Drilling holes?

[Cartierusm]

Howdy, I've got my CNC router finished and for now have just been cutting cheesy signs using a V cutting bit. But let's say I want to drill holes, for example let's say 1/2", 1/4" and 1/8". What I'm looking for are exmaples of how to cut them, not the programming part but speed and technique.

Basically I could drill the 1/4" and 1/2" with a 1/4" endmill or router bit. as for the 1/8" I could drill with a 1/8" endmill or router bit with a 1/2" shank.

But what I was thinking is I could get a drill chuck with a 1/2" shank to fit my router, then I could use any drill bit I want. Is this the best way to go or will I get more accurate drill hole results with endmill or router bits?

If I go with the drill chuck idea should I abid like normal and run the router at regular drill speed, say 1100 rpms for a 1/4" drill bit or should I run it faster. As a side note I don't know if my Harbor freight router speed control would go that slow, but I just got off ebay a really trick laser handheld tachometer so I could get accurate rpm ratings.

[dertsap]

for small holes you could use pin chucks and anything bigger interpolate it , drill chucks arent balanced so you would probably be looking at having a lot of vibration , pin chucks are what ive had in mind for mine

[Rhodan]

How slow can you get your router to go? Thats the real kicker. Try drilling wood with a 1/2" bit at 10K rpm and watch how fast the bit dulls and the wood smokes (been there!). I seem to do ok with 1/8th bit at the slowest speed (10K) and peck drilling (drill 1/4 deep then back out and back in). This lets things cool a bit and clears the tailings that normally seem to get stuck in the drill web. Still though, the 1/8th bit dulls very quickly so best to use inexpensive bits and sharpen them yourself frequently.

Drilling with endmills is a bad idea. The center of the endmill cannot cut and pushing that into the material can do damage. In wood its not so bad but metal can break things. Better to use the next smaller router bit and hole-pocket. This is how I make 0.159 holes for 10-32 machine screws in aluminium since hole pocketing isn't limited to the tool diameter. Its actually quite fast and easy, just make sure you use a helical feed with a low angle (I use 1-2 degrees) or you'll be shoving that non-cutting center into the metal.

I've been thinking of picking up a Sherline or Taig spindle and motor to mount on my machine in order to get slower speeds with high accuracy (ER collet sets) and the ability to fit a large range of drill bits. Still in the future though as they ain't cheap! Might even try a router speed controller with a non speed-controlled router if I can find one dirt cheap.

[Cartierusm]

Ok so I shouldn't go with a drill chuck extension on my router. How should I drill various holes in aluminum? I can get my router down to 3000 rpms, I used my Tachometer to measure.

Basically what I'm doing is using my old x and z axis to make a new one with a better design. Should I just bolt my aluminum to the router table and use a center drill bit and just mark like .1 down with the center drill and then finish up by hand on my drill press?

[solodex2151]

I agree with Rhodan that a router spins a drill bit way too fast. Check out this drilling chart and you'll see what we mean. I would use a 4 flute end mill bit and route the hole like you would any other pocket. If the hole is smaller than your end mill bit, then you need to drill the hole by hand.

If you really wanted to, you could create an x/y cnc table to mount on your drill press, have that move to the location of the holes, and you drill them manually...

[Cartierusm]

I have a bridgeport but I wanted to avoid having to drill so many hole. I think I might just use the cnc router to drill with a center drill bit and then use the drill press and have the drill naturally find the center of the pilot hole.

[ger21]

You could get a collet chuck, like this.
http://www.use-enco.com/CGI/INSRIT?PARTPG=INLMKD&PMPXNO=8708664&PMAKA=308-0018

But a router's bearings are not designed for drilling aluminum, and may not last long.

[Cartierusm]

I found a $20 air drill at harbor freight, aluminum body. I'm just goig to weld some mounts onto the drill or make a mount. That way I can drill holes properly.

[Cartierusm]

OK Here are the drilling tips and observations I noticed while machining. Fist off I have a Surplus Center Vacuum pump. The aluminum holds real tight to my melamine CNC Router top. I am making a new Z and X axis for my router table that is a little more rigid. I haven't noticed any defelection caused by the Router it's self as of yet, but I can flex the Z axis a teensy bit by hand. Making a new one will allow me to make it perfect as I'm using the CNC Router to make the new parts.

