Lots of 7/8" holes in aliminum

Mud · Jul 19, 2017

Lots of 7/8" holes in aluminum

I need a new tool for drilling shallow .875 dia. holes in 6061-T6. We've been using an Iscar Chamdrill, now I'm looking for something faster. The holes are through .500 to 1.0 thickness, we're drilling from solid, the diameter tolerance is +.005 - .000. We need a decent surface finish on the finished hole without a secondary operation. No spec, just has to look ok to us. Right now the Chamdrill is running 1800 rpm and 33ipm because any faster causes lots of squealing and chatter. What are you using in similar operations? I have 25 hp, up to 10,000 rpm and low pressure (200 psi) TSC. Drilling 36 holes per cycle.

XD341 · Jul 19, 2017

That doesn't seem all that fast, why the chatter I wonder? Surface feet seems a little on the low side but I've never run a chamdrill. If you have a real rigid setup it seems like you should be able to go faster. If it was me I'd start with faster SFM and play with the feed until the chips looked happy and nothing sounded horrible.

I've had good luck with sumitomo indexable drills, the sky seems to be the limit in aluminum with those tools.

plastikdreams · Jul 19, 2017

2 flute 3/4 endmill and helical interp...?

ManualEd · Jul 19, 2017

I would try the Iscar SumochamIQ. The IQ has a new tip design that seems really impressive.
ISCAR HCP vs ICP slowmotion - YouTube

If the job is big enough, I'd have a custom one made up at 2xD (if they don't have one standard)

I agree with XD341 though, unless you're running an 8XD drill I wouldn't expect any chatter at all.

Job Shopper TN · Jul 19, 2017

I know this will sound nuts, but I have seen HSS drills run at similar parameters to what your insert drill is running... it's really pushing it nonetheless, but.

A distributor rep came in one time with OSG carbide drills, solid and inserted, and we found that they take a lot more force to go through a part than touched-up HSS. Makes sense, really. Not as "sharp". Too much force, for us, in fact, due to that particular part and fixturing.

I'm sure you can get faster if you can make sure you get coolant to the right drill. Heck - see if you can get a short spade drill and try that. I usually see spade drills fed pretty darn hard.

precisionmetal · Jul 19, 2017

I'm with plastikdreams on this one -- maybe 1/2" or 5/8" end mill and helical tool path. Then just a quick final skim pass to hit size.

Might even use a rougher with slight interruptions (like the ones Helical makes) just to lighten the tool load a bit.

PM

TeachMePlease · Jul 19, 2017

Only 400SFM? I run that with coated carbide and no coolant/air blast in aluminum on a bridgeport.

My guess is that you're upping your RPM and not upping your feed to match. Chatter = either slow it down, or feed it harder... And you don't really need to slow it down....

I haven't used one in this size, because most of my parts are about the size of the chips you get off an .875 drill, but I've used MA Ford 2 and 3 flute Altima coated carbide drills to easily nail size and position locations tighter than what you're asking for, with a great finish, for thousands of parts per tool. The small ones aren't expensive... No idea what a big one costs, but it's probably worth it.

Mtndew · Jul 20, 2017

You should be going at least 800sfpm and around 77ipm
that's 3500rpm and .022ipr. If it's still squealing and leaving chatter, look into a 3 flute hss drill.

Bobw · Jul 20, 2017

precisionmetal said:
I'm with plastikdreams on this one -- maybe 1/2" or 5/8" end mill and helical tool path. Then just a quick final skim pass to hit size.

Might even use a rougher with slight interruptions (like the ones Helical makes) just to lighten the tool load a bit.

PM

He's running 33ipm.. He's making a 1" deep hole in approximately 2 seconds... And he wants to speed it up...
I really don't think that milling the hole is going to be faster than 2 seconds.

dodgin · Jul 20, 2017

Mud said:
I need a new tool for drilling shallow .875 dia. holes in 6061-T6. We've been using an Iscar Chamdrill, now I'm looking for something faster. The holes are through .500 to 1.0 thickness, we're drilling from solid, the diameter tolerance is +.005 - .000. We need a decent surface finish on the finished hole without a secondary operation. No spec, just has to look ok to us. Right now the Chamdrill is running 1800 rpm and 33ipm because any faster causes lots of squealing and chatter. What are you using in similar operations? I have 25 hp, up to 10,000 rpm and low pressure (200 psi) TSC. Drilling 36 holes per cycle.

We just switched one of our low volume production jobs from Iscar Chamdrills to OSG Mega Muscles - 35/64" and 21/32", 36 holes of each in the operation, through exactly 1" of material (mild steel). Went from running each drill around the 1500 - 2000 RPM range to about 3000 - 3500 RPM, and up from around 20 IPM to about 80 IPM. They're expensive, but after a handful of regrinds we're saving some money on tooling also. Finish looks great and they hold size really well also.

Mud · Jul 20, 2017

dodgin said:
We just switched one of our low volume production jobs from Iscar Chamdrills to OSG Mega Muscles - 35/64" and 21/32", 36 holes of each in the operation, through exactly 1" of material (mild steel). Went from running each drill around the 1500 - 2000 RPM range to about 3000 - 3500 RPM, and up from around 20 IPM to about 80 IPM. They're expensive, but after a handful of regrinds we're saving some money on tooling also. Finish looks great and they hold size really well also.

