What's new
What's new

Engraving with a 1/32 ball mill

Atomkinder

Titanium
Joined
May 8, 2012
Location
Mid-Iowa, USA
Exactly as the title states. Material is 304 laser cut, machine is a Haas VF-6SS with a 12k spindle. Obviously spinning at 12k, but what would everyone's feed be at .01" deep? HSMAdvisor always seems to me to be very low on these numbers (1.41 IPM? Yes this is with chip thinning turned on). Tool has a 1/4" shank and a real short flute length, solid carbide AlTiN coated.
 
10 IPM is only .0002" per flute, any 1/32 worth it's salt should be able to handle at least that. Watch your entry feed, most of the 1/32s I blow up are on the entries not the engraving itself.
 
Not sure of your part specs, but the Micro 100 engraving tools sure work well.. I just finished up some tiny numbers engraved on hard S-7 at 55 RC.

Gotta happen tonight. Only learned of the job last night (relatively typical around here) and it's cosmetic lettering. Nothing horribly special, but has to look good. I have two cutters to play with. That means I won't break one, right? :crazy:
 
Normal engraving for me is 10k and 10 IPM with a 4 flute (.00025 ipt) so if those two extra inches matter for quantity...

Edit: looks like it's a onesie-twosie.
 
I used to always use a ball endmill but recently I've been using a #1 carbide center drill and been very happy with the results.
#1 carbide about .003-.004 deep and you can really go fast.
 
That sounds deep to me as well. I end up going only a few thou deep to get a pretty decent width line. Sneak up on it, and either ramp in or slow down the plunge like Haazart said.
 
Normal engraving for me is 10k and 10 IPM with a 4 flute (.00025 ipt) so if those two extra inches matter for quantity...

Edit: looks like it's a onesie-twosie.

Just a onesie.

I used to always use a ball endmill but recently I've been using a #1 carbide center drill and been very happy with the results.
#1 carbide about .003-.004 deep and you can really go fast.

Don't have any of those.

Why .010 deep with a 1/32? Why not .005 with a 1/16 and triple your feedrate?

I can do that too, but then work will have to buy me a new one (not that that's a problem).

That sounds deep to me as well. I end up going only a few thou deep to get a pretty decent width line. Sneak up on it, and either ramp in or slow down the plunge like Haazart said.

Plunge right now is set to ~1.4 IPM.
 
Just ran the numbers and was going to lambast you for going so deep, but others have done it for me.

HSMAdvisor would probably suggest higher feed and lower depth of cut.

IMO. 0.01" deep with a 0.03" tool in 304SS is way too deep. Hence it suggests such a low feedrate.

Otherwise you would probably snap the cutter right away.
 
I found that 0.003 to 0.004 was adequate for engraving with a 1/32 mill. The trick is that the surface has to be dead flat for such a shallow cut otherwise the letter widths will be all over the place.
 
I'm going to change it to .005" with a 1/16" cutter. This is going straight on the subplate, so if it varies I'm going to blame Chick Workholding. Which I wouldn't mind doing anyway :D

Edit: got the part indicated with a tenths test indicator (I have a VERY short flat to work with) within two tenths end to end, and checked the flatness of the part. Around the area to be engraved it's all within five tenths. Should work okay.
 
We regularly do deeper engraving @ 0.015 deep so it shows up after being painted, and sometimes even deeper so we can paint it, then fill in the remaining volume with a lacquer stick or contrasting paint.

Looking at the last few we did, depending on situation, it was .003 - .005 depth per cut down to .015 depth, .0002" per tooth, and ~5ipm @ 10k rpm. That's with a 1/32 ball mill as well. The strategy might be 'playing it safe' but it's also a "onesie, twosie" where it had about $30k in each part before the engraving. Risk assessment resulted in taking it a little easy on the engraving with a 1/32 ball mill - acceptable time cost.

ETA: Whoops, missed your followup post. Glad you had good success.
 
I'm here at work on my day off doing a different version because the engraving came out so nicely, so they're paying me OT to make them now. :cheers:
 








 
Back
Top