PDA

View Full Version : Drilling a precision hole on a milling machine...??



krems
10-28-2007, 07:10 PM
I need to get the tooling set up to drill a precision hole through Aluminum. What is the correct way to drill a hole with any degree of accuracy. I am looking at drilling 3 holes through 2 pieces of aluminum 1/2 - 3/ 4" thick. I need the holes to line up perfect because I will be using locating pins so the blocks will close the same with very precise alignment. Do I use a spotting drill, undersize drill bit, then final ream to dimension or is their a better way w/ less steps. I need the final dimension to be .250" (1/4"). I will need to use some sort of press fit locating pins as well.

I need to buy the tooling and got confused at all the choices. What cutting angle on the bit, 118 degree / 130 degree??, HSS, carbide, cobalt. Coated or uncoated, What angle on the spotting drill should I get etc. What about the reamer..straight or spiral etc.

Confused in Montana!.................Thanks for the help in advance.

Forrest Addy
10-28-2007, 07:36 PM
It's tough to go into a technical endevor of any kind without a handy mentor to guide you over the rough spots. Dante had Virgil to guide him through the Inferno; you should have some old retired fart willing to swill coffee and spin you yarns of how it used to be in between chewing your butt. Try to find one. Ask around for retired machinists.

Vocaulary is absolutely everything when learning a new endevor. You need to clearify a few terms.

"Drilling" is making holes with a twist drill on any of a dozen varients. Drilling is done usually "from the solid" you put a hole where ther wasn't one before. Drilling is not a very precise operation. The hole location and size can vary somewhat.

"Reaming" enlarges an existing hole. The amount of reaming stock is small varying from 1/6" to 1/16" depending on the size of the reamer. A reamer will make the hole right on size but since it's a bit flexible will follow the existing hole if it's mislocated.

"Boring" uses a single point tool to enlarge an existing hole. In a milling machine this requires a boring bar often mounted in a boring head. The boring head mounts in the spindle of the milling machine and has a little slide you can offset to regulate the depth of the cut. Boring is best done with a mechanical feed - that is the head progresses into the bore at a fixed rate selected from several available to the operator. Boring will precisely locate and determine the size of the hole regardless of small errors in drilling the original.

If you have an endmill that's to size and in good shape you can bore the hole with it however you may find the hole to be a trifle oversize. Much depends on the accuracy of your spindle tooling. If the cutter is eccentric in the spindle tooling then the hole will finish oversize accordingly.

What I suggest you do is stack those two parts and bore the holes you need for the locating pins. That way accurate locations are relative and you don't need to sweat table and saddle offsets. For that you'll eventually need a boring head. Work one hole at a time, pre-drill with a center drill, drill each a bit undersize then drill out the remainder of the stock with an on-size drill. You'll probably get pretty much what you want unless you desire a closr fit. If that's the case, you'll have to bore out an undesize hole.

I don't know how you are equipped but if your machie is practically bare you could find a kit containing collets, a clamp and step block kit, a boring head, and a vise for about half the monthly rent.

Uncle O
10-28-2007, 07:41 PM
Always spot your holes. Some people use center drills, some don't like them and use spotting drills instead. Next, drill undersize, then ream. Get a .249, or a .2495 reamer and use cutting oil. If both pieces of stock are the same size you can stack them both in the vice and do them both at the same time.
If you cant do that, use a work stop so at least you won't have to pick-up the edge again. Note that sometimes reamers cut a little over and or undersize.

Get a couple .250 dowel pins

SGW
10-28-2007, 07:53 PM
As usual, Forrest said it better than I could.

mechanicalmagic
10-28-2007, 08:07 PM
To suggest the proper tooling I need to know:

How close do these parts need to repeat?

If I was doing this, and +- .001" is good enough:
Stack the parts in the vise, do both at once, making sure the proper faces are together.
Spot using a center drill, #5
Drill using .201" dia. #7
Enlarge to .242, D size
Ream .2490" thru
Ream .2510" thru ONE part.

When reaming, half the speed, twice the feed.
Use cutting lube on all operations.

Yes, pushing a dowel pin in that small a hole is a bit tougher than one that's .2500" but I do it. Align the two blocks, and use the oversize top block to stabilize the pin, until it's correctly started.

Dawai
10-28-2007, 09:29 PM
five minutes laying tooling out,
fifteen minutes clamping part down, spotting corner for X,y offset. setting tool depths by "feel and guestimation"
Five minutes to write G81 code spots,
Two minutes run spotting drills Madman gave me.
M6 tool change to drill.
Two minutes drilling holes
Ten minutes cleaning machine off.

Just because it is a cnc don't mean it shoots the holes where you tell it to, I have saw 1/4 drills bend in a U and drill off at a tangent. Stainless is the worst, want it turning really slow and a lot of down pressure.

Madman said to just spot drill it in the cnc, then drill it in the drill press. I wire machinery and knock about for my money and he does it for a living so I guess he is right. Most the time. A electricians Unibit makes a hell of a spotter.

J.Ramsey
10-28-2007, 09:59 PM
Buy a DRO and install it on your mill.

rkepler
10-28-2007, 10:22 PM
Buy a DRO and install it on your mill.

A DRO won't put the hole in the right place, but it'll put the table in the right place. A spot drill will help (more the stubbier and stiffer it is) but a drill can still catch the flutes and move off center, or a change in the material can cause it to move, etc. Loads of reasons the other end of the hole might be offset from the start.

