Deep hole drilling

[tutran]

Hi all,

I'm having a problem with the deep holes(it's walk on me at the end), so maybe someone can help.

The hole dia. is .125+-.002 4.500 deep.Mat. ALu.

Here are how I do it:

_spot drill

-drill .120 about .750 deep

-drill with .125 2fl.endmill .500 deep

_drill .125 regular jober to 1.7 deep

_drill the rest with .125 extra long

The hole dia. is within the tolerance, but the

holes is walk around .008 at the end.

Are there any methods that is better, beside gundrill?. Thanks ahead.

[George Simmons]

If this is on a lathe, I'd drill the hole first and then turn the OD between centers, making everything concentric. On the Mill, 3 flute drills work pretty well, but if you drill a smaller pilot hole thru, the 3 fluter will tend not to walk... That's what core drills are for.

[Moldmaker74]

I would look into a Parabolic drill and use the manufacturers feed and speed. Probably much faster than a standard drill bit.

 

I would also skip the end milling part because with spot drilling, you should not have trouble maintaining the location on the top surface.

[SBerg]

Titex and osg have some good drill selection programs on their web sites. Do you have a coolant thru spindle? http://www.titex.com/sandvik/3432/Internet...B8700412A0AC125 6CCB002EA86B&banner=/sandvik/3432/Internet/DE07001.nsf/LookupAdm/BannerForm%3FOpenDocument

[Tinhman]

Making sure your feed and Speed are OK then try to keep the tip of the drill in side the hole at all time ( your may need the long format for your drill). 4.5 deep with Alu. is not that bad.

Hope it help.

Tinhman

--------------------

Mc X & Sw07

[mold100]

I drill 1/8 holes in alum alot, I probably would not step drill, soft materials, like alum, copper, and plastics, you should start out with you largest diameter. I use titex drills and if that deep I use a regular length as deep as could then go to the longer drill and spot drill instead of center drill. be sure your feeding the drill fast enough putting pressure down and not allowing run out to double cut the hole out of tolerance, On the consrvative side to reduce chatter sounds I use a lower rpm generally 2800 rpms and 14 to 17 ipms with a .07 peck with the longer drill. .125 with the standard drill using chip breaker and full out pecks with the deeper drill.

[Lars Christensen]

If this is for production run, I would look into straight flute carbide, but it proberbly have to be custom made for 36XD reach.