[nodott]

So recently I watched the video with NYC CNC where he used a 3/64 Ball EM for engraving on an AR15 lower. I like the outcome and so I ordered some of these EM's for myself. However there is no information on the LSC website that would help in determining proper feed and speeds for such small EM's.

Does anyone have such information that would be helpful?

[Lasher]

I know it's not the same but maybe it will help. I use 1/16 ball for engraving and i run it at 5100rpm, 7ipm plunge and 10ipm feed at .005 - .008" depth depending on what it is. So if I were to do it and i'm not saying it's correct, I would run it at 5ipm feed and work my way up to 7 to 10.

[Steve Seebold]

I engraved a plaque about 5 years ago. I made the plaque out of a piece of 1/8 X4X8 inch brass. I did it with a .010 end mill and I engraved the plaque .03 deep.

I took it down at .0025 per pass at about 10 IPM AND 5000 RPM. the whole project took about 12 hours but it was for my mother in law when had passed away. It was a way for me to honor her.

[Tbkahuna]

I use short 1/16" and 1/32" ball end mills for engraving. My best results and most common practice is to use those small end mills in my Kress add-on spindle (I have a Series 2 1100 upgraded to Series 3) at 25,000 rpm. The faster the better. I use WD-40 for keeping the tiny chips out of the cutters way and to lube it. The results are very good. I typically adjust the depth from about .003" - .005" to as much as I need to get the line width I like which might be .030 or .040" deep for larger letters. The feed rate depends on how deep you cut.

Those little end mills work great and last a lot longer than I would have guessed as long as you don't push too hard. From my experience, the biggest issue is with the plunge feed rate. I dial the plunge feed rate down to around 10% to 50% of the cut feed rate. I might start at like a 6 ipm engraving feed rate with a 2 ipm plunge.

I occasionally use the 1100 spindle and run it at 5000 rpm and start at about 3 or 4 ipm and adjust it to what looks the best. The WD40 really helps.

[joshetect]

I have found Kyocera endmills hold up better than the LSC ones. I do really like LSC's 20* .02 dia ball endmill for text and other stuff. PIC

I engrave in aluminum 5ipm @ 5100 RPM and a 2ipm plunge and 1 pass at .018 deep. you could probably push harder, but it just hurts the wallet too much to break them.

In steel same speeds, but .009 depth so 2 passes.

All with flood coolant. You also need to try your best to get as little runout as possible when going this small.

[cmparts]

#1 c'drill - 3200 rpm - F1. down - F4. cut - Tormach 770
Cheers

[nodott]

#1 c'drill - 3200 rpm - F1. down - F4. cut - Tormach 770
Cheers

Very impressive. I have heard of using center drills for engraving and have acquired a few myself but have not tested them yet.

[nodott]

I have found Kyocera endmills hold up better than the LSC ones. I do really like LSC's 20* .02 dia ball endmill for text and other stuff. PIC

I engrave in aluminum 5ipm @ 5100 RPM and a 2ipm plunge and 1 pass at .018 deep. you could probably push harder, but it just hurts the wallet too much to break them.

In steel same speeds, but .009 depth so 2 passes.

All with flood coolant. You also need to try your best to get as little runout as possible when going this small.

As well I am impressed by the quality of the engraving. thanks for the feed and speeds. I will give them a try.

[nodott]

I use short 1/16" and 1/32" ball end mills for engraving. My best results and most common practice is to use those small end mills in my Kress add-on spindle (I have a Series 2 1100 upgraded to Series 3) at 25,000 rpm. The faster the better. I use WD-40 for keeping the tiny chips out of the cutters way and to lube it. The results are very good. I typically adjust the depth from about .003" - .005" to as much as I need to get the line width I like which might be .030 or .040" deep for larger letters. The feed rate depends on how deep you cut.

Those little end mills work great and last a lot longer than I would have guessed as long as you don't push too hard. From my experience, the biggest issue is with the plunge feed rate. I dial the plunge feed rate down to around 10% to 50% of the cut feed rate. I might start at like a 6 ipm engraving feed rate with a 2 ipm plunge.

I occasionally use the 1100 spindle and run it at 5000 rpm and start at about 3 or 4 ipm and adjust it to what looks the best. The WD40 really helps.

Thanks for the info. I unfortunately do not have any of the high speed spindles but will still try the recommended speeds with the 3/64 BEM that you used at 5000rpm

[nodott]

I know it's not the same but maybe it will help. I use 1/16 ball for engraving and i run it at 5100rpm, 7ipm plunge and 10ipm feed at .005 - .008" depth depending on what it is. So if I were to do it and i'm not saying it's correct, I would run it at 5ipm feed and work my way up to 7 to 10.

The material that I want to use this EM is 6061-T6. I do appreciate all the info and will also try your recommended speeds.