Dive milling.

[M-man]

I am milling out some kind of deep pocket and were thinking about dive milling it with a drill with inserts.(ive got a rigid one). Anyone that got any experince with this kind of operation. how big step overs etc (tool dia approx. 1")...The material to be cut are aluminium, ss6082-T6.

[rwwink]

Most of the people I've seen do this use a big two or three flute, center cutting end mill and step over 1/4 to 1/2 of the diameter. A drill, with the pointed end, will be forced off center by the unequal cutting forces and will break..like trying to drill half a hole

[Geof]

Some machines have a pocket milling canned cycle which makes it easy, just drill a hole at the center and then use a two flute center cutting mill and program a step over as rwwink suggests depending on how much spindle power you have available and make the depth of cut maybe two thirds the step over. Make sure you have plenty of fast moving coolant to flush the chips as much as possible.

If you are writing the pocket sequence there are a few ways which I think are more personal preference than anything. Zig zag your way across, start at the center and step out or start at the perimeter and step in. Doing a plunge straight down even with a center cutting mill can make things shake a bit so either drill a start hole and plunge there or ramp down during a straight move about five times as long as the depth of cut.

[RICHARD ZASTROW]

This technique is also refered to as "plunge milling". Originally, cutters were developed by Ingersoll but are now available from almost all cutter suppliers. The tech section of their catalogs, and probably on line as well, show all the step over amounts for a given diameter cutter. The neat thing about plunge milling, I believe, they can remove more cu.in./hp than peripheral milling with end mills.

try www.secotools.com

[RICHARD ZASTROW]

I just ran the plunge milling video on the Seco site. VERY IMPRESSIVE!!!

[roninB4]

A lot depends upon the machinery and cutting tools you have available. When I did core/cavity work we would often use spade drills to just remove as much metal as possible and then switch to a milling cutter to plunge/ramp in Z into the cavity. If you have coolant through spade drills you can waste a lot of metal in short order. It may be an outdated habit but I still do this on manual machines. Drill what I can and save the endmills for shapes/sizes. A lot of times it most advantageous to get the chips the heck out of the way, avoiding re-cut that mars finishes and wears the cutter. I like getting as much metal out of my way as possible so I don't have to deal with vibration of heavy cuts or prolonged passes to approach the final wall. Drills are efficient fast ways to remove the excess in your shape and can be resharpened easier/faster than an end mill. Maybe I'm too 20th century. Whatever method you use, get the chips out of the cutter path. If you're milling the excess then use a 2 flute with air/coolant flooded away from the direction of cut. Pockets get filled quickly so have a small wooden dowel on hand to shovel out the overflow during the cut. Hope this was of some help.

[RICHARD ZASTROW]

roninB4, Plunge milling cutters were actually invented for heavy metal removal on mold cavities. I suggest you look up the Seco site and look at the plunge milling videos. Like you suggested, start with a spade drill. Personally, I'd then switch to the plunge cutters, they really chew out the chips. keep on kutn

[Geof]

Originally Posted by RICHARD ZASTROW I just ran the plunge milling video on the Seco site. VERY IMPRESSIVE!!!

Yes it is impressive but may not necessarily carry over into aluminum. They are cutting dry with an air blast. This allows very high speed and feed because the steel chips come off red hot; the tensile strength is gone so in effect the cutter is working on very soft material. In addition the depth of cut is very small so there is little chance of plugging the cutter with chips; steel chips are not likely to plug the cutter anyway because they come off in strings or nice curls.

With aluminum running at appropriately scaled up speeds, feeds and depth of cut, coolant would be essential and probably more flute clearance would be needed for the larger chips that would be created.

Incidentally if you look closely the cutter does not plunge straight down between each circuit around the pocket; it either does a small circle or a small straight move so it is ramping down the plunge depth.

[Tony the Ferret]

Hi Guys, glad you have looked at plunge roughing and yes you are correct it can reduce roughing by more than 60%. But some of you are a little misinformed about the types of stratergy's available.

1. some cutters are centre cutting, so do not need the holes created with spade drills
2. Some cutters do need the pilot hole first
3. Some cutters are like trepaning tools, and also do not need spade drills

WorkNC has a toolpath for all of these types within the HVR toolpath.
In answer to the member who asked about stepover and advancement forward. (www.foregonesolutions.co.uk) has a screen shot of this in action.
Step forward is recomended to be less than the tip length, side step will depend on the quality of roughing required (30% to 50% of tool diameter). Another thing to consider. The tips are seated on a pocket in the tool which gives the tip support when plunging down, BUT when the tool is retracting there is a good chance of the side wall of the cut material disturbing the tip in the seat. WorkNC has overcome this with a small offset move AWAY from the material BEFORE the retract stroke

[RICHARD ZASTROW]

I think that retract is what roninB4 is seeing. I never did that and didn't loose an insert. Not saying it couldn't happen though. If it's there, use it. We were plunging horizontally so the chips fell out and we did blast air at the cutter both for cooling and chip evacuation. Plunge was straight in except near outside walls of cavity which were tapered.

[Gary55Ford]

I've been using A TRAK DPM bed mill with PROTO-TRAK programing & it has canned pocket programs for circle rectangle,and iregular pockets. I use a center cutting 2 flute end mill on 6061-T6 aluminum with no problems & an excellent finish. No starting hole is nessecary.

[sten]

Hi!

Coromant has indexable drills R416.22-xx with short chiprooms dedicated
spec. for plunge milling , they also have cutters R210-xx dedicated for
plungemilling and highfeed milling .

www.coromant.sandvik.com/

Regards/sae