Keyless Drill Chuck on 3HP Columbo

[johnny]

I have a 1/2 inch keyless Jacobs drill chuck ready to put into my Columbo, does anyone think this is a bad idea? I have a 3hp 1phase motor. The chuck weight is almost 2.5 lbs.

[bjwat@comcast.net]

Johnny...

Yes, you would be correct in assuming that a 1/2" Jacobs chuck is the wrong collet for use on a high RPM spindle. It is not meant to be run over 6,000 RPM and not only that but, that weight on the end of your finely balanced spindle will wear out your bearings in a heartbeat. It's not made to handle that sort of thing.

One thing that I don't understand is the reluctance to using 2 wrenches to remove a tool from the collet. Quick change collets are just a bad idea all around, unless they are designed for use with that spindle. I can change a tool out on my Colombo and Z-Zero it in about 2 minutes.

Sorry for the rant, but I'd hate to hear about someone getting hurt from a 2.5# chuck exploding at high RPM.

-Brady

[elcruisr]

I'm with Brady. If you didn't get hurt you'll trash your spindle in short order and get no sympathy from the manufacturer. On top of that you'll be losing useable z-axis, increasing tool deflection and introducing unacceptable runout. If you don't think that is important realise that most experienced people in the cnc world throw out their collets and replace them at 200 hours. I know it makes a difference I can see and hear, and we are just talking about a thousandth or so. Your chuck would introduce many thousandths of problems.

[elcruisr]

I'm with Brady. If you didn't get hurt you'll trash your spindle in short order and get no sympathy from the manufacturer. On top of that you'll be losing useable z-axis, increasing tool deflection and introducing unacceptable runout. If you don't think that is important realise that most experienced people in the cnc world throw out their collets and replace them at 200 hours. I know it makes a difference I can see and hear, and we are just talking about a thousandth or so. Your chuck would introduce many thousandths of problems.

[sheldon@dingwallguitars.com]

The keyless drill chucks loosten with vibration.

I tried the Jacobs wrenchless router collet and it had tons of runnout.

[johnny]

Sorry gents, I should have given a little more information. I am using the drill chuck for drilling - at lower rpm. I will change out the entire chuck like I would router bits, when I need to route. The machining will all be done in the z movement.

I understand about the wearing out my bearings, but are you guys thinking if I was cutting x and y too? How about at the lower RPM and only in z? I am worried about the wieght of the chuck and the high frequency stuff and low rpms and all the stuff I don't get about how this kind of motor works.

Does the Columbo always maintain the same frequency/rpm under load? So if i am running the chuck at a low rpm (like 600), will it still cut (drill) well or is it going to dog out?

Also, I havent used my router in awhile, but is there a way to approximate the rpm on the spindle? The control box for the spindle has a LED readout on it, but it doesn't show RPMs. I read awhile back that you can take the number on the readout and times it by something.

Thanks again.

[johnny]

Brady - what is your web address? I would like to see your setup.

[bjwat@comcast.net]

Johnny,
The lowest I have ever run my spindle is 3,000 RPM in wax...and I don't advise cutting parrafin wax on the CNC EVER!! I am still scraping shavings off of the machine!

For drilling I have successfully run it at 5,500 RPM using 1/8, 1/4 and 1/2 inch bits. I just selected the collet to match the bit...Of course that is no good if I am drilling an odd size, say a #29 drill for instance. I also drilled into soft melamine/formica and not metal. I wouldn't advise drilling metal with the spindle without coolant...and that makes a real mess.

I guess the 2 questions I have for you are 1) What are you drilling into & how thick, and 2) What size bit are you using? (Hopefully you are not going to come back and say a 6" holesaw...LOL!) That will dictate whether or not I would run the spindle that low of an RPM. Just like an engine, the spindle generates usable torque within a certain RPM range. My concern would be smoking the motor because it needed more torque to bore through a tough material at low RPM. The electric motor driving the spindle can burn up if it arcs on the stator trying to maintain RPM.

To gauge RPM with the Delta HF box that came with my 5HP Colombo, I simply press the Mode button 2 times and it displays RPM. The frequency scale on mine is between 0 and 400, translated to 0 to 24,000 RPM. The other way to determine RPM is to take the displayed number...Say 250 and multiply it by 60. That would give you 15,000 RPM.

I don't have any other pics online at the moment of Big Bertha...but there are a few on the Indexer post on this week's list. There's another pic link on here for my plasma water table as well if you search this site.

