Replace Spindle/Router with Metal Milling Head?

[gerryv]

Has anyone replaced their router/high speed spindle with a milling head or perhaps added some sort of speed reducer head so that standard metal milling machine tooling can be used? My standard Buddy with PC router has an extended axis so there would be room for a speed reducer of some sort.

The thought is that this would allow us to use this machine exclusively for metals and stay isolated from the PRT alpha machine and other woodworking operations so we don't get contamination from metal fragments. The application would mostly be for the machining of variously shaped brass and stainless steel feet and accessories for custom made premium furniture. The pieces would still be hand polished and finished so we don't need to worry about getting the kind of resolution or simultaneous 4 axis machining one expects from milling machines.

While I'm aware that soft metals like brass can be machined with the standard routers and spindles and if we'd be willing to forego the SS, the impressions (which could well be wrong) I've formed from reading archived posts is that one cannot "hog" as much metal in a given amount of time and that router/spindle tooling costs due to wear and breakage would like be much higher.

The other impression I've come away with is that while spindle speeds can theoretically be dialled down quite low, they don't run well at their bottom end speeds for some reason - perhaps not enough torque to power something like a 1/2" diameter tool? Is anyone using a spindle with success for this type of application? If yes, has anyone found suitable bits/procedures for doing SS, even slowly...successfully?

It would seem to be a pretty simple adaptation to pull off the router and holder and replace them with the head from a smallish bench top square column mill and tram it with shims. A lot quieter too :-)

[knight_toolworks]

it's not the head that's the issue it is the rigidity and the mass and slop that would be an issue.
Metal is very hard to mill well because it is hard (G) even my 600# mill/drill can only take light cuts to keep vibration down and accuracy up.
when you look at this
http://cdn8.grizzly.com/pics/jpeg500/s/sb1024.jpg
do you see a shopbot? even getting .01 on a shopbot on a regular basis can be a battle in metal it would be far worse.

[gerryv]

Yes, you're right on that Steve, I had metalworking equipment before we switched to woodwork. The key of course is that in our case there is no need to push speeds at all because there is no volume expected being a custom hardwood furniture shop doing mostly one-off pieces. Also, because the Buddy 32 has such as short Y axis but uses the same extrusion as the 4' and 5' ones there is actually a lot of rigidity there and there is the added benefit of the gantry being fixed. Heck, the extrusion and support members alone likely weigh 20 x what my little Sherline mill weighs :-)

I also had one of those Chinese lathe/mill/drills and I know from experience that the quills on those things are terribly sloppy and at full extension, might as well be a boat mast - yet some guys still manage to produce pretty fine hobby work on them by going slow and using extra care. Hell of a lot better than a vise, chisel and file anyway (chuckle).

Also, we'll not being needing to hit the same tolerances as a decent milling machine as these pieces will be hand finished; kind of like what a traditional toolmaker does - now those guys were/are skilled!

What I really want is CNC capability that can give us within a 32nd or, hopefully, 64th with the "final passes" being done by hand. My son is first a fine fine furniture builder who wants to maintain the fully hand built wherever possible but at least hand finished. I'm simply looking for a way to speed up the roughing aspect and make use of our existing machines and software (Aspire 3) for those pieces that are commissioned as hand-finished only.

The PRT Alpha will actually be used as a parallel business operating in the same facility with someone else doing fairly low volume hardwood and plywood products as a sideline to help keep the lights on so that my son can chase his passion :-) We're actually looking for that someone now but, finding an available 'botter is not proving to be easy.

Like I said though, I agree with you fully that it could not be expected to do the job of a HAAS or even a refurbished Bridgeport or any of the offshore knee mills like the one you posted.

Thanks much. Gerry

[michael_schwartz]

Use the right tool for the job, I don't think a shopbot would be well suited for this. Vibration, flex, wear and tear aside, I doubt the motors would even have enough torque.

I would buy an old milling machine for scrap price and convert it to CNC.

[Gary Campbell]

Gerry...
The frame on the SB is much too light to function well as a mill. High RPM routing doesnt load the machine near as much as a mill would. Like Mike says, use the right tool for the job.

