Holder/drill combo for tight tolerance drilling in aluminum

[GiroDyno]

Like the title says... what is the best style holder and tool for "tight tolerance" holes?
.3165 dia, +/-0.0008, .315-.355 deep, through the part, 6061. This hole needs a slip fit for a pin, so we need a reasonably smooth surface finish to boot.
This is a feature we have interpolated for years but I'm sure there is some sort of holder/tool combo that will let us blast them out in a lot less time, especially considering we're running these through a Brother w/16k spindle.
We do 100k's of these holes so something that will hold size and doesn't have to be swapped regularly is a huge bonus.
PCD tipped drill? Regular ol' solid carbide good enough? Coated or bright?
We don't have a shrinkfit or rego machine, is a collet chuck going to be good enough? SK vs ER?

 

[TKassoc]

Accuromm's g-drills will do that with ease. Get a few PCD drills made and you won't touch them for years. https://www.accuromm.com/products/round-tooling

 

[michiganbuck]

I'm not the CNC guy but think a bright carbide or PDC drill or reamer made to .3157 would cut at .3159 after a pre drill and be in spec for a good long time, with over .001 of safety.
Perhaps a 3 flute drill might be good.

 

[GiroDyno]

Accuromm's g-drills will do that with ease. Get a few PCD drills made and you won't touch them for years. https://www.accuromm.com/products/round-tooling

Question about ordering a custom tool like that: Would you match the drill diameter to the exact hole dimension, or would you try to compensate for the hole coming out larger/smaller than the nominal drill diameter?

 

[michiganbuck]

QT: (would you try to compensate for the hole coming out larger/smaller than the nominal drill diameter?)
Very often a drill (with a pre-drill) / reamer / gun drill or gun reamer will finish at .0002 over the cutter size.

The back taper OD will make them grow smaller in diameter as they are sharpened shorter, so a balance of the first hole and after sharpened a number of times is considered to get the best tool life...
All of these have a cylindrical OD grind, unlike an end mill that is sharp on the OD and so tries to cut the OD larger with any spindle or holder run out.

I suspect a G-drill would be like a single flute gun drill so would do the same.

 

[GiroDyno]

I got some off the shelf solid carbide drills in and have done some preliminary testing. So far holding size +/-0.00075" using an MA Ford 3 flute 229 drill and ER collet doesn't seem to be an issue which is great. I also have similar Guhring and OSG drills to test when I can get time on the machine.

The problem of finish is a bit trickier...
All the tests so far leave an undesirable (but still 100% functional) finish inside the hole, for right now I think it still counts as a win. What is a problem is the chips are also scratching the top surface and one adjacent to the hole.

I've tried a few different methods such as feeding out vs rapid, different chipload, and pecking but haven't had any success.

Is there a particular drill geometry that would prevent the chips from "whipping" out of the hole? Spade drill? Straight flute? Regular old endmill?

These parts all get anodized black so maybe that will hide these blemishes... I plan on sending all my test parts out once they're finished but that's kind of my plan B, I'd rather not scratch them in the first place if possible.

 

[Superbowl]

I got some off the shelf solid carbide drills in and have done some preliminary testing. So far holding size +/-0.00075" using an MA Ford 3 flute 229 drill and ER collet doesn't seem to be an issue which is great. I also have similar Guhring and OSG drills to test when I can get time on the machine.

The problem of finish is a bit trickier...
All the tests so far leave an undesirable (but still 100% functional) finish inside the hole, for right now I think it still counts as a win. What is a problem is the chips are also scratching the top surface and one adjacent to the hole.
View attachment 390849
I've tried a few different methods such as feeding out vs rapid, different chipload, and pecking but haven't had any success.

Is there a particular drill geometry that would prevent the chips from "whipping" out of the hole? Spade drill? Straight flute? Regular old endmill?


These parts all get anodized black so maybe that will hide these blemishes... I plan on sending all my test parts out once they're finished but that's kind of my plan B, I'd rather not scratch them in the first place if possible.

Can you put a strip of blue painter's tape over the hole area to prevent scratching?

 

[GiroDyno]

I had the same thought, but doing that 100x a day everyday sounds labor intensive and really tedious. I also considered leaving .005" stock on the vertical face and doing a quick cleanup pass following the hole drilling ops...

The vertical face right next to the hole is actually hidden by the head of the pin that goes in the hole in the final assembly, so those are in the same category as the pin hole surface finish-not great but also not a deal breaker.

The scratches on the angled face above it will be visible so they need to be eliminated or reduced if possible. I was told they will probably be hidden by the anodizing but that feels like a band-aid rather than a real solution.

 

[Milland]

I think doing a finish pass on the diameter will be the answer. That, or changing your process so you drill from the other side.

I'd keep testing drills if surface finish in the hole is an issue, or bite the bullet and drill, then ream.

 

[David Ferguson]

peck drilling is usually the solution to long stringy chips when drilling.

 

[dandrummerman21]

I had the same thought, but doing that 100x a day everyday sounds labor intensive and really tedious. I also considered leaving .005" stock on the vertical face and doing a quick cleanup pass following the hole drilling ops...

The vertical face right next to the hole is actually hidden by the head of the pin that goes in the hole in the final assembly, so those are in the same category as the pin hole surface finish-not great but also not a deal breaker.

The scratches on the angled face above it will be visible so they need to be eliminated or reduced if possible. I was told they will probably be hidden by the anodizing but that feels like a band-aid rather than a real solution.

Looks like a turned part that you're now dropping in the mill?

If so, make a really thin plastic ring that you just drop over that diameter. No fuss with tape. Drop over and go.
Make it a snug fit.
Or rubber. A wide rubber band or similar.


