Slightly sizing down a carbide drill

I have a job that will need about 150 holes drilled in 3mm thick carbon plate. The holes need to be 4.33mm +/- .01mm. It's right between common sizes of 4.3mm and 4.365mm. Normally I get my carbide drills for these jobs from drillbitsunlimited for just a couple bucks a peice and they work great. I found a couple 4.33mm elsewhere but they are around 25 bucks and hss. Could I possibly grind a 4.365 down to 4.33? Was thinking maybe just chuck it up in my cnc and slowly step into a grinding stone in my vise. Only needs to drill through 3mm, so only a small portion needs to be ground. These drills are only 10mm long flute to begin with so it should have good rigidity as I rub it up against the stone. Will it work?

First I think I would go back to the engineer and have a chat, maybe a more standard size would work. It seems a bit strange that the spec would be an odd size.

The odds of a hole being drilled exactly to the bit size is small at best, drilling is a roughing operation. Due to the nature of carbon fiber, I would expect the hole to drill a bit smaller than the bit due to spring back.

That being said, I would try a #18 or a 11/64 drill bit. Both are pretty close. Then there is the problem of actually measuring the hole once it's drilled. Do you have a Go/NoGo gauge set or pin gauges to measure the hole?

I think some experimenting is in order.

I don't think you have a chance of trying to grind the drill bit.

+\- 0.0004 is a lot to ask from a drill bit.

I can't find a drill bit in that range of specifications. The best I can find is a .1705 reamer. MSC part # 03371234, M.A. Ford, carbide.

Best of Luck.

Quote:

---

Originally Posted by Jim Dawson

First I think I would go back to the engineer and have a chat, maybe a more standard size would work. It seems a bit strange that the spec would be an odd size.

The odds of a hole being drilled exactly to the bit size is small at best, drilling is a roughing operation. Due to the nature of carbon fiber, I would expect the hole to drill a bit smaller than the bit due to spring back.

That being said, I would try a #18 or a 11/64 drill bit. Both are pretty close. Then there is the problem of actually measuring the hole once it's drilled. Do you have a Go/NoGo gauge set or pin gauges to measure the hole?

I think some experimenting is in order.

I don't think you have a chance of trying to grind the drill bit.

---

So far the other size drills I've used have given a dead on hole size in the cf. Remember, these are only 10mm long flute carbide drills. Only slightly more than a half inch sticking out of the spindle, so its not your average wobbly drilling op that has a general lack of precision. These tiny carbide drills hit pretty much dead on location and size in the cf plate.

I've already talked to the designer about it. They are using a press in flanged threaded insert that is actually designed for sheet metal. Probably not the best engineering choice, but that's what I have to deal with. He said at 4.3mm the insert will start delaminating the cf when pressing in, and at 4.36mm it will be loose and fall out. So I guess +/- .01mm is a bit overstating. +/-.02 would be The max. The flange on the insert is what takes the actual load, the press fit is just so the insert stays in until the customer assembles the frame.

So keeping in mind that these drills are extremely short and rigid, would it really be impossible to grind about a thou off it? It isn't the end of the world if I need to order a 25 dollar drill, I just don't know if hss will stay sharp enough for 150 holes in cf. As it is, I already swap out the carbide ones every 200 holes or so to keep them from fraying the cf since they're only 1.78 a peice

How about a #18, 4.305mm?

$18 at McMaster Carr, so probably can be found even cheaper.

Quote:

---

Originally Posted by ger21

How about a #18, 4.305mm?

$18 at McMaster Carr, so probably can be found even cheaper.

---

Yeah, that's the lower size I could find. He said at 4.3 it will be too tight and delaminate the cf when pressing in.

Maybe the designer should be introduced to LocTite products or cyanoacrylate adhesives :D

At <$2.00 each grinding would be worth a try I guess.

Quote:

---

Originally Posted by Jim Dawson

Maybe the designer should be introduced to LocTite products or cyanoacrylate adhesives :D

At <$2.00 each grinding would be worth a try I guess.

