LinkBack URL
About LinkBacks
Small drills require higher spindle speeds. I would go as fast as your spindle would allow.
| | |
Lord help me from breaking anymore drills! Whats the trick? I am drilling into Aluminum going about 1000rpm and barely pecking into the parts with jobbers on a series 1 Bridgeport using a Wire Gauge Drill Chuck (note I cant hold it near the flutes). I have to set up to drill at least 1.5" length too.
Small drills require higher spindle speeds. I would go as fast as your spindle would allow.
At 200sfm, a 1mm drill in aluminum should be going 19,000 Rpm. Your lack of spindle speed is most likely breaking your drills.
my machine only goes up to 3500rpm!
Then I would go 3500 rpm and peck it @ 7.0 IPM, if your drills continue to snap, reduce feedrate. With that deep of a hole, you're going to have to return the drill to the rapid plane to clear the chips every .05 or so to keep the flutes from packing with chips.
Ok what type of tool holder do you all suggest? We are currently using a Wire Gauge Drill Chuck and collet. It appears that there is a lot of wobble as the drill enters after each peck. I was thinking of using a pin vise so I could gasp closer to the flutes.
Also and particular flavor drill for aluminum?
Center drill your holes first, the pin vise should work, and any jobber or parabolic flute (non-tin coated) drill will work.
I have drilled deep holes like this before with long small diameter drills. I had to set up a fixture(bolted to the back of a Kurt vice) above the part to use a drill bushing that helped stablize the drill. I also needed to keep the drill wet with WD40 or the like and continuously draw out the chips to keep the flutes clear.
If you cannot grip it nearer the flutes, cut off some of the shank?
Another trick with tapping holes this small is to pack the hole with soft wax or grease. As the tap sinks in, the packing pushes the chips out.
DC
Learn cause and effect through experience. Mastering those relationships is the "Common Sense" ability within the art of any trade.
ok how does one use a drill bushing?
That ultimately depends on how you get the part in and out of your workholding. But, basically if you have a plate, arm or deck above your part, drill and ream a press fit hole size of the bushing OD on location you expect the hole to be in the part below it. The bushing ID will be that of your drill bit size.Originally Posted by star1280
A drill bushing is nothing more than a hardened steel liner to guide the drill. If need be, you can have a bushing with another sleeve to accept different size drill bushings. Like, say, spot drill size and then replace it for drill or reamer sizes. These are quite common for drill press fixture operations without the need for a more precision positioning machine. The precision is built into the fixture and locates hole relationships with fair repeatability. Very productive on a bank set of drill presses.
DC
Learn cause and effect through experience. Mastering those relationships is the "Common Sense" ability within the art of any trade.
I have drilled and tapped a lot of 0-80 threads in aluminum. I would suggest using a form tap if you can. Obviously, there are no chips when using a form tap. The less obvious advantage is the drill is larger (.055" for a form tap vs. .0469" for a cut tap) which makes it stronger.
I start with a 1/8" 90* spot drill .040" deep. Then, a .055" drill at 7500rpm with .015" pecks and 5ipm. I run the 0-80 form tap at 1500rpm. Flood coolant is important.
Posting Permissions
| | |
