What's new
What's new

Need help with tooling, specifically drill

EyeEmTrash

Aluminum
Joined
Feb 24, 2023
I hope I am posting this in the right place in the forums. I need to drill a hole, .625 inch OD, to a depth of 6.5 inches. I am looking for a reasonably priced drill. I believe it needs to have through coolant drilling that deep. I found a couple drills online, they were $1,064. I started looking into spade drills and I'm thinking this is the route I should go. It would probably come out to around $300 with the insert and drill. Does this sound like my best option? Do I need to peck drill with a spade drill going that deep considering the diameter of hole? Does anyone have any other suggestions? Just for clarity, it will be run on a CNC lathe, and I also drill holes with ODs of .750, .875, 1.125, 1.5 with depths up to 5.5 inches. The 1.125 and 1.5 I have insert and spade drills for already. Thanks in advance.

Edit:The problem I am having now, on the .625 drill is that the material is getting too hot and burning the plastic. I use a G74 peck drilling cycle. Judging by some of the experiments I have done, my guess is that its the coolant not being able to get through or something with chip evacuation or both. I have went into the parameters and increased how far the drill moves back for chip evacuation, I changed spindle speeds, feeds and depth of cut. I have had to reduce the peck to .02 cuts at a time because any deeper and it burns up. A travesty, I know. This machine is old and one that just runs in the background. They don't really care how long it takes but I do. This drilling cycle taking 10+ minutes is ridiculous. Maybe I am asking the wrong question. Maybe the drill I have is fine but my technique is wrong.
 
Last edited:
I hope I am posting this in the right place in the forums. I need to drill a hole, .625 inch OD, to a depth of 6.5 inches. I am looking for a reasonably priced drill. I believe it needs to have through coolant drilling that deep. I found a couple drills online, they were $1,064. I started looking into spade drills and I'm thinking this is the route I should go. It would probably come out to around $300 with the insert and drill. Does this sound like my best option? Do I need to peck drill with a spade drill going that deep considering the diameter of hole? Does anyone have any other suggestions? Just for clarity, it will be run on a CNC lathe, and I also drill holes with ODs of .750, .875, 1.125, 1.5 with depths up to 5.5 inches. The 1.125 and 1.5 I have insert and spade drills for already. Thanks in advance.
No-one can help ya if you don't specify the material you're drilling bub
 
Just for clarity, it will be run on a CNC lathe, and I also drill holes with ODs of .750, .875, 1.125, 1.5 with depths up to 5.5 inches. The 1.125 and 1.5 I have insert and spade drills for already. Thanks in advance.

What kind of finish are you wanting the drilled holes to have? Solid carbide drills will give you the best finish, but I wouldn't use those on a lathe unless I had no other choice.
Carbide indexable will be faster than a spade but again you're limited on size to the drill you're using.
Allied spade drills would be your best option since they are flexible on insert sizes. But for those hole sizes you list, you're going to need 2-3 drill bodies I would imagine.
As for pecking, you'll have to see what the chips look like, if they are 6's and 9's and exit the hole easily then send it, if they have a hard time exiting then you want a full retract pecking cycle as they will just bind up and create a ton of heat.
 
and, how many holes?

Could always just get a HSS drill and get it done.

Can't speak for this listing, price doesn't suggest to me "made in usa" but maybe.


If you look on ebay, you're bound to come across a 5/8 drill "new old stock usa made" for under 50$ for the length you want.

It doesn't "need" coolant that deep, but if using a spade or carbide, you really should have it. HSS? Just gotta peck it to keep it cool, and go slower.
 
What coolant pump does your CNC lathe have? Standard low pressure, or a high-pressure?

How precise do the holes have to be, and what surface finish?

Regards.

Mike
I believe it's just a standard pump. The holes dont have to be exact and the finish just has to look and feel relatively smooth.
 
I have a 5/8 dia solid carbide coolant thru in my marketplace. $340.00


If you dont have enough pressure you will need to peck! Especially on a lathe where the drill is not spinning.
I am using a G74. I edited my original post, if you wouldn't mind rereading it and letting me know what you think. Drill looks good but its about the same price as spade drill which I think would give a little more variety.
 
