PDA

View Full Version : Bolt circle help



daveo
03-26-2011, 06:04 PM
Im trying to drill a bolt circle, in 2 inch thick aluminum (6061) Im using a .250 drill. My question is , if everything is set up perfect on top. I do all my drilling and flip it over , Its .050 off in every direction on the bottom?

Black_Moons
03-26-2011, 06:35 PM
A few problems could be occuring.

What RPM are you doing? What feed rate? (Just roughly how many seconds it takes to drill 1 inch deep)

Are you peck drilling? (Withdrawing to remove chips from the flutes), How often if so?

Are you center punching or spot drilling first with a short, rigid drill like a spot drill or center drill?

I found one of my biggest problems was the drill would skate just a few mils before it would bite into the material, this 'bends' the drill and then it follows the angle of the bend, not the angle of your drill press. This can produce a VERY off hole after 2" with just the tinyest amount of skating, Using any drill thats too stubby to bend REALLY helps this, if just to start the hole and prevent the next drill from skating. (Basicly, any drill with next to no *flute* length and fits nearly all the way in your chuck. Flutes REALLY weaken a drill)

Feed rate is also very important as if you feed too fast for the RPM, you'll push the drill off center. Too much chip buildup can do the same, as can having a poorly ground drill to a lesser extent.

At 1/4", 1000rpm gives you 65SFM, So anywhere beween 1000 and 2000rpm should be fine in aluminum. (Maybe even a little slow, But I perfer slow, keeps from burning out drills)
(More like 800~1200 for steel btw. Bigger drills require MUCH less rpms. Allways go by calculated SFM)

Walter
03-26-2011, 06:51 PM
Daveo,


Its .050 off in every direction
Can you clarify the "Every Direction" portion of that statement please.

.050 over two inches is alot, an awful lot. But in this case it matters "how" it's off... every direction would lead me to question both the drill and the method. Honestly you shouldn't have that much drift with a .25 drill.

IS it properly sharpened? If not that can and will cause drift.

Second, the method itself. How are you drilling these holes? Hand drill, Drill press, Mill...? IF your using a machine tool, check the tram.

Deep holes in aluminum at .25 should be a cake walk. Peck after the first 1/2 inch of depth, use a lubricant. Kerosene, WD 40, Tap Magic... doesn't really matter, as long as you have something.

Black hit on some real good stuff too.

luthor
03-26-2011, 07:54 PM
How can it be .050' off in all directions?
Is the head of the Mill or Drill trammed correctly ?

Dr Stan
03-26-2011, 08:03 PM
By "every direction" I'm going to assume you mean it is random.

Blue Moons & Walter have said every thing I would, so follow their advice.

GKman
03-26-2011, 08:28 PM
How can it be .050' off in all directions?
Is the head of the Mill or Drill trammed correctly ?

Hell, my first question was how can it be so good?

daveo
03-26-2011, 09:15 PM
Im trying for.005... It is a mill and it is trammed. I was peck drilling, but after some suggestions, I dont think the drill is as sharp as it could have been. Thank you guys for the input!

Black_Moons
03-26-2011, 09:29 PM
Hell, my first question was how can it be so good?

Hehe. You'd think drilling a hole would be the easyest of all tasks... But it really does require more skill and math then the average drill operator is willing to admit if you want to drill a high accuracy hole, and get good life outta your drill bits.

I can now drill dozens of holes, inchs deep, with the same bit without dulling it. Even in steel. I used to as a kid dull a drill to nothing but rubbing in 1/4" thick steel before getting through. I actualy thought steel was too hard to drill as a kid. (And it never helped that most the drills I had from my dad where duller then nails, He did'nt know how to drill either... and mainly did woodwork, So dull as nails was pertty sharp for his work.. even if the wood did smoke often)

Now that I have learned how to drill efficently, speed and tool life wise, I need to learn more about accuracy. Go figure, all these years and im still learning how to drill a hole :)

As for accuracy... after 2" deep, 0.05" or more was what I was getting from about 0.01" or less of drill skate at the top of the hole. (Random exotic hardwoods/acrylics, 7mm drill (Near enough to 1/4") I barley even noticed when retracting and inserting the drill that the hole was not totaly in line with the relaxed position of the drill.

Center punch, spot drill/center drill, or 'raming' the unspinning drill into the work (Then turning the drill press on with the drill still in contact) all seemed to greatly reduce the skate error. I don't recommed raming on anything harder then wood or plastic however. And its likey not a good idea, just a fast one. :P Feeding too fast also amplifyed error. (More RPM's let you feed faster, Its Feed per Revolution thats important. Too many RPM's (SFM really) overheats the drill, (and in the case of plastic for example) and material.

With spot drilling, very slow feed, often pecking, highish rpms, 0.005" should be achivable with a decent machine at 2" in aluminum with a 1/4" drill.. IMO
0.010" Should be pertty easy.

SGW
03-26-2011, 10:08 PM
It may help to locate, then pilot drill the holes maybe 3/16" dia 1/2" deep, then go back and open them out to 1/4" for that 1/2" depth with a 1/4" center-cutting end mill. That will get the first 1/2" of all the holes spot-on location and provide a guide for drilling the rest of the way.

And using a sharp, accurately-ground top-quality drill bit is a huge help. If the two flutes aren't ground the same you're probably doomed to less than ideal results no matter what you do.

Tobias-B
03-26-2011, 10:12 PM
I find that using some sort of a stub drill- even just a countersink-
improves things by an order of magnitude. The web on a twist
drill loves to wander, sometimes even around a punch mark.

