Help drill Stainless bolts

I'm pulling hair out over this and at my wits end.

Hurricane bolts (sidewalk bolts) 18-8 stainless. 3/8"-16 threads, 1/2" long. All I need to do is drill a 1/4" hole through it length wise. Problem is the hole is so close to thread minor that any work hardening and the last 2 threads get pushed out and a nut no longer threads on. If I program any amount of peck or chip break I get massive thread deformation and looks like holes walks off center line but its actually just bending the thread section. Cheap chinesium stainless.

I tried carbide drills from Mari, chipped on first part. Best luck so far is a Tin coated cobalt stub length drill from Mcmaster. I once was able to get 40 done on one bit, now I cant seem to get 5 done and just deforming threads too much.

I dont have through tool coolant which is probably the biggest detractor. I have soft jaws cut in lathe chuck to grab head of bolt and clearance over threads so as not to damage them from jaws. Center drill, then go in with the 1/4" drill. My best luck was at 600 rpm and 0.0035" ipr, now down to 450 rpm same feed and still issues.

I thought about flipping them around so threads stick out of chuck, but problem there is lengths vary by quite a bit so hard to put proper spot drill mark in without facing first and then more issues arise.

I should of just quoted turning them from solid then could drill the hole first, then thread. I have something like 150 more to do with more batches to come if I can do it.

Try drilling with two sizes, first 3/16", then 1/4". The smaller drill goes in say 1/2", then follow with the 1/4", then keep alternating. The smaller drill will not push away the last threads on the bolt, the larger drill will have little force because most of the material is already removed.

I'd stay with the coated cobalt stubs. You can try 7/32" over 3/16" if you want as much beef there before the final size, but I wouldn't go bigger than that.

Edit: Thought the bolts were longer, at 1/2" you could try in one or two ops.

You could try putting a nut on the end threads which might reduce the thread distortion to reasonable levels.

do you have coolant at the turret? If yes, you can have coolant thru. I would try a steel threaded fixture to hold them while drilling that may help the threads from expanding

I’ve modified commodity hardware many times over the years.
I’ve learned to turn those jobs down. It never runs the same way twice.

PTD cobalt screw machine length (stub) drills.
By center drill you mean a 1/4" spot drill right? otherwise that may be part of the problem if you're using an actual center drill with 60°.

Sometimes I set that kind of job on the manual mill with a 5C collet, easy to get lots of good cutting oil in there which helps a lot with work hardened stainless. Also better feel for when its starting to get unhappy before anything goes to crap.

Any chance on chucking up the threaded portion in a collet? It'll help keep the drill concentric to the threads versus the head of the bolt. I know your wall at the root of the thread isn't much, but it may be enough surface area to keep from crushing them.

A lot of good responses here. I like the idea of putting a nut over the threads to prevent them from bulging out.

The problem with previously worked stainless parts is you wont know where it was worked and stressed previously. You wont get consistency.

As far as the Center Drill/Spot Drill goes. Most center drills are 120 degree. You want a 90 degree spot drill. Your drill could be wandering off center and is getting too close to the surface.

Many different things it could be. Many different solutions. With Stainless always try to machine the best quality SS you can. It will save you money and aggravation in the long run.

Yes, using a 90 deg spot 3/8" dia, just deep enough to leave a small chamfer on the hole when done. Also helps the drill get through the straight screw driver slot in head of bolt. The end always seems to be fine and the hss spot drill is lasting great. The nut over the threads is good idea, but takes too much time. I ordered some smaller drills, will try drilling it in 2 sizes tomorrow.

They appear to be rolled threads so Im sure there is some work hardening there. I do have coolant at turret, but not much pressure thats going to do much on a 1/4" drill bit.

I think the 2 drills will work, and seems so simple idea, but when you're in the deep of it and getting frustrated its hard to think of those some times.

JP Machining said:

I think the 2 drills will work, and seems so simple idea, but when you're in the deep of it and getting frustrated its hard to think of those some times.

Click to expand...

I'm good with simple stuff, it's the complicated bits that leave me confuseled.


Be sure to not dwell if you have to do "long pecks", avoiding the work hardening at the end of the drill is important. This also means changing out the drills before they get too dull.

