Will this work?

[t28c34]

Will it work, taking a jacobs chuck and making a threaded 1/2" shaft for it to be able to chuck up to my spindle to use as a drill head?

[gerryv]

The spindle spins many times too fast. These chucks are not balanced nearly well enough to do that. The highest you're likely to spin a drill chuck is maybe 3,000 rpm with a small bit; lower for larger diameters. Your spindle runs up to 18,000 likely.

My guess is that it would quickly ruin the bearings or worse, tear the spindle apart before you could shut down. I'd not want to be standing anywhere in the area without a concrete wall between me and the machine.

[t28c34]

Thats kind of the same thought i had. Not sure how slow i can slow down my spindle.

[Simops]

Thats kind of the same thought i had. Not sure how slow i can slow down my spindle.

My spindle won't go below 6000

Ciao

[Brian Harnett]

It would be easy just to make a mount to attach to the z axes for a drill I am pretty sure the bearings in a spindle are not designed for constant vertical loading.

[t28c34]

Yea I didn't think of the vertical load on the bearings, any ideas for a drill mount for a 05 PRT Alpha?

[gundog]

They make collet chucks designed for high speed machining but that won't help your bearings with the radial load.

Mike

[scottp55]

Terry, What size holes, how deep? Can't you profile or pocket toolpath and spiral an appropriate bit in?

[t28c34]

The the 1/4" and 1/8" holes are no problem with the spindle. But now they want a .109" (7/64") holes, 1/4" deep. Thats not a hole lot of load on the spindle i would think. I bought a cheap elecric drill today, i dont think it will fit in the carraige on my bot. I would have to midify the handle of the drill. I dont really want to go with a air drill.

[Brian Harnett]

For something that small you can machine your own collet or have a shop with a lathe do it I use brass or aluminum though preferably brass for my custom collets.

I don't have a picture of one of my collets but you can get an idea from these bit extenders.

The collet would have a slot cut down one side for compression.
http://i.imgur.com/XoLQ4Nz.jpg

[Burkhardt]

The the 1/4" and 1/8" holes are no problem with the spindle. But now they want a .109" (7/64") holes, 1/4" deep. Thats not a hole lot of load on the spindle i would think. I bought a cheap elecric drill today, i dont think it will fit in the carraige on my bot. I would have to midify the handle of the drill. I dont really want to go with a air drill.

Not sure how fast you need to drill them but I pocket small holes with such 1/16" bits (http://www.ebay.com/itm/380774607310) or 3/32" bits (http://www.ebay.com/itm/151251944889). These happen to have 1/4" flutes but I have seen them with 5/16 flutes as well. Obviously somewhat fragile and if you need to punch a lot of holes in short time not an option.

[burchbot]

You can find Micro End Mills here. Would these work for you? http://american-carbide.com/MicroEndMills/MEStandardProducts.php
Dan

[coryatjohn]

I like the Kyocera micro endmills. They are robust and inexpensive. The 1/16" bits are workhorses. They are not solid carbide but hold up well. I bought a set of 10 for $25 (or something like that). Haven't broken one yet.

[scottp55]

Terry, Kyocera has two good advocates. We drill hundreds of cribbage holes .1155"D to .257" depth in hardwood and use a 7/64" 2F end mill from Carbide plus and no problems at 1/2Diameter,.5,15K. Did use the PreciseBit .117" 2F fishtail and were very happy until we went to new pegs and had to go to 7/64" for smaller diameter. All good clean holes and bit stays cool. Here's 2 more suppliers we use and are happy with.http://www.precisebits.com/products/carbidebits/precisebit-soft.asp

http://www.precisebits.com/products/carbidebits/precisebit-soft.asp

[t28c34]

Thanks guys, so you have no problems using a spindle as a drill for such small holes?

[Burkhardt]

Thanks guys, so you have no problems using a spindle as a drill for such small holes?

No problem if using a smaller bit that allows to eject the chips. I never use actual correct size drills that will probably have to run much slower and/or with pecking.
If the bit is bigger or equal than half the hole diameter you don't need a pocket toolpath, just a simple inside profile, preferably with spiral ramp. Feed rate must be rather slow. I use 30-40 ipm horizontal and plunge feed for holes up to 1/4" . For holes smaller than 1/8" maybe even slower.
If the rate is too fast the movement becomes very jerky and somewhat inaccurate on my machine due to the small radius. Spindle speed is about 13-18 krpm.

[curtiss]

Seems someone, somewhere makes various bits 7/64's with a 1/8 inch shank

Not sure what material you are drilling, but you can always mark the holes with the Bot and drill them out later with a drill.

[scottp55]

Get bit somewhere around 60-70% of your hole diameter. Use some scrap of the same material as the job and do a linear array and try half dozen holes at a time to check chip size and heat. Ash and cherry both cut well at 1.2, .5, 15K with a 7/64" for a .1155"D hole. Haven't done maple yet and you're going to be using smaller bit. Only smoked one bit by being to conservative with speeds. Maybe G. , or John can get you closer with their 1/16" experience if you tell them material. Always get a little nervous doing something Brady says not to do(Drilling), but then again it's not REALLY drilling. No problems with Desktop doing it YET(Probably cursed myself). Much faster profiling inside with a spiral that peck drilling.