Email me if you have any questions.

bjwat@comcast.net (mailto:bjwat@comcast.net)

[johnny]

Brady - Thanks for the reply. I try to use standard cutters (1/8,1/2, etc.) when I make holes, but this job has many non standard hole sizes. Luckily it is in MDF, so I can run at a decent RPM. I have been wanting to work with aluminum though. So if you have any heads up for that, I would appreciate it.

So do you think using the chuck just to drill through MDF is okay, or make due with 1/8 router bits. That wouldn't help if I need to "drill" odd sizes in metal though.

Actually, I forgot, I need to drill some tiny holes for this job and they are on a part that has no square sides or straight edges, so measuring for manually drilled holes is less desirable than finding a drill chuck solution, unless it messes up my router.

-Johnny

[grandpas@ix.netcom.com]

I have a Milwaukee core drill mounted on my second z-axis and drill holes all day long. I am drilling 2 inch oak, poplar and ash. Speed for the core drill is 600 rpm and I use standard wood bits. Yesterday I ran 3500 holes in tool blocks for leather workers. you can see the finished product on my web site. www.grandpas-pastime.com.
The Milwauhee core drill runs around $300.00 and has a steel bracket i drilled holes to mount to the z-axis plate. It's the only drill motor I found with a steel plate mount. I have used it for over 4 years and only replace motor brushes twice in that time frame. Z motion is set at 0.5 and prevents tear out in the holes that are 1/2 inch apart. speed is governed by hole spacing and material density. Drill bits are all same length and come from Forrest city bit company. If you need a picture e-mail me and I will send one to you

[johnny]

Holy Cow! You sure do drill a lot of holes - saw your site.

I will email you for a pic - just to see - because doesn't sound like you use a chuck on a Columbo.
-Johnny

[elcruisr]

Johnny,
remember that the lower the rpm the lower the horsepower on your spindle. Before I ran it at 600 rpm I'd want the OK from the manufacturer. BTW they are great people to deal with and always glad to help. There are drillbits designed for use with spindles in many sizes with standard shank sizes available. Try Onsrud, they have some availale. Collets are also available in pretty much every size. MSC is one supplier, and good machinist supply should have them but only use good high precision collets, NOT the cheapies.

[mrdovey]

Johnny,

I have several parts that are hole intensive; and deal with the problem by using a bit the same size or smaller than the smallest hole - then wrote code to simulate a drilling operation.

I plunge at the center of the hole and if the hole is larger than the bit, cut a spiral path to the outside edge, then make a circular pass to ensure "roundness" of the hole.

When the hole is too deep to cut in a single pass, I plunge farther and repeat until the hole is done.

It took me a while to work out the math; but was worth the effort. The current version uses a tolerance parameter and calculates a minimal toolpath (the smallest number of J2's consistant with the tolerance) and is fast enough to be faster than changing bits even just once.

This approach is particularly nice for "compound" holes - counterbored holes and the like - and a countersinking routine is on my ToDo list, so that I can add a uniform conical top to a hole to improve both appearance and quality of screw assembly.

I looked at the chuck approach as well; and decided that this approach was actually faster than changing bits with a keyless chuck. The trick is learning to work /with/ the ShopBot to take advantage of its strengths, rather than trying to rebuild it into some other tool with which we're more familiar. (I know from my own experience that this isn't always easy :-)

Morris

[donchandler]

Use this routine in Vector to route all your holes. I mounted a Milwalkee mag drill press motor on my second axis. It worked, but if the material is hard to drill, it would lift the Y axis off the rails, loose steps, etc. Shopbot uses limit switches and they go down until the switch trips and then it goes up. They don't worry about the lost steps. I found that routing the holes using the ShopBot software to spiral down is faster and no bit changes!
move to the center of the hole you want to drill and it will drill.
&D=|ask('DIAMETER OF HOLE','0.375')| 'Diameter of hole
&P=|ask('PLUNGE PER TURN','.1')| 'Plunge per turn
&N=|ask('NUMBER OF TURNS ','3')| 'Number of turns
&C=|ask('CUTTER DIAMETER','.25')| 'Cutter diameter
'When Ready Press Any Key
PAUSE
'Cutting Hole
SA
SC,2
VC, &C,,,.5
G00 @c 'this is the center of the hole
GOSUB HOLE
Pause 1
END
HOLE:
SC,2
CP, &D, %(1), %(2),i, 1, 0, 0, -&P, &N, 1, 1, 4, 1, 1
jz, .5
RETURN