engraving

[rgollar]

I was wondering what people used to engrave part numbers there parts. We usually use center drills. Plus how fast and deep are you going for steel and alumimum? I have tried ingraving bits but they tend to chip the tips. Just wondering how others are doing it. I got to believe there is a better way than a center drill. Thanks

[uncle_dolan]

I was wondering what people used to engrave part numbers there parts. We usually use center drills. Plus how fast and deep are you going for steel and alumimum? I have tried ingraving bits but they tend to chip the tips. Just wondering how others are doing it. I got to believe there is a better way than a center drill. Thanks

Depending on the requirements of the engraving a 2mm dia ballnose cutter works very well and looks nice. Not so good if engraved lines need to be paint filled.

 

Brendan

[darko herak]

Sure it is important to see the spcification requirements, if you just engrave numbers as such good tool for that is 60 degree

tool with small r on tip e.g. 0.3 (metric values).

[rgollar]

Thank you for the suggestion.

[jeff]

I use a 1/16" ballnose 10000 rpm, .01 IPM .004-.005 deep

[Odin]

I use GARR Mold Cutters. 1/32" ball mill at 15000 rpm, .002-.003" DOC and at about 10"-15" IPM, Or a 1/16" ball mill at 14000 rpm. .005" DOC and at 15"-20" IPM. Those work really well and last quite some time.

[spade117]

I've used all of the above, and unless it's customer specific, I've had a lot of success with a centerdrill.

[Mic6]

Yea, well I usually run a .002 bem at 1,000,000 rpm, 5k ipm

[bal]

We use a tipped of scribe from Harvey Tool 12000rpm @ 5ipm

[K2csq7]

Yea, well I usually run a .002 bem at 1,000,000 rpm, 5k ipm

:lol:

I use broken carbide tools, no really, I grind 3 faces at about a 45 deg angle so the point looks like a pyramid, 10 IPM 3K rpm take a few passes to get to 0.010 deep then a spring pass will get rid of the burr, They look great and paint fills in nice...

I have tried ingraving bits but they tend to chip the tips.

Set your clearance to .030 above the part and plunge rate of 0.1IPM should keep the tip from chipping.

[McLaren]

1/32", 3/64", or 1/16" 4fl. ball endmill

10k, 30ipm, ~.005" deep, 6º plunge angle.

[rgollar]

Thanks for all the suggestion. Mclaren that engraving looks very nice.

[robk]

Harvey has a nice selection of engraving cutters.

[Tinhman]

How about this "Spring Loaded Engraving Tool"?

 

link: http://www.2linc.com/engraving.htm

[overthecrossbar]

I use 1/8" 2 flute chamfer mills