Marking steel parts on lathe with live tooling

Tungsten Carbide · Feb 28, 2020

I have tried carbide ball end mills, drill mills, Harvey marking tools...the carbide always chips pre-maturely. 5500 Rpm, 4 IPM plunge, 11 IPM feed. Anybody have a system that works well on marking low carbon steel?

dandrummerman21 · Feb 28, 2020

Recently did a whole bunch of engraving some 303 stainless parts on a mill.

We have an old 2L (pronounced "tool") spring loaded engraving tool. 2L inc., Engraving Tools, Spring Loaded Engraving Tools, End Mills, Vacuum Chucks and Pumps, Engraving Software, CNC Countersink Tools

The thing was crashed years ago, so the tool runs out about .003 at the tip, maybe more?

I am unable to run the pointy "single flute" engraving tools on it, they chip right away. But a 3/32" ball endmill worked perfect for hundreds of parts (maybe engraved 20 1/4" tall characters on each of about 250 parts)

Just looked at the program, 5000rpm 10ipm plunge, 15ipm feed
We use a macro variable to control the "depth", we had about .025" of infeed to get about .015" deep roughly.

Not saying there isn't a better solution out there.

Tungsten Carbide · Feb 28, 2020

Thanks for the input. I have tried 1/32 ball endmills and the little 1/32 extension snaps right off after a few parts. 3/32 would be stronger, but I think it might make too wide of a mark. I have seen others talk about marking with 1/32 ball endmills, but I don't know how they keep them from breaking.

dpolseno41 · Feb 28, 2020

I almost exclusively use ball end mills to engrave, ranging from .020" to .045" and have never had one break. On a mill I run 10,000 rpm at 25 ipm, plunging/ cutting without issue. Sounds like something is going on with your setup.

FredC · Feb 28, 2020

Onsrud makes engraving cutters. They have worked for me as well as common center drills 00 or 000.

CarbideBob · Feb 28, 2020

+1 for center drills.

dallack · Feb 29, 2020

There is a thread a few weeks old about a tool with a spring loaded carbide point that drags over the part with the spindle stopped.
We have used the same tool on a live tool lathe.

Red James · Feb 29, 2020

OP: Don't try to engrave full depth of the ball radius. I use a 1/16" ball end mill at 8000 rpm, 0.0015" per rev, but only cut 0.003 deep. Yields a width of about 0.025 Can't hardly wear it out.

aarongough · Feb 29, 2020

I use one of the spring loaded diamond point 'drag engravers' from WidgetWorksUnlimited, it has worked really well for me. It makes very clean crisp looking marks even down to tiny tiny sized letters. It's used with the spindle off. I use mine on tool steel hardened to 63HRC every day and get 500-600 parts per marking tip:

Diamond Drag Engraving Bit for CNC Machines - Use Your CNC Machine to Engrave Metal, Plastic, Glass, and Granite - WidgetWorks Unlimited

I'm sure it would last even longer on soft steel. 2L have a carbide point version but I don't think it's really much cheaper.

zerok666 · Feb 29, 2020

I normally use a #2 carbide center drill.

majohnson · Feb 29, 2020

What about the Tipped off cutters, the one the are 1/2 the cutter width. I used them on CNC routers for engraving. Mirco 100 page 209, 2019 catolog.

ChipSplitter · Mar 2, 2020

If you need big bold text, try Iscar's MM HDF series. They really work well for us on the mill and since they're 90 degrees, we use them for chamfering and back-chamfering, too. For engraving, we run 7500 RPM and 60 IPM for plunge and feed.

AARONT · Mar 2, 2020

I use drill mills if I need it to be deep, otherwise just a 1/16" bem .005" deep at max. Max spindle speed with about an .0008"-.001"ipt. I plunge at 3-10ipm depending on material and rpm from a .01" clearance plane

Tungsten Carbide · Mar 3, 2020

Thanks guys. Carbide 90 degree drill/mill is the winner so far, but it only lasts about 50-60 parts at .005 depth. It is a bonus that it can do chamfering, but I'd like to see better life. Maybe I'll try the 1/16" ball endmill, but the 1/32" one was breaking after 1 or 2 parts. It is a 16" long 4.5" diameter part being held with 5" long soft jaws in a lathe chuck. Maybe since I'm marking on the end face, it is not a rigid enough setup for carbide tools?

litlerob1 · Mar 3, 2020

I'm assuming that you do the engraving on the same op, that the part is Turned and Faced. Not a second Chucking....

R

SeymourDumore · Mar 3, 2020

My go-to engraving tool is a carbide, ball-end 15deg runner cutter.

But like rob said, you better have a known, consistent surface to start with, meaning: cut it on the same op!!!

vr6 · Mar 4, 2020

just a suggestion. we sell a lot of the FAK tools each month for users doing your exact application, take a look when you get a chance

FAK (Triangle Insert)

Tungsten Carbide · Mar 11, 2020

Yes, same op.

camhead420 · Mar 11, 2020

Tungsten Carbide said:
I have tried carbide ball end mills, drill mills, Harvey marking tools...the carbide always chips pre-maturely. 5500 Rpm, 4 IPM plunge, 11 IPM feed. Anybody have a system that works well on marking low carbon steel?

I have been using Harvey engraving tool w/ .010" tip. 6000rpm feed .001 ipm into part then feed at .004-.006 ipm.

ChipSplitter · Mar 12, 2020

mr.greenman said:
Feed .001 ipm into part then feed at .004-.006 ipm.

Wait......what??

Shirley you mean .001 per rev., not minute........

Marking steel parts on lathe with live tooling

Aluminum

Stainless

Aluminum

Aluminum

Diamond

Diamond

Aluminum

Stainless

Stainless

Plastic

Cast Iron

Titanium

Stainless

Aluminum

Diamond

Diamond

Aluminum

Aluminum

Cast Iron

Titanium

Similar threads