PDA

View Full Version : How to drill faster in brass



Boyan Silyavski
19-07-2016, 11:39 AM
Hi,
have to drill a lot of holes in brass, on the CNC i mean. 3mm as i thread them later to M4. Something similar to grounding bars , where each piece has 15 M4+15 3mm pass trough holes.

Till now i was drilling them using 3mm mill and 16000rpm feed rate like 15ipm and some pech tool path for the sticky chips to go out, which is leftover from the time when i did not use brass bar but very gummy aluminum bars. But now i have 500x30=15000 holes to make so have to speed up quite a bit.

Any ideas? if i remove the peck drilling path things will be speeded, but is it needed for brass ? 8mm square brass bar. Normally i use 2 flute spiral 30 degree fishtail 3mm bit. Problem is i am busy with other work so no time for experiments.


18888

magicniner
19-07-2016, 11:54 AM
Brass chips very nicely, you may find you don't get any issues but if you use very localised air you can shift enough chips for holes that depth, I use clip-together coolant pipe with a medical canula needle bonded into the nozzle from the inside,
Regards,
Nick

Clive S
19-07-2016, 12:53 PM
Boyan Would a 3.3mm drill be better than a 3mm in Brass?

Boyan Silyavski
19-07-2016, 01:56 PM
Brass chips very nicely, you may find you don't get any issues but if you use very localised air you can shift enough chips for holes that depth, I use clip-together coolant pipe with a medical canula needle bonded into the nozzle from the inside,
Regards,
Nick

So you are saying to try 24000 rpm, no peck drilling, blow air and try how fast things could go with that carbide cutter i have?


Boyan Would a 3.3mm drill be better than a 3mm in Brass?

yes, actually i am using 1/8 . was using 3mm on my old flimsy machine cause due to vibrations it was making a 1/8 hole :-)

Anyways i use a spiral pointed machine tap which further drill opens the hole if necessary.

Boyan Silyavski
19-07-2016, 02:00 PM
Or would using a drill will be faster? Instead of a milling cutter?

Lee Roberts
19-07-2016, 02:43 PM
Or would using a drill will be faster? Instead of a milling cutter?
I would have thought so, the right tool for the job and all that?

Milling cutters are for cutting sideways no?

.Me

ptjw7uk
19-07-2016, 11:42 PM
You should also check the drills geometry as a normal drill used on brass can break as it will pull into the hole, possibly not that relevant on a cnc machine as the drill will be restrained by the z axis.
Normally if you drill a lot of brass you can remove the cutting edge with a 'stone'.

Peter

Boyan Silyavski
20-07-2016, 12:21 AM
I had a talk with the HSMadvisor maker, so it seems i had that functionality but did not know how to find it.

So according to the calculator it seems drill / HSS/ or mill/carbide/ is almost the same feed rate. But if drill is cobalt or carbide then 1.5x faster. 1000mm/min and 1500mm /min respectively.

I use the general option " Other non ferrous alloys" in stead of "low lead brass " or similar as the latest give me too slow feed , slower than aluminum. So it seems my brass is different, as i know for a fact that it machines and drills much faster than aluminum.

Will experiment tomorrow to see how fast it could go in real life and report back.

189071890818909

magicniner
20-07-2016, 11:43 AM
Boyan,
I'd definitely use a drill bit, not a milling cutter,
Regards,
Nick

sinnsvak
20-07-2016, 09:44 PM
And pecking could be reduced to short-stops to just break the chips.

Boyan Silyavski
21-07-2016, 08:52 AM
Boyan,
I'd definitely use a drill bit, not a milling cutter,
Regards,
Nick

I will buy, but unfortunately have to order from the net and wait for them, as i live in a very small tourist town . So from calcs it seems carbide drills would be best. Even faster with parabolic ones, whatever that is.


And pecking could be reduced to short-stops to just break the chips.

I was thinking something similar. Though at the end decided to use no peching following the HSMAdvisor prescription, see snip above where says " pecking not necessary.



So instead of wasting more time thinking, today i tested the HSMAdvisor suggestions. 18000rpm, 3mm 2 flute carbide end mill, ~40IPM or 1000mm/min. I started reducing to 30% the feed to see what happens, then raised slowly to 70 , then 100%.




Hat down to the HSMAdviser. Drilled like cheese. At the suggested speeds and feeds all noise disappeared. You could see from video how smoothly all went. I think for DIY machine to drill 15 holes 9 mm deep in metal for <20 seconds all, is a quite an achievement. At least in my world.


I would use the chance to recommend again HSMAdviser. The support is great. I have the 3 year subscription. The guy updates the program constantly and every 2 updates or so resets the trial counter, so it could be used almost on trial. Plus i see now that he decided to let you have full functionality once a subscription expires :beer:. With some HP restriction. I am not affiliated in any way, just think that its a great tool worth the money.




https://www.youtube.com/watch?v=4SEQIuS0Rq4

Clive S
21-07-2016, 10:04 AM
Boyan Very nice. Does the brass bar bend at the ends as you are drilling? On the last hole! as that could snap the bit.

Boyan Silyavski
21-07-2016, 10:52 AM
Boyan Very nice. Does the brass bar bend at the ends as you are drilling? On the last hole! as that could snap the bit.

You have really sharp eyes Clive! i see what you meant. In reality - i don't think its a problem. I believe that was some artefact from the video. If you note at the beginning it does not happen, having in mind the distance is the same both sides.

By the way i just realised that HSMAdvisor did recommend peck drilling, i just have missed before to fill how deep my hole is. Fortunately this brass is a very nice material to work with, that's why on first place i abandoned aluminum for the bridge of the instrument i make.

18915