Today I was playing with some techniques for making a square blank into a round blank on the rotary. I know that if you move primarily in the X axis (mine is set X+), rotating a bit between passes, you end up with an N-gon instead of a cylinder (i.e. the result is faceted).
So I tried moving primarily in the A axis - spiralling from X0A0 to X5A12960 (or the equivalent). After tweaking that a bit, and pondering the not-flatness, it occurred to me that router bits are not flat on the bottom - the cutting edges are angled a bit so that the center doesn’t rub/burn. But that means if you run the bit right at Y=0 you actually mill a triangular spiral, like a very flat thread, because the center of the path is slightly higher.
I ended up offsetting the bit in the Y direction a little, and using smaller passes, so that I’m milling away from the center of the bit, but it’s not perfect.
I suspect there’s no intersection of “normal router bit” and “desired cylinder” that’s straight… so is this a fool’s errand? Or is there some magical bit or technique that will do this job correctly?
The best way I’ve seen this done is using the spiral toolpath you mentioned, but with a fairly large flattening bit. With a small stepover, it presents a large flat cutting edge that peels away the outside layer of the desired cylinder.
Vectric has a couple of gadgets that do a nice job with a rounding toolpath on a rectangle. The first couple of cuts take off the corners and then it does a spiral toolpath for rounding. Certainly, a piece of cake for Fusion too.
I found the best method for creating rounds it to use a pocket based on the corner to corner of the square dimension, cutting to final round diameter in 3 passes. The first pass will cut some air as it cuts off the corners. The final cut is smoother than using a spiral cuts or offset cuts with a planer bit.
The nice thing about a pocket is you don’t have to allow for the bit offset.
I use a 1/2" 3-flute spiral bit.
Most of my rounds are used in making two piece walking sticks (see Vectric’s Aspire Gallery). I started making sticks in 2000, these were profile cuts and full length.
The last 15+ years they are 2-piece with 3d art carvings. I have completed hundreds of them, gifts to people with medical needs without charge.
10% (could be higher with good sharp bits) usinng a down-cut 1/2 3-flute spiral bit
18K+ rpm
150% - 175% feed rate
Different woods, different settings…
~ .25" cut, 3 passes
Dale
Ah, that explains it. If you try closer to 90% you’d see the effects I was talking about; at 10% you’re only cutting with the tip of the bottom edge, but taking 9 times as long to finish.
You are probably wondering about all the sawdust when I have a vacuum system.
Running a 5 HP vacuum while cutting with small bits makes for an expensive cut.
I made a box using 3/16 Luan plyywood, full size under the rotary.
Then I put a strip of cardboard in the groove on the machine frame which deflects most of the sawdust into the box. It leans outward at about a 60 degree angle so it clears the spindle and dust head.
To make the box with thin wood I use quarter round on the inside corners
You could make one using the Vectric box gadget but I would still add quarter round
True, but my original query was more theoretical - a 100% pass on a flat pocket gives a flat pocket. A 100% pass on a flat cylinder gives a ridged cyilnder. Reducing the pass size makes the ridges arbitrarily small, but not flat, because only the tips of the cutter are at Z=0, with the rest angled up slightly.
True, just like a straight line is a curve with an infinite radius. The only difference in smoothness is how much time you allow the machine to do the work. I only use 3-flute spiral bits, both up and down cut. Then decide, more finishing time or more machine time… the machine usually wins…
Even if the bottom of the bit isn’t flat, it will be closer to flat near that tangent edge. The step-over for a Y offset of 0.4*bit_diam would be something like 60%. You would still get ridges, which is unavoidable with a non-flat bit, but they would be much smaller. It also cuts more along the grain, which might yield a better finish even with a flat-bottom bit.
Unless it specifically says otherwise, assume those have a half degree or so of clearance towards the center, so that the part that’s doing the actual cutting is closer to the specified cutting speed.
They’re more flat, but it’s unlikely they’re actually flat.