[gundog]

Gerald,
I have considered doing this myself for machining aluminum I think SS would need a heavier machine unless you take light cuts. I also do machine work and there is no substitute for heavy rigid machines when machining steel & SS.

Here is a head I have thought about buying for mine and making a mount to take the place of a spindle. If I had room for another machine I would probably do it.

http://littlemachineshop.com/products/product_view.php?ProductID=2517&category=

They convert these mini mills to CNC and as you can see they are very light and no more rigid than a SB but you can't take heavy cuts with one. I think one of these small heads would work they weigh about the same as a spindle but turn the appropriate speeds for milling metals. They also do not cost any more than a good router.

Mike

[gerryv]

Hi Michael,

Yes, that's the type of head I was thinking about. It's been awhile since I've purchased anything from LMS so had forgotten they had these units.

I certainly agree with you, Gary, Steve and Michael S. about the benefits of of mass/rigidity when it comes to mills so no issue there. I've has quite a number of metalworking machines right from the little Taig and Sherline lathes and mills on up to compact tool room units that weighed in on the plus side of a thousand pounds and there's no question which were more rigid and could handle heavier cuts. That said, my little manual Sherline mill (not yet CNC'd) can hold pretty darned tight tolerances even though I can literally pick it up with one finger - as long as I cut slowly and lightly enough.

That's probably where I didn't explain myself so well earlier. While I agree that it's best to use the right machine for the job, I also need to consider other factors. (1) How many pounds of metal will I likely remove in a whole year? Probably less than 20 lbs. (2) I do need CNC due to the nature of the shapes being cut, which means a learning curve. I have only 12% of my short term memory on a good day due to a disabling accident. That's the part used for learning new stuff so I've struggled some and had lots of false starts even getting into the basics of Shopbot & Vectric, which are considered the easiest to learn so I sure don't want to now take on Mach as well (3) I already own the Buddy, sitting alone and bored and feeling rejected in the corner, haha but would need to spend $ to get what I agree is the right machine for the job so, at 15-20 lbs a year of removal, is it the wise choice of machine for the job so-o-o... IF I can go slowly and lightly with the Buddy (I'm retired and in no rush) then, hmm... the router on my Buddy pulls 1.5 Kw and the spindle on the head you pointed out pulls 0.5 Kw ... the stepper torque on the small tabletop mills and lathes is about 240 oz/inches while the Buddy's is more in the range of 600 or more?

Gary nails it of course by pointing out the fact that the much higher RPM router/spindle doesn't load the machine so much and this to me is the biggest factor. However, where most of the 'botters tend to work and think in terms like 3-5 inches per second, I'm thinking in terms of 3-5 inches per minute :eek: like I do on my little Austrian EMCO lathe. Heck, the planing bit for levelling the tabletop on my Buddy is about 2" so I can't help wondering that IF I were to stick to a <0.25" round nose mill bit at say 10 in/min and small step overs, just how bad would these roughing passes be recalling that the pieces will be hand finished anyway. Steve also made the important point about vibration which I know from experience can end up with "a whole lot of shakin' goin' on" when using the lower RPM and larger diameter milling cutters :-)

I guess I just keep thinking about how UNrigid and sloppy the quill was on my awful and gone Chinese 3-in-1 lathe/mill/drill compared to the Z axis on the Buddy and yet, with care and time I could produce to higher tolerances than I actually need here although I have to admit that was on mild steels, plastics, etc. and some of the Stainless's are certainly a different animal regardless of machine.

Actually guys, I think it may just be more about the fun of trying to see what's possible for this retired old geezer rather than trying to change well established paradigms and truths. So please accept that I really am hearing and don't question your advise. I was mostly just wondering if any other silly fellow like me has actually tried it to determine what it could do in a pinch.:o

[Brady Watson]

I've got one of these heads on my old PRT gantry. Still in the R&D stages since we just bought a farm and I put a lot of things on hold (that's where I've been!)...It will reach the table for milling purposes, but I am modifying it in Z to be able to put a tapping head on it. The RPM of my 5hp spindle is too high for a tapping head.

