Hey all, Ive been trying to engrave some text, and while its coming out OK, its not perfect. the problem is that the edges of the letters and paths have a burl or flash on them, raised above the surface. Like my tool isn't fully cutting the material, its half cutting then pushing it up out of the way.

I need .125 high letters, I tried .oo5 depth (not too good) and .007 depth (better, atl east I was able to use my fingernail and scrape the flash off here)

Im using a carbide 60degree 2 flute v bit, .0625 diameter, .005 flat, from precisebits.com. I run .003 depth per pass at 15 IPM, around 27k rpm. Maybe 5 thou per pass instead of 3?

any tips with rotary engraving of alum? which bits have worked best for you?

thanks for any insight and experienced tips!!

~Steve

Steve,
I have been using a small die grinder running at +/-50K with a 1/8" carbide "slotting drill" 90° and getting acceptable results. Because the pencil grinder doesn't have much power, I have been running about 3IPM and .002 depth in aluminum. worked great until the other day when I "think" a piece of rust or something got into it from the air line. Stalled out and now have to tear it apart to see what went wrong:{(

I have been cutting to .011" deep in 6061 and in steel, cut the paramaters to .001" deep and 1 or 2 IPM

also, use flood coolant!

Tried not using coolant and ran into all kinds of problems.

hmmmm thanks for your insight there Bubba. Im going to experiment around a bit more with depths of cut and speeds feeds, and see how it goes.
Id like to use coolant but I don't even want to think of the mess!

keep it comin anyone

thanks
~Steve

Have you tried Melin Conical Blanks. They are Carbide and come in sizes from 1/8 to 1/2 diameters. It is a single flute though. The tips vary from .005 to .02 and they also have 30, 60 and 90 degree included angles.

I use these a lot for engraving plastics, and aluminums.

http://www.endmill.com/pages/catalogs/2005/pdf/038.pdf

I use a 1/8 carbide ball endmill,5000 rpm,.005 depth,works fine.

i use a 1mm carbide ball nose running mid speed in a dremel .1mm depth wd 40 for coolant ,also works fine

I used to have similar issues with standard conical cutters until I began grinding them to have a positive face. This requires that the face is ground back past the normal point (which is on center). This makes for a somewhat frail cutter but the results are worth it - it drastically improves the cut quality. Grinding behind center also prohibits you from achieving a infinately small valley as the point becomes essentially a micro fly cutter so if that's really a concern then this method is not for you.

It also helps to spin these at rediculous speeds - I am fortunate enough to have access to a 50,000 RPM spindle. With said spindle, my cutting rates are still only between 10-12IPM with a .010" depth, but I get very little burr. Using a die grinder is another viable method for getting some pretty good speeds - I believe you can get pancil grinders that spin over 100K RPM (turbine type) but they might be a bit pricey.....

Someone out there has got to offer a conical cutter with positive rake, but I haven't looked. The neutral (standard) is just not adequate for aluminum in my opinion.

Scott

I had the best luck with engraving SS when my single point carbide 60* tool chipped. I was irritated so I just raised the table a couple of thou and let it go, worked great, 20ipm, .003 per pass, 2 passes. I reccomend using carbide ballmills.
Michael

Are you doing a finish cut?

I was having similar problems and did a final light pass with tool compensation on and told the CAM program that the tool was slightly smaller diameter than the roughing passes so that it "pushed" the tool over a bit further.