4130 Annealed Hard Spots??!

[magudaman]

So I purchased a piece of Annealed 4130 that I had intended to machine but after facing a couple pieces my cutter really started to create a lot of noise. I shut everything down and found I was starting to dull pretty bad. These are of course cheapy Chinese HSS TiN 4 flute cutters but I figured with flood and nice slow speeds they would be able to face okay. So now I am concerned that I may have hit a hard spot in my metal and burned up my cutter. I had made some initial cuts using a carbide tipped metal circular saw along one edge but it seemed to do okay and didn't seem to heat the metal too much. There is also an edge that must be from where they rolled the metal out because it is rather rough and sort of rounds.

Is it possibly as I moved though the surface near one of these edges it basically ruined my bit? Do I have to use carbide for this project? The two piece I had already faced didn't have that rough edge or had been cut with the carbide blades.

[dertsap]

if your having to break thru scale or rust then it tends to be fairly abrasive on the tooling

[magudaman]

if your having to break thru scale or rust then it tends to be fairly abrasive on the tooling

That is a very good point. I am basically just taking that stuff off and another millimeter or two. I now ended up just cutting off that rough area just to be safe. One guy at the shop said that area maybe work hardened. It was also brought up to me that I may have been making too sallow of cuts and therefor putting a lot of stress on my bits.

The background I left out earlier:
This is 1/2 4130 plate, I was running 600RPM with a feed of 5 IPM and a depth of cut of about 0.04 in on a tormach with 3/4in 4 Flute.


I have a Niagara 1/2in 4 Flute C430 TiAln Cutter showing up tomorrow and will try finishing up the parts. I used the angle grinder with a sanding wheel to remove most of the scale on the remaining parts so hopefully that will help some.

I ordered the Metal from Industrial Metal Sales, so hopefully their annealed rating is true. From what I found that means it should be about B82 hardness and would be around 300SFM with carbide TiAln.

Really like this chart: JM Machine Co Metals

That calculates to 2200 RPM @ 55IPM, say a 10% DOC = .05 per pass. I'll do 40% step over. From what I am reading I maybe better off running no coolant, that sort of scares me.

[magudaman]

I was just looking at the numbers and I am going to be very close to my horsepower number for the 1100 Tormach so I may change my step over a bit.

[jimhurlburt]

You want to get well under the surface scale the first pass.

I'd recommend about .025 doc for the first pass, a fairly fast feed, then reduce the load as needed by reducing the stepover.

I would definitly use coolant, if nothing else, hand sprayed WD40.
You want to get well below the surface the first pass, hot roll 4140 is more than a bit nasty for the first .010 or so, worse than a36 hot roll because the scale and hard spots are stronger than mild steel. If you can't afford the .025 material removal, you may have to figure on using up more tools.

I would use carbide myself, perhaps an insert fly cutter for the surfacing pass so the tooling wear is cheaper.

If you need to do this as a regular thing, you might look at the ceramic inserts that can cut hardened steel. They might survive the abrasion better.

Jim

[dertsap]

at 6000 rpm you've simply ran it much too fast and burned the tool , if you've got a Niagara cutter on the way then contact them or look on their site in order to get the proper speeds and feeds for that particular cutter because I don't see the cutter lasting for long at what you've calculated

[magudaman]

at 6000 rpm you've simply ran it much too fast and burned the tool , if you've got a Niagara cutter on the way then contact them or look on their site in order to get the proper speeds and feeds for that particular cutter because I don't see the cutter lasting for long at what you've calculated

The above was at 600rpm not 6000, I did looking into niagara website and came up very close to what I calculated for tialN cutter. I decided to back off some on the cut per tooth. Apparently dry is the way to go for tialn and actually activates the coating. I'm cutting in a couple hours and will let you know how it all goes.

[magudaman]

As per usual: The right tool for the job makes life easy. So while I wasted a day removing trival amounts of material with bad surface finish earlier but with my new cutter everything went absolutely smooth. Beautiful finish much higher removal rates and I still feel I was being conservative and could ramp up to a higher level.

So my final number were 2500 RPM, 35IPM, No Coolant, 20% stepover, and the max I did was .05 Depth since my cuts didn't call for more. So its a bit subjective but even after going through a significant amount of material, the edges and finish felt and looked amazing on the tool. So I think I got it down. No more fear for working in steel!

One of the guys came by and side if I saw too much blue chips I will want to slow it down a bit. But I though with carbide and good coating if it wasn't blue then you were going to slow?

Check out the video of making some chips:



Thanks for all the help and information!

[dertsap]

The above was at 600rpm not 6000, I did looking into niagara website and came up very close to what I calculated for tialN cutter. I decided to back off some on the cut per tooth. Apparently dry is the way to go for tialn and actually activates the coating. I'm cutting in a couple hours and will let you know how it all goes.

oops about the 6000
that material should be fairly easy machining but unless the tool had a corner rad then the chipload at 55 ipm seemed a bit heavier than I would push it to start with , I've seem too many corners get knocked of due to excessive chip loads .
Dry running tialn isn't always the way to go , and many have a misconception that you should never run coolant on these tools but if the heat gets hot enough to break down the coating then the tool will be toasted pretty quickly . So more or less it depends upon the application , when it comes to end mills then I prefer to see clean colored chips at high or low speeds , insert tools I'll aim for blue when I'm pushing for high speeds .