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:

morsetaper2

Diamond
Joined
Jul 2, 2002
Location
Gaithersburg, MD USA
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?
 

thermite

Diamond
Joined
Sep 21, 2011
Location
Sol, Terra
I believe the material is invar 36 FM.

"FM" is the Selenium "doped" "Free Machining" version. and as good it gets.

Such as that is.

Page Not Found | All Metals & Forge Group

Have had Invar goods but have never had to machine it.

I'd expect it to have characteristics similar to Nickel-Aluminium Bronze, which I've worked plenty of.

That responds well to uber-uber sharp HSS-Cobalt / Stellite - slicing not bulldozing. M.A. Ford's best drills?

I would expect nasty exit into the ID. Not sure how practical drilling under size then reaming would be.

A) How did the LAST successful hand do it under your own roof, on the equipment and tooling you already have to-hand??

B) If no "useful local history" available in-house? Can you not lay-hand on some material with which to TEST your tooling, speeds, feeds, coolant, to vet your chosen approach BEFORE applying it to the final-final on already value-add parts?

That last point would be my highest priority if the parts are the least bit critical. Even if you have to purchase some "scrap" to try it out on.
 

boslab

Titanium
Joined
Jan 6, 2007
Location
wales.uk
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
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
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.
 

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
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.
 

car2

Stainless
Joined
Sep 19, 2009
Location
Apex, NC
Sensitive feed drill chuck in a good collet, spot with short carbide drill, drill thru with a short cobalt drill (can probably use a carbide drill with the sensitive feed, but as mentioned, they can grab when breaking thru).
 

CITIZEN F16

Titanium
Joined
May 2, 2021
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!
 

morsetaper2

Diamond
Joined
Jul 2, 2002
Location
Gaithersburg, MD USA
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?
 

thermite

Diamond
Joined
Sep 21, 2011
Location
Sol, Terra
80 years old, and still functioning like a child.

Regression, or attained his limits early on? The world may never know.

Or care.

Not so. We still care aboucha a LITTLE bit.

Scientific curiosity if nowt else.

Wondering if anyone EVER recovers from TDS?
 

morsetaper2

Diamond
Joined
Jul 2, 2002
Location
Gaithersburg, MD USA
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.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
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.
 

thermite

Diamond
Joined
Sep 21, 2011
Location
Sol, Terra
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 this 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 frequebtly. 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.

.043 is a #57 HSS drill. Fair certain I have ONLY one CTD "jobbers' prolly M42, and "maybe" one extra-long under roof. You won't have the kind of sharpener needed under-roof, so unless M.A. Ford or a Swiss outfit, you'll want no fewer than three drills to insure you don't push 'em dulled?

BirdPort clone is nice for positioning, but short on feel and RPM.

I can toss a variable-speed Electro-Mechano W-105 sensitive drillpress in the SUV and lend it to yah at yer carpark, but it absolutely, positively needs a prick-punch, then decent center punch mark for each hole.

Or a spot CNC'ed to place accurately? But if you had THAT.. you could JF drill it.

Fair chance you could scrap (at least) one part if you haven't the "feel" for the material?

Page Two:

These holes might happen to need tapped for Metric screws, next?

TIGHT f**kers, if so. #55 for 50%, #56 for 75% ...# 57 for bust your taps in this material?

If you were not previously aware of it, the most common characteristic shared amongst top-teir craftsmen is to make difficult things look easy.... so the clever devil is a SERIOUSLY "tough act to follow".

If your Machinist has been "JFDI" on this tasking, no whimpering?
It could be a trap!

Embarassing an "Engineer" is more fun than sex to the Old Timers, and not a choice even young ones want to have to "pick only ONE" of!

I kid you not.

:D
 

mnl

Cast Iron
Joined
Sep 7, 2007
Location
Maryland near DC
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.
 

thermite

Diamond
Joined
Sep 21, 2011
Location
Sol, Terra
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.

Dumore not. Boley, mayhap?

Or P&W's Sigourney, Or a Muehlmatt/Hamilton.

Unless used with an add-on rising-table, the E-M is actually clumsy by comparison what with the extra mass of that stone-age variable speed rig - same physics - AFAIK - as the one on my old-but-good Hobart heavy-lifter kitchen mixer. Which does have a crank operated rising BOWL on Z-axis dovetail ways!

More HP than the Burke #4 mill as well. Then again, talk about "earning your crust"?

My ex could crank out round loaves of bread on that machine as if feeding a Roman Legion!
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
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.
 








 
Top