Hello all. I've got a Haas VF-1, and I have a run of 12 pieces I'm doing. Not sure what the best way of going about doing them would be.

They are 3.07" long, and I need a hole 1.5" DIA all the way through. It doesn't need to be a good hole, it's just a clearance hole.

Material is 6061-T6

So far, I see myself having a couple options.

1. A 1" drill (with a .5" shank, in a .5" end mill holder, as a guy more experienced than myself recommended to not mount such a long tool in a drill chuck. Drill chuck is ~3.5" long, drill is ~4.5" long.)

So, would you first pre drill the hole with say a 3/8 drill, or just do it all with the 1".

It's a HSS bit, and I've never really used a drill this large before. SS of ~2000rpm and feed of 5 IPM? Peck drill at .25" increments? I'll be using flood cooling, part will be clamped on a mount flange at the bottom which is 3/8 thick. Then using a 3/4" end mill, with 2" flute cutting length, mill out the top half to the 1.5" OD with a G13 stepping down .5 per pass. Flip the part over, and finish the rest of the hole. I do have a 3/4" 4 flute end mill with 3.5" flute cutting length, but it chatters quite a bit.

I need to flip the part anyway to drill some holes 4 smaller holes.

2. Using a 2 flute 3/4" end mill meant for aluminium, peck drill out the middle, then G13 the rest of the way down, flip it, peck the rest, then G13 to finish it off?

Which one would you choose? Any other options? Pre drill for a 1" drilll?

Thanks for any suggestions.

I would do one side 1.6" deep using a 4" long 1/2" diameter GAR 242M two flutecutter, 45degree helix cutter with 2" flutes running at 10000 rpm and about 60 ipm feed on a helical interpolation taking Z-0.20" per circle at a depth of cut of 0.45 for the first pass then 0.35 (0.75 radius) for the second.
Same thing after flipping. We do thousands of holes a year, 2" deep, through and blind 7/8" to 2" diameter. Flood cooling ... and I mean flood!!! .... is essential or you finish up with a stub of tool spinning in the spindle with the rest embedded in re-solidified aluminum.

Thanks for the reply Geof.

I do have a nice 3 flute 3/4 carb end mill I could use, but I'm not sure how rigid the part will be, so I think I'll start off with a 2 flute 3/4" HSS end mill.

I'll have all 4 coolant nozzles pointed at the tool, with the max flow a haas VF-1 can pump out.

Do you plunge at a slower feed? Or do you keep the same feed throughout the entire run?

All my end mills sound horrible when plunging, and draw a heck of a lot of spindle load. Is that normal for end mills, even that are 'supposed' to be center cutting?

us a 1.5" drill with the biggest shank you can get (min of 3/4" shank) and punch thru. I use a spade drill to drill thru aluminum all the time my typical hole depth is anywhere from 1" to 4" deep.

Flood coolant is a must for these hogs. a 1.5" Allied spade drill can go maybe 875rpm at 10ipm with normal flood and faster if you have TSC flood.

Although if your fixturing is weak then maybe 4-6ipm and peck after the first 2".

One of the reasons we use the GAR 242M is that they are very free cutting and have good flute clearance; the 45 degree helix lifts the chips quite well.

On our VF2 at that rpm and feed the spindle load will be around 50% or less. Part of the reason for using 1/2" diameter and two passes on large holes is to keep the spindle load down. Our programs go down on a helical ramp; we do not use the G13 which plunges then moves out to the radius. A typical code for a hole is:

Position tool at center of hole and .02 above surface
G91 G42 D01 G00 Y0.45 Move to radius with tool comp
G91 G03 I0. J-0.45 Z-0.21 F60.0 L10 Do ten counterclockwise circles ramping down 0.2 for each circle to reach Z-2.0
G90 G03 I0. J-0.45 Z-2.0 F100.0 L1 Clean up the bottom at Z-2.0
G00 Z0.02 Move back to top for second cut

Have any insert drills? That would be the fastest way. I would use an 1 3/8 insert drill and an endmill that has enough LOC to finish in at one depth. Leave some mat'l for a skim pass if you need too....:cheers:

Have any insert drills? That would be the fastest way. I would use an 1 3/8 insert drill and an endmill that has enough LOC to finish in at one depth. Leave some mat'l for a skim pass if you need too....:cheers:


Thanks for the suggestion. Sadly we're just starting up, and I dried up the budget long before even being able to think about insert drills.

Center cutting endmills do not cut on center. The SFM drops to zero at dead center. Do the math. For twleve parts in AL I would use the reduced shank drill in a collet. Pilot drill the hole to reduce cutting forces and push hard.

Just a clearance hole in 6061?

Center Drill and drill to size man!!!!!!!

Don't mess around, just DO IT!!!!!!!

Cheers

big mak has drilled the correct

All my end mills sound horrible when plunging, and draw a heck of a lot of spindle load. Is that normal for end mills, even that are 'supposed' to be center cutting?Try programing a helix to plunge with instead of driving the cutter straight down. It seems to work well for me.

If you need to run an endmill, I'd go with helical interpolation, but I'd still go with the SPot and Drill method.

Generally drills are the most efficient tools for metal removal.

THink I saw that in a text somewhere.