Drilling a 1mm bore in C110 copper

[teemfan93]

Hey folks,

I have a part that is 1.5mm thick (C110 copper) I am hoping to drill/ream a 1mm bore about 4mm deep. I purchased a number of different drill bits (between 65-70 drill sizes) but am having a bear of a time getting anywhere. I purchased several of each size as I knew this was going to be challenging. I also have a couple 1mm reamers and a few .037" reamers to try once I have successfully drilled the pilot hole .

In terms of equipment I am pretty limited in what I have to use. We have a manual bridgeport and a tormach, both of which I have tried (unsuccessfully). I have given it a shot with a drill chuck as well as an ER collet holder (the tormach tooling system if you are familiar with it). After getting ~2mm deep my drill bit is always snapping. I did try spotting with a spot drill, but that didn't help much either, and I did see the drill walk a bit when it was starting the hole.

I am mostly looking for recommendations of a few other things to try. I am just a hobby machinist and this one is really giving me trouble. As of right now everything has been manually pecking, any thoughts about trying to program in a pecking cycle with the tormach? Should I not spot drill and allow the drill to find its own center? For reference the drillbits I purchased from Mcmaster were from this series:

McMaster-Carr

McMaster-Carr is the complete source for your plant with over 595,000 products. 98% of products ordered ship from stock and deliver same or next day.

www.mcmaster.com

 

[WizardOfBoz]

So you are drilling into the face of the part that is 1.5mm wide with a 1mm drill, leaving 0.25mm (about 0.01") on each side?
In soft copper?
That is somewhat ambitious in my view.
Others have more experience but I will say that drilling into copper per se presents an issue. It's so soft that it grabs the drill and pulls it in. It hogs the drill. For larger drills I've done the recommended changing the angle of attack (?) of the drill with a stone. Kind of like dulling the edge, but what you are really doing is ensuring that the drill scrapes material away and does not dig in, pulling the bit out or moving the part. Not sure how I'd do that on a 0.5mm cutting edges of the 1mm drill.
But maybe people do do this. Any voices of experience?

 

[Mtndew]

I have a part that is 1.5mm thick (C110 copper) I am hoping to drill/ream a 1mm bore about 4mm deep.

Sandwich the 2 faces between 2 other pcs of copper so that it can't bulge out while drilling.
And if you need to ream it or size it after drilling, maybe try one of these:
https://www.harveytool.com/products/tool-details-2541m

 

[jim rozen]

I do jobs like this on a Dumore high speed drill press. For a 0.040 diameter drill you want to have the spindle running very fast. My go-to cutting fluid for copper is 50/50 lard oil/kerosene mix. Centerpunch the location and allow the drill to pick that up. Manual peck a few times as you get more than 1 drill diamter deep. You are probably running the drill too slow and over-feeding it.

Brass will catch and hog drills, copper does not. Do not use a zero rake drill for this.

 

[teemfan93]

I appreciate all the advice everyone. I figured this was an ambitious (but hopefully feasible?) task. I knew the .25mm wall was going to cause me issues, but wasn't sure how big of a deal that would end up being.

I do jobs like this on a Dumore high speed drill press. For a 0.040 diameter drill you want to have the spindle running very fast. My go-to cutting fluid for copper is 50/50 lard oil/kerosene mix. Centerpunch the location and allow the drill to pick that up. Manual peck a few times as you get more than 1 drill diamter deep. You are probably running the drill too slow and over-feeding it.

Brass will catch and hog drills, copper does not. Do not use a zero rake drill for this.

Do you have an alternate drill from Mcmaster you would recommend? That is our go-to supplier unfortunately and I am probably limited to ordering through them. I figured the alum/brass/bronze drill would be the way to go, but that may have been a mistake.

We do have a high speed sensitive drill press, I could look at spotting it on the CNC and then drilling through with the drill press?

 

[kenton]

Program your tormach to full retract peck every .005" or .13mm to clear the chips. I would start at .0008" or .02mm per rev and maximum RPM.

You may need to babysit it to clear chips and brush on oil every retract. Set your rapid override to 10% so you have more time to clear chips and add oil if you need to.

 

[implmex]

Hi teemfan93:
You have a few things working against you, and one of the biggest ones is that your gear, especially your CNC gear is marginal for a job like this.
But you can make it work with enough persistence.
The secret I've found in situations like this is to lubricate the tool really well, peck in very small increments, and keep your cutting tool in pristine condition.

So on the Bridgeport...I peck with the quill stop, so my left thumb is on the stop and I rotate the stop a bit, then peck down onto it, lift the quill rotate a bit more, peck down again and etc etc.
This limits how deep you can peck and is a bacon saver.

On the Tormach...set your peck increment really small...I will go as low as 0.0005" per peck, and just accept it's not very fast.

On both, always always always get a spot into the part before you drop in your drill... you need it to get the point of the drill to stay where it's supposed to.
Chuck up the drill so it's sticking out only a bit farther than you need but watch out you don't end up with the flutes that go up in the collet packed full of chips.
I can re-point my drills easily, so I just cut them off as short as I need for the job.

Next you can petition the customer to change the grade of copper from C110 to Telco.
Telco is doped with tellurium, which transforms its ability to be machined and will make your job vastly easier.

Last you MUST use a good lubricant, generously....enough to keep your drill clean and sloppy wet.
I am a fan of Relton's Rapidtap, but there are plenty of others.
Some advocate buttermilk for machining copper...apparently it works but without a really thorough cleanup afterward it will go rancid and your machine will begin to stink unmercifully.
I've never tried it...Rapidtap has always done it just fine for me.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[WizardOfBoz]

Brass will catch and hog drills, copper does not. Do not use a zero rake drill for this.

