Rpm and feed rates

[connie]

I want to cut maple and spruce. I care about quality of finish cut and I don't need to cut many parts. I'm not a production shop, I have a 1/4" Onsrud bit and a 2.5 hp spindle. Anyone have experience with these 2 woods that could give me a good starting rpm's and inches/sec cut rate recommendation for each type. Thanks.

[connie]

Also any rules on plunge rates for Spruce and Maple using the 1/4" ball nose onsrud bit?
thanks

[richards]

Connie,
There's an excellent Chip Load Calculator that can be found under the Tools tab in SB3. You might want to try 5-6 ips at 15,000 RPM as a start if your cutter is 2-flute. A 1-flute cutter would be run at 2.5 - 3 ips at 15,000 RPM. That would give you a chip load of 0.010, which is much finer than the 0.015 to 0.020 that I aim for with composite materials. Most likely, 0.010 would give you a fine cut without too much heat build-up.

[terryd]

Connie,
The key to machining maple is to cut fast enough so that it doesn't burn. You have to keep in mind that the chipload number is the same regardless how deep you plunge into the material. Use Mikes suggestions but stepdown about 1/8" per pass and cut as fast as possible. Never had problems with spruce except for the "fuzzies". Depends on the tree. Smaller growth rings mean a more dense wood and vice-versa. Do a test using a 0.025 chipload then speed up or slow down your cut speed dependant on the results. Fuzzy- slow down, Glassy- speed up.

[connie]

What about curly maple (that's eastern hard curly maple)? Finish is the most important concern, any good starting rpm and feed rates? Has anyone cut curly maple and have some starting points?

[connie]

Mike, thanks for your post. I'm using a 2-flute solid carbide up cut. Would that 5-6 ips at 15,000 RPM be a good starting point for maple or spruce?

[Gary Campbell]

Connie.
When I was in Northern Mich. we processed a lot of curly, burl and birds-eye maple. it was impossible to plane with a straight blade planer. We had to switch to a spiral head to get an acceptable surface. Try using multiple quick passes as Terry says above with a .010 offset and then do a final pass at full depth to remove the last .010 at half the move speed of the cutting passes. I would use a compression for the last pass to reduce tearout. (or all the way, as it is a spiral up for the bottom portion of the bit)
Gary

[Brady Watson]

Try climb milling instead of conventional to avoid tear-out in maple. It works wonders...

-B