End mills bigger than shank for deep pockets?

[Jim27]

Very new to milling and have a general question about milling tools. I have a small Servo Products mill that has a max collet size of 1/4" but think the question would apply to larger machines too. I picked up a few end mills and they have fairly short cutting length - for example, a 1/4" diameter with 1/4" shank and 1/2" cutting length. What is good practice for milling a 1" deep pocket? I can get up to 3/4" cutting length and maybe a bit longer but the point is for a pocket deeper than readily available end mills cutting length. (I realize there will be deflection on this small shank at this depth so will need to take small cuts.) If I go deeper then the shank may rub against the side of the pocket and the chip exit will be restricted too - how bad is this? Are end mills bigger than the shanks readily available? Or is there some other solution to this?

Similar Threads:

• Need help routing/ reaching deep pockets.
• Need Help!- Eroding deep pockets
• Chip removal from deep pockets?
• Deep pockets
• Deep Pockets

[Jim Dawson]

You can buy 1/4 inch with 1 inch cut ''endmills'' at your local hardware store. They are solid carbide router bits, they work great in all materials if you are careful. And the best part is you can get them on a Saturday afternoon. I normally keep a few in the drawer.

Longer length end mills are readily available from various vendors. Google ''endmills'' for vendors, there are hundreds of them. End mills with a larger cut than shank are also readily available. Carbide tipped router bits work well also, and again available from your local hardware store.

[Kenny Duval]

The only issue with Homeless Despot router bits is they will be straight flute bits with no ability to center cut. If your DOC is .250 then that's .250 of cutter face slamming into the material all at once. Ok for wood...not so ok for metals. Go .500 deep and the problem only gets worse. They will work if you are in a bind but you are better off with end mills designed for cutting metal.

If you need to go an inch down then order 2 1/4 inch carbide end mills. One with a .500 flute length and the second with the full 1 inch flute length. Rough the hole with the shorter flute length end mill in multiple depth passes and leave .005 material radially then run a finish pass with the second end mill at full depth to clean up the walls of the pocket to the finished dimension. Your results will be better.

They do have these that would work in a pinch.

Diablo 1/4 in. x 1 in. Carbide Up Spiral Router Bit-DR75102 - The Home Depot

[dertsap]

, a 1/4" diameter with 1/4" shank and 1/2" cutting length. What is good practice for milling a 1" deep pocket?

grind some relief in the shank above the cutting edges .

[awerby]

This might work with wood (using router bits as was previously suggested) but it's not advisable in metal. The reason your mill's spindle won't accommodate a tool with a shank size more than 1/4" is probably because it doesn't have the torque to spin one that's wider than that. Trying to do it anyway will likely result in either the tool getting stuck in the material while the motor stalls or the belts start burning, or the collet spinning while the tool remains stuck. There's a reason you often see metal-cutting tools with a flute diameter that's smaller than the shank, but rarely the other way around. If you need to make a pocket that's an inch deep, use a 1/4" carbide tool with a flute depth that's long enough, and take it easy, so you don't snap it off.

[alan_3301]

I've had good luck with the Diablo 1/4 carbide upcut spirals. Even with the 1" flute length, I was able to cut 30mm AL plate with it with a slightly rubbing shank. In one job, I went through about 400 inches of it 0.080" at a time, or about 6000 inches of cutting, with 2 bits. (broke the first one due to chip clogging).
If I could find a comparable bit online for a little cheaper, I would go that route, but that $20 bit does fine for me in AL and wood.

The only issue with Homeless Despot router bits is they will be straight flute bits with no ability to center cut. If your DOC is .250 then that's .250 of cutter face slamming into the material all at once. Ok for wood...not so ok for metals. Go .500 deep and the problem only gets worse. They will work if you are in a bind but you are better off with end mills designed for cutting metal.

If you need to go an inch down then order 2 1/4 inch carbide end mills. One with a .500 flute length and the second with the full 1 inch flute length. Rough the hole with the shorter flute length end mill in multiple depth passes and leave .005 material radially then run a finish pass with the second end mill at full depth to clean up the walls of the pocket to the finished dimension. Your results will be better.

They do have these that would work in a pinch.

Diablo 1/4 in. x 1 in. Carbide Up Spiral Router Bit-DR75102 - The Home Depot

[warrenb]

There are some companies that have the shank ground. Lakeshore carbide is on of them. You can also find cutters with smaller shanks at MSC.

[Jim Dawson]

The spiral upcut Diablo bits from Home Depot are center cutting as are the Botch equivalent from Lowes. Measure the cutting diameter before using, I have found that the 1/4 bits can be as small as 0.239 on the cutting end, but the shanks are always dead on. When not ramping into a cut, I normally pre-drill a pilot hole where the cut is starting, that way the bit is not plunging into the material and is a lot easier on the bit and machine. I always do this for end mills also.

The straight flute, carbide tipped bits work well in plastic and wood, but not so good in metal. Having said that, I have done some deep pocketing in aluminum with straight flute, carbide tipped router bits. But a pilot hole is required to start a pocket.

On your machine, I proabaly would not use any bit with a cutting diameter greater than 3/8, and make allowances for the increased cutting forces. In all cases you have to make allowances for the machine you are using regarding depth of cut and stepover. Solid carbide bits are a lot less forgiving than HSS bits and they like rigid setups and stable machines to minimize breakage.

[dertsap]

Edit

mistook something ,

[vertcnc]

Here are some reduced shank end mills from MariTool. They are great for deep pockets. https://www.maritool.com/Cutting-Too...219/index.html

[Eldon_Joh]

I have cut A36 steel 5/8" thick with a 1/8th inch 4 flute carbide end mill, .25" length of cut. due to the chatter and chip re-cutting and runout the end mill cuts a slot wider than its shank.

A straight flute router bit requires hundreds of times more cutting torque and force to shave off a chip that is as wide as the cutting length, vs a thin ribbon. while the hp averages out, small milling machines don't have the rotational inertia and mass or stiffness to resist the cutting force. this is the same reason why dovetail cutting tools are such a pain to use. i did find a company that makes helical dovetail cutters, but they don't appear to keep any on hand, custom only.