Cutting Aluminum Bar

[Kenny_BTFP]

I'm getting my first shopbot this month. I have the airdrill along with the spindle and will be cutting and punching holes in the aluminum bar. the bar is 1/2" and 5/8" thick. it will be cut to length on a bandsaw and then trimmed on the router table. there will be 5/8" holes punch through the aluminum using the airdrill, and then cleaning up/ tapering the edges with the spindle. in the 1/2" pieces i will be punching holes that will then be threaded.

my only concern is what bits to use. Im looking through the ONSRUD catalog and i dont know what i need. downcuts, upcuts, single flute, double flute... the diameters i can figure out, but the type of cutter i need to use for each of these is really what i need help with. at least a starting place, i figured i would get several to test and figure which one works best for each application i have.

does anyone have any advice?

[Brady Watson]

Don't plan on drilling anything other than melamine/flakeboard with the air drill. It is designed for cabinet production. It absolutely positively will not work for your application.

You can 'drill' holes by using a smaller bit and spiral into the cut with a smaller diameter cutter, using a inside profile toolpath strategy. This is the preferred method of drilling holes in AL on a CNC router. You must *never* plunge straight down into a cut - It must be ramped.

As for cutting, you really need to think about how you are going to hold the parts down. This is nearly the ENTIRE JOB in CNC machining & one that needs to be carefully thought through. You can use a single spiral-O bit to do all of your cutting, but the best would be to have an Onsrud dealer come to your shop and recommend tooling to you - or at the very least, you take a trip to his store.

-B

[letterman7]

Brady is an incredible source of inspiration and knowledge. But in this case I have to disagree with the drilling procedure. Yes, you have to ramp if you're using a bit, but you can also simply chuck the appropriate size drill bit into the spindle. I did this for years on an industrial CNC (albeit the thickest we milled was 1/2"), and you can drill the holes with either a very slow downfeed or a 'peck and retreat' method which clears the chaff just as well. On the thicker stuff you may want to use a lubricant - WD40 works well. I preferred the 'peck and retreat' where the spindle drops just a bit at a time - maybe 1/8" total each time. You might be surprised how clean a hole you can get with that method!

[Brady Watson]

Rick,
Thanks for the acknowledgement...However, the HSD & Colombo spindles sold with ShopBot tools have bearings that are not approved for drilling. They do not like heavy down pressures or shock loads because the bearings favor radial precision over thrust loads. Additionally, spindles are wound to run at a useful RPM of 10,000+. Anything lower than this, and torque goes way down & amperage goes way up.

I'm not saying that what you suggest cannot be done...but to run a brand new tool right out of the box in this way is not advised. It also really isn't the right tool for the job. A CNC mill would be more appropriate for this type of work...but you can get by with intelligent toolpathing and the correct tooling.

-B

[letterman7]

I hadn't realized that the spindles aren't approved for that type of work, but I can't see why it wouldn't work if the procedure was slow(ed) for direct drilling or the peck type drill toolpath was used. The Vytek router I used to run had a 3hp (if I remember correctly) spindle and this was something we did routinely and never had an issue using "regular" HSS bits... though I insisted on the cobalt bits for longevity.

But you're right - for a first time user it's probably not a good idea to push the machine before you know it's limits. Repeatability is always nice, but you can get the same results setting up a jig milled by the 'Bot to place over the aluminum stock.

[beacon14]

Brady, not to contradict, but I asked the HSD reps at the IWF a few years back about this and and they flat out told me they did not know what I was talking about. They stated that the HSD spindle bearings will work fine for plunging as well as sideways cutting. What you say may be very true about the Columbo spindles, but I think the ShopBot community made the assumption years back that this applied to all spindles, and it may not be the case. Of course I ramp all my plunges anyway, but just to relay what I was told.

Also, if we are talking about using the airdrill to drill the holes, then the spindle bearings aren't being used for the drilling operation. I have no experience with the current air drill setup so I can't comment on whether or not I think it would work.

[Kenny_BTFP]

I know that the spindles cannot be plunged, or so i am told and shall not test. But Brady, you mention the airdrill only in your first reply, and everyone else has seemed to ignore that this is the piece of equipment i plan to use for drilling. If i drill the holes in a stepped plunge (peck and repeat), would that not work to drill the holes and preserve the airdrill? also, when i was at ShopBot for training and on the hunt for answers, the airdrill is what was recommended to me. I even had the aluminum bar with me to show the technicians there.

[Brady Watson]

Kenny,
The air drill is meant to drill down in one shot, with a substantial amount of impact on the surface of the material, due to the pneumatic actuator's plunge action. The air drill is really not set up to peck drill, but you could probably customize it to do so - but it would most likely have to run constantly. You need a good solid 10-15 CFM compressor to prevent the need to pause in your file for the air to catch up. It wastes a LOT of energy, in terms of electrical input vs actual work done just to drill holes. Why run 5hp of air just to drill holes?

Regardless of what was recommended to you, I still hold my opinion about using the air drill in this application. It just isn't made to handle drilling AL with those tiny bearings. The correct tool for the job is a 2nd Z axis with a drill head, such as a Milwaukee drill or something to that effect. It is made for drilling, plus is cheap and durable. You really can't alter the speed on the air drill without either spinning it too fast (higher psi than recommended) or dialing it down low, with loss of torque - of which it doesn't have much to begin with. You want the ability to dial in the correct drilling speed.

So...in saying all of this, I would never run the air drill in my shop to do what you want to do. The point in me posting is to help you avoid being disappointed. If anyone reading this is drilling AL with the air drill in a production scenario, I'd like to see your results and hear about your experience.

-B

[Kenny_BTFP]

Brady,

Thank you. I don't have a plan as of yet. We have multiple projects that we will be using it for. Primarily it will be for the AL Bar. In addition we will be manufacturing work trunks and road cases for our production needs (wood/ laminate based). when i was at ShopBot i saw a duel Z with a Milwaukee drill in the second Z, one technician had recommended that, said it would be perfect for all my applications. When my PM called in a week later to get an official quote he was informed that the airdrill is what we wanted, and that it was all the same, so we could get the airdrill and save table space rather than getting the Duel Z. I dont have anything running yet, still waiting on an electrician before i can test the table.

[Brady Watson]

The Milwaukee is the way to go. With a 5' table width, you'd have room to park the 2nd Z and still have a 4' machinable area.

-B