If you're milling that diameter (doesn't look like it), mill it after the holes are there

I don't think you'll see it once black

 

[GiroDyno]

I've drilled a few hundred (thousand?) test holes with different tools, feeds, pecks, etc... and am now just waiting for some parts to come back from anodizing and see what the finish is like.
In the meantime I'm also considering improving the interpolation process we already use. An interpolated hole obviously won't be as fast as a drilled one, but it certainly does a better job of keeping the adjacent surfaces pristine.
A more rigid tool (5/16 vs 1/4) designed for aggressive ramping might get it down to 2<3 seconds/hole vs 6 which would still be a huge gain.

Anybody have recommendations for an aluminum endmill that will ramp like crazy, but can also leave a quality finish on the walls? The SwiftCarb Rampmill came up right away but I'm not sure what kind of finish they leave.

 

[crossthread82]

I've drilled a few hundred (thousand?) test holes with different tools, feeds, pecks, etc... and am now just waiting for some parts to come back from anodizing and see what the finish is like.
In the meantime I'm also considering improving the interpolation process we already use. An interpolated hole obviously won't be as fast as a drilled one, but it certainly does a better job of keeping the adjacent surfaces pristine.
A more rigid tool (5/16 vs 1/4) designed for aggressive ramping might get it down to 2<3 seconds/hole vs 6 which would still be a huge gain.

Anybody have recommendations for an aluminum endmill that will ramp like crazy, but can also leave a quality finish on the walls? The SwiftCarb Rampmill came up right away but I'm not sure what kind of finish they leave.

I've had good luck getting decent finishes with a DLC coated alumigator from GWS their ART series tool. With a 3/8 tool going down 0.100 per pass or so.

Are you pre drilling or helixing in blind?

 

[GiroDyno]

In my testing I was drilling straight to size but the drill chips were whipping as they came out and would scratch the turned surfaces adjacent to the hole, heavier feed broke the chips so they weren't long and whipping but instead they were thick and would create gouges.

After testing a bunch of tools I was able to find a tool/process that left a perfect finish but the cycle time is long enough it made me reconsider interpolating the holes.
I'd like to ramp in at 80* and then do a spring pass at full depth to eliminate taper and clean up any marks from the entry.

There is a mating mating cast iron part that I've been working on simultaneously and I was able to find a tool with a ramp/spring pass fast enough that it beat drilling a pilot and interpolating the hole because of the extra tool change/spindle ramp (On a Haas VF3SS, not a Brother) so I'm trying to do the same with this aluminum part now.

 

[dandrummerman21]

I mean, an 80 degree ramp is still basically just drilling a hole. You'd still have similar drill-type chips coming out as well as regular chips, I *think*, although I also think they'd be shorter in general.

I don't think a rampmill will do what you want? Don't those just have a thru hole on center?

You mention 5/16 or 1/4 but a quick look at the swiftcarb catalog suggests they start at 3/8"

Disclaimer, I've never used one of those endmills, nor have I ever tried interpolating anywhere near that steep in solid metal.

 

[crossthread82]

In my testing I was drilling straight to size but the drill chips were whipping as they came out and would scratch the turned surfaces adjacent to the hole, heavier feed broke the chips so they weren't long and whipping but instead they were thick and would create gouges.

After testing a bunch of tools I was able to find a tool/process that left a perfect finish but the cycle time is long enough it made me reconsider interpolating the holes.
I'd like to ramp in at 80* and then do a spring pass at full depth to eliminate taper and clean up any marks from the entry.

There is a mating mating cast iron part that I've been working on simultaneously and I was able to find a tool with a ramp/spring pass fast enough that it beat drilling a pilot and interpolating the hole because of the extra tool change/spindle ramp (On a Haas VF3SS, not a Brother) so I'm trying to do the same with this aluminum part now.

max ramp angle on an alumigator is 45degree rampmill is around 15-18 degree. Alumigator will ramp consistently at 45 degrees to 2xD through solid if you have enough flood coolant on it. Rampmill has tsc hole so better chip evac if that's an issue. below is a chart that shows minimum entry hole size for the rampmill. Both are going to leave a pretty gnarly finishes if done at final depth. You'd have to ramp the finish as well to get the teeth marks to disappear.

 

[GiroDyno]

I just got off the phone with SwiftCarb they pointed me towards that chart with the minimum hole size.
I will get a GWS to test out, thanks for the recommendation.

 

[crossthread82]

I just got off the phone with SwiftCarb they pointed me towards that chart with the minimum hole size.
I will get a GWS to test out, thanks for the recommendation.

Make sure to get it dlc coated, you have to ask. It greatly reduces the chance of chip welding when ramping aggressively. Plus I think it leaves a slightly better surface finish over the uncoated tool.

 

[crossthread82]

I just got off the phone with SwiftCarb they pointed me towards that chart with the minimum hole size.
I will get a GWS to test out, thanks for the recommendation.

Also, you should get the 1/4 one not the 5/16 because it's not going to like basically plunging since it won't hardly have any radius to the helix going into a 0.316" hole. Maybe even go to the 3/16 size.

 

[GiroDyno]

Also, you should get the 1/4 one not the 5/16 because it's not going to like basically plunging since it won't hardly have any radius to the helix going into a 0.316" hole. Maybe even go to the 3/16 size.

It has to stick out of the holder 2" which is why I wanted to try a larger/stiffer tool; we have to baby our 1/4" tool since its hanging way out there. I have both 1/4" and 5/16" extended reach w/stubby LoC tools coming to test.

Hopefully I get parts back from anodizing in a few days and it turns out we can just drill the holes but I'd rather try some more tools out while I wait.