Micro carbide drill help

I am curious if anyone out there is having any success drilling 6061 with micro carbide drills.

All the factory speeds are well over my 24k max and rated for copper that is softer. I need to peck drill through .1875" bar stock. So far using a maglube MQL, 24k rpm 5 ipm .019" pecks with full retract I’m getting 2/3 of the way and then breaking. My gut says take smaller pecks but I don’t want my lack of XP to kill my last 3 drills so I figure I will see if anyone has real world micro drill XP they can share.

Hmm, possible causes…
Chips left in hole (perhaps a short dwell at the bottom of each peck)
Heat (lots of lube, air, mist, )
Runout - is the stock round? Maybe centerdrill the holes first? Vee-bit or centerdrill. Tram the Z axis to make sure it’s moving perfectly straight up & down.

What are these holes for? dimension critical? Could they be drilled from 2 sides?

1 Like

I don’t drill that small but I’ve made pockets just above 1mm with a 1mm bit with a much shorter fluted length. In fact, this particular endmill is surprisingly tough in brass and aluminium. Low DOC (0.2-0.5mm) helps. Unfortunately is just shy of your depth.

Not a particularly helpful response but more one that adds weight to the theory that the shorter the thin part, the stronger the endmill.


A microdrilling video just came out on NYCCNC that I did on a Tormach.

IMO lower your peck depth or use a peck reduction. In my experience, misting was not great for microdrilling, you want to crank it way up. I would say start out with 1/3D for peck depth (wouldn’t hurt to go 1/4 to be safe) and make sure your retract isn’t super fast.

Perfect tram, proper spot, and runout sub 0.0005 but as close to 0 as you can. Check and adjust with tap method.

edit Your feed per rev is a little low at 0.0002"
Harvey Tool specs around 0.001" feed per rev at that diameter (aluminum) and Ive personally had success running 0.001" per rev with a 0.032" carbide drill

In 4140 steel, a 0.0157" carbide drill runs well at 0.0002" feed per rev to put things into scale.


I’ve got some of these:

and I can give it a shot when I get home tonight. I have some 1/4" 6061 plate I can drill into. I have 99% IPA which is what I use when cutting aluminum, (but never tried drilling aluminum with such a small drill) and RapidTap tapping fluid I can use as well if you want me to try it, but that might be a bit thick for such a small hole. I probably have WD-40 as well, if you want me to try that as well.

I do think that it is worth checking the tram of your spindle / router, as others have mentioned. If it is off, the force could be too much once the bit gets into the hole and the lateral force gets to be too much from the offset angle.

Edit: Just let me know if you want me to give it a shot.

1 Like

First off it’s crazy some times how the universe works. I just now needed to do micro drilling and it just so happens the day I’m trying it out Vince is uploading a video on it at the exact moment I need with no prior request from me.

I started at 20 ipm to get close to .001 and it ghosted that bit on the 2nd peck. I did have retract set high at like 40 ipm so that can be slowed way down and might be where I failed along with too deep of a peck and I did not spot drill.

Flat bar stock, 1 side machining, not critical as long as it is not under sized. It’s a hole to capture one end of a return spring for an adaptive reacher for quadriplegics that opens the jaws.

All help is welcome if you don’t mind volunteering time.

The reason I’m doing all this work for my friend is because his tools changed my life and allow me to live independently for the past 10 years. He has been hand drilling and making these reachers his father designed for the past 20 years to help quads and I’m getting him into CNC so he can stop killing himself manually milling and drilling these tools one at a time.Making a reacher for quadriplegics - YouTube

1 Like

Okay. I’ll watch @Vince.Fab video, go tram my spindle and give it a shot.

I just replaced my v-wheels yesterday because my spindle / Z-axis assembly shudders when cutting from left to right.

Took a couple days to get figure out recipes and ghosted quite a few of them myself too! In fact, I wasn’t able to run one of the drill in a hard material due to run-out. The high helix of the bits you have should clear chips decently but maybe thing about lowering the rpm or switching to a HSS drill. Can be much harder to hold but will but much more forgiving with run-out as they are more flexible.

Recipe 944 is a Nomad 3 running a 1/16 HSS 2F drill in 6061.
930 is a 1/64 HSS in 6061

1 Like

Okay, I apologize for the delay. It took forever** to tram my spindle. But I think it’s good.

Left to right:

Front to back:

This is a little bottle I got from TAP Plastics for dispensing the water thin acrylic solvent. It originally had a blunt needle tip, but that broke off a long time ago. I like it because it can spray a very fine jet of 99% IPA and it doesn’t use a lot, but works great.

Here is the video of 10 holes being drilled. Turn off your sound! I do not have a drill start, so I just went for it. I have a dial gauge, but not a dial test indicator, so I have not checked my runout yet. A test indicator is on my “to-get” list.

The good news is, it drilled all 10 holes without issue with just the 99% IPA coolant.

RPM: 24K
Peck Depth: 0.010"
Plunge: 10IPM
Total depth: 0.1875"

Online calculator says that is 0.0004IPR

The bit afterwards:

**Forever does not necessarily mean forever, but most likely means an hour and a half or so, because “maff is hard” when putting in shims to calculate angles.


Are you paying $6.58/ea For your drill bits?

Drillman1 has that size drill bit 10 for $9.00.


Pecking could actually be bad for the bits, especially something that small. With pecking, you’re repeatedly going from no load on the bit to some finite load in a short period of time. Which carbide especially might not like due to its brittleness. This page recommends not pecking until you hit 3X the drill diameter worth of depth:


An older thread about carbide circuit board drills in aluminum (not quite as small as 0.043"):



So after a few tests and ghosting 4 out of 5 new drills in the process Slowing down to

10 IPM
.01 peck WITH full retract
24k RPM

This seems to work reliably and so far has drilled over 70 holes through .1875" 6061 so thank you to everyone who gave input.

I have 5 more drills on the way to continue testing on my machine while my friend is up and running his first batch of tool blanks.

I am also now a huge fan of using a MQL. We installed a Maglube single pump system on his 24r and the tools are room temp after cutting. Even when taking .1875" Doc .125" Woc at 20k Rpm with a .1875 square end mill and only using a few Oz of fluid after several hours of milling. It also left no real residue or any drips on the MDF or cause any swelling. The chips and parts were dry after machining.

I have a Unist cool lubricator Jr coming for my HDM with their cool lube 2210AL and can’t wait to see how much it helps.


Thanks for the info. I use MeshCam for most of my drill paths, so I’ll have to see if I can find a good (lazy) way to implement that type of drill path.

This topic was automatically closed after 30 days. New replies are no longer allowed.