What's new
What's new

Any advice for 1/32" Carbide Drill at 10x Depth?

Paul Mark

Plastic
Joined
Oct 6, 2015
Location
Mableton, Georgia
I could use some advice for using a 1/32" carbide drill (2 Flute Carbide, 0.400" Flute Length). I have a specific job that I use this drill for but it's only a couple times a year so I don't have a lot of data to determine what parameters I need to modify.

The job details is drilling Cast Aluminum Mic 6 Plate that is 0.3125" thick. Each plate requires about 800 holes. Coolant is Trim Microsol 585XT at 10%. Machine is a 2008 Fadal 4020 with 10,000 RPM Spindle.

A couple years ago, I used a Feed of 9 IPM and 10,000 RPM with a peck depth of 0.030" and that would last for about 2,000 holes but then the drill bits started breaking more often. So I lowered the feed to 6 IPM and that worked for a while but now it's breaking the bits again after drilling about 1,000 holes.

I know it's a lot of holes but for it to break after an hour of cutting time doesn't seem right.
 
We made some very similar sounding parts: vacuum hold down plates, tooling plate, etc. Make sure you're using collets and not drill chucks and choke up on all drill shank you can. Check the run-out. Maybe even consider spotting all the hole locations first. You're trying to avoid the drill walking at all before it starts. The point gets a little wear, it wiggles on entry and then it's all over.

I'd also consider backing off the RPM. Yes, small bit, wants RPM, etc, etc. If the tip starves for coolant at all, it's going to melt, pack with aluminum and then it's over. 7000-8000 RPM might be enough to make it a more reliable process.
 
For sure runout is key. If you're using ER collets you will want to make sure you're using one that's exact size to your drill shank.

It could be worthwhile to get a loupe/microscope and inspect the drill tips before they break, to see how they're wearing. I haven't worked too much with cast aluminum but I'm pretty sure I've seen it mentioned somewhere that it can be abrasive.

Another idea would be to start the process with a shorter drill and go in with the longer drill to finish the holes.
 
Agree, runout is key. Have you measured it?

I've had the best luck with tiny 1/8 shank drills in a good quality solid 1/8 side lock holder, believe it or not, versus any Er or similar collet.

Shrink would be nice too, but shrink 1/8 tool holders are a proper PITA to get the tool back out after it breaks.

I've had the best luck with MA Ford drills. What drill brand are you running?
 
Eh, at that size, a super conservative 100sfm is about 12k rpm.

For ~80sfm/10000rpm and 1/32" drill, I'd just use HSS or Cobalt at the same speeds and feeds. Less likely to break imo? dunno what your tool life would be in mic6 but should be 1000-2000 holes. Maybe just change it out every part just in case.

What do you do when you break a drill? Is the part junk?
 
Thanks guys. I should have mentioned that I'm using a Maritool ER16 Collet and the bits have a 1/8" shank.

I tried measuring runout at the tip but it flexes too much. The runout on the 1/8" shank was 0.0001"

The part is for a thermoforming mold and is 5/16" x 24" x 24". I use a vacuum fixture to hold it while machining the mold features (takes about 6 hours) and then I'll clamp it to do all the drilling. Depending on which feature the drill breaks at, then I have to scrap the part. And trust me....you don't want to forget to turn off the vacuum fixture while drilling the through holes or else you'll end up with coolant all over the place.

I had been using SGS but I also have some MA Fords. The SGS rep actually responded to me this afternoon and suggested eliminating as much pecking as possible and doing the peck cycle such at, 5xD, 2xD, 2xD, 1xD. I tried that but it immediately broke the next bit.

Currently, I'm trying a hybrid approach based on all these suggestions. Right now the drill is running at 8,000 RPM, 6 IPM, 0.070" First Peck and 0.050" for all other pecks. So far it's made it through the first plate of 800 holes and the second plate is running now.
 
For tiny little circuitboard drills with standard 1/8" or 3mm shank, I've found Kyocera to be absolute little beasts. And cheap, too.
 
Most are going into a recessed groove that was made with a 1/8" Diameter Ballnose but some are going in on flat surfaces.
What kind of surfaces are you entering with these drills? Are any of them slanted?

Methinks you might be getting into a bit of walking and fatiguing the life out of the little guys like Donkey mentioned
 
Thank you guys for the help. The new settings of 8,000 RPM, 6 IPM, 0.070" First Peck and 0.050" for all other pecks has worked the best. It went through 2,400 holes and then broke. The next drill after that only lasted 10 holes and the only thing I noticed that was different was I probably had the flood coolant pressure too high which I assumed caused the drill to walk on entry. Kind of makes me wonder if the coolant pressure was what was causing the issues to begin with.
 








 
Back
Top