Drilling with end mills?

[sp1nm0nkey]

I've heard I should never ever drill a hole with an end mill if there isn't already a hole at the center for the chips to clear. Why can't the end mill clear the chips and how deep can I plunge with it at a time (if I'm cutting a pocket)

[dertsap]

http://en.wikipedia.org/wiki/Endmill
an endmill is an endmill a drill is a drill , you just cant use one for the other , can you not add a ramp move rather than plunging ?

[nwrepair1]

I drill with an end mill all the time. The reason being the endmill is also an edge rounding tool. I also use it to put pin holes in the cutting boards I make. I use phenolic material, wood grade x, never had a problem. I just finished building a grid vacuum table 57" x 114" for my router. It is 1" cast K100s aluminum with 220 3/8" holes that were drilled through with an end mill. I plunge slow, 10 " per minute, at 9000 rpm. I also use an air vortex to cool the bit.

[mrainey]

Some end mills are designed to center-cut and some aren't, but none of them will make holes (plunge) nearly as fast as a drill of the same diameter.

[LeeWay]

I sometimes use a drill mill.



They are quite versatile little tools.
Here is a video of me using one for several different milling ops. This was just after I set me mill up the first time and was some initial part runs. I have since redone most of the mill and moved it to the other side of my shop on concrete.

http://www.youtube.com/watch?v=YG7j_u5Ffgs

http://www.youtube.com/watch?v=YG7j_u5Ffgs

[Geof]

Originally Posted by sp1nm0nkey I've heard I should never ever drill a hole with an end mill if there isn't already a hole at the center for the chips to clear. Why can't the end mill clear the chips and how deep can I plunge with it at a time (if I'm cutting a pocket)

To answer this question have a look at the end of an end mill that is ground for center cutting. The clearance behind the bottom cutting edges is much less than the clearance behind the side cutting edges. There is simply not enough space for a chip to occupy and also there is no way for the chip to get out. If you do very, very short pecks you can drill with and endmill but it is much better to ramp down in a helical path. For doing a pocket it will be best to predrill a hole but if you want to avoid a tool change instead of drilling with the endmill slot down using a little ramp back and forth. Move the tool sideway about 1/2 its diameter while going down about 1/8 the diameter; this creates room for the chips to get out. It is not ideal but it works.

[fatal-exception]

I also drill with end mills all the time. They leave a very nice finish on the inside of the hole. You will have to go slower than a drill, but there's no problem evacuating the chips. Mostly, it's done when you want a flat bottom hole such as a counterbore. As far as depth of plunge, about half the tool diameter is standard. Sometimes more or less to end up with the least amount of passes to achieve final depth.

Also, thin materials can easily be drilled with endmill, where a drill bit would grab and tear at the piece, the endmill just sizzles through it and leaves a round hole rather than a triangular one.

[kalmah]

http://www.nachi-fujikoshi.co.jp/eng...mil/index.html

Nachi produce end mill wich can easily drill and slot. It works perfectly in steel.
The feed is 4 times lower than a drill.

Warning, it doesn't work with other end mill manufacturer. It have a special flute design in order to allow the drilling.

[dertsap]

the thing is it can be done , but in production i am a firm beleaver that it is a poor practice , i've seen far too many melt downs , oversized holes chipped tools etc due to guys plunging endmills , we rarely have spare parts , normally we have exact material to cover the customers order , there is no room for error , i always love a shortcut but this is an area i won t adventure in

[sp1nm0nkey]

Yeah, I already chipped a cutter so I'm never ever doing it again. I was just curious why and how pocketing works without drilling a hole.

[dertsap]

as Geof said , ramp it side to side in or helical interpolation ramp

[kduffy]

As Leeway said in post #5 those are the way to go for production if you don't need a flat bottom hole (combination drill and taps are made for thru holes by most tap manufacturers). Fortunately for Hobby folks and general jobbing shops, they are easily made from those two flute endmills that lose a corner or dull (at the typical end cutting region) and are too small to justify a regrind. You surely regrind a drill, dont' you? It can be done to a four flute, but it will likely not cut on all four unless ground on a machine, so simply remove them farther back and make it a two flute drill / four flute side cutting endmill (for slotting plate). The obvious thing to look for is a center cuttting endmill of course (if it is ground to the center looking at the end, does not look like it has been center drilled).

Often I have found that the carbide endmill will cut a very nice clean hole in hardened die steel, especially on weld repaired dies where an existing ejector pin or core hole must be located. Locate the hole, dog it down, then do the weld repair in the machine, (Probably shouldn't try this on a CNC, works well on manual machines) after welding, you just recut the hole, which would not have been round enough for drilling accurately.

For thin sheet metal, as mentioned earlier the endmill would be the choice unless a brad point drill is available. For true flat bottom holes, an end mill would have to be custom made to eliminate the center relief of 2-5 degrees that is ground in. It should also not have the center exactly on center, a few thousandths past center with one flute will clean the center all the way. I guess the poor have poor ways, but we still get it done in our own time. For simple endmill regrinds, try using a surface grinder endmill grinding fixture in the mill, with a cup wheel on the spindle. This is a case where you won't likely have enough spindle speed, so replace it with wheel diameter, Surface Feet Per Minute is what you are looking for after all. It will of course require a rigid machine. A little slow will still work just not perfect, VERY light passes, remember you are grinding, not milling.