[cp8071]

What type bits should I be using for routing out Printed Circuit Boards? Currently I'm using an Engraving Spindle which uses 1/8" cutters. I've tried 0.005" and 0.010" bits and both have broken while cutting boards. These types of cutters have an angle to them (not like end mills) so setting the depth and width can also be difficult. I guess they are really only designed for cutting plastic, but I though that being carbide would be good enough for cutting copper/fiberglass.

What are you using?

CP

[alphatroniqu]

hi

check http://www.precisecut.com it have low cost pcb router bit ..

im use it every day and work verry nice

it also have pcb milling bit to

http://www.precisecut.com/products/f...I1.x=13&I1.y=8

[Jwallis]

Hello,

I use second hand dental burrs... They work really well and are plentiful at the local dentist. I have found that the trick is to plunge through the copper layer at a reasonable rate before giving any sideways motion. When I first started routing PCB's I had the bit skimming the copper and they broke without fail. Now that I plunge through the copper there is no problem. The most common bits I use are 0.6mm diameter and 0.8mm diameter and they work perfectly.

Hope you find some that work for you.

Regards,

Jayson
(Horsham, Australia)

[abasir]

Also make sure the spindle is running at high speed. Professional system runs in 20,000 rpm range.

[alphatroniqu]

hi

20,000 rpm is near of the minimum

on my system it set for 30,000 rpm

tool[14].name=Contour Router 2.0 mm (79 mil)
opt_rotation_speed=30000
opt_milling_speed=3 (one ink per 3 segond)

most of pcb shop run faster that this ...

for trace milling "Universal Cutter 0.2 mm"
opt_rotation_speed=40000
opt_milling_speed=0 (one ink per segond)

Ther tool data come from my Protomat C60 PCB milling

Marc Lalonde
Alphatronique

[lwhodson]

For routing out PCB's the best tool to use is either a Chipbreaker or Diamond Cut style carbide router bit. Pictures of either style can be found here: PCB Routers & PCB Router Bits - MCT
Don't use a fluted tool such as an end mill as they will burn up quickly and leave a poor finish. In practice the diamond style is used industry wide by a factor of 100 to 1 over the chipbreaker style.

For speeds and feeds if you have a machine capable of it you'd want to run your spindle up to 36,000 RPM for a 1/16" (1.60mm) bit and feedrate of 40 to 50 inches per minute. A 3/32" (2.40mm) bit should turn about 30,000 RPM and a feedrate of 45 to 60 IPM. If your spindle doesn't operate that high just run it at 90% of maximum RPM and a .0015" Chip-load. In other words if you are turning 12,000 RPM feed at 18 IPM for a starting point. Vary you feedrate up or down to achieve a good finish and tolerance. Don't run too slow a feedrate or you will heat the bit up causing a shorter tool life. Use a vacuum source to remove chips rather than compressed air. The fiberglass chips can cause skin irritation as well as mess up your equipment.

Try to stay away from small diameter router bits as obviously they break a lot easier. Your best bet is to use a "Fishtail" over a "Drill-point" end style. It will leave a square bottom vacuum path and if for some reason you don't penetrate thru the work piece quite enough it will allow you a second chance to cut the part. Drill-point end style bits also need to penetrate deeper, especially 1/8" and larger bits.

Hope this helps
[email protected]
PCB Cutting & Etching Tools - MCT

[CitizenOfDreams]

I think the original post, 8 years ago, was about routing traces on the circuit board. My personal favorite bit for that is a 30-degree V-cutter:

[smarbaga]

check this out
https://www.youtube.com/watch?v=7EctuSTL7-w

[joeavaerage]

Hi,
I use both angled engraving bits for normal 1oz copper board but also use very small diameter endmills with thick copper board.

While it is tempting to use narrow angle (10⁰, 15⁰, 20⁰) engraving bits because the cut is that much straighter
and therefore the width of cut less dependent on the depth they are too tender and break too easily. I personally find that 30⁰ is a good compromise
but notice that many others use 45⁰ with good results. It is also tempting to use 0.1mm and 0.2mm tipped engraving bits but they are
tender and break. If you need really fine traces then you have to use these tender tools but if you don't have to....then do yourself a favor and use tools with
a larger tip.

I have some very specialized PCB with 12oz (420um) thick copper for high current boards. Because the depth of cut is required to be so deep
an angled cut would badly compromise the width of the trace. I elected to use small diameter (0.5mm) endmills. I found it necessary to
use Autoleveller, a software utility that probes the PCB blank and make small adjustments to the Z depth Gcode commands to accommodate
any bow/warp in the PCB or unevenness of the spoil board. I found it important to avoid any excess cutting of the underlying fiberglass in order
to maximize tool life. I found also that tool life could be extended by many hours by using flood cooling, ostensibly to rinse away the chips. These two
techniques allow me to get about 6 to 8 hours cutting per tool. I was able to buy these tools (on special) for $2.65US each, I bought 30. Wish I'd bought
more now! They are good tools made by Kyocera Tycom and are marketed to PCB makers.

The quality of the cut (lack of burrs) is so good that I now use endmills for ordinary 1oz board as well.

https://www.ebay.com/itm/5-0-50mm-01...cAAOxy1VlRFPam

Autoleveller – CNC Millings, Levelled

Craig

[reg.miller]

check this out
https://www.youtube.com/watch?v=7EctuSTL7-w

Wow, that is pure magic to watch. Thanks, If I can cut half a good as that I'll be happy.