I am using a Husky brand air drill. I wen with the air dril as the front collar is round at about 1 5/8" in diameter; making it easy to drill a hole and split it and add a bolt to clamp the drill in and then bolt it up onto my Router. This went according to plan except that the 1 5/8" hole was a little small and after clamping left it a little skewed, but alas I was able to put a drill bit in it and move the drill into position by using a preceision machining square to line up the drill bit in reference to the CNC Router table. Then I clamped it down tight and move the gantry around and rechecked for square and everything was OK.

I am milling about 16 6mm holes in a piece of 6061 6" x 10" x 3/4" aluminum to hold the linear bearings. I designed it in ArtCAM. I used the drilling operation and just made the drill bit the same size as the holes I needed that way ArtCAM wouldn't drill the hole pocket style. I realized it doesn't actual have a way to add drill bits into the arsenal of tools, it just assumes ALL machining will be made by end mill or router bits and will actually cut like a very small circular pocket. I didn't want that but maybe in retrospect I should have done it that way.

I set up the materials and used a laser center finder to find the edges and zeroed out my DRO. I ran the progam with the drill running at 1800 RPMs. I couldn't get it any slower or it would bog down. I setup the drilling operations in ArtCAM to drill the holes at .0625 steps at a time and use peck drilling. I was plunge cutting at 1 ipm. Any faster and the it would be way to fast. I noticed right away that the drill bit was wondering. Oh, BTW I just bought brand new high end drill bits to use from my machine supply shop, no cheap drills here. So the bit was deflecting not the CNC Router. I stoped and retried at .5 IPM, real slow. Still it wandered. I then tried using a center drilling bit, you know for center drilling for lathe operations, very rigid and accurate bits. No luck it was wondering too. I know it was the bit not the router. I figure it's either the way you hand feed drills on a mill people use "feel" and it makes for more accurate holes,or the drill wasn't PERFECTLY perpendicular to the table and going in at a very slight angle causing it to deflect, but my square said it was right on before starting and after. So I figure maybe drill bits are just not that accurate and I never noticed as I ususally do all my exact driliing with an endmill on my bridgeport. Anyway, I ended up letting the bit wander but used a 3/16" drill bit. Then I used a 6mm end mill in my drill to clean up the holes. At first the 6mm endmill wandered when first plunging into the 3/16" hole because the hole was slightly off center becasue of the wandering drill bit I piloted with. But as i was cutting real slow and an endmill side cuts it self corrected.

So now I need to make some more. My options are to start with a 3/16" end mill and cut the majority of material away and then clean up with the 6mm endmill as a drilling function. OR predrill with a 3/16" endmill and then use a 4 or 5 mm endmill and use Artcam to cut the holes as a circular pocket? Any suggesstions would be helpful. Thanks for reading.

[Rhodan]

Well those center drills are quite short and stout and I can't see it bending enough to make the bit wander. It should be easier to bite in the go sideways. Are you sure the Z isn't tilting back from the down-pressure?

Hmm, I wonder... If Artcam doesn't have drills, maybe its trying to pocket anyway with a built-in minimum helix diameter? See the other steppers moving at all? Shot in the dark heh.

[Cartierusm]

No nothing is moving except the bit. I was 5" away from it with good light. I wonder if I could be feeding too slow; allowing it to wander? I wonder if I feed faster if it would just bite into the aluminum? I'll try that tomorrow.

[Cartierusm]

Well the saga continues. I want to drill holes and not pocket them as I'm not sure the Z axis is rigid enough, hence the drilling of holes to make a new Z axis.

I ended up returning the air drill I bought because it blew out my compressor; a very big and very powerful 80 gallon compressor which I now have to figure out why it won't run. Luckily I was able to find a cheap $60 black and deckker hammer drill with a uniform collar I can bold up to a new jig attachment I made and will resume drilling operations as soon as I can align the new drill properly.

I was able to drill without all the wandering yesterday. What I did was go back to my machine tool distributor and bought stubby split point drills. They are short drill usually associated with screw press operations for less flex and they are split point which the catalog describes them as self centering for less wandering. Sounds like a movie title, "self centering for less wandering" ...coming soon to theaters everywhere.

Anyway, gettting closer. I guess I should have converted my Bridgeport first instead of after, oh well. I would just do that but I need the new ballscrews for it and they are $800+. But I do have to say with all my analness the spacing and accuracy of the holes are very good.