What's new
What's new

Technique For Drilling Small .043 Inch Holes in Invar

morsetaper2

Diamond
Joined
Jul 2, 2002
Location
Gaithersburg, MD USA
Invar: Drilling Small .043 Inch Holes

Machinist at work is out for an extended period. I'm a mechanical engineer, but when odd-ball fixes need to be done I get tapped to do them when its an emergency and machinist is out. I'm no journeyman machinist by any means. Competent in alum, steel, brass, some stainless, various plastics, etc.

I have zero experience working with invar.

I believe the material is invar 36 FM. And the parts are nickel plated. I need to drill 3 small .043 diameter holes in five parts (15 holes). These are expensive optical mounts so I don't want to ruin them.

I'll be using .043 carbide drills. Exact hole size and position is not critical. I read some posts about drilling invar. But none were for drilling small drill holes. Read that it work hardens. I'll be drilling into a tube that is hexagonal on the outside with a round ID. Where the hole needs to go wall thickness is about .100 thick.

Any advice so I don't screw this up? Work will be done on a Bridgeport clone.

Drill RPM for .043 carbide drill?

Drill RPM for .043 HSS drill?

Coolant: oil or water based?

Will it act unusual when drill breaks through to ID?

Thanks.
 
Last edited:
And adding....

So I planned to spot each hole w/ a #0 center drill (.032 tip). And since it work hardens I know I don't want the drill to dwell. Should I peck or just push through?
 
I was told soap bar on the drill, it was an instrument maker I knew, never tried it as I have zero Invar on my junk shelf, it did work for bismuth, what that was for I know not but chemists ask for some odd stuff
Mark
 
I've done a fair amount of Invar/Kovar, although it's been a while. I would not use carbide drills (especially when breaking through a tube), buy some quality cobalt split-point stub drills.

Sharp wins, so change drills if you notice any dulling. You'll want a sensitive "feel" when breaking through the tube (don't wind up jamming the drill down on breakthrough, you'll snap the drill). Use a good oil, around 3K rpm, and don't dwell - either cut, or withdraw the drill.

Think gummier 3xx stainless for behavior, not too bad to cut.
 
Glad it's not me...small pecks, light downfeed, lots of coolant, clear the chips, small pecks, clear the chips...you get the point lol.

Technically speaking a Bridgeport is just not going to have the rpms and feed control to use carbide drills. We put .041 holes about .400 deep in superalloy castings at 12000 rpm, .001 pecks l, and like 1 ipm. Sometimes you get 8 castings per bit, sometimes you don't get one lol.
 
Maybe it's me but I would not want to use that small of a carbide drill on a manual machine, hopefully you have a steadier hand than I do. Good luck!
 
OK so common theme here is carbide drill not preffered in a manual mill. Not sure if we'll have cobalt drills? What about using plain ole HSS?

What kind of rpm w/ HSS?

Use water base coolant or oil w/ HSS?
 
Buy some cobalt stub split-point drills.

Do it.

I command you!

Lord Emperor Zog, Ceti Alpha 3

I am partially retired. I only work Mon, Tue, & Wed. I get a desperate call this aft from the engineering mgr (my boss) that the assy of one portion of a laser module has stopped. And can I come in and drill these holes into these optical mounts. Machinist will be out for a period.

So I'm going in tomorrow to work on these parts.

So I start asking questions about the parts and we get a tele-conference going, I'm looking at the CAD models. And then it becomes clear. This isn't as easy as it sounds. I didn't have time to order anything. I don't know if there is a sensitive drill chuck available. Although I know our machinist does these kinds of things frequently. But he is very experienced in all of this... me, not really.

So I'll be walking in kinda cold on this having never worked a part (5 parts & drill 15 holes) made from invar. Kinda not looking forward to it, esp on my normal day off. But if I can pull it off I'll be a hero at least.
 
Understood. See if there's an industrial supplier in your area that has them, the reason I'm pushing them is they're better suited for what you're trying to do that either "normal" HSS or carbide.

The split point will cut better in a high-nickel material than the chisel (blunt) edge of a regular drill, so less prone to work hardening. The harder cobalt alloy will retain edge condition better than HSS too. Both are wins for Invar.

