Speeds and Feeds

[#Rekd™]

Hi,

 

I am enraving a sign (10" x 20" x .062" 304 s.s.) .015" deep. I have tried both 2 and 4 flute solid cabide 1/4" 90 degree chamfer mills.

 

I have been running 3000 rpm, feed rate of 4 and a plunge rate of 2.5. The tip keeps coming of the endmill (it is to a perfect point to start with).

 

I am using a Daewoo DMV 3016L with a Fanuc control and drives.

 

Are my feed and speeds correct? Should I be using highspeed machining? I am running the file as a sub from my flash card.

 

Thank you

 

John Ford

Mastercam V9.1, Mill, Lathe, Wire, Design, Art, Engraving and MastercamX

[#Rekd™]

Hi Again,

 

Are there better solid carbide endmills or differnt grades?

 

Thank you

 

John Ford

[DavidB]

Instead of using a Chamfering tool try a Engraving tool.

I use Dixi

[Chris Rizzo]

Another maker of engraving tools is micro 100 .

 

can you rough the pocket out a bit with a regular small endmill (set pocket to "tapered" with the taper value 1/2 the included angle of your tool), and then use engraving as a remachining operation. Sounds like your tool might just not like getting plunged into stock.

 

mc2

[BernieT]

Also, why not ramp the tool into the stock? Much easier on tools. I suggest 1/2 to 1 degree ramp on sst.

[robk]

I agree that you should ramp into the workpiece. I prefer to use engraving cutters that are not ground to a point, but are tipped off. Harvey is another manufacturer of engraving cutters, but I prefer to use their carbide drill/end mills to do my engraving with (we put a .010 flat on the bottom of the cutter) just because they are in the machine already to be used as chamfer tools.

I use the same principle as a regular end mill to get my speeds & feeds. Not sure what your max RPM on the machine is, but I am limited to 12K. I would start with .0005 FPT @ 94 SFM that would bring me up to 1196 RPM @ 12 IPM running the cutter at the full .015" depth (which gives it .030 Dia.). That was for a 2 flute tool. If your machine is allowed higher RPM's then keep experimenting with your SFM, but I would leave the FPT alone. Give 150 SFM a shot & see what those #'s look like.

 

[ 02-15-2006, 05:56 AM: Message edited by: robk ]

[htm01]

also you could try ball end mills ,i use a 1/16 ball when the engraving is wide enough

[summit fever]

I agree with the idea of ramping. The engravers I use have a .025 rad or flat on the end. This way the sharp tip doesn't break on the first move. By the way, I engrave at 4500rpm at 7ipm in alum., and 4ipm in steel.

[chowquoe^]

We use a .5MM Ball endmill on 17-4 PH Stainless Rpm=10000 Feed=2.5 tool life is great. Hope this helps