Plunge cuts/drilling with a spindle query

[johnm]

Folks -

I understand that you're supposed to ramp into cuts and corkscrew (pocket??) into drilled holes to reduce end load stress on the spindle.

If the cutter (say a straight bit) has a cutter at the base to remove waste from the bottom of the cut (as in a dado) would it be okay to do a slow straight plunge? It sure seems odd that a ~$3,500 spindle can't do straight plunges without extra work. How hard could it be to design the unit to take end loads?

Finally, for drilling holes, couldn't you use a brad point bit? - I understand that you'd have to use one the same size as the collet - I've never seen brad point bits with fixed shank sizes and different cutter diameters.

I certainly don't want to push my bran-spankin' new spindle into doing things it isn't designed for, but I am wondering what thresholds I am working with. Drilling a bunch of 1/4" shelf pin holes 3/8" deep in MDF with a slow plunge doesn't seem like it would be asking for much....

I'd appreciate any input on this, and a source for any fixed shank size brad point bits if you have any ideas.

Thanks!

John Moorhead

[ron brown]

John,

Spindles usually have collets available in almost any size. At one time KBC tools had an imported line that were quite reasonable. At low spindles speeds I would not hesitate to use screw-length drills in the proper collet.

Ron

[richards]

Be sure that the carbide on the cutter extends at least 1/2 the diameter of the cutter. Most of my carbide tipped cutters were not designed for plunge cutting. A solid carbide spiral cutter (at least the ones that I use) usually has the proper configuration for plunging.

Also, I try to drill my holes using a separate file so that I can slow the spindle down - usually around 5,000 RPM instead of the usual 13,000 - 15,000 RPM.

[mrdovey]

John...

I do straight plunges all the time. If you're drilling a deep hole, you might back the bit out midway and re-plunge deeper - to allow chips to escape and to avoid too much heat buildup. A spiral up-cut bit works well.

When you're making holes with a router bit, you can make any size hole the same size or larger than your router bit.

If you're using a router bit, it should be a plunge-type bit - and if you're using an end mill, it should be a center-cutting type.

If you chuck up a 1/4" spiral bit, you can drill lines of perfectly-spaced shelf pin holes with ease.

I like the Lee Valley carbide tipped lipped brad point bits; but haven't ever felt the need to use one on the 'Bot.

...Morris

[gerald_d]

Why do you guys feel the need to slow the spindle for drilling? Is it for the bearings or the burning in the hole? Do you also slow down for plunges before a straight cut? Somehow I have never had the urge to slow down the cutter's rotating speed.....

[richards]

Gerald,
For me, it's a two part answer. First, Colombo suggests reducing the feed rate to 10% of normal when doing a 90-degree plunge cut. So, instead of running at 6-ips I run at 0.6-ips. Secondly, to get the proper chip-load at the slower speed, I slow down the spindle; however, I normally use 4,000 - 5,000 RPM as my drill speed - based on sound. At slower speeds, the cut sounds way too rough. At higher speeds, there is evidence of burning.