I know, I know, yet another feed and speed post…
I’ve created a spreadsheet to calculate feed rate based on my understanding of Amana’s specs. For this post consider the following;
46170-K Amana Compression Spiral 1/4 Dia x 7/8 x 1/4 Inch Shank
Chip Load .0031
Based on the above, I get a calculated feed rate of 74.4 for wood. Amana’s recommendations are the same for wood and plywood.
While these settings have worked ok with plywood, last night I ran a job using poplar, and then the same job in what I believe to be white oak. I’m not exactly sure; I get scraps from a local cabinet shop and glue them up for odd projects. Anyway, let’s assume white oak. It is very hard and heavy, and I was concerned about these settings, as machining the poplar seemed a bit tough. For the white oak I slowed the ipm down to 35. The job completed, but wow, did it sound awful, like about to disintegrate at any moment awful! I also got some breaking/chipping of the wood at some of the thinner areas.
Regarding the .25 DOC, that’s what Amana recommends. I could certainly do a much shallower DOC, but that would defeat the purpose of the compression bit. Correct?
Any thoughts on this? I’m really trying to follow appropriate guidelines, but I have to believe I’m doing something really wrong here.
Oak chipping: I’ve used oak with and without cnc and it can be a mare as the grain wanders around.
I also concur on Oak being easily chipped, in fact in hand held routers, I use a climb cut to help in some areas then do a clean up pass in conventional direction, and probably could do that with Vectric, but not sure of the same outcome.
As to the speeds, I think 12,000 rpm is too slow, and would at least go to 16,000 or perhaps better. This would lower your chip load, so you should adjust the travel speed (ipm) higher. I shoot for a chip load of .006 in oak and .010 in poplar. I think the awful sound you hear is a “polishing” of the oak due to slow feed rate instead of “cutting” the oak. Look for the chips themselves, if they are smaller than about 1/16 of an inch, then you definitely are polishing the wood to death instead of carving the wood. The chips bing expelled will tell the whole story.
Seems to me there’s a little bit of “art” to this - the calculated numbers get you close, but feel free to make adjustments to them and experiment a little. The numbers I end up with are usually closer to .002 for chip load - but I’m not trying to push my machine to the maximum.
I usually start with 100 ipm with a 18,000 RPM - same .003 chip load but letting the spindle use its power more efficiently. From there, I’d back down on the ipm, and the DOC, for harder woods. Going down to 50-70 ipm with 18K RPM is likely where I’d start. That’s about the same chip load as you were at with 12K RPM and 35 ipm.
You’re right that a compression bit needs a minimum DOC to be effective. If you need to go with a lighter DOC maybe start with a down-cut bit - you’re not cutting through as you start out, so a lighter pass can work OK. Then switch out to an up-cut (or compression) for the last pass that cuts through the bottom.