Aluminum Hole Drilling

[piperpilot]

I've done a search and can't seem to find the info. I'm sure this has been asked before, but I wanted to throw it out there again in its own thread.

I have the need to drill some holes in aluminum. This will be a repetitive task drilling mounting holes in an enclosure and I will do it 100s of times. I have my drill press and could do it the old fashioned way, but was hoping to use my CNC for the job. So my question is this:

1. If I use a speed controller to reduce the router RPM to say 5000-7000 RPM or so, is there a way to use a standard drill bit? These are relatively small holes for #6 or #8 size screws.

2. If I can't use a standard drill bit, I'm guessing an end mill is the best tool for the job? Do end mills come in the differnt sizes? The spec for a #6 screw says the drill bit size is a 31 and the hole diameter is 0.120".

3. I'll be using vCarve Pro and Mach3 to do the drilling, I assume they handle the drilling profile properly to make sure chips get cleared, etc?

Thanks for the help!

PiperPilot

[Mr H]

I also have a question about working with aluminum, I see a variety of endmills, 1-2-4-flute etc and also upward or downward. Can someone give me some advice on what type of mills to use. Most of what I'll be doing is .063 to .125 alum. I will be doing some thicker 3/8" stuff in the future. I to have a particular project that requires lots of holes and would be interested in the drilling aspects of it. Any info would be appreciated. (I have a Precix 4x8 industrial router with Perske power head, no tool changer)


Thx

Mark

[Diverdude]

Mr. H, I have seen a guys set up that he was milling aluminium with his cnc router, He was using a Belin single flute bit and using a Kool Mist system to lubricate it. I have ordered the same set up just haven't recieved the bit yet so I can't say how it works first hand.

[jsheerin]

I've drilled mdf and plywood with a 1/4" drill in my router. It burns the holes but works okay. I use a screw machine drill which is shorter. Personally I would not try aluminum. You could pocket the holes, but that's a pretty small hole to pocket...

As far as clearing chips / software, Mach only does what you tell it to via your g-code. V-carve may or may not have various drilling programs (pecking, etc.), but I doubt it has anything to calculate appropriate speeds and feeds for various materials. So no, you have to know what to tell it to do. You can find recommendations for surface speed and the equations to convert that to rpm on the web or in Machinery's Handbook.

[DonFrambach]

I've done a search and can't seem to find the info. I'm sure this has been asked before, but I wanted to throw it out there again in its own thread.

I have the need to drill some holes in aluminum. This will be a repetitive task drilling mounting holes in an enclosure and I will do it 100s of times. I have my drill press and could do it the old fashioned way, but was hoping to use my CNC for the job. So my question is this:

1. If I use a speed controller to reduce the router RPM to say 5000-7000 RPM or so, is there a way to use a standard drill bit? These are relatively small holes for #6 or #8 size screws.

2. If I can't use a standard drill bit, I'm guessing an end mill is the best tool for the job? Do end mills come in the differnt sizes? The spec for a #6 screw says the drill bit size is a 31 and the hole diameter is 0.120".

3. I'll be using vCarve Pro and Mach3 to do the drilling, I assume they handle the drilling profile properly to make sure chips get cleared, etc?

Thanks for the help!

PiperPilot

I think you'll have difficulty using a standard drill bit at 5k rpm. I have used a Taig spindle at 1k rpm and sucessfully drilled 1/4" holes up to 1" deep in 6061 aluminum but it is a pain. What I try to do now is use my CNC to mark out the holes with a "center and coutersink" drill (also at 1k rpm) and finish drilling the hole with my drill press. If I need a large hole, I mark it with my CNC, drill it to 1/4" or so with my drill press and then enlarge it to whatever I need with my CNC. Here's a link for the "center and countersink" drills I use: Enco - Guaranteed Lowest Prices on Machinery, Measuring Tools, Cutting Tools and Shop Supplies

If you need to precisely locate a number of holes, I suggest you try to mark the holes with your CNC (at the slowest possible speed) and then drill the holes with your drill press.

[piperpilot]

Thanks guys for the suggestions. I only need to go 0.18" deep so will probably go with a 0.120" end mill. I did a quick search and found a few options. Hopefully it will work out. I won't need to do any tapping as I'll use thread cutting screws for these holes...its basically just for circuit board and mosfet mounting to the heat sink top of an extruded enclosure.

I'll post more to this thread as I test it out!

Thanks again!

PiperPilot

[louieatienza]

You should easily be able to peck-drill with an endmill; or you can use a drill-mill if they have one the size you need.

I started a thread on different bits and endmills and their uses with information on speeds and feeds as well.

http://www.cnczone.com/forums/diy-cn...criptions.html

I made a carriage plate for my new router build, where I had to drill 32 holes for the profile rails, 2 sets of 8 per rail, and needed to get at least .005" tolerance spacing on center. I used a .125" endmill at my slowerst speed , 5krpm, and peck-drilled through 5/8" aluminum. These holes were accurate enough, that when I screwed up on a couple threads, I flipped the plate over and the holes still lined up!

[Mr H]

Thanks guys for the info, I'm running bobcad so I have a canned peck drilling cycle that I can use. Piperpilot, let me know how that cutter works for you.

Thx

Mark

[CarveOne]

If you use an end mill, make sure it is a center cutting type that cuts while going straight down. The end cutting edges go to the center of the cutter. A non center cutting end mill has a "hole" in the middle that does no cutting. These are ok for spiraling into a larger hole than the end mill.

If using a drill, use a 135 degree split point drill for the same reason. A standard drill's center web does as much rubbing as cutting.

[adprinter]

I haven't tried aluminum drilling yet, but this is the work-around I use for drilling holes.
I use Corel Draw for artwork creation, and when the need arises for drilling holes - what I do in CD is draw circles at the desired hole locations in the drawing. And then alter their diameters to be 0.001" (effectively resulting in points in the drawing). Then export the file as a HPGL.PLT file to preserve the proper scaling.
I then use LazyCAM to import the Vector file (*.PLT) into LazyCAM. For the drill tool, I specify a "depth per pass" of say 0.008". And post to Mach3. This results in a "peck drilling" G code, which cuts circles with a 0.001" diameter. An end mill with a diameter which is slightly smaller than the desired hole diameter is used as the actual cutter.
And since the depth per pass is set so shallow, it results in a "simulated" peck drilling cycle. Since it retracts the tool between each pass, this extracts the chips from the hole. The result is nice clean, round holes in the wood materials I work with.
As I said, I haven't tried to do this in aluminum yet. But I see no reason the same method wouldn't work for any material. For the small diameter holes you are describing, I would set the depth per pass in LazyCAM to be very shallow- maybe 0.003" per pass to prevent bit breakage. And the feed rate very slow- maybe 10 IPM. Hope this helps!

[brucer]

use a carbide drill and compressed air..

[BLAMOUR]

If you go with an end mill, make sure it has chamfered or radiused corners. Much stronger for drilling. Hanita makes a good one.