Miniature Engraving

[JAMMAN]

Trying to engrave something smaller than usual in a quantity larger than usual. What are others using for an engraving tool, need about .03 wide path max and I'm limited in RPM to about 4,000 unfortunately. This haas screams even at 4000, I think 5000 is max and that would scare me.

 

Current ball nose (.05 ball nose .006 deep) is loading up in aluminum even with heavy flush.

 

If it were a one off I would creep it and get-er-done but I have 60 of these freaks to run. Getting a lot of fuzz after a few parts as u can see.

[crazy^millman]

Might try a an engraving tool from Micro-100 or Harvey tool. Might look at getting a Die Grinder and bolting it to the side of a tool holder that way you got some RPMs. That slow with small tools and you are going to get what you get.

[Millertime]

what are you feeding that cutter at?Is it 2fl or 4fl?

[JAMMAN]

OK I'm a harvey user to the max, I didn't know they carried small engraving tools. The end mill is a harvey but unfortunately the job came through quickly and a 4 flute was all I had.

 

I'll order a 49710 since it will give me an even smaller slot at .006 deep than I currently have.

 

I think I'm down to 10 on the feed.

 

I've done the die grinder thing on an anilam knee mill for small hole drilling. We are engraving more and more projects as time goes on, I should plan a little better for this.

 

Thank you

[#Rekd™]

Drill/Mill combo from McMaster-Carr will work well.

[Pilot Plant Supervisor]

If you want indexable, Everede tool company has a line called nine9 that has some really slick little engraving tools.

[JAMMAN]

Just checked out Everede tool company, nice stuff going to give them a call but I already have a harvey on the way. I think I have a mill drill already, I'll try that too.

 

Thank you!

[Mr. M]

I always liked the Harvey miniature spot drills for engraving like that (.045 dia)

[Newbeeee™]

and maybe worth taking a re-cut with a facemill (minus a thou) after engraving to clean the face off

[JAMMAN]

That would make them pretty for sure. Only face mill I have is on a R8 though. I'm trying the tumbler today, parts are done for this run.

[cincy k]

I've always used a 2 fl ball mill with very good success. Use an application/material specific geometry and coating. Something like 27831-C8. The coating should help with welding. About 10 ipm would be a good feed rate. Look into an air turbine spindle or even an electric spindle if you're going to be doing a bunch of it. http://www.hpt-drivesystems.com OR http://www.airturbinetools.com/ You could get your feed rate up to 100 ipm or so.

[ablucra]

I have used the Harvey cutters for years with good results.

Recently purchased a spring loaded holder for engraving and polishing

from here 2linc.com. Works great on uneven surfaces and the cutters

have held up well. They have a speed and feed chart as well.

[Bucky Cornstarch]

I engrave stuff like this on every part we make (6061,) and occasionally have to use the slow (6000rpm) mill. I use a 1/16 2fl BEM, 6000RPM, .005 DOC, 10 IPM with flood coolant. Isn't the fastest way to get things done, but it works. BTW, this leaves me with about a .035" engrave width, so you might want to try a 3/64 BEM.

[Brad St.]

Another trick I use is not necessarily the tooling but the path chaining. I'll chain as much of the path in one opps and keep the tool engaged to ensure cutting forces. I'll chain it using the partial chain with waiting and reverse back on legs even a little to keep the tool in and moving. It's a lot more time sometimes up front but look at how many parts you have the every time that tool has to plunge if your doing bigger runs of parts. Saves tooling and finish. If your tool can handle a single depth of cut your golden, usually then I just have to maybe wrap a piece of sandpaper around a honing stone and give it a nice quick draw polish.

[chrisdavala]

i haven't ordered on in awhile but harvey used to have an engraving cutter that was slightly off center so it would knock the burr off as it went. down side was it had a small flat on tip so your depth might not allow that

[JAMMAN]

Harvey is awesome, I buy so much crap from them they sent me a t-shirt.

 

By that logic CNC software should send me a car......

[jeff]

http://www.2linc.com/engraving_tools.htm

These guys have a nice selection, even have a micro engraving tool with a .002 tip width

[35K chipper]

Jamman,

Here are the Harvey tools i use 75102 & 75102-c3.

they are runner 2 flt cutters i run at 35000 rpms @ 43.75 ipm @ 0.003>0.004 doc

in aluminum.

.

.

35k

[TK-32™]

I would try two, (or even 3) depth cuts. You can increase federate and ultimately you can have a shorter cycle time. Also facing the material before engraving tool helps because extrusion is not flat.

 

One time I engraved with a 1/8 45 deg em from McMaster car (DesignRite?) and I was feeding lose to 25ipm.

[M. Anderson]

I do a lot of engraving on aluminum parts - logos to ser. numbers.

 

I have tried everything - ball endmills - engraving cutters (Onsrud-Harvey-Ect.) - custom grind (me).

 

Damn near every part I run for one customer has engraving.

 

I use a Accupro 60deg 1/8 2fl Chamfer tool (82892498) for most all parts.

 

Sometimes I will use the same thing in a 90deg cutter, depends on depth.

 

The only thing you have to watch is the cutters will sometimes come in with a messed up point.

Don't really know how to describe it - anyway I usually take the cutters when they come in and grind them to a <.005 flat on the end.

I run them in 6061 at 12 to 15 ipm at 4200 rpm at .012 depth, in a Schunk Hyd. holder. ( no runout!)

The cutters usually last 300+ parts.

 

I even use these on some 304 and 316 parts for serial numbers. (alot slower!)

 

Best solution I have found in a while.

 

HTH

 

Mark