Compared to my Bridgeport, the PRT is flimsy...It will be fine as long as it is operated within 'milling speeds' not routing speeds & you limit your bite in all axes. Ditch the plastic gears in that head and get a belt drive. You'll get a wider RPM band and eliminate broken gears. I had to make a solid 2" aluminum mount/adapter to mount to the t-rail. The head is NOT a bolt on deal - there is some engineering and work to be done to mount it. Also, you'll have to remove and re-mount the e-stop button that comes with it to clear the Y car. It absolutely will not fit in a PRT gantry as a 2nd Z. It needs the whole bay.

Plus...you'll want to up the ante on the Z motor if you are running anything less than a 7.2:1 Alpha. I am running a 25:1 harmonic geared Alpha on it for increased torque & positional accuracy. Not sure if I will incorporate the brake on it yet or not. Also...The 'spoilboard' should be metal - ideally aluminum. You'll flatten it with a mill just like MDF, except it should have provisions for clamps or threaded studs/screws. You will want or need to run either coolant or lube when cutting most metals, and MDF ain't gonna cut it...

This setup will add a lot of versatility to your machine, but as Dirty Harry says, "A man's gotta know his limitations" - A Bridgport mill or HAAS it ain't...

Pics when it's done...It's a mess right now!

-B

[jeffreymcgrew]

We cut aluminum all the time since we got our spindle. With the right tooling, we don't even use lubricant or air, we just cut dry and it works great. We've been taking shallow passes of .125" at 1.5 IPS and it works great. We do roughing passes .005 out and then one final cleaning pass at zero. And we've just got an older PRT with a 4G upgrade, not a PRS or Buddy.

It works so well that things I thought about before maybe making out of steel and getting cut somewhere else, or cutting with our small plasma torch, I now make out of aluminum.

However, with that said, hold down and vibration are totally killers here. After cutting aluminum it's not uncommon for something to have loosened up on the machine somewhere. We have the machine make safe holes in the sheet first, and then screw it down all over the place. No way could you walk away while it's cutting and do something else, either, for things go wrong really fast when cutting aluminum. Also, our table is stiffer than the stock Shopbot table, heavier too, so maybe that helps.

What I would do is unless you really want milling, i.e. pockets and other features, I'd fine someone local with a waterjet that will run small jobs for you, and get your steel cut that way. Laser is good too, but if you're planning on welding anything after it can be a pain for the heat of the laser can temper the edges of the metal and make it harder to weld. But a waterjet or laser will be so much faster than any mill that even paying someone else to cut it for you might be cheaper than having your 'bot spend hours doing a job something else can to in less then ten minutes.

We looked into adding a bigger head for steel, or picking up a smaller CNC mill like the Tormach, and in the end the numbers said that we should just farm out our steel cutting for now to a bigger shop with the right tools to do it.

[frank134]

What cutter do you used for cutting almuminum?
How thick of a piece can you cut?

[Brady Watson]

There's certainly no issue cutting AL on the Bot - thin sheet or thicker parts up to let's say 1.5" thick - that are held down well, can produce good results.

If you need to do production in thick AL or steel that requires lube & coolant - then farming it out or investing in a CNC mill like a Tormach is a wise decision...although I have to say, farming it out is no fun for guys who like tinkering or the occasional Saturday metal project.

With the Colombo, I use a spiral-O bit up to about 1/2" thick. If doing extensive area clears/pocketing, I will use a HSS end mill with a geometry suitable for milling AL. The HSS absorbs some of the harmonic vibration that you can get when milling AL with solid carbide end mills in certain diameters & feeds. Plus HSS will bend in situations where carbide will snap or shatter.

You can mill 2D and 3D in most non-ferrous metals with your router. As Jeff pointed out, you can't walk away when milling this stuff & you can't be asleep at the wheel while programming or operating.

-B

[jeffreymcgrew]

We've been using Amana Tool's polishing flute aluminum cutters, and they work great.

We do roughing passes down to an onion skin 0.005 offset, then a cleanup pass with no offset and full depth. We run 1.5 IPS with .14" passes at 18,000 RPM with a 2.2 HP spindle.

Tabs hold like crazy in aluminum, so you don't need very many to keep the part in place while cutting this way.