That's exactly the sort of thing I'm looking for. Who does the regrinding for you?

dodgin · Jul 20, 2017

Mud said:
That's exactly the sort of thing I'm looking for. Who does the regrinding for you?

There was an OSG recommended regrind shop not far from us that does it for a good price. On those particular drills OSG will regrind (and do their own coating, which is new) out of Chicago, but if you have less than 3 drills to regrind they hit you with a set up fee and that makes it a little less economic. If OSG does the regrind for you I think they charge around 50% of what you originally paid for the drill for each regrind, but they'll guarantee so many linear inches of material removal as well. We're getting about 2000 to 2500 linear inches with those drills in mild steel. We actually got the first set in on test and the edges wore down a little quicker than they promised, but they set us up with trial drills until we got them tweaked in to running where they promised and we needed.

I'm just wondering about size offerings. 7/8" has to be pretty damn close to the cutoff for what they offer.

doug925 · Jul 20, 2017

Mud said:
I need a new tool for drilling shallow .875 dia. holes in 6061-T6. We've been using an Iscar Chamdrill, now I'm looking for something faster. The holes are through .500 to 1.0 thickness, we're drilling from solid, the diameter tolerance is +.005 - .000. We need a decent surface finish on the finished hole without a secondary operation. No spec, just has to look ok to us. Right now the Chamdrill is running 1800 rpm and 33ipm because any faster causes lots of squealing and chatter. What are you using in similar operations? I have 25 hp, up to 10,000 rpm and low pressure (200 psi) TSC. Drilling 36 holes per cycle.

Have a look at the Guhring, series 5518. Specifically the "GS 200 G"
Guhring, Inc. - Tool List
It is a 3 flute, 130° point, ground for aluminum and cast iron.
The drill should run around 550-600 sfm (external coolant only) and 0.02 - 0.025" IPR.
RPM= 2619, 65IPM
Assuming 1/2" plate, 0.05" clearance, and feeding to Z-.68 (130° point depth included) makes for 0.7 seconds /hole.
That's not too shabby.....

Doug.

precisionmetal · Jul 20, 2017

Bobw said:
He's running 33ipm.. He's making a 1" deep hole in approximately 2 seconds... And he wants to speed it up...
I really don't think that milling the hole is going to be faster than 2 seconds.

Understood completely -- he never said how many total holes he was drilling, so I guess my "small thinking" defers to chip control, size control, and tool life.

LockNut · Jul 20, 2017

Do you have support under the parts, especially the .500 ones? If not, that will cause chatter. Also, Cham drills "like" being pushed hard. More SFPM until you get good performance. Of course, the part needs to be supported well, no flexing.

Paul

DMF_TomB · Jul 20, 2017

Bobw said:
He's running 33ipm.. He's making a 1" deep hole in approximately 2 seconds... And he wants to speed it up...
I really don't think that milling the hole is going to be faster than 2 seconds.

.
usually the chips often wrapping around drill bit and needing to stop and remove them takes longer than 2 seconds to remove

Rstewart · Jul 20, 2017

DMF_TomB said:
.
usually the chips often wrapping around drill bit and needing to stop and remove them takes longer than 2 seconds to remove

If your wrapping chips around your drill, your doing it wrong or Chinese material...

Mtndew · Jul 20, 2017

doug925 said:
Have a look at the Guhring, series 5518. Specifically the "GS 200 G"
Guhring, Inc. - Tool List
It is a 3 flute, 130° point, ground for aluminum and cast iron.
The drill should run around 550-600 sfm (external coolant only) and 0.02 - 0.025" IPR.
RPM= 2619, 65IPM
Assuming 1/2" plate, 0.05" clearance, and feeding to Z-.68 (130° point depth included) makes for 0.7 seconds /hole.
That's not too shabby.....

Doug.

That was going to be my suggestion also, but the sizes don't go up to 7/8.

Bobw · Jul 20, 2017

DMF_TomB said:
.
usually the chips often wrapping around drill bit and needing to stop and remove them takes longer than 2 seconds to remove

At .018 a rev on an insert drill... He better be breaking the chips, and if not, that's going to be too fat of
a stringer to wrap around anything, its going to be more like a piece of mangled welding rod.

Mud · Jul 20, 2017

LockNut said:
Do you have support under the parts, especially the .500 ones? If not, that will cause chatter. Also, Cham drills "like" being pushed hard. More SFPM until you get good performance. Of course, the part needs to be supported well, no flexing.

Paul

The material is a 6" dia sawed slug held in soft jaws in Chick vises, It can flex only as much as a 6" dia X .560" th. plate can flex. We experimented a fair amount in a previous machine and settled on these parameters as a best compromise. We're doing new programming for a different machine and trying to optimize things for this machine. Chip nests aren't a problem. We do about 1000 holes per run. These holes are the slowest part of this particular part, looks like a good place to put some effort. I initially did them with a custom HSS step drill, found it was faster to sink a through hole with carbide then come back and hit the top with a 1" endmill to counterbore .100 deep. If I cut the drilling time in half I'm only saving less than 16 minutes on a 1000 hole run which is about $0.10 per part, but I'm still trying.

Lots of 7/8" holes in aliminum

Diamond

Hot Rolled

Diamond

Stainless

Cast Iron

Stainless

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Hot Rolled

Titanium

Stainless

Stainless

Diamond

Stainless

Diamond

Diamond

Diamond

Similar threads