What kind of finish are you wanting the drilled holes to have? Solid carbide drills will give you the best finish, but I wouldn't use those on a lathe unless I had no other choice.
Carbide indexable will be faster than a spade but again you're limited on size to the drill you're using.
Allied spade drills would be your best option since they are flexible on insert sizes. But for those hole sizes you list, you're going to need 2-3 drill bodies I would imagine.
As for pecking, you'll have to see what the chips look like, if they are 6's and 9's and exit the hole easily then send it, if they have a hard time exiting then you want a full retract pecking cycle as they will just bind up and create a ton of heat.
I edited my original post. What you said sounds like my problem. What do you mean by "6s and 9s"?
 
and, how many holes?

Could always just get a HSS drill and get it done.

Can't speak for this listing, price doesn't suggest to me "made in usa" but maybe.


If you look on ebay, you're bound to come across a 5/8 drill "new old stock usa made" for under 50$ for the length you want.

It doesn't "need" coolant that deep, but if using a spade or carbide, you really should have it. HSS? Just gotta peck it to keep it cool, and go slower.
I am at that point now. I have to take .02 cuts. I am using a G74 and it seems like anything over .04 is a problem. I adjusted feeds and speeds, right now I think I am running spindle at 1000rpm and .005-.01 feed. It would be a nightmare if my boss was breathing down my neck but they're not thankfully. I even went into parameters and adjusted the retract but judging by someone else's comment maybe I need to do more. I'm just scared that the plastic is gonna melt onto the drill again and I'm gonna have to break out the torch.
 
I edited my original post. What you said sounds like my problem. What do you mean by "6s and 9s"?
the shape of the chips look like little 6's and 9's. Common term for "the perfect chip formation".

machining-steels-lead-768x432.jpg
 
I'd say you should be running a Parabolc fluted drill and get your feed up to about 0.03" per rev. or more. Start with a Parabolic Screw Machine drill to get yourself started straight then switch to the long one for the balance. Still may have to peck every couple diameters.
At 10+ diameters, coolant thru would be great. You might even consider a Gun Drill, though I'm not sure if they're made for plastics. Plus they'll want HPC whereas a Spade Drill, if you were to go that route, likes volume more so than pressure.
 
Sounds like you're drilling plastic and not getting coolant deep enough.

My post creates a peck cycle that retracts the same amount each peck which often does not clear chips or allow coolant access in deeper holes. For those I just add a rapid back to zero after each peck. I just edit it manually, it usually only takes a few seconds. Gets your chips out and allows coolant on the drill and into the hole.

X0.Z0.02
G01Z-0.3943F0.005
G00Z0.
Z-0.3743
G01Z-0.6443
G00Z0.
Z-0.6243
G01Z-0.8943
 
I am at that point now. I have to take .02 cuts. I am using a G74 and it seems like anything over .04 is a problem. I adjusted feeds and speeds, right now I think I am running spindle at 1000rpm and .005-.01 feed. It would be a nightmare if my boss was breathing down my neck but they're not thankfully. I even went into parameters and adjusted the retract but judging by someone else's comment maybe I need to do more. I'm just scared that the plastic is gonna melt onto the drill again and I'm gonna have to break out the torch.
Ah yeah, plastic.

Your feed should be at .020 or more as suggested above.

Parabolic or spade will be fine. spade has an advantage over most HSS drills because of the coolant thru, but there are HSS drills that have thru coolant, like this one: https://www.ebay.com/itm/143196703269?hash=item2157304a25:g:KnMAAOSw5cNYcTpk
 
You will have little luck drilling plastic thinking about metal. Can you dwell peck? Try more aggressive feed with lower RPM. Crazy more? Friction makes plastic melt and fooking aggressive feed keeps the tool forced against cool material as it sets it free. And dwell peck for a single revolution breaks the chips and lets them fly. For sure I would not think coolant. Not needed.
Para drill for sure and you need flute space left over at depth.
 








 
Back
Top