---

Yeah, for prototyping he may just have to put some ca on them unless he wants to pay more for a special tool. Thing is, this insert is already used on many other models they already have. Large production runs are done in china. I assume it's mostly waterjet, but they must have a 4.33mm drill for the holes. I just do the quick turn around small batches.

I ordered a couple 4.305 and 4.365. I'll probably drill with the 4.305 and then chase with the ground down bit if I can get that to work. I also ordered a 4.33 gauge pin. Who knows, maybe I can grind some flutes into that and use it to ream/form the 4.305 hole to 4.33. Only needs to get a thou bigger. Probably not even that much. Maybe I can tap some runout into the 4.305 to gain a little lol. Or just use one of my old cheap er collets. Probably already has a thou of runout

Hi, at 4mm + you could get a masonry drill and use a diamond lap to wear it down to size.
Ian.

Quote:

---

Originally Posted by handlewanker

Hi, at 4mm + you could get a masonry drill and use a diamond lap to wear it down to size.
Ian.

---

Whatever I do, it has to be quick and efficient. The ones I already did, I just interpolated with my 2mm cutter. It works, but it takes extra time to dial it in and also have to recheck every 50 holes or so since the tools wear very fast on cf and diameter of tool can easily go down .01mm in 50 holes. Getting them round is also a challenge when interpolating with a 2mm cutter because of flex and the fact that radial tool engagement changes as it starts and moves through the cut. I have to do spring pass to help with that, which makes the wear problem even worse.

I'm glad I didn't waste 25 bucks on a hss 4.33mm drill. Last night I did some small m3 countersinks using a 1/4 hss spot drill, tried anyway. It ate the tool in literally 20 countersinks. Hss is definitely a no go for cf, even with very short term usage. Had to finish the countersinks by interpolating with a carbide chamfer. Looks like the only reliable efficient way to do these holes is with a carbide 4.33 drill. Really hoping I'll be able to grind down the 4.365 bits. If not, I'll just have to keep dealing with the pain of interpolating. My new cutters i have coming should at least help with that

I suspect what you want is a carbide reamer.

Since you seem happy with interpolated holes, I also suspect you don´t achieve 0.01 mm +/- in size cylindricity and straightness.
Do you have go / no go gages of 0.01 mm size difference to qualify size and straighness of the holes ?

No Q. intepolated holes can do 0.01 mm, but on high end machines with industrial tooling.

Hi, now if you had a Deckle SO D bit grinder you could take a long round carbide blank and grind it to a hex shape for 10mm or so......you drill first with a normal drill and use the ground drill to take out the last couple of thou…….the hex shape will cut just as good as a real reamer but you can custom grind it to whatever size you need.....the hex shape or even a square one automatically has clearance behind the cutting edge......a hex one just has more edges.

The other dodge would be to use a boring head with a single flute carbide end mill.
Ian.

Quote:

---

Originally Posted by hanermo

I suspect what you want is a carbide reamer.

Since you seem happy with interpolated holes, I also suspect you don´t achieve 0.01 mm +/- in size cylindricity and straightness.
Do you have go / no go gages of 0.01 mm size difference to qualify size and straighness of the holes ?

No Q. intepolated holes can do 0.01 mm, but on high end machines with industrial tooling.

---

Yeah, +/- .01mm diameter and round was a bit overstating. That's what id like to shoot for, but doesn't need to be quite that perfect. Let's say +/- .015mm. The holes that I interpolated with spring passes were measuring 4.33 to 4.34 at different positions, probably .01mm oblong in many cases and an occasional 4.32 and 4.35. This was accurate enough, just a pain to keep chasing the cutter wear. When I get the couple bits I ordered, I'm gonna throw the 4.305 in a cheap Chinese collet I have with some runout and see what the hole looks like. If I can push a 4.32 pin in it, I'm calling it good enough

So I ran the 4.305 bit in some holes. In one of my old cheap collets I got it chucked up with about 7 tenths runout. Worked great. 4.32 pin passes, 4.34 does not. Close enough. Not very scientific, but it works. Obviously an average drill bit would just center itself, but at only 10mm long flute and 165deg point, it seems to hold the runout and enlarge the hole.