Can I fake lathe work on my VMC without proper tool comp?

Done this a few times when the lathe was tied up and it works fine, but skip the automatic comp entirely. The control's comp assumes the round thing is the tool, and once the work is the part spinning it just gets confusing. Easiest path is to program it the old school way, to the theoretical sharp tool point, and build the nose radius in by hand. For the chamfers that means aiming the tool at a point shifted off the finished angle by the nose radius, measured square to the surface being cut. For the blend on the shoulder, program the tool nose centre to swing an arc one nose radius larger than the finished one and it comes out clean. Do the maths on paper once and reuse the offsets for the whole batch.

For touch-off, the spinning bar is actually your friend. Feed the tool in untill it just kisses the stock and marks it, and that gives you your radial zero against whatever diameter you turned the bar to first. Find the axial zero off the end of the bar with a feeler or the edge finder. One thing that matters more than people expect: the tool tip has to sit dead on spindle centreline. If it's high or low the diameters drift and you get a pip anywhere a face is cut. And to whoever suggested just milling it, that only works with a rotary axis. On plain round bar in a vise you can't get a true turned surface all the way round, so spinning the work is the right call for a Friday deadline.

I did a version of this last year turning down a couple of bushings on the mill while our lathe was out of action, and the thing that bit me was the tool not sitting square to the spindle axis. Diameter came out a hair tapered end to end and it took two parts before I figured out it wasn't my maths. Now I sweep an indicator along the tool before I start. One thing I'm still unsure about though, do you run the spindle slow for this? I was timid with mine and it still threw chips everywhere since I had no good way to aim coolant at it.

One thing I'd add to the toolholding side of this, because it bit me the first time I tried the same trick on a stubby bit of bar, is that a regular machine vise is a genuinely poor home for a lathe tool since the cutting loads are trying to lever it straight out of the jaws. I ended up bolting a square toolholder to a plate clamped to the table with two toe clamps and the finish improved noticeably. I also kept the spindle speed low, maybe a couple of hundred rpm, so any wobble in the grip did not get amplified. How long are these rollers, because the overhang out of the chuck will decide wether you need a support at the far end.

Ran a job like this once and the thing that saved me was keeping the rpm way down. Feels wrong on a mill but that bar whipping round at a few thousand rpm with any runout in it is a whole diferent animal. A couple hundred rpm was plenty for stock removal and the finish was fine after a slow spring pass. Also left a couple thou on the diameter for the first test cut, saved me a scrap.

Ha, this goes way back before CNC, we used to swing big rings on the horizontal boring bar by spinning the work and feeding the head, same idea. One thing I'd watch is the chips. On a proper lathe they clear themselves, here they pile up right on top of the tool and pack into the workpiece, and a packed chip will tear the finish on that blend radius before you know it. Hit it with coolant or blast it with air between passes and keep it clear. Also worth a think, how long are these rollers? If they're long relative to the diameter, deflection between the two ends of the cut will show up as a taper no matter how good your offsets are.