# Beware: Stay away from Dormer/PTD Cobalt drills.



## ChrisAttebery (Feb 25, 2020)

Let me start over. I typing this up between real bill paying day job work and it was a bit disjointed to say least.

I've been fighting with a mildly deep hole (.205" x 1") in 6061-T6 aluminum lately. I'm running them at 4500 RPM and 18IPT. Both of these numbers are around 50% of what FS Wizard recommended. I'm peck drilling starting with .200" depth and reducing by .050" with a minimum peck depth of .050". I'm using a home brew fog buster with KoolMist 77. When I deep drill I crank up the coolant so it's very wet and point it right down the hole. I had been using PTD black stub length drills and they worked OK, but they did chip weld at the bottom of the hole occasionally.  

I asked my tool store if they had a better drill for the job and they gave me Dormer/PTD stub length M41 cobalt drills (PTD 041305). I tried them out and found that they would barely drill into the material and were walking all over the place. I tried going down to 2250 RPM and 9 IPM (.002 IPT) and it was still having trouble. 

I called Oemeta and spoke to a rep who recommended I add 10% Oemeta Hytap 12 soluble oil to the mister. I tried it and it made minimal difference.

At this point I was shocked at how bad these drills were working so I grabbed one of my old discarded black PTD drills, chucked it up and watched it blast right through the same hole at the same speeds and feeds. 

I took the two drills to my lathe and drilled a full depth hole in aluminum with both drills at 2000 rpm. The black drill cut like butter, the cobalt drill struggled to cut and I needed a lot more pressure on the tailstock to get it to cut. 

Here's a picture of the tip of the drill. This one was brand new when I tried it out.


----------



## Winegrower (Feb 25, 2020)

I guess I am surprised at the specs here.   Maybe somebody can help me.  You don't mention the material, which is maybe the most fundamental question that could be asked.   Assuming steel,  I would start with about 400/0.2=2000RPM and I am sure I could not get a 1/2" per second rate of feed.   What would be reasonable for a Bridgeport mill in mild steel?   And, what is your material above?


----------



## ChrisAttebery (Feb 25, 2020)

Oops, sorry. It's made from 6061-T6. I use it on 99% of everything that I make.


----------



## middle.road (Feb 25, 2020)

Any lubricant? 6061 is kind of 'gummy' to begin with, and @4500RPM? Without lube...
118° instead of 135° perhaps?
Bad batch of 6061?


----------



## pontiac428 (Feb 25, 2020)

Bad drills?  If the HSS cut and the cobalt didn't, I'd inspect the grind job on the drill points.  I do think your feed rate is high, but I'm sure it's within the performance envelope of the drill- the machine is an unknown.  Usually you can blast through aluminum.  Hey, was your spindle turning the right direction?  That's a simple error that would definitely cause this fault.


----------



## darkzero (Feb 25, 2020)

middle.road said:


> 118° instead of 135° perhaps



That could be a factor. Don't need cobalt drills for aluminum & cobalt drills usually come with 135° points. I was taught in general to use 135° on harder materials & 118° is better for softer materials. I don't have an issue with either or but then again I don't have anything that will drill at speeds higher than 2000 RPM nor do I use high/max feed rates. But it does seem that 118° works better for me on aluminum.


----------



## ChrisAttebery (Feb 25, 2020)

I'm using a homebrewed fog buster. I'm using KoolMist 77 with 10% soluble oil. 

I think it was a bad batch. I've been using their black oxide stub length drills for a while and I've been happy with them.



middle.road said:


> Any lubricant? 6061 is kind of 'gummy' to begin with, and @4500RPM? Without lube...
> 118° instead of 135° perhaps?
> Bad batch of 6061?


----------



## ChrisAttebery (Feb 25, 2020)

FSWizard recommends 9400 RPM and 63 IPM (.0033 IPT). I usually run 6750 RPM on all of my drills 3/16 and under. I've been using 4500 RPM and 18IPT on my 1/4" drills for quite a while. That's pretty conservative for a CNC machine.


----------



## mattthemuppet2 (Feb 25, 2020)

I don't have enough to compare, but I've always read that cobalt drills have a thicker web as they're more brittle (if that's the word) than HSS. At that size, maybe the difference is enough to prevent decent chip evacuation? What was the coating on the cobalt drills? I've found bright HSS to work the best with 6061 and flooding the hole with kerosene. Otherwise chip welding to the drill lips is pretty common. Black oxide is ok, other coatings (TiN) don't play well at all with 6061. Not pushing them as hard as you are, but those were some of the things that came to mind.


