[LockTech]

Looking to see what everyone throught would be the best approach to milling a part. The part is 2x2x2 steel. I need to cut out a 2x1x1 out of the side of it, basically making it a L shape.

Being that its steel, does it make more sense to use a larger bit say 1/2in. and just keep surfacing it until I get to the desired depth? Or use a smaller bit say .1875 to cut slots in the steel to meet at the desired points therfore removing a corner chunk of the steel.

I usually work with aluminum and just wondered if there was a recommended method for harder metals?

Thanks

[txcncman]

Basically you are talking about a trepanning method, which will take 2 set ups and might cause binding on the tool and tool breakage. Most people would do this in one set up with a larger tool. Machining time will probably be close to the same either way. You will lose time on the 2nd set up.

[fizzissist]

Band saw, I say.

This is just for one part? Lay it out with Dykem, rough it out with a band saw, then finish mill it with the 1/2" mill. That way, you're not spending time turning it into chips and you've got a small blank for some other purpose.

Like txcncman says, you run the risk of binding with the 3/16 tool, and you're slotting way deep with it..... always problematic.

Assuming this is on a CNC (this is, after all, a CNC forum ) and production... Then get a carbide 1/2 mill and turn it into chips. A good, solid setup, a stubby 3fl @ 300SFM and .006/rev feed and at least 40% stepover.... You're at 2 roughing passes and 1 finish pass. You're done, and with time to worry about more important stuff.... Like what's for lunch.

[LockTech]

Thanks for the input. Yes it is a Haas Mini and that makes sense on the slotting too deep. I dont have a bandsaw so I guess its off to making chips

I see you mention a 3 flute, I have always used 3 flute for cutting aluminum quite often but was always under the impression the more flutes on steel the better? For example I have some .5 5flute carbide bits that I use from time to time. Is there a reason you suggested 3 flute?

[RICHARD ZASTROW]

Chip clearance and evacuation, same for Alum. Too many teeth engaged in the cut will also squeal and depending on cutter dia., not have sufficient room for chips.

Dick Z

[glovebox20]

If I have a 40 tapper CNC Mill, I would just use a inserted cutter (2.00 my favorite) and mill the step out. If I was on a manual mill, I like the bandsaw Idea follow by machining to size on the mill if needed. using a inserted cutter or regular EM.

I don't think you will have much luck sloting it out, but if you drill a bunch of holes first, then you could go back and clean it up with an EM. I find it easier to sharpen drill bits by hand than end mills, so if you have more time than money, I probly go this route.