hand with a bench grinder.
Agree it takes some practice to make the OD clearance on the drill portion by hand.
 
Last edited:
6061? lowish qtys...........I drill and straight to the endmill........just feed to depth and mill(no helical).............large qtys...........drill and then plow with a stubby flat bottom drill............I push it hard so the chips won't wrap around the tool.........I do thousands of holes this way..............these are CB's after all............99.99% of the time the tolerance allows for quick and dirty results...............
 
There are some variations that can help decide on average though,
for instance sometimes the counter bore is extremely deep.

My usual-

I slightly undersize drill the counter bore first to a depth enough to leave a chamfer on the smaller through hole.

Then drill the smaller through hole, counter bore material removed so I rapid down to within .020" from bottom before starting drilling,
and only peck clearance if needed up to bottom of counter bore depth.

Then rapid end mill down into counterbore within .020" from previous counter bore drill angle bottom,
then helix down to depth, and then out to diameter.

Previous through hole allows coolant and chips out the bottom of through hole.

If its a tapped hole instead of through, I tap it before milling so chips aren't clogging the c-bore or the tap drill hole, then mill.

Just my process out loud. :D :cheers:
 
As the title suggests, I'm curious what people's opinions are on this subject. I bore almost all counterbores by helical interpolation with an endmill after drilling the hole. Is this the fastest way or perhaps one of these other options:

1. drill thru hole, drill counterbore, finish with endmill
2. drill thru hole, drill counterbore, flat bottom drill to finish
3. same as above, but drill counterbore before thru hole
4. drill thru hole, use counterbore tool
5. Custom drill/counterbore combo
6. something else?

Which is the fastest option? Second fastest? Material is 6061 aluminum. Does the answer change if the material is 316 stainless? Assume a 2.5 second chip to chip.
And to answer your question of, you helical interpolate the bore, that is slower, and uses the tip of the end mill cutting downward, not optimal cutting conditions for end mills, it's slow, I try to avoid helical ramping into material because it's slow.
2 cents.
 
For infinite quantities, a custom step drill is the best. If you countersink both the top of the counter bore and the drilled hole then it gets even better. The downside is the chip gullets get rather small for the drill so you really want to make sure the drill is ground correctly for its size. I know it's wishful thinking but I have wished for it many times. Did a lot of those holes on pre cnc turret lathes.

The first tooling task I did past lever pusher was grinding 1/8" step drills for the counterbored holes in 1/4" 304 rods I was making. The owner/toolmaker hated doing it so was happy to have me do it. That was the first toe in the door of tool and die making for me. Instead of 5-50 holes per drill I was getting over 200 with the ones I made.
 
There are some variations that can help decide on average though,
for instance sometimes the counter bore is extremely deep.

My usual-

I slightly undersize drill the counter bore first to a depth enough to leave a chamfer on the smaller through hole.

Then drill the smaller through hole, counter bore material removed so I rapid down to within .020" from bottom before starting drilling,
and only peck clearance if needed up to bottom of counter bore depth.

Then rapid end mill down into counterbore within .020" from previous counter bore drill angle bottom,
then helix down to depth, and then out to diameter.

Previous through hole allows coolant and chips out the bottom of through hole.

If its a tapped hole instead of through, I tap it before milling so chips aren't clogging the c-bore or the tap drill hole, then mill.

Just my process out loud. :D :cheers:


I like this. I typically have machined the counter bore before the tapping thinking it would help with the tapping, but the chips possibly getting down in the hole to be tapped makes sense. The drilling only of both the tapped hole and counter bore would pull the chips out...hmmm. Need to remember this
 
We can assume for the purpose of the exercise that the quantities are infinite.
Your screen name implies you've done F35 machining. In that case, something like exterior panels and doors would be a similar application, except now you're doing countersinks. I believe they use integrated drill and countersink tools for aircraft panels so they don't have to rely on a 5-axis machine needing to unwind, change the tool and come back to the same location a second time. Less chance for positional error.
 
On quantity a custom tool. Plunge in to depth then circular interpolate for counterbore diameter and chamfer on top and bottom. This is for parallel plate.
 
Speedio owner here. I spent some time playing with this on my machine with some M6 cap head counter bores.

I drill the through hole to size (even bought the correct size drill)

I then played with plunging a smaller end mill into the hole and cutting outward at constant engagement (plunging at full rapids 50,000mm of course! 😁). Try the "flat" tool path to program this in Fusion

However this took (much) longer than using a helix into the hole and a "contour" finish. The helix can take advantage that it's got a hole already, so you don't have full engagement. I tend to program about a 12-15 degrees helix with a 12mm endmill and you seem to get rid of material faster. For me it was about 2x as fast to run. No need for a finish pass.

I don't remember the exact numbers but let's say for 4 holes you need and 2-3 seconds total to drill the through holes. Then I think a bit over 1 second per counter bore? (Plus one tool change)
 
I used to make a bajillion 5" 1045 steel parts with 3" deep 1" counterbores.

I drilled 4" through with 37/64 drill then plunged a 6 flute HSS endmill. Worked great for me.

I drill and counterbore a ton of 1/2" holes with 1.25" counterbores in 6061. I should look into a custom tool.
 








 
Back
Top