What's your go to engraving cutter?

[kunfuzed]

I've got about 600 parts a month I just took on that need a small logo engraved on them. Customer spec is .005 min depth x .015 wide. (Intended for a .02 ballnose) in 1018 mild steel. These numbers can be fudged a little. 

Long story short, I have to take a couple depth cuts to get there, and can only crawl at 5ipm at 7500 max rpm.

I've used 60 deg cutters with a .005 r tip from Harvey befpre, but seems like they end up chipping as well.

What works for you in steel? Probably more ss is the answer... lol

[Mike@Dive Lab Inc.]

I've been using a 60 deg indexable one from 9 Nine. The inserts hold up well for me. I run it at 7500 rpm @14-17 IPM in 316 stainless. I usually end up about .006-.008 DOC.

http://everede.net/documents/archived_documents/2013_nine9_catalog.pdf

 

[Matthew Hajicek - Singularity]

Can you tilt it to cut with the part of the ball that's moving instead of the center that's just spinning?

[Matthew Hajicek - Singularity]

Or use a speeder head (air or electric)?

[kunfuzed]

Not unless I made a fixture for the indexer.  Something to think about though!

[kunfuzed]

Just now, Matthew Hajicek™ - Conventus said:

Or use a speeder head (air or electric)?

If this job keeps up, that might be the way to go.  I don't have TS air or coolant, so mechanical drive maybe the way I'd have to go.  Haven't seen any electric ones.  Will be interested to research those.

[kunfuzed]

As far as "Half Round" single flute vs a 2 flt engraving cutter, what is the difference in application there?

[Matthew Hajicek - Singularity]

Unfortunately electric speeders tend to be expensive.  You could probably improvise one with an 18000RPM trim router, but it probably wouldn't toolchange so you'd want a separate engraving op so you'd leave the tool in the spindle and swap parts.  Or have a bunch of parts on the table for a batch.  For that matter you could get a hobby grade benchtop CNC router with high RPM just for engraving.

[Matthew Hajicek - Singularity]

If you go the trim router speeder rout, I did some research a while ago on what to use as a spindle on a hobby mill and there's a strong consensus that the DeWalt DWP611 is the best.  I put one on a MAXNC with good results.  It's 18KRPM variable speed, has a nice machined aluminum cylindrical body to grab it by once you remove the base, and has good bearings that will last and keep it running true.  Holds up to 1/4" shanks.  Just need to make a mount for it and you'd be good to go.

[Matthew Hajicek - Singularity]

double post

[nickbe10]

I usually use a center drill unless there is a reason not to. Strong, lasts forever, readily available in many sizes and inexpensive. I engraved tool steel the other week at 15 ipm, no problems.....aluminium at 25 - 30 ipm

[jeff]

I've tried a bunch of different brands, and so far these seem to hold up the best:

http://www.lakeshorecarbide.com/highperformanceengravingendmills.aspx

[geirsj]

This one is handy, comes in different angles so you also can use it as a chamfer tool.

If you use that brand you maybe get away with just the insert and not the holder. Otherwise its fast to change the tool if needed.

Works great in different materials, I use it both for engraving and chamfering holes before threading and also sometimes outside on the edges of 

the part.

INCH:

https://www.iscar.com/eCatalog/Family.aspx?fnum=3642&mapp=ML&app=0&GFSTYP=I

Metric:

http://www.iscar.com/eCatalog/Family.aspx?fnum=3642&mapp=ML&GFSTYP=M

G

Edited September 22, 2017 by geirsj
Links for metric and inch edited

[YoDoug®]

Do you have through spindle coolant? If so I would recommend an Iscar Spinjet.

[geirsj]

On 21.9.2017 at 6:03 PM, kunfuzed said:

Probably more ss is the answer

Hi!

I run the one i mentioned on 6000rpm, 11ipm and depth of cut 0.02I

in metric it would be S6000 F300 Z-0.6mm if the numbers seems off in Imperial...

if further cuts i have this depth of cut on engraving, on chamfering its max z-3.2 in metric and probably z-0.12 in imperial

 

I run both steel, aluminum and stainless on this speed, its always in the machine and we do both engraving and

chamfering with the tool. When the tool got on the market i knew of it before my supplier, and had asked of it many times if they had something like it.

Ordered it, put it in the machine and change when i see build up of deburrs, not often.

I could probably rum max spindle 12000 in my machine, but i prefer slower speed, feed could also be higher i guess, but i also prefer rather change the tip

than spindle......

 

[kunfuzed]

Unfortunately I think I'm going to have to stick with a solid 1/8" shank tool, as there is a little boss that I have to get right up next too.

[RonC.]

On 9/21/2017 at 1:54 PM, nickbe10 said:

I usually use a center drill unless there is a reason not to. Strong, lasts forever, readily available in many sizes and inexpensive. I engraved tool steel the other week at 15 ipm, no problems.....aluminium at 25 - 30 ipm

I too use #1 carbide center drill to do my engraving unless engraving get filled..

 

[gms1]

For all aluminum parts https://www.mscdirect.com/product/details/05479175?rItem=05479175
onsrud tipped engraver. Roughly .03" deep one pass 12 ipm.

For all steel (right now its 15-5ph ss) its a garr tapered ballnose edp #15220. .03" deep, .015" doc per pass 3 ipm.

[MrPrecision]

We have had very good luck with these: http://www.2linc.com/engraving_tools.htm We have mostly used these for an application where we are machining serrations into H900 17-4, and not much else works at all. We have used them for aluminum as well though (the aluminum specific ones..). 

 

The gear spindle speeders warm up like crazy (we bought a Nikken), so running them is not fun. We have a really long warmup cycle before we even try. The cutting depth drops about .004" from cold to warm. Coolant thru speeders are much better about warmup, but only if you have the setup for it obviously.  

[jeff]

On 10/4/2017 at 10:49 AM, MrPrecision said:

We have had very good luck with these: http://www.2linc.com/engraving_tools.htm We have mostly used these for an application where we are machining serrations into H900 17-4, and not much else works at all. We have used them for aluminum as well though (the aluminum specific ones..). 

 

The gear spindle speeders warm up like crazy (we bought a Nikken), so running them is not fun. We have a really long warmup cycle before we even try. The cutting depth drops about .004" from cold to warm. Coolant thru speeders are much better about warmup, but only if you have the setup for it obviously.  

We used to use those from 2Linc for years. Until I found the ones on Lakeshore Carbide's website. They give a much crisper cut. 

We only use them for lettering parts though, no "engraving" stuff.

[Sticky]

Small ballmills give much better tool life than the engraving specific cutters, while also giving a crisper edge.

[kunfuzed]

Update:

I was blowing through cutters left and right, getting about 24 parts per cutter at best (engraving one small logo per part, soft 1018 steel).  Was using some uncoated HTC 60deg 2fl cutters with a .01R tip at .008 deep, 7500rpm, 5ipm, with a ramp in of about 2 degrees.  After I had run out of cutters, I sourced some more from a local cutter grinder.  Fairly certain it wasn't these cutters themselves, but the other big change was I switched from coolant to dabbing on some dark thread cutting oil I picked up from the plumbing isle of Home Depot, lol.  All of the sudden now I've run 430 parts on one cutter!

[jaydenn]

 

On 10/10/2017 at 1:16 PM, Sticky said:

Small ballmills give much better tool life than the engraving specific cutters, while also giving a crisper edge.

I always use a 2mm ballnose endmill spinning at 10000-12000 rpms. Aluminim, steel, tool steel... always 10000 rpm.

The results are absolutely fantastic and the cutter will last for a million years (give or take...)

 

J