Re: [CAD_CAM_EDM_DRO] using a CNC mill to engrave metal

Hi David:
For the most part, the CNC milling approach to engraving will work, but
the Sherline doesn't have the spindle speed for tiny cutters.
Most engravers run at upwards of 25000 RPM.
Forget about trying to engrave letters 0.050" high in steel with a single
lip cutter; you'll be breaking cutters continuously.
If you confine your efforts to brass, Delrin or a hard grade of aluminum,
and if you don't push the cutter, you should be able to do creditable work.
As the letter size gets bigger, you will have better success (up to a limit
of course) because you will be able to use a larger cutter without obscuring
the shape of the letters.
A reasonable minimum would probably be around 0.100" tall letters cut with a
0.015" dia, 10 deg single lip carbide cutter.
Typically, you would engrave these letters 0.006" to 0.009" deep, in several
passes.
Keep your depth of cut below 0.0015", keep your feedrate below 5" per
minute, and you should be OK in brass.
Watch for plunges in your toolpaths; these will almost always murder your
cutter.
Ideally, you need to ramp in to your depth of cut; a 2 deg ramp over 1.5
times the cutter diameter is a good starting point; you can experiment as
you gain experience.
Obviously, with such a tiny depth of cut, you need to have a very flat
surface before you start; if the surface is only 0.003" out of parallel, you
could be doubling your depth of cut in places and just kissing the part in
others.
Best bet is to mill over the surface to be engraved just before you start ;
that way you know it is flat.
Seems complicated, I know; but it's really not too bad once you are actually
cutting.
Good luck with it!
Cheers

Marcus
-----Original Message-----
From: david albert <dalbert@...>
To: CAD_CAM_EDM_DRO@yahoogroups.com <CAD_CAM_EDM_DRO@yahoogroups.com>
Date: Monday, August 13, 2001 12:47 PM
Subject: [CAD_CAM_EDM_DRO] using a CNC mill to engrave metal

>I was wondering if anyone has any experience using a sherline mill
>with a CNC package as an engraver. Ideally, I would like to be able
>to type some text on a keyboard and have the mill enrave some metal
>down a few thousandths with what I typed. What end mill should I
>use? What CNC software? Any web site you could point me to? thanks
>in advance.
>
>
>Addresses:
>FAQ: http://www.ktmarketing.com/faq.html
>FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
>
>Post messages: CAD_CAM_EDM_DRO@yahoogroups.com
>Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
>Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
>List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@...
>Moderator: jmelson@... timg@... [Moderator]
>URL to this page: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
>bill,
>List Manager
>
>
>
>Your use of Yahoo! Groups is subject to http://docs.yahoo.com/info/terms/
>