[jlembas]

I'm fairly new to machining but I'm having a problem with peck drilling.

I'm tapping a 1/4-20 hole with a thread former on 6061. The thread former is doing just fine but the drill bit isn't. The drill bit is loading up the tip with aluminum. This is happening on the last few holes of the operation. I have also noticed the tip is getting dull. All this only after 50 or 60 holes.

Here is what I have going on:

1. spot drill
2. 0.228 drill (I think this is the size...going on memory)
3. 1/4-20 thread former
4. approx 7/8" deep hole
5. 4000 RPM on the drill bit
6. 9 IPM on the drill bit
7. peck drill (actually using the chip break program)
8. 0.05 pecks

[/LIST]


My speeds and feeds calc says to run the drill bit at 16-18 IPM@4000. Normally I wouldn't have a problem running a test setup but these parts are on there last op and 90% completed. I really don't want to disrupt the flow since this is my only machine.

So I guess my question is this: Should I run the drill bit @ 16-18 IPM and go for it? And what about the peck depth? I know 0.05" is a bit small but I was trying to break the chips up without loading the drill bit with "hairy shavings". Obviously I need to sharpen the bit before continuing.

thanks

[Matt@RFR]

I just got done running a similar sized drill in 6061 at 5600rpm and 70ipm. Keep pecking if you want, but make sure you've got good coolant coverage and turn the feed up!

[snowshovelbmx]

defiantly turn your feed up, you are running about .002" per rev. with a heavier feed you will probably have much better luck.

[mc-motorsports]

turn your feed up as mentioned and don't use coated drills.
Good luck

[Geof]

.......[*]peck drill (actually using the chip break program).....

Do you mean the drill is not retracting, just backing off a short distance but staying in the hole?

Use full retraction and if your machine can do it use 'retract above R' so you can get coolant down the hole. You should be able to go into 6061 much deeper than that at 15 to 20 ipm and do hundreds of holes per drill.

[jlembas]

Ok, I'll try increasing the feed. The higher feed just seemed too much for this drill. I need to stop fighten' the machinist bible and just go with it.

Now that I think about it, I think Geof is on to something too. This is the first time I was trying the Chip Break cycle instead of the full Peck Cycle. And yes Geof, the Chip Break cycle doesn't fully retract. That is probably why I'm hearing slight squeaky sounds towards the deeper end of the holes.

I really appreciate the help guys.

[neilw20]

Running at 3500 rpm, with flood coolant after drilling a 5mm hole in stainless steel
I accidentally (by not re zeroing the tool) I plunged a coated drill 6mm down into the 5mm hole at 1500 mm/min (60 IPM) and there was a hell of a shudder as the HP went up, but it seemed to finish the last 2mm of depth without any drama so I let it run.

Examined the hole. Perfect !
Examined the drill. Perfect !

That was a chip load of 0.2mm (0.008") per flute. Worked fine !
I think I am probably HP limited.

I have had a few rapid sequences before, (due to brain in neutral) and the only exciting one that busted a cutter was carbide 10mm cutter (ouch !) into a clamping bolt. The bolt unscrewed and the cutter shattered.
Same chip load in steel is a bit high for that size cutter.

Screaming through aluminum at 700mm/min (27 IPM) with a DOC of 1/3rd cutter diameter above appears quite exciting on my SX3.

Flood coolant must hide the impending noise is a must. I have rubber curtains, so I only know what happens after the noise !:withstupi

It is surprising how hard you can push things. The only thing that seems to limit you is the bending loads on smaller diameter cutters.

WIND UP THE FEED ! Wheee.....:wee:

[ALLtra Mach]

you don't want to disrupt flow...
What would be more disruptive, taking the time on a piece of scrap material to get your cutters running right, or scrapping one of the "90%" done parts?
Just a thought.
Geofs right, aluminum is soft, but abrasive. Your low feed rate combined with poor chip evacuation is rubbing the edge off of your drills.
lots of coolant, clear the hole often and keep your chip load up.

[jlembas]

ALLtra---you are right. I would rather use a piece of scrap and get things right, which I did originally and thought I had it right. But obviously I didn't. And "rubbing the edge off the drills" is exactly what is happening.

My current jig for these parts takes up most of my table and was a bit time consuming setting it up. I was really trying to cheat and rely on some of you experts before tearing down my jig setup to get this drilling sequence right. That is what I really meant by "not disrupting" the flow.

Anyway, this morning I'll be making some programming changes as you guys have suggested and continue while keeping a close eye on that drill bit.