I also found that a bad bearing in your spindle will thwart most attempts
at accuracy!

t

Evan
03-26-2011, 10:15 PM
I have some 1/4 inch deep hole aircraft step drills left. Would you like a few? This is what they are intended to drill and the result will be dead on. If you want some just shoot me a PM with your address and I will mail them out on Monday.

GKman
03-27-2011, 08:27 AM
Thanks to all. After over 50 years I'm learning something about drilling. What does "peck" mean exactly.

daveo
03-27-2011, 08:35 AM
In and out, in short increments. To clear the chips.

daveo
03-27-2011, 09:54 AM
Thanks Evan... I was going to reply to your PM but your box is full.

Im in no hurry. I dont want to ruin any more metal. So take your time and dont make a special trip if not needed. Thanks again! Dave

Evan
03-27-2011, 11:33 AM
You are welcome. My mailbox is cleared out too.

John Stevenson
03-27-2011, 11:50 AM
Go round twice, first time with a stub drill, second time with one that is long enough to drill to depth.

daveo
03-27-2011, 11:51 AM
Not to derail my own topic, but doesn't softer metals like alum and brass call for a different raked bit?

Just a thought?!

rohart
03-27-2011, 12:11 PM
Not ally. The different rake you may be thinking about is that brass should have no rake or the bit can dig in.

Another way, especially if you're drilling on a mill, is to use a centre cutting milling cutter for the first half inch, slightly under size, say 6mm. Then when you go in with the 1/4 inch drill if will cut straight for the 1/2 inch, and that portion will help support the rest.

Most holes I drill I do on the drill press with the work held in a vise, but the vise is free to find its own position on the table, with the help of my hand of course. I use a 1/8th pilot drill. I move the work around at the start of the operation till I see the pilot drill go in straight. I touch the pilot drill on the punch mark, and the next few touches clearly show the pilot drill bending if the hole isn't in alighment.

Carld
03-27-2011, 12:15 PM
Not necessarily daveo. It's more important that the cutting edges be exactly the same length and angle. If they are not the same length and angle the drill will drill oversize and/or off center.

As stated, use a short correctly sharpened drill to start the hole to a depth 2 to 3 times the diameter of the drill size. That way the drill is guided through the rest of the hole.

One thing to remember, a drilled hole is not a precision hole. If you want precision drill undersize and ream to size.

daveo
03-27-2011, 12:19 PM
True and thanks Carl! I will be happy getting these a lot closer than .050...

Rich Carlstedt
03-27-2011, 12:30 PM
The depth of the predrilling is dependant on the flute spiral angle of your drill
Check your drill flutes and note where the flutes make exactly 180 degress of travel (two flute drill). at that depth, the drill has full 360 degree support in a hole for stability. I have some 1/4 drills that require 3 diameters for this support.

Use a spotting drill, or a Ball endmill. Center drills are OK for lathe work, but not mill work.
WHAT ?.....You say ?
Right, center drills provide a spot for the lips of the drill flutes.
Spotting drills and Ball endmills (the best !) provide radial support to the flutes, which produces a straighter hole, especially if the lips are not ground perfect ( which is the case most times !) and you honor the rule above.

Black_Moons
03-27-2011, 04:46 PM
I allways thought center drills where fine to use. Not so much to provide proper support for the flutes of course, But more to 100% prevent skating as theres a giant pre hole for the tip, And the existing hole will help guide the drill down it as drills perfer to follow existing holes as thats easyest for them.

Much like drilling an undersized pilot hole first, Except the center bit acts as a very strong/rigid pilot bit.

Dawai
03-28-2011, 08:16 PM
Yeah,, I'm with Evan.. a beehive-step-knock out drill is a good start..

I kept one on my tail stock drill on the lathe for a year or so.. it'd start a no-wobble punch mark like quick like.. No worry.. close enough.

In the cnc.. it'd do the spotting just fine.. no wandering.

Not sure which "buddy" borrowed it.. as it has left the building..

madman
03-29-2011, 09:22 AM
I have sets of Stub Drills, I use first a Stub (thats short series drill) and peck away, I do NOT use spot drill or centre drill, just start slow carefull peck a LOT ,when all holes done (aka bolt circle) I change over to my Long series drill, the long series drill follows the stought stiff short series and generally comes out good nuff. If You drill in a rammy fashion the drills love to wander , ive had some amazing die block holes which sucked to fix by too much drill pressure. Rushing too much. Hopoe this helps mike

Carld
03-29-2011, 11:01 AM
When you hit the surface of the work with a drill, short or stub, the tip wanders. If you don't plunge, but peck at it the drill will center it's self and start running true. Many times it is absolutely necessary to use a stub drill to center the drill bit at the start.

Don't over look the fact that the drill bit has to be nearly perfectly sharpened so the flute cutting edges are equal length. A correctly sharpened drill bit is the most important thing when drilling a hole.

luthor
03-31-2011, 08:07 PM
Im trying for.005... It is a mill and it is trammed. I was peck drilling, but after some suggestions, I dont think the drill is as sharp as it could have been. Thank you guys for the input!

What procedure was used to Tram this milling machine?

Evan
03-31-2011, 09:40 PM
If the mill were out of alignment the offsets wouldn't be random.

madman
04-05-2011, 09:34 AM
The S point drill is designed to NOT use a centre drill first, Used them years ago in the shop on cnc mills, drilling lots of holes. They didnt wander and also a stub drill sharpened right doesnt wander either, Have done loads of holes and never had a quality issue, Keep in mind I worked on Aerospace and Nuclear and tool and die work so i think for home shop use the stub drills should be OK>? Just my Opinion.

Evan
04-05-2011, 09:46 AM
Your drills were in the mail last week so you should get them pretty soon.