[graemeian]

I need to drill several holes using a 1/16" drill bit at 0.72" deep.
My machine is good at 6000 rpm. I could go 7500 if needed.
I am doing the following:
Pre-drill using a 1/16" carbide bit to 0.03" deep
I then change to a new HSS bit at 6000 rpm and feed of 6 ipm.
Down at 0.06" increments and lifting 0.005" for a chip break.
I do that three times to get to -.18"
I keep the bit at/below 0.18" to avoid chips going into the hole.
I then peck at 0.06" increments and lifting the bit to -.18".
I use only feeds and retract at 88 ipm.
I then lower to .005 of the previous depth at 55 ipm and drill again at 6 ipm
My coolant is 6 jets from around the quill.

After 10 test holes, the bit is trash.
I am drilling at 0.001" per revolution.
What am I doing wrong?
For those interested...
My sub code is the following:
O223
(Chip Breaker
G0 X=VC5 Y0 (VC5 IS IN A TEST LOOP FOR X POSITION)
G0 Z.01
G1 Z0 F6
VC2=0
N200
VC2=VC2+.06
G1Z=-VC2
G1Z=-[VC2-.005]
IF [VC2 LT .18] GOTO N200
(Peck cycle
VC3=.18
N201
VC3=VC3+.06
G1 Z=-VC3 F6
G1 Z=-.18 F88
G1 Z=-[VC3-.005]F55
IF [VC3 LT .72] GOTO N201
G1 Z.1 F88
G0 Z.3
RTS

[graemeian]

I am drilling in 6061 aluminum.

[joeavaerage]

Hi,
what material are you drilling?

I suspect the real problem is the depth of the hole, its 12 times the diameter. I'd use the carbide drill alone, if it long enough.
I would peck regularly, and withdraw the drill to above the surface. I'd be less worried about chips falling back down the hole as much as getting
the chips already in the hole out.

Craig

[joeavaerage]

Hi,
if drilling aluminum then its all about chip clearance.

I use circular interpolating toolpaths regularly.

For instance I have some quite long (16mm flute length) 1.5mm two flute carbide endmills. If I want a hole for a 2mm screw, then I want a hole diameter of 1.6mm to 1.7mm, to have material to tap.
I would do this with a circular interpolation tool path with my 1.5mm endmills. The tools are pretty spindly and break easily, but with care you can drill 1.6mm holes 15mm deep in aluminum, brass and plastics.
The interpolated hole means its much easier for the coolant to flush the chips out.

You might think its a drag doing circular interpolation but it means you can use one endmill to do many different size holes, without having to stop and change drills all the time.
For example the circuit board I'm working on at the moment require five different size holes, ranging from 1.6mm (threaded for 2mm screw), 2.1mm (threaded for 2.5mm screw), 2.6mm (clearance for 2.5mm screw),
2.6mm (threaded for 3mm screw) and finally a 3.2mm hole (clearance for 3mm screw). It would drive me up the wall manually changing drills all the time, when I can interpolate holes and do them all
with one tool. Done it that way for years.

Craig

[graemeian]

Carbide not long as why it is used as a spot drill. I moved the coolant jets so they are not jetting directly towards the hole and that did not work. I am currently looking at bits with a loupe and trying the better ones. I may try with the door open and coolant and air blasting while slowing the retraction.

[graemeian]

I do helix for most other holes. I do not have an end mill for this.

[graemeian]

I ran with door open and blasting coolant just to the left of the bit. My coolant flow is much faster than the bit surface velocity. I ran 10 holes and 10 holes again. I also raised the step over so I could check for any remaining strings on the bit and blast them away with air if necessary. The bit tip still looks good. The factory grinding is not Titex quality. I have some common HSS bits arriving from McMaster Carr on Monday.

[ToolHIT]

The key thing in deep hole drilling is matching the drill point from the Spot to your Drill. Would you know the drill point angle of your 1/16" Drill Bit? Most HSS Drills are a 118 or 130 degree drill points and most Carbide Drills are a 140 degree drill point. The best move may be to go with a HSS or Cobalt Spot Drill that matches the drill point of your HSS or Cobalt 1/16" Drill.

Your speeds/feeds are good but I'd also look at lighter pecks. Usually we try to peck at 0.5 X Diameter so taking .031" Pecks can also make sure the chips are evacuating (with the depth a .020" peck may be better to ensure the chips are getting out).

Another thing you can do is go with a Parabolic Flute Drill so there is more room for the chips to evacuate. If you would like a recommendation on the drill or spot let me know and we can send over the ones we recommend.

Hopefully this helps!

Mike

[Algirdas]

Mitsubishi has that diameter drill with trough - hole coolant. You need high pressure coolant and 1µm ( or 5 µm ) coolant filters. Check if it's worth at your conditions.

[Superman]

You are using an Okuma...
Why not utilise the G83 cycle to do peck, peck, retract (use I J, not Q)
Ie G83 Z-0.72 R0.04 I0.036 J0.072 F12.