37X diameter drilling in 6061 using HSS

Bigbore050 · Jun 19, 2020

Curious if others have accomplished something similar and how it went.

Part is a manifold so straightness isn't critical but unfortunately the part quantity didn't justify buying high dollar tooling so I'm stuck with your standard HSS twist drill. All holes are blind depths.

My hole list and strategy so far:

-7/8 x 18" deep
Pilot with 7/8 CAM Drill 4.5" deep then drill to depth with HSS.

-3/4 x 12.5" deep
Pilot with 3/4 CAM Drill 2.5" deep then drill to depth with HSS.

-5/8 x 18" deep
Helix 5/8 pilot 1.25" deep, Bottom out HSS jobber 4" deep and take to depth with long HSS.

1/2 x 5.5" deep
Plung 1/2 pilot 1.25" deep and drill to depth with HSS, Not to worried with this one.

3/8 x 14" deep
Plung 3/8 pilot 1.0" deep, bottom out 3/8 ext length HSS drill 7" deep, then take to depth.

Will be holding all the drills in either ER32 or ER40 CAT50 holders and turning them with a 630mm CNC Horizontal.

I am slightly worried with how well the 3/8 and 5/8 holes will go. Anyone have any tips or suggestions for the feeds, speeds, and pecks on these long drills?

litlerob1 · Jun 19, 2020

You'll probably be fine with your strategy. What I do with deep holes is;

Spot
Drill with stub length drill
Drill with Jobber length drill
Drill to depth.

All the same diameter.

R

Milland · Jun 19, 2020

Couple things:

Drill droop may be an issue, and so may vibrations causing the drills to act as "tuning forks" for the longer lengths. Both could cause non-centration of the point as it tries to reenter the hole if using full-retract pecking. So either stop retract one or two diameters from actual exit, or leave some "clean up" material at the entry so you can face off any nicks.

This has the disadvantage of potentially leaving some chips in the flutes, so another option is to drop RPM to a low number, then ramp-up after reinsertion. Depending on control options this could mean manually coding the peck operation.

Along with this, use a pecking technique that stops the drill from rapiding back to the last cutting depth - stop about .1" or so away, feed to next depth to prevent impacting any chips that remained in the hole.

Figure out coolant impingement so that as much gets in the hole as possible, but minimizes pushing chips back into the hole. Tricky to balance sometimes...

Larry Dickman · Jun 20, 2020

i used to do 1/4" holes up to 23" deep. Started out like litlerob1 says, except we would go to depth using progressively longer drills. We had the best luck using aircraft extension drills, just a lobber length flute with a long shank. Peck at about 1/2d. Rpm depends a lot on drill length. You don't want to fire up a 24" long drill in high gear. On your long drills, grind a small flat along the shank to relieve coolant pressure.

Bigbore050 · Jun 20, 2020

Thanks for the suggestions. I bought drills with enough flute length to clear the hole depth but the aircraft drill definitely sounds like a good idea.

Should I be reducing the chip load on the long drills along with the rpm?

Milland · Jun 20, 2020

You can play with chip load or peck depth as you go, just make sure to not pack the flutes or starve the coolant. If there's some scrap material you can do a few test holes in, it might save a real workpiece.

ChipSplitter · Jun 20, 2020

Set a bottle of Moly-Dee beside the machine.

Makes a BIG difference according to some people......

Jokes aside, a good tapping lube can help if all else fails.

Milland · Jun 20, 2020

ChipSplitter said:
Set a bottle of Moly-Dee beside the machine.

Makes a BIG difference according to some people......

I wouldn't waste M-D on 6061, in fact I'd think cleanup would be a pain. Just a properly mixed coolant should be enough, it's delivery that's the issue.

Ox · Jun 20, 2020

I would second the fact of not pulling that 3/8 drill out at speed!
Lots of hand coding.

----------------

Think Snow Eh!
Ox

yardbird · Jun 20, 2020

Fuzz the deeper drills 3/8" to walk off center opening up the hole a bit to give the drill some room as it gets deeper and don't worry about withdrawal rpm. And thin the web too. Won't do any good to stubby drill on size then, maybe drill next size bigger first or long fine tuned drill from center drill to bottom. Aircraft drills or make extensions, no long ass fluted drills although in alumi you might get away with it? Don't cram it in there either.

Brent

Bigbore050 · Jun 20, 2020

Ox said:
I would second the fact of not pulling that 3/8 drill out at speed!
Lots of hand coding.

----------------

Think Snow Eh!
Ox

Looks like lots of hand coding is right.

Trying to program this today and now realizing Fanuc nor Mastercam has any standard/easy options for fine tuning drill cycles. I thought back in my OSP days Okuma has a easy way to control the peck retract point vs the drill start point.

Kinda frustrated its 2020 and Fanuc can't control the drill start separately from the peck retract point in a simple canned cycle.

