Hole drilling help

[stevehuckss396]

I have to drill 2 - .3125 holes in 1 inch aluminum round bar. These 2 holes need to be dead center and exactly 90 degrees apart and do NOT intersect.. I have made 2 attempts and the closest i came was a 4 degree error. The drill seems to be drifting.

Any tips or tricks. Should i drill small and try a reamer? Maybe drill with a smaller drill to pilot and then step up to the 5/16?

[lerman]

Assuming you have proper tools and fixtures, this should not be an issue.

Why don't you tell us how you are doing it?

Hint #1 if you are using a stub drill, it can't possible bend by 4 degrees. How are you holding the rod and how are you rotating it 90 degrees?

Ken

[stevehuckss396]

Originally Posted by lerman Assuming you have proper tools and fixtures, this should not be an issue. Why don't you tell us how you are doing it? Hint #1 if you are using a stub drill, it can't possible bend by 4 degrees. How are you holding the rod and how are you rotating it 90 degrees? Ken

I am holding the rod horizontaly in a rotary table with a chuck mounted to it. Getting 90 degrees is easy but the drill seems to be drifting.

Someone mentioned a screw machine bit would be a good choice along with spot drilling before hand. Another mentioned pre-drilling with a smaller drill and then finishing with the proper drill or an end mill.

What effect does drill RPM play here?

What do you think about

1. Indicate along X axis, find center, and Spot drill

2. Change mill to highest RPM possible

3. Drill thru with a .250 drill bit.

4. Finish with a .3125 2 flute endmill chucked in a collet.

Bad idea? Should i finish with a .3215 drill?

[martinw]

Originally Posted by stevehuckss396 I have to drill 2 - .3125 holes in 1 inch aluminum round bar. These 2 holes need to be dead center and exactly 90 degrees apart and do NOT intersect.. I have made 2 attempts and the closest i came was a 4 degree error. The drill seems to be drifting. Any tips or tricks. Should i drill small and try a reamer? Maybe drill with a smaller drill to pilot and then step up to the 5/16?

Dear Steve,

No expert, but here is what has worked for me in reasonably low precision applications, eg drill press stuff.

Drilling into round stock is a problem. You really must hold it securely.

The drill tip will skate everywhere if it has nothing to centre on.


IMVVHO, start with a centre drill. I nice big fat one. It will not wander. You only have to drill deep enough to provide a guide for the point of the next tool. Do not move the workpiece, and put your 0.3125 drill in the chuck.

When it comes to 90 degree alignment for the next hole, there are better men than me hereabouts.

Best wishes,

Martin

[Gary55Ford]

Are you center drilling before using the drill bit?

[stevehuckss396]

Originally Posted by Gary55Ford Are you center drilling before using the drill bit?

I am now!! (Grin)

[lerman]

Another trick is to use a center cutting end mill to put a small flat on the rod before drilling.

Ken

[bigtoad170]

I had a job a few years back drilling in I think about 3/4 maybe an inch aluminum rod I remember doing a few hundred of those suckers anyway the operation I had to do was
1. Center drill with an over size drill like mentioned above by martinw
2. Drill with a stub drill I think about .050 undersize
3. Then with a two flute endmill in a collett not a drill chuck about .015 undersize
4. Finish with a reamer not pushed all the way in the collett maybe about an inch so it can float a little
Maybe someone else would have better input on rpm but I would probably stick around 700- 900 rpm for drilling maybe 300 for reaming It does just suck switching from drill chuck to collett but once you get a rythm probably chuck out 80-100 in ten hours

[keebler303]

If you are having problems after the above suggestions, an endmill as the finish tool can help as it does not wander. if an end mill tried to wander, it would cut and then come back to center. a drill cqan be pushed from side and move the hole over. An end mill will just cut on the side.

Matt

[martinw]

Originally Posted by lerman Another trick is to use a center cutting end mill to put a small flat on the rod before drilling. Ken

Dear Ken.

Yes indeed. I do not have a milling machine but I've hand filed a small flat on small diameter workpieces to discourage the drill from wandering.

Best wishes,

Martin

[martinw]

Originally Posted by martinw Dear Ken. Yes indeed. I do not have a milling machine but I've hand filed a small flat on small diameter workpieces to discourage the drill from wandering. Best wishes, Martin

Dear Ken,

This is slightly "off-topic", but putting a small flat on equal angle aluminium or steel profiles works well too if you want to drill a hole at 45 degrees to the section axes, and on the "point".

Sorry, machining experts (amongst whom I not numbered) will know this already. I was thrilled to discover this for myself a few months ago.

Best wishes,

Martin

[dapoling]

Steve most errors can be found in the setup.

How deep are you drilling as well ?

1. Recheck your setup with a test indicator while your material is being held to ensure your rod is being held in alignment of your Z axis.
2. Ensure your drill surface is prepped with a flat surface and use a center drill to start.
3. Drill undersized leaving about .015 on the diameter.
4. Bore or use a Boring endmill with a G85 (bore in and out) to finish the hole to size this will take out any wandering of the drill or reamer for that fact.
5. when you rotate 90 degrees check with your indicator to ensure your table has located properly. (I have been amazed on how many tables are warn and do not locate properly).

Never assume that a chuck or another holding device is right on the money, use that indicator so you know, once you verify then you're off and running.

Hopefully this will help.

not met to offend anyone but to ensure understanding I post the following.
(a reamer will only follow the hold that is made for it)
(boring endmill is ground so that only a small portion on one flute will be cutting)
(G85 can be used with a L2 or L3 (repeat) command for tight tolerance holes for repeatability)