Cutting Hardened Steel

I have to modify a slide for a Glock handgun. My company has a patent and we need to modify the slides to accept a new rear sight. If you research the material the Glock slide is made from:

"Glock barrels and slides are made from quality steel which has been treated with a special "Tenifer" process. This colorless carbo-nitrate formula enriches the steel with oxygen, sealing its pores. Tenifer makes the steel extremely hard (as hard as industrial diamond on the Rockwell scale) and corrosion resistant. The steel will not scratch or rust, period! In fact, the slide is so hard you can use it to sharpen your knives."

That comes straight from Glock's website. I know the hardening is only about 3 microns deep but I still need to mill thru that 3 microns so I was wondering if anybody has any experience with this and can recommend some cutting speeds. The endmills used are only .25", .1875", .125" diameters and a .25 x .125 keyway cutter so I know the chip load will have to be low but I have no idea about the SFM.

I know it's a long shot but if anybody has any recommendations for the speeds and feeds it would be greatly appreciated. Thanks in advance for any help.

You'd do best to grind such material. Or grind thru the case with a dremel and then mill it.

We used to use a steel reamer bushings treated with a nitroloy process that made a thin crust super hard. The crust was so hard they would spark when you knocked one to the other. That was part of the sales man’s presentation showing how they would spark but still would not mark each other. Likely this is the same process. We never had reason to do any machining on them.
Very likely you may find grinding the solution, at least to go through the the fine skin or all the way throuh the hardened. How wide is the cut and does it need a special form/shape?
Off hand I am thinking a surface grinder or a higher precision abrasive chop saw may be a possible solution. It is not difficult to dress an abrasive wheel to a special shape/form.

If possible you do all needed work in the soft and you send out for nitroloy tratment...

Doing fancy on a slide a CBN plated / special shaoe wheel might be good for slides..


Harness chart:
Plasma Nitriding Hardness Chart & Typical Results / North East Coating Technologies

What machine are you milling this on?

I am wondering if this might be a job for an EDM

no problem to mill a Glock slide at all I drill with carbide drills and thread mill the holes but no problem to mill
Don


Sent from my iPhone using Tapatalk Pro

D Nelson said:

no problem to mill a Glock slide at all I drill with carbide drills and thread mill the holes but no problem to mill 3/16 endmill 5000 rpm .02 depth of cut 7 percent step over. .125 endmill 6000 rpm .02 depth of cot 7 percent step over 15 inches per minute 3/16 ball endmill the grooves are .005 depth per psss they are not hard to cut
Don


Sent from my iPhone using Tapatalk Pro

Click to expand...

Sent from my iPhone using Tapatalk Pro

realityrat said:

I have to modify a slide for a Glock handgun. My company has a patent and we need to modify the slides to accept a new rear sight. If you research the material the Glock slide is made from:

"Glock barrels and slides are made from quality steel which has been treated with a special "Tenifer" process. This colorless carbo-nitrate formula enriches the steel with oxygen, sealing its pores. Tenifer makes the steel extremely hard (as hard as industrial diamond on the Rockwell scale) and corrosion resistant. The steel will not scratch or rust, period! In fact, the slide is so hard you can use it to sharpen your knives."

That comes straight from Glock's website.

Click to expand...

Glock has idiots writing for their website. It's not oxygen, it's mostly nitrogen and carbon that's used to create the thin, hard "case". And it's not "diamond hardness", not by a longshot, as per Michiganbuck's link.

Here's a Wiki article that gives better information on the process: Ferritic nitrocarburizing - Wikipedia

I would give a try to just milling them with carbide. Cutting anodized aluminum (aluminum oxide) eats cutters eventually but you can mill a fair amount before the cutter is trashed. I would start about the same SFM as you would run 316 stainless, maybe a bit slower.

No personal experience, just where I would start if that job came across my bench.

here is another one I cut. You won’t have any trouble with carbide endmills
Don


Sent from my iPhone using Tapatalk Pro

Thanks everyone for the responses. Just for more info, I'm doing this in a Haas VF6 with a rotary 4th Axis. The slide is mounted to a 3" dia steel fixture in the 4th axis. Its a pretty rigid setup but not as rigid as a vice. Its not my setup, the previous machinist made this fixture so I'm stuck with it unless I can prove it doesn't work. But since I'm using such small tools I think the setup will be ok. If anyone has experience with this a good starting SFM and chip load would be useful. I'm using a dynamic toolpath so the tool engagement will be full depth (max cut depth is .25") with minimal stepover ( approx. .010 - .03" depending on tool dia.). Thanks again everyone.

Nice pics Don. Those speeds you mentioned with your pic; it looks like you went with 200-250 SFM, are those just a matter of trial and error or did you find info that you followed?