----------



## Ulma Doctor (Feb 25, 2020)

mattthemuppet2 said:


> I don't have enough to compare, but I've always read that cobalt drills have a thicker web as they're more brittle (if that's the word) than HSS. At that size, maybe the difference is enough to prevent decent chip evacuation? What was the coating on the cobalt drills? I've found bright HSS to work the best with 6061 and flooding the hole with kerosene. Otherwise chip welding to the drill lips is pretty common. Black oxide is ok, other coatings (TiN) don't play well at all with 6061. Not pushing them as hard as you are, but those were some of the things that came to mind.


point of information...
Cobalt is HSS, with cobalt added to the HSS- i have seen 8 to 12% cobalt tooling


----------



## ChrisAttebery (Feb 25, 2020)

The spindle was turning in the correct direction. I only have it wired for RH rotation. All of the parameters were taken from the manufacturer's recommendations and cross checked with FS Wizard.



pontiac428 said:


> Bad drills?  If the HSS cut and the cobalt didn't, I'd inspect the grind job on the drill points.  I do think your feed rate is high, but I'm sure it's within the performance envelope of the drill- the machine is an unknown.  Usually you can blast through aluminum.  Hey, was your spindle turning the right direction?  That's a simple error that would definitely cause this fault.


----------



## ChrisAttebery (Feb 25, 2020)

I think you're thinking of carbide, not cobalt. 




mattthemuppet2 said:


> I don't have enough to compare, but I've always read that cobalt drills have a thicker web as they're more brittle (if that's the word) than HSS. At that size, maybe the difference is enough to prevent decent chip evacuation? What was the coating on the cobalt drills? I've found bright HSS to work the best with 6061 and flooding the hole with kerosene. Otherwise chip welding to the drill lips is pretty common. Black oxide is ok, other coatings (TiN) don't play well at all with 6061. Not pushing them as hard as you are, but those were some of the things that came to mind.


----------



## pstemari (Feb 26, 2020)

No, cobalt such as M42 or M44 has a thicker web for strength. The steel is also a substantially more brittle than straight HSS like M2. There's really no reason to use cobalt drills with aluminum.

Aluminum in general is incompatible with most tool coatings. IIRC, black oxide, TiCN, and ZrN are the only ones recommended by the manufacturers for use with aluminum. The aluminum-containing coatings are particularly bad. Good lubrication helps a lot with chip welding. I tend to use WD-40 because it's handy. I've also heard of good results with kerosene. KoolMist works well on aluminum ***if*** you can get it to the cutting edge. That means lots of pecking if you're drilling. Use the canned cycle that has a full retract (I think maybe G73?) and peck in 1D increments if you're going deep.

Supposedly parabolic flutes can get you around having to do so much pecking, but I haven't actually tried that myself.

Sent from my Pixel XL using Tapatalk


----------



## projectnut (Feb 26, 2020)

Here's a link to an older thread on the Practical Machinist site where someone was having a similar problem.






						Hints on Drilling/Tapping 6061 T6 ?
					

If I'm on the wrong forum, my apologies, and please advise.  I have a need to drill and tap M6 about 200 holes in one inch thick 6061T6 aluminum bar stock.  I've had difficulties in the past in this material with the drills gumming up - sometimes to the point where I have to take the drill bit...



					www.practicalmachinist.com
				




The basic takeaways are lots of coolant, lower speed, polished Parabolic drills, and retract the drill at least a couple times to clear the chips.  The type of coolant you use might also make a difference.  Some fluids cause the aluminum to seize to the drill.  For aluminum I use Tap Magic for Aluminum



			http://www.tapmagic.com/assets/uploads/2016/02/20160217160226-tmalumpdf.pdf
		


I can tell you from experience the non aluminum formula will make a mess of things.

While I do use lots of 6061 I don't attempt to drill at near the speed you are using.  I also have found that polished parabolic drills are much better at chip removal.


----------



## mattthemuppet2 (Feb 26, 2020)

ChrisAttebery said:


> I think you're thinking of carbide, not cobalt.


 well colour me not bothered to reply again.


----------



## projectnut (Feb 26, 2020)

mattthemuppet2 said:


> I don't have enough to compare, but I've always read that cobalt drills have a thicker web as they're more brittle (if that's the word) than HSS. At that size, maybe the difference is enough to prevent decent chip evacuation? What was the coating on the cobalt drills? I've found bright HSS to work the best with 6061 and flooding the hole with kerosene. Otherwise chip welding to the drill lips is pretty common. Black oxide is ok, other coatings (TiN) don't play well at all with 6061. Not pushing them as hard as you are, but those were some of the things that came to mind.



I m not sure all manufacturers use the same geometry, but cobalt drills manufactured by Viking do have a thicker web than their premium HSS drills.  Here's a link to some info from Viking.  Near the bottom of the page it shows the difference between the web of their premium HSS and cobalt drills.