If you absolutely, positively have to have the holes on size and position (to a tenth both ways): spot, drill under, bore close and ream to size. If you've got big ones and clank when you walk go ahead and bore to size, reaming is for pussies like me who hate to scrap things when the 50th hole goes a little oversize.

J.Ramsey
10-28-2007, 10:42 PM
A DRO won't put the hole in the right place, but it'll put the table in the right place. A spot drill will help (more the stubbier and stiffer it is) but a drill can still catch the flutes and move off center, or a change in the material can cause it to move, etc. Loads of reasons the other end of the hole might be offset from the start.

If you absolutely, positively have to have the holes on size and position (to a tenth both ways): spot, drill under, bore close and ream to size. If you've got big ones and clank when you walk go ahead and bore to size, reaming is for pussies like me who hate to scrap things when the 50th hole goes a little oversize.

I'd say you must be good enough to center punch individual pieces and spot drill with drill press and still have all the holes align.

Bguns
10-29-2007, 02:38 AM
I bet Krems wants to make bullet molds..... They are kind of thick for boring a ~.250 hole, roughly 1 to 1.5 in deep..for locating/alignment pins.

As long as the mold blocks pin holes were drilled and reamed with both blocks together, hole location is pretty loose tolerance wise..

Using a cherry (tool for cutting mold cavities) is the way most are done , (unless bullet profile allows boring blocks out in lathe , ie flat tip bullet) The Cherry is run sideways 1/2 way into mold blank and then 1/2 way into opposite blank.

I hope Krems knows even the oldest US bullet mold maker does not achieve that great of accuracy in cutting the molds... They state that the cavity may be as much as .002 too deep on one side or other .....

Most cast bullets are run through a lube/sizer after casting anyway...

Your Old Dog
10-29-2007, 06:41 AM
What I suggest you do is stack those two parts and bore the holes you need for the locating pins. That way accurate locations are relative and you don't need to sweat table and saddle offsets. For that you'll eventually need a boring head. Work one hole at a time, pre-drill with a center drill, drill each a bit undersize then drill out the remainder of the stock with an on-size drill.

This is the only way I've ever had any luck doing what you are trying to do. I get a pin in the first hole as soon as it's drilled to hold register for the following holes.

On a side note: Whenever I home brew a project, all screw holes are placed on multiples of 1/8th inch. Now I can just get a tape measure close to the drilled holes and tell you if they were 3/4 or 7/8's apart because I don't drill them anything other than 1/8's. (I mean you won't find me drilling holes at 27/64's off each other if it's a project I homebrewed myself.) Call it a shop standard for me.

This may or may not have anything to do with your question. If you're having trouble figuring out how far the holes are apart, Sir John suggested a simple way some time back. To measure the distance between two holes, put a properly sized pin in each hole, measure to the outside of each pin and then subtract the diameter of one pin. I milled a flat on the end of one pin to the center of it and use that to rest the caliper on as I measure over the amount needed for the center location of the second hole. It works surprizeing well for me.

oldtiffie
10-29-2007, 08:57 AM
Hi krems.

I haven't got time to respond to this today so I'll just use this interim post as a "bump" to keep this thread where I can find it tomorrrow - or the day after.

There are a few easy, effective ways that cost very little, require no reamers or boring and can be done with what you have on hand.

Some may say its too "Agricultural" - but we'll see.

rkepler
10-29-2007, 09:37 AM
I'd say you must be good enough to center punch individual pieces and spot drill with drill press and still have all the holes align.

Actually, I'm so bad lining things up by eye (be it center punch or drill) that I use the DRO for most everything. I can line up a wiggler but it's no faster than using an edge finder if there's a couple of edges.

But hole accuracy is overrated in the home shop - the only time I had to use jig boring techniques was when I was making new jaws for a Verti-Vise. Since the vise is vertical the parallels have 2 1/8" dowel pins on each end to fit into matching holes in the jaws. There I needed the holes very accurately placed to match the parallel ends and to be sure that the parallel remained, well, parallel to the table. There were quite a few holes (48 in all? might have been 64) that needed to be made, all in A2 (my favorite jaw making material). It all came together, all the parallels are nice push fits into the holes in the jaws.

aboard_epsilon
10-29-2007, 10:17 AM
i say spend all your time getting the first hole to line up ...
then put dowl through it ...or tight bolt ...line the rest up ...and spot drill

thats if im understanding where you are coming from.

all the best.mark

krems
10-29-2007, 06:45 PM
Yes...I'm Trying to make some bullet mould blocks. I'll have 3 alignment pins per set of blocks. I plan on having both blocks clamped together when they are either bored, drilled, or reamed. I'm trying to figure out what would be the best method to punch a 1/4" hole through both halves of the blocks and use some sort of a press fit dowell pin for alignment. Drill bit / reamer choices are endless. Because of the press fit pins I'll be using the hole needs to be straight and uniform in dimensions. I'm king of leaning toward drilling undersize then final ream to dimensions. The boreing bar scares me a little in that I might miss the dimension I was trying to get.

I can see getting a DRO eventually on the milling machine. I'm more concerned about being able to punch a precise hole through both blocks. Hole spacing can vary as long as I get 3 straight and true holes.

I'm sure there is more than one way to go about this. I was just curious how everyone else would do this and what tooling they would need.

Thanks for the great tips!................krems

Uncle O
10-29-2007, 09:37 PM
To facilitate mold seperation you will want to heed MechanicalMagics' advise and ream one half of the mold with slip-fit tolerances. Otherwise you will be SOL when it comes time to remove your bullet.