Last, I actually suggest not using the sensitive chuck. With smaller drills, sure, but .043" is big enough that will a little care the direct leverage on a quill will give better load application, and again, with a nickel alloy you want constant load to ensure cutting. With a sensitive drill, you'll have to lean on it a little more, which can make control trickier, especially during breakthrough.

But do what you gotta do. Good luck and let us know how it works out.

Edit: I just remembered that at that size, there's likely no split point (they tend to start at 1/16" and larger), but the higher hardness of cobalt is still a benefit if you can get them.
 
Just glad I don’t have to do it. My Electro-Mechano will spin it faster, but I think the Royal in the Aciera high speed head has better feel. Ideally I would want a couple of practice goes with each, probably with some sort of chlorinated cutting fluid. Once upon a time either Dumore or Boley made a really nice sensitive drilling machine. Far better than either of the above. I tried to find a picture of it and failed.
 
Hi morsetaper2:
If you are going to do this on a Bridgeport (or any manual mill with a quill stop) you will have best success if you use the quill stop to peck the drill down a few thou at a time.
You have to get into the rhythm of lift the quill, advance the stop, pull the quill against the stop, lift the quill, advance the stop, pull the quill against the stop etc etc.
Since you need to keep cutting pressure on the tip in Invar (but not too much) it's nice to have a stop against which you can feed the drill aggressively, but never overshoot.

The other thing you want is your favourite magic goo.
Invar likes a wet tool...you may interpret that any way you like:D, but the take home is to keep it from getting dry and rubbing painfully.
I'm a RapidTap fan, but you may pick from a wide offering that's out there.

Third, you need to keep the chips from accumulating around the hole and having one drop in by accident...it will smear at the bottom of the hole, work hardening it and making it really hard to get going again.
A gentle air blast rigged with a foot pedal is ideal, but you may not be able to justify rigging something so elaborate.

Fourth, all of you who have said "Keep the drills SHARP" are spot on...this shit makes gummy chips and is abrasive and workhardens with enthusiasm.
Whether you have to buy lots of drills or you need to get really good at grinding them doesn't matter...they MUST be as sharp as you can get.
If you push a drill even for a moment after its point is gone you'll snap it in a heartbeat...so resist the temptation to just finish that last bit of hole while ignoring the unhappy noise coming from the drill.

Other than that, those who compare it to 316 SS are right on...it's very similar.
You can do this...it's not rocket science...you just need to pay attention to the proper details.

Good luck with it...oh yeah, and buy lots of drill unless you've got an Optima or equivalent drill grinder.

If all else fails, Invar can be EDM machined without problems, so if you can find a guy with a sinker, you can offload the whole problem.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Oh yeah, one last thing:
The burs you make on the exit side of your holes will be epic.
You need to have a plan to get rid of them.
Plugging the main bore is dangerous...you may never get the plug back out once the burs lock it in.
 
McMaster usually delivers next day in most locations. Make sure you indicate the drill in no mater what you use to hold it. You want next to no runout on a drill that small.
 
Well I threw in the towel on this. Nothing but broken drills. Meanwhile, machinist covid test is negative. So he'll be in Monday to clean this up.

Better him than me. :D
 
Well I threw in the towel on this. Nothing but broken drills. Meanwhile, machinist covid test is negative. So he'll be in Monday to clean this up.

Better him than me. :D

At least you tried, not an easy job even for someone with a lot more experience than you. Little delicate tools, manual machining and exotic materials are a bad combination.
 
Hi again morsetaper2:
Did you try peck drilling it?

Cheers
Marcus

Yes I did. I was advised by everyone to peck drill it. But I peck drilled by hand, hadn't read your note about using the stop. By that time I had given up.

Called machinist on phone asking for advise, he said lots of lube, but I was running way too fast at 2800 rpm. Said I needed to be down around 500 rpm for HSS and a bit higher w/ carbide drill. Still broke carbide drills and/or dulled HSS drills. I just don't have the speeds and quill pressure right and am hesitant of ruining those $800 optical mounts. So just backed off, I just don't have experience w/ invar to have a good feel for it. And the drills are just tiny.

But thanks all, for your contributing advice.
 








 
Back
Top