						Viking Drill and Tool-America's Finest High-Speed Steel Cutting Tools™
					

Full line of Industrial Cutting Tools




					www.vikingdrill.com


----------



## ChrisAttebery (Feb 26, 2020)

Matt,

I'm sorry. I'm typing on my phone in the moments between real, bill paying work. I wasn't trying to be rude.


Chris



mattthemuppet2 said:


> well colour me not bothered to reply again.


----------



## ChrisAttebery (Feb 26, 2020)

*I rewrote my original post and tried to make it clearer. *

I went back to my tool dealer this morning and explained the trouble I was having with the PTD cobalt drills. They gave me a refund for the new drills I had left. I described the cut I was taking and told them I wanted a stub length parabolic drill that would work for aluminum. We found a YG SCREW MACHINE DRILL HSS-Co5% SCREW MACHINE DRILL PARABOLIC FLUTE in stock. They were about 25% cheaper than the PTD drills. They seem to be much sharper and I was able to shave a fingernail with one. I've been really happy with YGs HSS end mills for aluminum. I'll try them out and report back.

https://www.yg1usa.com/feature/itemdetail.asp?edpno=DN515205


----------



## ChrisAttebery (Feb 26, 2020)

I looked up the recommended speeds and feeds for the YG tools. They recommend 3200 RPM and 9.6 IPM to start with. From my experience they are very conservative with their recommendations though. I have programs where I run their HSS end mills for aluminum 20% faster than they recommend. I've run their end mills at those for hundreds of hours without any issues. Applying that logic to the drills would put me at 4300 RPM and 17 IPM. So maybe I was pushing the PTD drills too hard.


----------



## mattthemuppet2 (Feb 26, 2020)

ChrisAttebery said:


> Matt,
> 
> I'm sorry. I'm typing on my phone in the moments between real, bill paying work. I wasn't trying to be rude.
> 
> ...



no problem, I shouldn't be so quick to jumpt to conclusions!

another thing to try, if it's an option, is to vary the "peck interval". I often find myself drilling to 2 or 3D first, then 1/2 that, and then at most 1D each peck or the chips start packing and dragging on the walls of the hole. That's doing it manually but I did just finish drilling about 90 #19 holes, so I had plenty of time to get a feel for it


----------



## middle.road (Feb 26, 2020)

mattthemuppet2 said:


> no problem, I shouldn't be so quick to jumpt to conclusions!
> 
> another thing to try, if it's an option, is to vary the "peck interval". I often find myself drilling to 2 or 3D first, then 1/2 that, and then at most 1D each peck or the chips start packing and dragging on the walls of the hole. That's doing it manually but I did just finish drilling about 90 #19 holes, so I had plenty of time to get a feel for it


(90) #19's? I think my eyes just crossed and my shoulder started aching...


----------



## ChrisAttebery (Feb 26, 2020)

I decided to call YG and speak to a tech rep. I told him that the speeds and feeds looked pretty conservative for these drills. He looked up another drill that was HSS but metric and said "I'd run that drill at 4500 RPM and .0045" feed per rev (20.25 IPM)."  



ChrisAttebery said:


> I looked up the recommended speeds and feeds for the YG tools. They recommend 3200 RPM and 9.6 IPM to start with. From my experience they are very conservative with their recommendations though. I have programs where I run their HSS end mills for aluminum 20% faster than they recommend. I've run their end mills at those for hundreds of hours without any issues. Applying that logic to the drills would put me at 4300 RPM and 17 IPM. So maybe I was pushing the PTD drills too hard.


----------



## ChrisAttebery (Feb 27, 2020)

Last night I tried out the YG parabolic drills. They seem to cut more freely that the PTD drills on my lathe. I ran my test program at 2250 to 4500 RPM and feeds from .0015 to .00225 IPT. The drills handled them all, but I did start to see some chip welding at .00225 IPT. I'm going to stick with 4500 RPM at .0015 IPT. 

I also realized that even though I've been setting a reduction in peck depth in Fusion 360 Mach3 doesn't support that option. I've been using this option for a few years and never realized that it wasn't actually being used in my G code.


----------



## mattthemuppet2 (Feb 27, 2020)

middle.road said:


> (90) #19's? I think my eyes just crossed and my shoulder started aching...



18 QCTP holders with 5 10-32 threaded holes per holder  Drill held up well, one tip had a little chip but otherwise it's fine.


----------



## middle.road (Feb 27, 2020)

mattthemuppet2 said:


> 18 QCTP holders with 5 10-32 threaded holes per holder  Drill held up well, one tip had a little chip but otherwise it's fine.


And where are the picts of this project?


----------



## mattthemuppet2 (Feb 27, 2020)

on my camera waiting until i have time to post a thread  I have a blank holder to turn into a parting tool holder (tomorrow or Saturday) and then I'm going to try to give them a black oxide coat. once that's done, I promise I'll post up the results.


----------