Thanks Jim. True for all Cu alloys?

 

[BoxcarPete]

Thanks Jim. True for all Cu alloys?

Think about what you just asked for a few seconds, and you can answer it yourself.

 

[jim rozen]

(copper and zinc = brass)

So yes, zero rake for brass.
Postive rake for pure copper. Copper 110 and copper 101 are both pure copper from the standpoint of machining.

My favorite for this is Guhring parabolic flute drills. Apparently not available from McMaster Carr as far as I can tell. Can you source through MSC?

 

[Limy Sami]

(copper and zinc = brass)

So yes, zero rake for brass.
Postive rake for pure copper. Copper 110 and copper 101 are both pure copper from the standpoint of machining.

My favorite for this is Guhring parabolic flute drills. Apparently not available from McMaster Carr as far as I can tell. Can you source through MSC?

X 2 on those parabolics - love em, don't forget the old trick of milk for lube - been discussed on PM several times.

 

[Conrad Hoffman]

This just doesn't seem that difficult. The L/D ratio is only 4:1. The trick is in the lube and chip clearing. I'd be using Monroe Cool Tool II or maybe Crown Buttercutt, or some good veggie oil. Spot it with a centerpunch or spotting drill and peck in and out, keeping the hole flooded with oil. It's small enough that I wouldn't do anything special to the drill, just a regular HSS jobber or screw machine length. Should be easy enough on anything that spins, including a cheap import drill press. I wouldn't screw with reamers, at least not the ones we buy, as they aren't sharp enough to cut, but will tend to bind up and break.

 

[kenton]

When I started my current job one of my first jobs was a turned copper part. I made a comment about using whole milk as cutting fluid. One guy looked me dead in the eye and said "If you fill the lathe sump with rancid milk the whole shop will kick your ass".

That is my total experience using milk as cutting fluid.

 

[teemfan93]

Thank you for all the suggestions everyone. I will update on Monday when I am back in the office. I believe one of my bigger issues was runout (with the drill chuck) which is why I switched over to the ER collets. I am able to get 1-2mm deep before it breaks, which is probably a chip clearance issue. When the drill grabs I do have an issue with one side of the part bulging out, I like the idea of including some additional stock to support the thin walls. I will probably use some 1-2-3 blocks for this. The tormach is limited to 4500 RPM, but I will run it full speed next time I give it a shot, and try some of the very low peck drilling cycles. Run time is not a concern, I just have 2-3 of these to do, and plenty of spare parts to test on.

Marcus I appreciate the advice about peck drilling on the manual mill. That is so simple but I have never thought to do that before.

 

[jim rozen]

We machine a lot of copper on manual machines at my workplace. The lard oil kerosene works pretty well. Most folks who get in trouble are running the tools too slow and over-feeding it. As long as a good chip is getting spit out of the drill, it's going well. Go calculate the SFPM numbers for a 1 mm diameter drill in copper and you may be suprised. "That fast??"

 

[???]

Make sure the spot drills tip doesn't leave a flat in the center of the hole that's bigger than your drill bit. I normally spot with a solid carbide 3 corner bit that I grind to a sharp point on the tool and cutter grinder.

Bridgeport at top speed over CNC for feel, I also clear the chips with my fingers every retract. Coolant neat Hocut 795.

 

[Screwmachine]

Make sure the spot drills tip doesn't leave a flat in the center of the hole that's bigger than your drill bit. I normally spot with a solid carbide 3 corner bit that I grind to a sharp point on the tool and cutter grinder.

Bridgeport at top speed over CNC for feel, I also clear the chips with my fingers every retract. Coolant neat Hocut 795.

This is important. Most folks think of center drills as spotting drills, and they do work, but aren't ideal, and it gets really sketchy down at this size.I also grind up 3 corner carbide spotting tools, with the same angle as the drill lips, works great, and 1mm is on the large size of what I tend to drill.

Drill RPM isn't as important as feed rate; there's a tendency to overfeed with slower rpm and underfeed with high rpm. Figure out the chipload you want (0.01mm per lip/rev is a start, go down from there) and program that on the Tormach, or use the quill stop like Marcus mentioned, turning it to feed, on the Bridgeport. Figure out the time required to hit the feed rate per peck and turn the quill stop at a rate that simulates that.

Whether you try an animal lube like milk or lard, or something like Rapid Tap, you need to keep the drill lubed and chip-free. Frequent pecking and brushing of the drill will avoid chip packing, which causes heat, which jams the drill in the hole and breaks it.

Obviously the drill needs to be running pretty concentrically, but at 1mm with HSS and a long-ish drill you don't need to be in micron territory, just visibly concentric should be fine.

 

[WizardOfBoz]

Think about what you just asked for a few seconds, and you can answer it yourself.

Fair enough. Bronze and brass get there own rules. And beryllium copper. But when I asked I was thinking about the more pure Cu alloys. Didn't think the question through.

So after reading your note I looked arounds and found a monograph on machining copper alloys:

https://www.copper.org/applications/marine/cuni/pdf/DKI-Machining.pdf

It's German (Deutsches Kupferinstitut) so it must be good, right? There are a lot of words in the thing, and there may actually be useful info, but there's an awful lot of "everything depends upon the specific alloy, and no generalizations can be made". So the answer seems to be the universal answer: "It all depends". Which may have been your point....

 

[boslab]

A clamp on sleeve would limit the plastic deformation.
Try freezing it before drilling or reaming , pipe freeze spray helps cool it down
Mark