The more I get into machining, the more I respect it. Especially the old skool guys.

[Delw]

I use a .234 dia drill I run 8500 rpms 22.5ipm with pecks of .100, on the mill
the drill is a cobalt 135º screw machine drill I drill about 150-200 holes aday in 6061, I havent changed the drill in over a year( think its been about 14 months). its due at any time now as I can hear it pushing more than cutting over the last few weeks.

the whole key is coolant and chip build up usually I don't get chip build up after a 24 hole run, lately the 6061 I have been getting has been stringy on the 3/4 and 1" stock(last 3 lots) notices this on milling and drilling,
the rats nest cause the coolant to deflect.

when drilling alum its a must to have the drill retract completely from the part. as alum is very abrasive and will wear the edges about as fast as a diamond file touching it. its also important that you use a good coolant as lubricity keeps the edge from gettng worn.

[ALLtra Mach]

Nothing but respect for the Old Skoolers! Nothing can replace experience!
However, Machining(like all other technology) is a constantly progressive technology.
If you Stay hooked on the old ways too long, you'll find it hard to be competetive.
On the other hand, I don't like to jump on the newest stuff out there either. New technology is highest dollar. And in todays ultra competetive world of manufacturing, with harder than ever pushes for efficiency, alot of the "New" technology gets pushed into release before it is completely explored and perfected. Then as it is improved, manufactures aren't willing to "Invest the cost of a tooling change" for a "slight product improvement".
I prefer to give them some time to perfect the new technology, let others test and tune the tooling, pay the price of R&D, and when the "Next Great Idea" pops up, I gobble up the now old news, but very effective, well proven stuff at 1/2 the cost!

Not quite "old skool", not quite "cutting edge", I guess I'd be better classified as "Carefully Progressive"? LOL

[Geof]

....... lately the 6061 I have been getting has been stringy on the 3/4 and 1" stock(last 3 lots) notices this on milling and drilling,
the rats nest cause the coolant to deflect.......

Check that you received the correct temper; 6061 is available in different tempers and T6511 (I think that is the number) is the hardest and best for machining.

[ALLtra Mach]

If this is a hole you make quite often, I would consider a coolant thru drill. Will be pricey in that size, but may be worth the investment.

[jlembas]

I've been out of the shop for a few days, but I finally got to play with this yesterday afternoon.

I changed the feeds and speeds to around 5000 RPM at 20 IPM (can't remember the exact rpms). Drill seems to be doing better. I also changed back to full peck.

I have noticed that I'm getting the "rats nest" now. Sometimes it flings off the bit and sometimes it doesn't. When it stays on the bit the coolant obviously doesn't get where it needs to be and it seems to have a snowball effect.

Any advice here? Should I increase just the feedrate? I've played around with different peck depths but that doesn't seem to help much. Thanks again.

[Geof]

.....Any advice here? Should I increase just the feedrate? I've played around with different peck depths but that doesn't seem to help much. Thanks again.

If anything decrease the speed (not feed rate) to get a thicker chip that breaks easier.

And use the 'retract above R' feature if it is available on your machine.

Maybe also use the I and J options if they are available; I is the size of the first peck and J is the amount that each subsequent peck is reduced.

Corrected mis-statement.

[snowshovelbmx]

you mean increase the feed to get a thicker chip?

[Geof]

you mean increase the feed to get a thicker chip?

Whoops! Yes I typed it backwards. Actually not quite backwards I think I meant to type decrease the speed.

[jlembas]

Whew...I thought I was going crazy after reading Geof's original response. Thanks for correcting and returning my sanity. I'll give it a try.

I am using the I and J features now. The peck eventually decreases to a minimum peck of 0.1". As I said before, I've tried different peck depths etc. with not much luck getting rid of the occasional rats nest. So I'll try decreasing the RPM's to give more chipload on the bit.

Thanks for all the help guys.

[Delw]

just out of curiosity what kinda machne are you useing and what kinda drill.

a good cobalt drill only cost around a buck -2 bucks
you use your feed and peck depth to contol the chip.
on alum most factory twists are ok, hardware store drills suck and will give you problems like you describe.

right now it sounds like you might not have the drill drilling true and its walking, or your point on the drill is off center. are you using a center drill/spot drill? does the drill have a factory point or is it a regrind?

[Geof]

Whew...I thought I was going crazy after reading Geof's original response. Thanks for correcting and returning my sanity. I'll give it a try....

Sorry about that.

I have caused consternation at other times by flubbing a reply; I don't claim to be perfect.