3/4 Baltic Birch, 1/4 Downcut. Feeds? Speed? Plunge?

[BASiQ]

So, long story short, I have a recently acquired two CNC's. More or less just thrown in my lap.
I am 90% sure everything is ready for use except for the bit settings, which I know are quite important.
At this point I am going to be focusing on one machine, getting it working then moving to the second one
So... Straight to the details, here is what I am working with

1998 6x10 Multicam SF CNC Router.
Elettromeccanica Giordano Colombo 7.5HP RS-90 Spindle
1/8" ONSRUD 57-240 Straight Bit
1/4" Whiteside 1500 V Groove 90

I will be cutting 3/4 Baltic Birch almost exclusively so for the wood
The software I am using is Vectric Aspire 3.5

I am brand new to this and in an attempt to not break my bits or wreck the machine, I am hoping someone here can take pity and offer some suggestions.
I am clueless when it comes to seting things like Pass Depth, Final Pass Stepover, Clarence Pass Stepover, Spindle Speeds, Feed Rate or Plunge Rate

These are what settings I have so far for the VCarve Bit
http://img35.imageshack.us/img35/2590/bit1g.jpg
These are what settings I have so far for the Straight Bit
ImageShack® - Online Photo and Video Hosting

Is there something I should change? It this acceptable?

I also noticed on my spindle's spec page says that the spindle's RPM's are 18.000 - 24.000.
Should I still set the spindle speed to 16,000 like everything else? Or should it be 18,000

[BASiQ]

Hmm, it's amazing what variations of google search queries can result in if you stick with it
these links have been wonderfully helpful answering these questions, at least some of them.

http://www.multicamnw.com/support/ma...ting_guide.pdf
Calculating Feeds and Speeds - CNC Router Shop
Feed Rate Calculator

Also a particularly interesting one, where people are asking almost the same thing as me
Note, this thread was mainly about 1/4" bits. mine is a 1/8" so I assume this means different settings, to avoid shearing.
Cutting Birch and have Speed questions - Let's Talk ShopBot

Great stuff, but I am still looking for input from the people here

[ger21]

How are you cutting 3/4" plywood with a 1/2" long bit?

If you up the rpm to 18,000, you should be able to cut at about 200ipm or more.

If you are making deep cuts, I'd make one pass with the downcut, and use an upcut for the next passes up to the full depth.

[BASiQ]

How are you cutting 3/4" plywood with a 1/2" long bit?

Multiple passes I guess. I told the people who sold me the bits I was going to be cutting 3/4" Baltic Birch and they said the 57-240 should be fine.
I had planned on multiple passes anyways, especially with a 1/8" bit

If you up the rpm to 18,000, you should be able to cut at about 200ipm or more.

Forgive my ignorance, but I am assuming IPM is feed rate? Correct?

If you are making deep cuts, I'd make one pass with the downcut, and use an upcut for the next passes up to the full depth.

All I have is a downcut, but I want to pursue this for the future. What is "upcut"?
Is it a bit that you spin backwards? Or is it a bit that is just shaped differently?
Or am I completely off and it's just some kind of method of cutting using a downcut bit.

Also, had one more question.
My spindle says 18,000 - 24,000 RPM. Does this mean I can't cut at a slower speed?

[louieatienza]

The feed can be calculated, if you know the chipload of the bit. You should be able to find that online. I don't believe the 57-200 series is recommended for plywood. Fine for MDF. The recommeded chipload for a 1/8" bit is .005-.007. Just multiply the chipload by the spindle speed by the number of flutes, using .005 I get 180ipm, and .007 I get 252ipm. So that's the range, and should be achievable with that big spindle!

Really however the high performance bits are normally 3/8" and above, since they're more ridgid. A downcut might not be the best for plywood, I would probably use a compression spiral; with that powerful spindle you should be able to do one pass through plywood easily. The nuber of flutes would be determined by how fast you can run your machine. I've seen Onsrud's demo of a 4-flute compression spiral cutting hardwood plywood in one pass at 2800ipm! But this is with their Extreme Series, cast iron bridge and 40HP spindle!

I use a 1-flute mortise compression spiral for plywoods, since the short upcut section allows me to do 3/4" plywood in two passes, and still have the downcut section leave a clean finish on top. Onsrud recommends for hard plywoods compression spirals and roughers and rougher/finisher bits...

[BASiQ]

Tons of great information louieatienza. Thanks for the chipload information
Had one question I was not able to find out information about though.

Still wondering about the spindle speed though.
From the spindle manufacturers page, it said 18,000 - 24,000 RPM.
I am not sure if this means I can't cut at a slower speed?

[louieatienza]

Don't know much about Colombo spindles other than that they are one of the best. If you're cutting plywood only you'll be fine, as long as you keep the speed up. With a 3/8" chipbreaker compression spiral, you should be able to cut upwards of over 350ipm per flute, provided your machine can run that fast.

[ger21]

IPM = inches per minute

Does the tool have a 1/8" shank, or 1/4" shank? If it has a 1/8", it's OK.

Upcut bits cut with an upshear, and can cause splintering at the top edge, but they remove the chips better. Downcut bits will push the chips down, and pack the chips into the cut. Honestly, though, with an 1/8" bit, you won't notice much difference, as it's hard to get the chips out of a 1/8" cut.

Sorry, but I don't know anything about your spindle.

[BASiQ]

Got everything working so far.

For anyone else reading this, my settings I am using are

1/4" V-Carve bit. 1600rpm, 250ipm, 100 plunge.
1/8 Straight bit. 1600rom, 100imp, 30 plunge.
I am cutting 1/2" Baltic birch. 5'x5' sheets.

Thanks to louieatienza [below] for the chipload info and the formula.
Will certainly use it in the future

Nothing broken so far, running a cutting program as I type this, watching the cnc run around the table lol. Also to answer my own question, I have learned that using a lower speed is more then fine, apparently running 20k+ is bad for your bearings in the long run. So I am sticking with 16000rpm =)

[ger21]

Plunging is also bad for your bearings. Ideally, you should try to ramp in to the cut whenever possible.

[louieatienza]

Plunging is also bad for your bearings. Ideally, you should try to ramp in to the cut whenever possible.

I agree... Especially with a downcut spiral, the bottom edge is negative rake, so it takes more "force" for it to cut; again maybe not as much a problem with 7.5HP. We had a 5HP shaper that I was scared to death of.

Some bits are designed for plunging, some are not and should be ramped or helixed in. Many wide mortising bits (i.e. hinge mortising) have center clearance and should be ramped in. May insert bits should be ramped in unless they have a plunge tip; some insert and carbide tipped bits have an extra plunge tip section. The manufacturer's site will usuallly indicate such.