While test cutting some Baltic birch plywood for my sculptures recently, twice the router has gone off course resulting in some loud screeching and burning of the wood and ruining the job. I’m wondering if my feed rate is too high and or getting too much bit deflection Here;s the technical info: Newly assembled OOZnest 1500x1500 OX CNC Dewalt 611 1.25 hp router set at minimum 16,000 RPM Baltic Birch with a plastic laminate on the face side for a total thickness of 0.712 inches. Routing from the back side (plastic laminate face down). ¼” carbide compression bit with approx ¾” to 1” stick-out Feed rate 290 ipm (derived from trial version of G-Wizard) Software: Vectric Cut2D Pro with following parameters: Plunge rate 30 ipm 6 passes at 0.1187” at a time Lead in @ 45 degrees, 0.1” length with lead out of same length, overcut distance 0.1” Checkmarked: Ramps smooth Checkmarked: Ramp on lead in Order selection: L to R, Bottom to Top, Grid, shortest Checkmarked: sharp external corners Nesting setup: Tool diameter 0.25” Tool clearance 0.50 Border Gap: 1.0 Rotation step angle Allowance offset: 0.02 Final pass 0.00 The pieces being cut are very curvy (Bezier) . Both times that the diversion occurred, it was one of the deeper cuts of the six cuts. No other adjacent nested pieces were cut before the diversion and no objects were present to hinder the routers path. On one piece, I was able to see that there was a slight diversion at several higher steps but the router continued on course until the lower cuts and then it went off track. The other piece went off track on the deeper cut without any previous diversion at the higher level cuts. Any suggestions would be greatly appreciated.
Hi, From your feedrate i would say that is way too high, if i was doing that job i would start at around 1200mm/min. From a calculator i used to use, they would give a feedrate as if the machine was a perfect setup. But it had an extra input box, where you could enter a percentage of the feedrate you want to run at and it would recalculate the rest. Ryan
Ryan: From the other feed back I've been receiving on other forums, it does seem that my feed-rate is the most likely culprit. I've got a lot of pieces to cut. I usually have about 3-4 dozen per 4'x4' sheet. With the slower feed rate, it looks like this could run all day? Any strategy suggestions?
I would keep the feedrate, increase rpm a little (I regularly cut at 30000rpm) and decrease depth of cut (do 7 layers instead, maybe 8), and make sure the chips are vacuumed out of the slot before the next cut. recutting chips is very bad your compression bit will push chips down into the slot which can jam up and cause burning, stalling, and of course, going off course as the cutting force exceeds the stepper holding forces. maybe an UP spiral bit would be better, so it clears the chips? compression bits are supposed to cut the first cut deep enough so that the compression area is at the surface, to prevent breakout. I don't think 0.1" is deep enough for that. ??? Since you are cutting from the back anyway, maybe you don't need the compression feature? Compression Bits are Often the Right CNC Tooling Choice, But Not Always
You could do a roughing pass to remove the bulk of material, then come back through slower to tidy it up?
