Ideal spindle speed vs. feed rate

[BoscoToys@thebest.net]

I talke to an Onsrud tech today and he said that the best spindle speed for cutting 3/4 " plywood would be between 16,000-18,000 rpm's. I have a variable speed 3-1/4 hp Porter Cable router. I can reduce the spindle speed to that range, but I'm concerned about the machine having enough power at that speed. The Tech Rep said that spindle speeds higher than this cause dust instead of chips. The dust dulls the bits faster. He said the ideal speed at this rate would be 125ipm which translates to about 2 inches per second. He also said feeding much slower than this also will shorten the tool life, due to chips being in constant contact with the cutter. Does anyone know the fastest feed rate that the PC can be pushed at without causeing premature failure of the motor? Would I need to put an amp meter on it to really know the true load?

[bruce_clark]

Mr. Fisk,

I doubt that running your P/C at 16Krpm will hurt
it. I also believe that this is still in the
"power band" of that router, but I am really unsure.
I have a smaller PC (1.5hp) and a variable speed
Bosch (2hp). The Bosch has power in all but the
lowest setting.

As for doing damage, the WORSE that could happen
is that you would need to replace the brushes
sooner than normal. A 5 minute job on my P/C
router.

Oh, I did a calculation on the Onsrud bit. They
are recommending 2200 surface feet per minute (I
am assuming you are talking about a 1/2" bit)
which works out to a chip load per tooth of .007".
That is a pretty good "cut". If you keep your
RPMs constant, you could switch to a single flute
cutter and your IPM would drop by half (the
reverse is also true, and by switching to a 4
flute cutter your IPM would be about 250).

The last bit about dust and cutting too slow is
true for ANY cutting tool. I have learned in
my machine shop classes that more cutters are
broken/dulled by cutting too SLOW than by cutting
too fast!

Bruce Clark
bwclark@centurytel.net (mailto:bwclark@centurytel.net)

[vcabinet]

Does anybody know the rpm and cut speed that would be best for the columbo spindle cutting .75 maple plywood veneer core. Is it best to cut 1 or 2 passes.

Thanks Gary

[Brady Watson]

I usually cut 4/4 hard maple in 2 passes with a straight bit or upcut spiral on the Colombo. I go 1 to 1.4 IPS at 13,500 RPM. 13,000 seemed too slow and 14,000 seemed to burn.

-Brady

[vcabinet]

Brady, Thanks for the info. Do you have any idea about plywood, and about how long do the bits last. I am using a compression bit 1/4". Cutting at 2 ips. at 18000 rpm. It seams to cut fine but the info on the forum varies so much.

Thanks Gary

[kerrazy]

Gary,
Compression bits are great if you are cutting entirley through in one pass. The bueaty of compression bits is that they are Up cut (godd for reducing bottom veneer tear out) and down cut (good for reducing top surface tear out). You need to be able to do this operation in one pass though for best results allowing the bit to cut into the surface of your table or having your sheet rasied on vaccuum pucks.

If this can not happen, then decide which surface is the keeper and place it face up on o=your table then use a down cut spiral. The glues and resins in plywoods very, so bit life will depend on what you are cutting. I have had great success using a 52-240 onsrud upcut spiral on 1/2 inch CDX plywood cutting in one pass. feed rate of 1.25 in/sec and RPM of 16,000. I was able to do 30 sheets with one bit.

MDF is not the same, I use a 1/4 inch upcut (to extract the chips) and cut a 1/4 inch deep per pass with a 1.3 in/sev feed rate, again 16000PM.

Do not give up on double flute bits either. I just cut 4 sheets of 3/4 Maple veneer ply with a 1/4 inch 2 flute end mill and all edges were perfect. The client was very pleased.

Dale

[vcabinet]

Dale thanks for your help, I hope I can get more than 30 sheets out of one bit since I cut about 16 to 20 sheets per day.

Thanks Gary

[K. Simmerer (Unregistered Guest)]

Do a search on this forum for "Chipload calculator" and download. Scroll down to the end of the discussion for the final version. Pretty cool. Who would have thought of using a computer to help do the math? Anyways hats off for the programming effort and the slick slider interface! I LIKE it.

[Brad (Unregistered Guest)]

125 ipm? That is incredibly slow. I can cut 3/4" plywood all day, one pass, at 1200 ipm at 18000 rpm. I can stack cut 2 pieces of 3/4" plywood at 600 ipm. I can bump the spindle speed up to 24000 rpm and cut 2000 ipm. It is not with a SB though.

[daniel]

Hey Guys,
I'm new to this and gotta question about plunge depth.
I have the 2 1/4 makita. I'm running a quater inch bit at 18,000 rpm's with a feed rate of 1.7 ips through pine. The step down is .1 inch per pass. When I want to cut a profile total out can I cut the total cut depth of the bit? The bit has a half inch cut depth. Should I just slow down feed rate to cut with the entire depth of the bit.
Any help would be Great!

[Mayo]

Daniel, I regularly cut all the way through 1"x Pine (3/4" thick) with a quarter inch bit in one pass. Speed is around .85 to 1" per second and my Porter Cable is probably set around 19,000 rpm. Depending on the grain of the pine, I sometimes have fuzzy edges in places, but I'm frequently rounding over and sanding anyway. I use a carbide downcut spiral, usually single flute.

I'm wondering why you have such a small step down of just .1 inch per pass?

[ron brown]

Daniel,

Gee - lots of unknowns BUT, I cut 3/4" soft material all the time in one pass with a 1/4" bit. I'm not sure what your router/machine combination will do BUT, I doubt anyone can without actually seeing the material and the results from cutting with the actual bit you are using.

My normal cuts are about 2X diameter in wood. I cut 1/2" with a 1/4" bit and a bit more in soft wood. The power it takes to make the cut may be different from the speeds one should cut for proper bit feed and life.

Ron

[daniel]

Hey Thanks for the help. The .1 step down was a default set in the software I'm using, I can change it easily. I spent every penny I had on the machine and I can barely afford bits right now so I would rather ask before breaking a bit. I love this machine though! Thanks again!