4130 Feeds and Coolant?

[magudaman]

So I have a thread running over here where I got some great information on running my Annealed 4130 Cromoly. Reading around on the web I am seeing conflicting information on cutting 4130 with carbide end mills.

This one on Practical machinist is saying crazy numbers like 600SFM while most sources I see say 300SFM


Really like this chart: JM Machine Co Metals

Let me run the number by you guys just to confirm I don't ruin my new $40 dollar tool:

I have a Niagara 1/2in 4 Flute C430 TiAln Cutter showing up tomorrow and will try finishing up the parts.

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.

That calculates to 2200 RPM @ 55IPM, say a 10% DOC??? = .05 per pass. I'll do 40% step over.

From the posts in practical machinist it sounded like the general feel was run no coolant. Anytime I have done that in the past (in aluminum) I almost instantly broke a cutter.

Coolant or no?

EDIT:
ARG looks like this should have went in the metalworking tooling :-/ GRRR

[Geof]

4130 is very different to aluminum. Try running aluminum alloys with a decent DOC and feed without coolant and you are almost certain to load up and break the tool, especially if it is a four flute.

However, running a TiAlN coated cutter in 4130 should be done dry. The coating needs to get very hot to activate it's lubricating properties.

600fpm with TiAlN is not really crazy depending on the DOC, stepover and feed. With a 1/2" four flute you should be able to run at this speed with a DOC of .4", maybe more, a stepover of no more than 20% and feed of 0.005" per tooth.

The goal with TiAlN coated cutters is to get a fast moving hot chip that does not efficiently conduct heat to the part or the tool. But the tool must not be buried deeply in the cut, however with the small stepover you benefit from radial chip thinning so the feed per tooth can be cranked to get very rapid metal removal.

You should do a search on trochoidal milling and peel milling to find out how fast you can run with the correct combination of tool, DOC, stepover and feed.

[magudaman]

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 said 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 and I think I can ramp it up even further!