Cutting Brass Sheet

[CNYDWW]

.060 half hard brass sheet, polished one side. Cut face down with vacuum and widgetworks pressure foot. Bit is onsrud .125 dia x 1/4" zero flute. I can't remember the number off the top of my head. It is actually an acrylic/plastic bit rather then for non ferrous metals. I have been cutting brass for a little more then six months on and off. This bit performs better. Less heat, better finish and longer life then the "proper" bit. This includes a less aggressive angle grind on the tip compared to the non ferrous metal bit. Bit is zeroed to the top of material with a cut depth of .125". This allows for the center of the bit to be used rather then the tip. Allows for cooler running bit cutting at a stronger point of the cut length. Plunge rate is 30 IPM, Feed rate is 100 IPM.

http://youtu.be/LCuO7UieZf4

[tom_fiddler]

WOW I would have thought that would have broke.
What RPM?
Looks great
Thanks

[scottp55]

Randy, searching for that bit. Was it a straight or upcut? Wondering if it was 61-040 that came with Desktop starter set(that little bit does LOTS of stuff its not supposed to). Hopefully cutting branding iron soon, be nice if it was.

[CNYDWW]

Randy, searching for that bit. Was it a straight or upcut? Wondering if it was 61-040 that came with Desktop starter set(that little bit does LOTS of stuff its not supposed to). Hopefully cutting branding iron soon, be nice if it was.

The bit is an upcut 0flute. I've tracked down the number, Onsrud 63-510 1/8 dia 1/4" length of cut and 2" overall length. As i said, it's meant for acrylic. It also has a less aggressive shear angle on the tip for plunge cutting and less "ribs" on the outside of the spiral compared to the bits meant for brass and aluminum. As i mentioned, it lasts longer and has less breakage. I can cut two-three sheets of smaller parts then shown in the video ( 36x96 sheets) with more detail then this project on the same bit. Considering Grainger sells them for $45 each, it's not bad at all for costs. This also cuts down on the hand work due to the smaller radius in the corners. Everything needs to be square at the corners for the bending break to do it's job properly.

[scottp55]

Thanks Randy.

[CNYDWW]

Thanks Randy.

No problem, glad to share.

[CNYDWW]

WOW I would have thought that would have broke.
What RPM?
Looks great
Thanks

The spindle is set to Mhz. I had a base line of 4500 Rpm @ 300 Mhz and 1500 Rpm @ 100 Mhz approx. It cut best at 186Mhz on the spindle control. The overall trick to cutting with such a small dia bit is plunging down half the depth of the length of cut. The bit has a 1/4" length of cut and I was cutting a single pass depth of 1/8" from the surface of the material. I had large chips that evacuated the heat. One issue i had was the chip build up on the pressure foot. It was melting the plastic unless it was cleared properly with the air.