Carbide drill hole size variance

Duc · Jul 23, 2018

Looking to reduce a machining op from 3 tools down to 1 hopefully by using a carbide drill. Very small production batch of 100-300 parts for a home shop using a Fadal 4020 with 10K spindle. Not the quickest tool changer in the world and already knocked more than a few hours off the process by switching to a vacuum fixture.

Material: 6061-T6
.400 Depth of Thru hole.
.250 Dia -/+ .0015
Positional: -/+ .030
No surface finish call out - Part is hard anodize later.
Flat surface to start.

Would a carbide drill from Maritool or Guhring be able to meet the -/+ .0015 spec? Would love to remove the center drill, drill and ream operation from this.

Milland · Jul 23, 2018

Short drill and holder, clean and true spindle taper interface, Z-axis ways in good shape - yes, shouldn't have any trouble as a straight-shot.

Mtndew · Jul 23, 2018

Duc said:
Would a carbide drill from Maritool or Guhring be able to meet the -/+ .0015 spec?

Yes, but you also have to take into account the tool runout.
Do you have a good holder? How's your collet?

Duc · Jul 23, 2018

Tool holders are new from Maritool in either ER16 or TG100. Brand of ER16 is unknown at this point but no issue picking up a 1/4 collet while purchasing drill bit. I also have a fairly new integral drill chuck from Accupro that can be used.

Milland · Jul 23, 2018

Do not use the drill chuck, use the collet system, clean and properly assembled.

Duc · Jul 23, 2018

Sounds like a plan for moving forward. Thanks everyone for the info.

Finegrain · Jul 23, 2018

No need for carbide. OSG EX-Gold will hit that tolerance in 6061 no problem, and one of them will drill thousands of holes with no perceptible wear. Hold it in a collet chuck. You can start the hole slow and light, to emulate a spot drill, then retract a bit and hit it.

Regards.

Mike

Mtndew · Jul 23, 2018

Finegrain said:
No need for carbide.

It's only a .250" drill, buying a carbide drill that size won't break the bank. And it will be more stable, especially if he wants to bypass the spotting op.

lastrada · Jul 23, 2018

If your mill has TSC, then a heat shrink holder and a coolant thru carbide drill is the cat's meow.

doug925 · Jul 23, 2018

Duc said:
100-300 parts
using a Fadal 4020 with 10K spindle
6061-T6
Thru hole.
.250 Dia -/+ .0015
Positional: -/+ .030
No surface finish call out - Part is hard anodize later.
Flat surface to start.

All day long, and then some.
No spot.
Short projection holder, and drill.
Coolant.
You should be able to hold you position and diameter tolerance without issue.

Doug.

robert123 · Jul 23, 2018

Assuming anodize is per MIL-A-8625, unless otherwise specified, standard Type III (hard anodize) thickness is .002" per surface with approximately half of the growth making your hole smaller. Thus the anodize will make your hole ~.002" smaller, so you should probably make your holes about .252" if you want them to be in tolerance. 6.4mm could work.

Duc · Jul 23, 2018

lastrada said:
If your mill has TSC, then a heat shrink holder and a coolant thru carbide drill is the cat's meow.

The mill does have TSC and in the future I will be purchasing some tooling to use it. Before I scrap a 80 dollar drill I will take a swing at $15 carbide drill. Still purchasing some nicer equipment for the mill such as a Haimer 3D and more tool holders.

Mtndew said:
It's only a .250" drill, buying a carbide drill that size won't break the bank. And it will be more stable, especially if he wants to bypass the spotting op.

I was a little surprised how cheap the drills are.

Milland · Jul 23, 2018

robert123 said:
Assuming anodize is per MIL-A-8625, unless otherwise specified, standard Type III (hard anodize) thickness is .002" per surface with approximately half of the growth making your hole smaller. Thus the anodize will make your hole ~.002" smaller, so you should probably make your holes about .252" if you want them to be in tolerance. 6.4mm could work.

OP should check with the customer, usually they're supposed to account for any coatings and adjust drawing callout to suit (i.e. make it to print before anodize).

But it never hurts to confirm.

robert123 · Jul 23, 2018

Milland said:
OP should check with the customer, usually they're supposed to account for any coatings and adjust drawing callout to suit (i.e. make it to print before anodize).

But it never hurts to confirm.

I disagree that dimensions are usually before (or after) coating. In this case, MIL-A-8625 (I'm assuming this is the called out spec but could be wrong) specifically states that drawing dimensions apply after anodize unless otherwise specified.

In general, industry standard ANSI Y14.5 states that the drawing should specify in some manner whether dimensions apply before or after coatings. There is no default method. I see plenty of poor drawings that will reference ANSI Y14.5, zinc or some other plating, and fail to specify if dimensions are before or after plating. In my experience with aerospace work, I would say it is maybe a little more common for dimensions to apply after plating but before primer or paint.

Milland · Jul 24, 2018

Fair enough. The drawings I get call out specifics on before or after anodize dimensions, if they don't and I know the part will get anodized I ask. I'd rather be safe than have to recut hard anodize.

litlerob1 · Jul 24, 2018

At .4" deep, you don't need TSC. It's a bonus for sure. If you aren't doing any Toolchanges great, but if you are, it's going to take longer to get the coolant going and shut off, than it will to Drill the bloody hole.

I use Guhring GS 200 U. My hole would be finished in 33 milliseconds (1/3 of a 1 second). 10,000 RPM, .006" chipload. 'Course I know yours isn't a Speedio or the like.

Robert

Job Shopper TN · Jul 24, 2018

One can hit tenths tolerances with carbide drills, you just have to be smart about it. Minimal runout (hydraulic holder) and a good quality drill can make it feasible to hit tolerances down to less than .0005. Reamers would be more reliable, of course, but drilling can work at that level.

johneezreno · Jul 24, 2018

Screw machine length drills. 6061 size tolerance no problems.

Sent from my SM-G950U using Tapatalk

litlerob1 · Jul 24, 2018

Job Shopper TN said:
One can hit tenths tolerances with carbide drills, you just have to be smart about it. Minimal runout (hydraulic holder) and a good quality drill can make it feasible to hit tolerances down to less than .0005. Reamers would be more reliable, of course, but drilling can work at that level.

This is the CNC sub-forum. WTF is a Reamer??? Oh you mean one of those POS, dated, half functioning, deals that require more care than a PCD Endmill?? Fuck that. Fuck Reamers. Fuck Reamer drawers and storage, and all the money wasted on every last possible size variant, flute variation, OAL length variation, shank size variation, material variation. Do you realize what it would take to be fully stocked from 1/64 to 1"????$$$$$ I can keep under .0005" with a Drill 98% of the time, the other 2% I'd rather just make everything else grow around the hole. Literally the last option AFAIC.

R

Matt@RFR · Jul 24, 2018

Hey Rob. I was wondering if you have any input on the use of reamers in today's modern CNC machine shop.

Carbide drill hole size variance

Aluminum

Diamond

Diamond

Aluminum

Diamond

Aluminum

Diamond

Diamond

Aluminum

Titanium

Stainless

Aluminum

Diamond

Stainless

Diamond

Diamond

Cast Iron

Aluminum

Diamond

Titanium

Similar threads