Anyone have a simple macro for this kind of thing?

Larry Dickman · Jun 20, 2020

Bigbore050 said:
Looks like lots of hand coding is right.

Trying to program this today and now realizing Fanuc nor Mastercam has any standard/easy options for fine tuning drill cycles. I thought back in my OSP days Okuma has a easy way to control the peck retract point vs the drill start point.

Kinda frustrated its 2020 and Fanuc can't control the drill start separately from the peck retract point in a simple canned cycle.

Anyone have a simple macro for this kind of thing?

only think i ever found that works. In mastercam you can disable canned cycles, then it will post long hand. Then you can set the retract plane, start depth, etc. wherever you want.

Bigbore050 · Jun 20, 2020

Larry Dickman said:
only think i ever found that works. In mastercam you can disable canned cycles, then it will post long hand. Then you can set the retract plane, start depth, etc. wherever you want.

I gave that a try but I can only get it to start drilling at where my retract value is set.

Were you able to get MC to start drilling at say Z-7.0 but then peck retract to Z-.25? Im using X8 for solidworks witch could be part of my problem.

edit: I was able to get it to work by just using a simple replace all after posting and manually changing the z retract depths to where I want them. That will at least get me started until I can get a macro working.

Larry Dickman · Jun 20, 2020

Bigbore050 said:
I gave that a try but I can only get it to start drilling at where my retract value is set.

Were you able to get MC to start drilling at say Z-7.0 but then peck retract to Z-.25? Im using X8 for solidworks witch could be part of my problem.

edit: I was able to get it to work by just using a simple replace all after posting and manually changing the z retract depths to where I want them. That will at least get me started until I can get a macro working.

I haven't used MC in years, but if I remember correctly, there's a box for initial peck and subsequent peck. So if you wanted to start at Z-5.000 with a peck of .125, use .125 for subsequent peck, -4.875 for initial peck. That will create an air cut that you can delete.

Ox · Jun 20, 2020

Make sure that you have already G0 to your X/Y location, and then just set your ref plane to Z-.75.
But that's not going to allow you to enter the hole at a lesser S tho I don't think.

???

------------------

Think Snow Eh!
Ox

mmurray70 · Jun 20, 2020

I would not mess with all the different sizes, do the whole thing 3/8. If you have a larger hole halfway down, the chips will fall out of flutes instead of being lifted all the way out of the hole when you peck. If the design requires these steps I would go full depth with smallest, then work your way bigger.

Run as much RPM as your comfortable with at that length and peck 0.100 or so, full retract. Be patient and it should be fine.

Ever sharpen a drill by hand and notice it cuts a little larger the the drill diameter? This can be your friend with super long drills too. I ran a bunch of 3/16 holes, 7" deep (ironically 37x diameter) in 4140HT a while ago and got WAY better results with a chinese 12" drill from the hardware store then I did with a nice new precision twist drill. Reason being the shitty hardware store drill was poorly made and cut a little oversize giving me some extra clearance. Good luck with it!

Milland · Jun 20, 2020

mmurray70 said:
I would not mess with all the different sizes, do the whole thing 3/8. If you have a larger hole halfway down, the chips will fall out of flutes instead of being lifted all the way out of the hole when you peck.

OP is using a horizontal.

"Will be holding all the drills in either ER32 or ER40 CAT50 holders and turning them with a 630mm CNC Horizontal."

mmurray70 · Jun 20, 2020

Milland said:
OP is using a horizontal.

"Will be holding all the drills in either ER32 or ER40 CAT50 holders and turning them with a 630mm CNC Horizontal."

Should be piece of cake in that case. Definitely easier with horizontal.

yardbird · Jun 21, 2020

#1=.025(FEED SHORT OF)
#2=.1(PECK EVERY)
#3=.0(START DRILLING AND LOCAL VARIABLE)
#4=18.(STOP DRILLING)
#5=.2(RAPID BACK SHORT OF)
#6=.010(FEED RATE)

S175M3
G0X0Y0
G0Z1.M8
G0Z-[#3]
#3=[#3+#2]
N200
G1Z-[#3]F[#6]
G0Z.1
G0Z-[#3-#5]
G1Z-[#3-#1]F.2
#3=[#3+#2]
IF[#3LT#4]GOTO200
G1Z-[#4]F[#6]
G0Z1.
M9

Brent

Ox · Jun 21, 2020

How about S up and down too?

--------

Think Snow Eh!
Ox

37X diameter drilling in 6061 using HSS

Aluminum

Diamond

Diamond

Titanium

Aluminum

Diamond

Titanium

Diamond

Diamond

Titanium

Aluminum

Titanium

Aluminum

Titanium

Diamond

Stainless

Diamond

Stainless

Titanium

Diamond

Similar threads