Carbide end mill in steel

[CJdave]

Ok, I will admit that I have next to no machine background. Everything I learned was from here or watching and listening, or just trying it myself. but I have ben doing that for the past 3 years.

So Here's the problem, I can't get carbide end mills to last in steel. Right now I have a part I am trying to make and I just can't seem to get the em's to last. Material is 1045, 1.625 dia round stock. I need to mill a flat on the end of the stock to half the dia and 1" back. I am starting with a 4fl carbide rougher (uncoated) and finishing with a 4fl carbide uncoated finisher. I started at around 480sfm and .002 per tooth at .050 deep flood coolant. That chipped the edge of the tooth. so I stepped back and slowed down a little, 275 sfm and .0015 per tooth, still sounds bad, so I thought I had too much steppover, and reduced to .120, and upped the doc to .12. Still sounds bad...
Can someone please enlighten me on where I should start with speed, feed, and doc? What about coolant?
Thanks
Oh, machine is a Millport bed mill 5hp spindle with a centroid control.

[Konrad]

I'm not a carbide lover in something like this,.. take a good 1 1/8 or 1 1/4" rougher HSS, full depth one pass,...100 pieces should be possible, carbide endmill has a hard time to beat this.

Konrad

[HuFlungDung]

Flood coolant is probably not a good idea for the roughing stage, as there is enough heat generated in the cut zone that the carbide may just crack, losing your keen edge.

Also, it sounds as though you are not getting much benefit from using the rougher at those shallow depths. They are designed to be run at perhaps 1 diameter deep or so. You might be using a 1/2" diameter tool. I'd pick TiALN coated for milling steel, never uncoated because built up edge can also rob your tool of its edge life.

You should have enough HP to remove 1.25 cubic inches per minute. So adjust your feed to accomplish that, if the machine is sturdy enough to handle it. Run at maybe 350SFM if you want to be conservative and extend the tool life. Rough at almost full depth so that you can take advantage of the helical flute, and try cutting at 60% stepover of tool diameter. Feedrate perhaps 30ipm or more if your machine doesn't bog down. Use an air blast to clear the chips from the cut zone. This chip clearing action needs excellent reliability, you don't want to ever hear crunching sounds coming from the cut zone as chips get recut.

If the machine is literally shaking itself to bits, maybe you need to ensure that your setup is rigid (not a vise sitting on an indexing baseplate). Or perhaps the spindle bearings are getting old and tired, and have lost preload a little bit, resulting in a looser than optimal spindle.

I have not roughed a lot in open situations like yours with roughing mills. I use Iscar inserted endmills. A 3/4" endmill makes a pretty good rough cutter. What you lose in diameter you make up for in rpms. There is always a tradeoff, of course, but you can run the 3/4" at 2500 rpm and 50 or more ipm and they will last for many cubic inches of material removal. C1045 isn't even tough

Inserts for steel cutting come honed, meaning the edge is a little bit rounded. This means the tool is not so free cutting but also a little bit more durable. The tip radius on the corner of the insert is also a bit more generous than solid carbide mills, and this keeps the tool in cutting condition for a longer time. These tools will hammer a bit more than a solid carbide rougher.