[jbrookes]

It's a 1/8 drill. I am drilling into eco-brass at 1500 and .006, wih G83 and .18 peck. The bit slips in the collet longitudinally. Here is my current understanding, which I gleaned from Rego-fix and Practical Machinist. I am using Castrol water-based coolant, and the first thing to is to remove the coolant from the collet and chuck surfaces. I plan to do that with a series of solvent baths: wd-40, ethanol, and acetone. Torque is supposed to be 40 ft-lbs. Finally, I have ordered some Rego-fix collets, though Mritool looks very good as well.

Any comments? Thanks.

[jbrookes]

Maritool, that is.

[txcncman]

Are you using a new drill bit that is sharp? What angle - 118 - 135? Split point? Are you using a new collet? If the collet is not new, has it ever been crashed (broken tool) before? 0.006" per flute? Probably too aggressive for brass.

[78nova]

I would make sure you have the correct size collet and that you tighten it down more. Also make sure the collet is snapped into the cap all the way.
We have 3 different kinds to ER16 holder styles. One has a cap on it that accepts a 1.0" standard US wrench, this is the one I prefer. One has the notches around the cap that takes a special wimpy wrench and the other has just two wrench flats on the cap.
I have never used a torque setting when tightening down tools. I use what feels tight and it works. I know this may sound crude but it works when you have a good feel for it. More tools come loose from "NOT" being tightened down Enough! You would most likely have to put a cheater bar on the tool you use to tighten with, in order to crack the cap. Cracking a collet is not very likely.

(chair)

[jbrookes]

I would make sure you have the correct size collet and that you tighten it down more. Also make sure the collet is snapped into the cap all the way.
We have 3 different kinds to ER16 holder styles. One has a cap on it that accepts a 1.0" standard US wrench, this is the one I prefer. One has the notches around the cap that takes a special wimpy wrench and the other has just two wrench flats on the cap.
I have never used a torque setting when tightening down tools. I use what feels tight and it works. I know this may sound crude but it works when you have a good feel for it. More tools come loose from "NOT" being tightened down Enough! You would most likely have to put a cheater bar on the tool you use to tighten with, in order to crack the cap. Cracking a collet is not very likely.

(chair)

....I read the Rego-fix website directions, and they say to clean it and assemble it correctly. I did that, and it seems to cure drill slippage.

Another problem I am having is drill wandering. I am drilling a 1 inch hole 1/8 diameter. I am using a Guhring GT-100 taper length drill with parabolic flutes. HSS. I had the drilling working fine, but now am having it wander and break out through the wall of the tube. I am pushing the bleeding edge, as the walls are only .010, but was successful before.

The drill wandering may be caused by any of these:
-crappy collets. I have some collets with what looks like "SYC" engraved on them. Another has a triangle.
-The G83 woodpecker scenario was not coming back far enough, and drill was not getting coolant on it.

That's about it. I will next try to improve the coolant wash on the drill via G83. Then I will try a better collet. I have a mix of cheap imported and more expensive US made. My suspicion falls on the imports here.


Question:

Anyone have any indicator approaches to getting the drill bit centered? I have used a last word plus a carbide rod in the past. This is redious, and it would be nice to invent a method that is easy to do...

[jbrookes]

I would make sure you have the correct size collet and that you tighten it down more. Also make sure the collet is snapped into the cap all the way.
We have 3 different kinds to ER16 holder styles. One has a cap on it that accepts a 1.0" standard US wrench, this is the one I prefer. One has the notches around the cap that takes a special wimpy wrench and the other has just two wrench flats on the cap.
I have never used a torque setting when tightening down tools. I use what feels tight and it works. I know this may sound crude but it works when you have a good feel for it. More tools come loose from "NOT" being tightened down Enough! You would most likely have to put a cheater bar on the tool you use to tighten with, in order to crack the cap. Cracking a collet is not very likely.

(chair)

I'm using the slotted mini-nut style, to save space on the table.

[jbrookes]

Are you using a new drill bit that is sharp? What angle - 118 - 135? Split point? Are you using a new collet? If the collet is not new, has it ever been crashed (broken tool) before? 0.006" per flute? Probably too aggressive for brass.

.006 is .003 per flute. I am using new guhring GT-100 parabolic taper length drills. Not sure what angle they are - think 135.

Not sure what type of collet I am using. Could be an import. I have to sort out my collets and keep the expensive ones separate.

The best deal seems to be maritool at $17 or so apiece.

[78nova]

I have not used guhring GT-100 parabolic taper length drills & Guhring does make some good stuff it is just kind of pricey. First off, I have never had any luck with Parbolic flute drills when drilling holes under a 1/2" and I do not think they are very self centering. Either get yourself a good made 140 degree self centering drill and or add a center drill to start it straight. Dormer Precision Twist drills work good and so do Sandvick & OSG. I mainly use carbide drills in the Aluminum parts we make & we use Fullerton drills. 3-flute self centering.

