Driiling .020 holes in .05" thick brass .. Plunge/ Feed and RPM Help!!

I need help from some experienced cnc'rs...I am drilling 61 holes that are .020" OD into .05" thick brass. I put my spindle rpm to about 3000 and doing .4" Plunge rate into .05" thick brass. I am using my cnc mill but I notice my drill bits keep breaking.

I did notice that when I blew the brass chips off that it seemed to stop the breaking. Could brass swarf , even small as .020 drilling into .5" thick brass, at a .4" plunge rate, cause the drill bits to get stuck and break? Or is there a better Plunge rate and RPM that I should be using? Also, should I spot drill the 61 holes first?

I am new to this , so I am thinking maybe I should be having to blow air to clear the small brass swarf while drilling? Any help please as I need to make quantity pieces doing this 61 hole drill set up. Thank you for any information/help and your time doing so!

What is your maximum RPM on your machine? You should be at max for a drill that small.

Are you spot drilling first? What drill are you using?

Give us more info and we can help.

Your photo is some funny looking brass.

mpix00 said:

Also, should I spot drill the 61 holes first?

Click to expand...

Yes, this. A .02" drill has little chance of running on-point without a spot to get it started.

Wait, .05" deep,. or .5" deep? You say both. If .5" deep, then you are at 10xD and most definitely need to spot first as you will be having to use a snaky 10xD drill.

Also, if .5" deep, are you pecking? Probably have to .

What do you mean by ".4" plunge rate"? 0.4 IPM? At 3000 RPM I make that to be .00013" per rev, which is pretty dainty.

Regards.

Mike

Finegrain said:

Yes, this. A .02" drill has little chance of running on-point without a spot to get it started.

Wait, .05" deep,. or .5" deep? You say both. If .5" deep, then you are at 10xD and most definitely need to spot first as you will be having to use a snaky 10xD drill.

Also, if .5" deep, are you pecking? Probably have to .

What do you mean by ".4" plunge rate"? 0.4 IPM? At 3000 RPM I make that to be .00013" per rev, which is pretty dainty.

Regards.

Mike

Click to expand...

+1 on that and check how true the drill is running, ....for spotting holes that small I don't use a drill, just a pointed piece if HSS ground to the same angle as the drill, ..a small true ''divot'' is all you need.

P.S. your surface finish on that brass isn't helping you one little bit - far too rough and will cause any tiny drill to wander. .....if you need a rough surface m/c a smooth one, drill, the re machine to rough after drilling.

Yes Mike, I meant .05" deep and I am running my mill at 3000 rpm. Yes, .4 IPM.... When I spot drill, about how deep should I spot drill, and at 3000 rpm, what would be an ideal IPM?

Thanks for the tip on the spot drill. I have a 60 degree angled tip for engraving I am going to use. Thank you about the finish. I faced it by hand , so I will use my cnc motors to finish it for a better finish. I just need to figure out the best rpm and PIN rate now. I'm currently at 3000 rpns with .4 IPM which someone said is to dainty, so I just Ned to figure that value out. Any suggestion? Thank you for your time and help

No I did not spot drill, but i will do so. I changed the picture color of the brass to try and get a better view of the holes. My drill bits are carbide . I have a cnc hf x2 mini mill with belt upgrade. It goes very fast. Should i turn it to as fast as it will go?

I would not use a 60º spot drill (or engraving tool) for a spot, but if that's what it is and you are going to do anyway, spot the absolute minimum for a .02" diameter spot you would drill .0209" deep with 60º cutter, I would go half that. The alternative is using a spot drill that is very close to the same angle as the drill you are using and still spot very shallow.

Use all the RPM that machine has...I wouldn't worry too much about the feed rate unless you are going into production, it isn't like you are going to harden the material.

The brass in the picture looks suspect are you sure it is yellow brass?

R

I am going into production, so what should the IPM be or how fast should the drill plunge Into the brass when drilling? Thank you for your help and advice.

Were talking Harbor Freight equipment here never mind.

This little cnc HF can handle this job no problem as long as I can get the right info. Looks like I had a few issues.

1:the brass finish needs to be better
2: spot drill needed
3: HSS Steel Bits needed as I was using carbide. I just purchased the HSS Steel Bits.. Thank you for the much needed info TOOLROOMGUY!
4: I need Air to blow out swarf
5: I need faster RPMS

This should be good to get everything down. Thank you for the helpful information and time to help out everyone!

You need on more thing. You should find a piece of drill rod that is not too much bigger than you drill diameter and make a point on this rod larger than the drill bit point angle (118* or 135* so 120 and 140, or if you can be precise, then match the angle). Then grind half of the diameter of the drill rod off to create a spade point (just like and engraving tool). If you had an engraving bit with a larger angle then this would be perfect and you could avoid making your own.
tom's techniques drilling brass - YouTube
Center- and spotting drills - YouTube

.020" hole in brass .050" deep shouldn't be too bad. I drill mountains of .010" holes in harder material, much deeper all the time.

Find the right drill. Do not get a flute length any longer than you need to make the hole.

Spot drilling is important. I have used an .03125 ball end mill, .004 deep gives a .005" edge break on the hole.

Check the runout on your drill. You are running a mill with a potentially bad spindle with poor tool holding. This will make it tough. You will need the correct size collet for this operation. The small drills usually have metric size shanks. Also explore the small circuit board drills. They have a 1/8" shank and are cheap. A Jacobs chuck won't do it.

I usually run my .010" drills at 6,000 RPMs, .5 Inches Per Minute, with a .005" peck. This is not optimized for production, but it has not failed me in a lot of holes, and when I break a drill it is the last op on a 10 hour injection mold half so I'm a bit cautious.

You need something the clear the chips and add a bit of lubrication to clear the chip. I use flood coolant, but I would be willing to gamble on a spray mist system if I was running an open mill without flood.