Takes some round stock, chuck it up, and cut some female threads so you can screw the bolt in to hold it. When done machining you have a nice hex head to get a wrench on to loosen to remove. Never pull the threaded round stock out of the chuck until you are done running the job. Since you are bottoming the heads onto the round stock your datum will only vary as much as the head thicknesses. I would rather locate off the threads for center vs the head any way I could. Just my 2 cents.

2 diameters deep without a peck or tsc is certainly pushing it with ss.

A pneumatic impact driver with a butterfly lever would sure speed up driving in and removing the parts if you're doing enough of them.

This is what these bolts look like McMaster-Carr

Slow it down and use a lot of coolant, 200 rpm slow feed and flood it to wash the chips away...Phil

I have drilled my share through roll formed threaded items. Find a vendor nearby with Schtluk cutting fluid. I am told it works wonders. I can't buy it around here. I just buy more tooling and toss when timed out.

Lots of times when I have had problems with thin wall stuff swelling I grab a gun drill. Just short pilot bore with a stub then plow through with the gun drill.

I've made a couple of different sized emergency collets with threaded bores. Screw the bolt in and then clamp the collet. I think this will give better heat transfer from the bolt to the chuck and will help reduce overheating the inner end of the bolt while drilling.

I don't think 2 drills will work very well, it'll be a bitch on the second drill. Run slower rpm and heavier feed most of the way, then reduce the feed for the last part of the hole.

HuFlungDung said:

I don't think 2 drills will work very well, it'll be a bitch on the second drill. Run slower rpm and heavier feed most of the way, then reduce the feed for the last part of the hole.

Click to expand...

If he's using a spot drill to get an over 1/4" entry, I don't think it'll be too bad. Might need to slow the RPM for the second drill, I'd not known this was a slotted screw from the OP. But still, I've done similar processes and not killed the larger drill.

Used to do alot of this stuff a long while ago. 500-3000 at a time, most of bolts came from copper state some mc mastercarr. basically all the same bolt stock 18-8.

you said hex head 3/8 at 1st then you link shows a 5/16 slotted.

you must center drill it enough to make it even on the slot or the dimple in the head, if its a hex head I generally skim it with a facing tool, the outside edges of the drill cannot touch a interupted cut or you scrap drills extreamly fast.
if you can face the head a Hi-roc will work perfectly and last a ton of parts 100-200 easy with rich coolant slow rpms.

those who said use a collet or a threaded fixture are right on. if your locating on the hex your screwed. reason being is the run out and while if might be good where you start, its crappy where you finish and thats what reduce's drill life 10 folds.
The part needs to run perfect true.
Another thing to do is make sure your drill is centered with in a few tenths anything over a .001 your drill will fail quickly.
I use the old brooke field adjustable V block holders.
I prefer HUFlungdungs way with the emergency collet on very thin walls, sometimes we had to us a boring bar to bore them close depending on the cell out and thread dia.

Generaly Im at 500 RPM somtimes i'm at 1000 but thats rare with that material on drilling.

one other thing if your not breaking bown the drill corners by one of those high dollar made for stainless solid carbide stubby twist drills from Mc matercarr. They actually work extreamly well (alot better than I ever thought) but your need to have run out less than .001 on the entire part cant have uneven end surfaces but your feed rate and rpms can be doubled.

If edges are chipping on your drills...try a nice quality HSS drill. Run it slow with a high end feed, gotta see where chips are coming out best. No exact speeds and feeds as it's outside the norm, but this has saved my butt on a few troublesome SS jobs. Including a recent 304 sheared plate job with thousands of holes drilled and tapped. One or two plates with cobalt drills, less then one plate with carbide and hundreds of plates using simple HSS drills. Yes it ran longer, but it ran.

Longer as compared to 304 True bar I priced the job with and ran half till no longer available so HAD to make the Plate work.
I found this out years ago when having to cross drill threads and holes in Aquamet 22 (Nitronic 50) by hand. Afte busting all the good drills on a job that hand to go I fell back to the old HSS draw of drills and to my surprise the job moved forward very nicely...actually faster turning dead slow and leaning hard on the drill to produce chips...easing up as I broke through.

In short...if it don't work...change it till it does.

I did not know about the slot at first. This probably is already work hardened on the head. Tool wear will be significant. All it takes is 1 cut with a dull drill to ruin things.

Sharpe new drills is key. Change them before they wear out at all.