tpulley:
Cool; thanks for the information. Now we can really start to look at the numbers
.
Just remember: the chart-supplied numbers are for machines of substantial rigidity. Using just that table, you don't really have a way to understand the torque and power that a cut will produce, as you choose those numbers. Even a moderate amount of torque on the HDs leads to diving and jutter and jumping.
"Mild" is of course relative. On the Brinell hardness scale (
https://en.wikipedia.org/wiki/Brinell_scale), 1040 steel is 187, while 6061-T651 Al is 95. So, the mild steel is actually fully twice as hard, for machining purposes, compared to the aluminum.
On our HDs, cuts like this should ONLY be made in the "pull" direction. That is, the gantry moves in the direction away from the spindle, dragging it across the material, versus forcing it into the material. If you need a back-and-forth cutting motion, then along the gantry width is the best choice. This will help immensely with the success of these cuts.
Remember that, regardless of your depth-of-cut and stepover, if the first cut is a slot, you'll need to use full-slotting F&S, which are much slower than a typical profile cut.
On our machines, one of the things you'll notice is that the exact height-location of the cut surface top is directly related to how much deflection occurs, which is directly related to how "hard" the cut is. How "hard" the cut is varies not only when the cutter changes direction, but also as the cutter enters and leaves the material. What you'll notice by sight and sound is that, there will be odd tool markings on the far end of the cut, right at the moment that the force starts to go down, as the bit comes off the edge of the material. I wish I had a technique to cancel it out, but it's perceptible even on 0.002" deep finishing cuts in aluminum. So, don't freak out if you see that...
.
3500RPM @ 28IPM only gets you 229 SFM, but 1020 steel (low-carbon, cold-drawn, low-temp relieved) wants 345 SFM. I'd recommend going with 5000 RPM @ 28IPM, for 327 SFM, though myself I'd probably do something more like 4000 RPM and 18 IPM. Note that plunge rates are in the 1.5-1.8 IPPM range, so be wary there. That gives about 1/3 the chipload recommended, so it's a nice easy cut. I used 0.05" DOC and 0.01" step over. If you haven't already, and your VFD has a setting for "low RPM (power/current) boost", you might want to increase it for a little more ability to push through the cut at that 4k RPM.
As a first test, I'd run one at 0.025" DOC and 0.008" step over. If that works, move up to the other, increasing stepover slightly first, then depth, then stepover, etc.
Full slotting F&S for 0.025" DOC are 4500 RPM, 8.1 IPM and 2.0 IPPM (plunge). That seems reasonable, but I could also see it going horribly wrong.
And finally, are you familiar with the "color" test of the chips? (a good chip-reading article is here:
http://www.mmsonline.com/articles/read-your-chips) There are cutting conditions that inject so much heat into the cutter that it loses its temper, goes dull and then just starts rubbing. Also, chip re-cutting in steel is a far bigger issue than in aluminum. Steel work-hardens to a much greater degree. When those hardened-steel chips get lodged between the cutter and stock, it is very common to chip the cutting edge. For you, that might mean rigging up the back-end of the shop-vac for a temporary chip-blower.
While you're doing this, stand by with a squeeze or spray bottle of some sort with light motor or machining oil. I wouldn't worry about flooding the cuts, but having misted-drops of lubricant on the surface and the bit can make cuts like this a lot safer. In the real-world, after all, most cuts in steel are done with flood cooling being poured on a rate of multiple gallons per minute. Nowadays, that coolant is delivered by a high-pressure stream that goes through the length of the bit itself: through-spindle cooling they call it. Flood cooling at that volume might be an issue on our machines
.
I'm excited for you; I've stayed away from steel on my machine, so I'm interested to see how it comes out. You're a trailblazer, man!
Regards,
Thom