[jbrookes]

I have not used guhring GT-100 parabolic taper length drills & Guhring does make some good stuff it is just kind of pricey. First off, I have never had any luck with Parbolic flute drills when drilling holes under a 1/2" and I do not think they are very self centering. Either get yourself a good made 140 degree self centering drill and or add a center drill to start it straight. Dormer Precision Twist drills work good and so do Sandvick & OSG. I mainly use carbide drills in the Aluminum parts we make & we use Fullerton drills. 3-flute self centering.

Thanks. How deep are you drilling depth/dia ? I am driling 8-20 ratio using peck, but would like to get rid of peck.
JB

[uli12us]

I use only ER16 Collets with an adjusting screw, behind the end of the collet. If your drill is in contact with the screw, it can't slip into the collet.

[jbrookes]

I use only ER16 Collets with an adjusting screw, behind the end of the collet. If your drill is in contact with the screw, it can't slip into the collet.

is this a set screw?

[jbrookes]

I have not used guhring GT-100 parabolic taper length drills & Guhring does make some good stuff it is just kind of pricey. First off, I have never had any luck with Parbolic flute drills when drilling holes under a 1/2" and I do not think they are very self centering. Either get yourself a good made 140 degree self centering drill and or add a center drill to start it straight. Dormer Precision Twist drills work good and so do Sandvick & OSG. I mainly use carbide drills in the Aluminum parts we make & we use Fullerton drills. 3-flute self centering.

The Dormers and OSG: are you using a peck cycle?
The 3 flute carbide drills: wat speeds and feeds do you use?
as well, I have some coolant through drils which I may deploy.
jb

[jbrookes]

I have not used guhring GT-100 parabolic taper length drills & Guhring does make some good stuff it is just kind of pricey. First off, I have never had any luck with Parbolic flute drills when drilling holes under a 1/2" and I do not think they are very self centering. Either get yourself a good made 140 degree self centering drill and or add a center drill to start it straight. Dormer Precision Twist drills work good and so do Sandvick & OSG. I mainly use carbide drills in the Aluminum parts we make & we use Fullerton drills. 3-flute self centering.

I followed your advice about center drill, and it looks like it may have cured the wander problem.
I am interested in your feeds and speeds on the 3FL Fullertons. I have some 1/8 carbide USA 3FL drills I am itching to try. The fit and finish on them is very good. The cutting angle of tip looks almost 180. The tip almost looks like a milling cutter end-mill.
I am cutting eco brass so I magine I can try speeds like 4000 rpm at this drill dia. Just curious about your F and S.

[uli12us]

Yes, its a setting screw to adjust the offset of your tool, in some toolpresetters you can drive a the allen head with a long hexshaft from below, but on some collets you can have a thread on the inner end of the collet in which you can screw special tools. But I don't know if you can buy ERs with such feature. I fear that option is only available for single sided slotted collets.

[78nova]

JB,

I do not use ipm or ipr when determining what feeds & speeds I use when running Fullerton 3 flute drills. There are several factors to look at when I determine just how fast I want to go which are, tool effective length out of holder or type of extension used, hole diameter & positional tolerance.
I am limited to 5000 RPM with the older machines I run.
Fullerton recommended SFM is 300 - 600 in AL & feeds as follows;
1/16 .008 ipr
.125 .003 ipr
.250 .007 ipr
.500 .012 ipr
.750 .015 ipr

The actual drill effective length will determine just how fast you can go with good results. If you have 1.0" -2.0" effective set lengths you can go fairly fast & your feeds & speeds. The longer the drill sticks out will limit your rpm & feedrates. Again, this is all relative to your own setups & varibles you work with. I normally run Fullerton drills, .067 - .0937 diameter up to 5000 rpm, but the larger the size will have me backing off the diameter as I go up in size & as I mentioned before the length of the tool.
What I will recommend is testing, testing & more testing. Use a scrap part or a block of material and test your speeds, feeds to the size drills you are using with the tool setups you have.
The only reason I never used sfm, ipr & ipm is I was never taught that way. When I first started machining in 1973, I just used the speeds & feeds provided to me. If what I was given did not work I played around with the feeds I speeds until I found what worked best. I have done very little manual machining. I have been doing CNC machining & tape proofing for over 30 years so I have had several programmers to work with over the years, some better than others. Through all of this, I have been able to see what works & what does not over & over again. This is how I learned my feeds & speeds to help me get a good feel for what works for the particular tool setup, part setup & machining detail.

[neilw20]

Rough up the drill a bit.
12v on an old carbide insert.
Spark it all over the shank. Leaves what looks like little pits.
Look under microscope and see tiny bits of carbide sticking up!!
Works a treat in lathe jaws to stop hard materials slipping too.:idea: