number of passes to cut pockets and roughing cuts

[boatman811]

I am working on a number of projects that require profile cuts in .5 inch and ,75 inch hardwoods, specifically mahogany, oak and walnut. My bit supplier has indicated that I can make these cuts in a single pass especially in the .5 inch materials. his rationale is that making multiple shallow passes puts undue stress on the very tip of the bit creating undue excess heat. Shallow passes do not create chip sizes necessary to carry away the heat. Currently I am using a .1875 inch 2 flute bit at 10000 rpms and 100 inches per minute feed rate. He suggests a faster feed rate, a 3/8 bit and single pass or at most 2 passes. Any thoughts? What are your experiences?

[ger21]

Shallow passes do not generate more heat. But they do wear the bit more, because the same small section of the bit is doing all the cutting.

Your machine's rigidity will usually be the limiting factor in how deep and fast that you can cut, as the deeper the cut, the higher the forces, which can cause a lot of machine flex on smaller hobby machines.

With tools 1/4" and smaller, I like to keep depths to tool diameter or less. Once you get to 3/8" and larger bits, you can easily cut 3/4" deep or more in one pass, IF your machine (and spindle) can handle it.

[Tailmaker]

For simple pockets (square or circular) I try to cut a small starter pocket (essentially a hole) to the pocket depth in the middle and then cut the rest of the pocket inside-out in a single pass, as far as the flute length allows. However, that means a smaller stepover to avoid breaking the bit or stalling the machine. Usually this is a faster way to cut the pocket, avoiding several retract movements and it is making the best use of the flute length. I wish vectric would offer this strategy as an option for the pocket tool path. Oh, it also reduces the long slivers of wood that are torn out when pocketing along the grain in the conventional direction and which can clog the dust collector.

For complex pockets or roughing tool paths this gets too complicated and I use the normal method of stepping down in layers.

[Xxray]

Usually best to go with the recommendations of a supplier, but obviously not always.
As Gerry states, machine flex might well be an issue doing deep cuts in hardwood on a hobby machine - 2 other things are just as possible, bit breakage and hold down failure. I personally would start conservatively and not exceed .25 per pass. If that cuts like butter then by all means, increase the depth. Not optimistic about you cutting thick slabs in 1 pass, all you can really do is try it if so inclined and report back the results. As far as rpm/feed, again, no one here is really in a position to go against the recommendations of the supplier, too many variables involved. Do what is suggested and if you have bad results, you'll know not to listen to him anymore.

Regardless of who says what, much in CNC comes down to trial and error and building up experience. I don't know your experience level or your machine, that is why I suggest being conservative. You are not saving that much time in the scheme of things using 3 passes instead of 1, unless you are making 100's of copies. 1 thing is certain - If you bite off more than your machine can chew, you'll know it quickly.

[Mikehell]

His recommendation made no sense until you got to the part where he recommended a 3/8 or larger bit. One pass on 1/2 inch hardwood with a decent bit seems right