Drilling holes on CNC Machines

Hello CD, I’m a member of team 449 and as some of you may remember we have recently gotten a Omio X8 for our shop. After quite a while of trial and error and some help from CD and CncZone, we’ve finally gotten used to cutting aluminum and making some nice parts. Theres still a little work with tweaking the feeds and speeds, but regardless, were ready to take it to the next step of drilling some holes. I’ve heard that twist drilling is the best way to get nice holes while maintaining tool life. Were mostly going to be drilling 5/32" holes for rivets and 1/4" for bolts. If you guys could help with the general feeds and speeds for a machine of this caliber and any tips for tooling and how to attack the cut (chip breaking, retracting, etc.) I would be very thankful.

Split point drill bits and chip breaking are highly suggested. The split point drills reduce the downward thrust required and the chip breaking cycles help prevent “birds nesting” around your bit.

+1 on split point drills, they’re also great for hand use. I don’t know when I wouldn’t use a split point drill honestly, except maybe if I need a prick-punched hole to be super accurate for some reason. McMaster sells screw machine length drill bits (basically short drill bits) with split points for $2-3 each. I’m planning on picking a bunch up for 1072 and 299 soon.

Small holes: split point drill bit, chip break a little more frequently than you think you need.

Large holes (e.g. bearing fits): Pocket it (or contour it) with an endmill. Do this on a test piece the first time you do it so you can compensate for how your particular mill behaves with regards to precision.

It’s not too hard to get it right either way, if you’re already familiar with the basics of your machine.

The Machinery Handbook contains recommended speeds and feeds for different materials, tooling and operations.

For 6000 Series Aluminum and a 1/4" HSS Drill Bit, the optimal spindle speed is 3,340 rpm, and feed rate is 0.0031 in/rev.

Cutting Fluid or a coolant spraying mister will prolong tooling life. We just buy our standard #7 drill bits in bulk and replace them often at under $3 each in HSS.

On that machine, honestly I’d just do everything with an Onsrud 1/8" single flute bit and interpolate the holes with a small helical entry.

We just drill the smaller holes with a single flute end mill like Sanddrag said. We cam it with helical drill motion. Try to avoid the down and rotate motions. Depends on what cam software your using.

It’s a CNC router. Throw out the machinery handbook. The spindle will stall at 3’340 RPM as it produces no torque at that RPM and you could potentially damage the spindle bearings.

Crank up the speed to at least 12K RPM and drill at a reasonable feed. You’ll have to experiment. 6-10 IPM should be ok.

Personally if a part has more than one hole size I just use the most common drill (usually a .196" screw machine length) to spot anything of a different size and then drill it out later. It’s rarely worth changing tools in a router.

this is very close to what we do.

The two post above this are good. The machine you have is listed as an engraver so it will be very limited as to what it can do when cutting or drilling aluminum. If you need accuracy use a carbide spot drill, it wont walk or bend when it first hits the work. Then you can spot all your holes and finish on drill press.

Also 4638 can help if you need something machined, we have a tormach 1100 and would be happy to give you access if you need a part done.

Like feeds and speeds are not very applicable here but if your curious G-wizard is a great tool. That will do all the math for you. We use it as a guide http://www.cnccookbook.com/FeedSpeedsCalculator/CCGWizard.html

Don’t judge a book by it’s cover.

Omio mistakenly refers to the machine as an engraver because of a Chinese to English translation error. It is the strongest, fastest and best machine for cutting aluminium in it’s category/price range.

The omio is the only router we used for our 2017 season.

Cut a boatload of 1/16-1/4" plate without issue at reasonable speeds.

Respectfully speaking, its still limited thus your qualifier “strongest, fastest and best machine for cutting aluminium in it’s category/price range”

That may be but its still limited when milling. I am not knocking it, I was just pointing out that there wont be a direct correlation to speeds and feeds that you would see on a real mill. The mass is not there not to mention the power. It may be great and I am sure it does great work,but the op asked for feeds, speeds, and procedures. The OP or any owner of these would have more knowledge via trial and error than by general CNC mill practice.

In the world of CNC mill you can judge a large % of a book by its cover by simply looking at mass. CNC mills have a lot of mass as I am sure you know. This does not. I am not saying its not great for what we do in FRC. I am sure its is a perfect tool for price and function.

It depends on what your goals are. I know a lot of people who would consider a Tormach a “toy” but I’d bet limited to a 1/8" endmill and aluminium you could achieve a significantly higher material removal rate compared to tons of machines twice or even four times it’s size/mass simply due to a higher spindle RPM. Another example of this is the Datron line of CNC machines. They utilize extremely high RPMs and vibration dampening epoxy granite to achieve great results in a lightweight machine.

I can engrave parts with a dremel, an engraver, a CNC router, a Tormach or a Mazak. Simply saying that because the manufacturer lists the machine (incorrectly) as an engraver and therefore limited is inaccurate and misleading. It’s just a different machine and like every machine may require different parameters.

When I drill with my machine, I always use peck drilling. This is where you advance at maybe 6 to 8 ipm but only take about 50 thou or so of a bite before backing off briefly and repeating. But Julian quarter inch and 5/16 holes for rivets with an 1/8th inch onsrud bit is probably the best advice.

If that works for you, that’s good, but pecking at 1xD or more for any reasonable sized drill is far faster and will cause less tool wear.

Is this true for routers and thin sheets as well? A 1XD depth peck will punch straight through 1/8" sheet for 0.196" holes, not to mention the super high RPMs involved. Is that more likely to make a chip weld to the bit or otherwise screw up the holes/bits?

I didn’t take into consideration the fact that routers are way higher RPM. That would probably be a concern.

The way my system does it is almost like a chatter, only a brief retraction. The slowest my router will go is 8000 RPM