Cutting Birch and have Speed questions

[groovinjello]

Brand new and have been having a blast with the ShopBot! Just have a question to hammer out.

I'm cutting into 1/2" Birch Plywood with 1/4", 2 flute, carbide, straight, upcut end mill.

I am cutting in 2 passes.

My settings have been:

Spindle Speed 8000 rpm
Feed Rate .75 inch/sec
Plunge Rate .12 inch/sec

I just downloaded a project I want to try out from the project wizard and the settings set there are:

Spindle Speed: 18000 rpm
Feed Speed: 1.75 inches/sec
plunge Rate: .5 inches/sec

It is set for a 3/4" piece of plywood but still using a 1/4" end mill with 3 passes. Obviously the settings are much higher than what I've been using.

Have I been going to slow? Should I up my speed on this and future projects?

After reading through the forums, I get the feeling that I am going to slow, but I just want confirmation.

[shoeshine]

Hi Nathan, and welcome. This is a great space for questions.

to answer, Absolutely, especially if you have a spindle. I run a PC router and I regularly cut birch at 2-3 IPS depending on bit. actually I'm surprised you aren't getting burning/char on the wood at slow speeds.

I will leave it to the wizards here to calculate chiploads (I generally go by sound), but the idea is to get chips not dust. too slow and you generate a lot more heat which is the bane of carbide.

[myxpykalix]

The (non)answer is "maybe". To my point though,
I have had my shopbot 4 years and i still go slow or at least slower than some guys.

What you will learn is to listen to the shopbot and tune your ears so that you will know whether it is getting bogged down or spinning too fast for the speed.
There are speed and feed charts for different bits/materials combinations but the best teacher is going to be your eyes and ears.

Do you know how to adjust the speed manually while the file is cutting? (shift < or > ) and i would start out slowly and gradually increase the speed and watch and listen.
I don't believe there is one magic setting and the different bit/material combos from mfg to mfg will vary. Also the type of cut (2d or 3d) so experience is going to be your best teacher.
You would be far better off asking questions then breaking bits or damaging material because you didn't know so don't be afraid to ask the same questions (we've all) asked 100 times before.
I'm reminded of quote from one of my teachers, a short green guy with big ears...

"You have much to learn young padiwan..."
i'll try...
"Do or do not...there is no try...." lol
good luck

[shoeshine]

OK Jack, I take your point and it is very true, every bit/material combo is its own animal.

Ditto on the learning to see and hear.

I will say however that when I started I was hesitant and cutting MDF at .2 IPS and damn near set the stuff on fire.

[groovinjello]

Ok... now I've got more questions.

I was getting dust, which means I'm moving at to slow a feed rate I take it?

Both Chris and Jack suggest listening as key. What am I listening for? I assume hi-pitch screaming? If that is the case is it going to fast or to slow?

You guys are awesome, thanks for the help!

[shoeshine]

Hmm, OK easy to experience hard to describe.

As far as the dust goes, When I am cutting BB, (if I feel I am tuned in right) I get a sort of velvety sawdust with tiny little curlys in the mix. It comes up in handfuls rather than sifting through my fingers.

as far as sound, I can only attest to what I hear with my PC router which is a very different beastie than the spindles SB sells.

What are you running?

[groovinjello]

I have no clue what I'm running... how would I tell?

[myxpykalix]

It is hard to describe what you should be listening for as every bit/material/speed-feed combo will produce something different.

I will agree with chris on a point that you would be better off cutting mdf faster then slower because remember that you basicaly are cutting paper.
Look to this pic withthe arrows. That is your speeds. Those speeds are generally determined by the tool selection and things like stepover and stepdown values you select in the tool selection menu.

4936

[shoeshine]

sorry, the question should have been...What tool did you buy when you bought your shopbot? a porter cable router, or one of the industrial spindles.

The router is a black plastic motor housing w/ the PC logo on it. 5 speeds from 10k to 21k.

The spindle is one of several options from shopbot with a whole lot more power and speed control than the setup I've got.

I am assuming you bought a spindle as The PC router does not have the option to go down to 8k RPM.

That is why I said my sound experince might not apply. The router is notoriously louder than any of the spindle options, and regardless, operates at a very different frequency.

Chris

[eaglesplsh]

Nathan -

Chris and Jack are right that you will have to learn to listen to your machine to fine tune things as you gain experience. But that's going to take a fair bit of trial and error on your part. I'm not sure why no one has piped up with a simple "run it at this speed" answer to get you making parts today...

We have a new Alpha machine with a PC Router. When I'm cutting Baltic Birch Ply with a 1/4" bit I use:

Spindle Speed: 19,000
Feed Rate: 5 ips
Plunge Rate: 3 ips

I cut the material in 2 passes 0.250 deep, because the chips don't eject right and the bit will deflect (bend) if I cut deeper - then your mortises will come out narrow. I also use a 22.5 degree ramped plunge to ease into my cuts.

You'll find that your upcut spiral will leave splinters on the top of your part. It may not do this new out of the box, but they all do it as soon as they start to dull even a little. Most folks would cut this material with a mortise compression bit. (Unless you need to drill holes smaller than 0.313" as part of your file - then you need the upcut to avoid burning, which is worse than sanding off splinters.) The compression bits are designed to eliminate the splintering on the top and bottom of your parts.

Most pros have switched to 3/8" diameter bits for the majority of their cutting. You can cut deeper without deflection/chip ejection problems and they clear out pockets 50% faster. Sometimes you still need do use a 1/4" bit to get into tight radius details.

[groovinjello]

Nice,

Thanks guys. Will let you know how it goes.

[brcguy]

Nathan,
I've cut almost 2,000 sheets of birch through my alpha in the last year. I mostly use 3/8th or 1/2 bits, but sometimes 1/4. With a 3/8th bit in 1/2 thick BB, I run 16,500 rpm at 6-8 ips (single pass). My bits last a good while (30-50 sheets) before they need to be sharpened. With a 1/4" bit I'll usually take two passes and start a little slower.

I use amana or onsrud compression spiral bits. Single flute bits give a higher feed rate, but the two flute bits give a slightly cleaner finish.

Learn to use your chip load calculator until you get comfortable with the material you're using. Also check out onsrud's website for a very good tutorial on feeds and speeds

Good Luck!

-Dave

[dlcw]

Nathan,

I've cut many sheets of 5/8" baltic birch for drawer box parts. I set it up to cut using a climb cut on the first pass and leave a 1/32" skin. I then do a second pass using a conventional cut direction to cut 1/64" into the spoil board. I do all this with a 1/4" mortise compression bit.

My settings for the first pass are:

Spindle RPM 12,000
Feed rate 5" per minute

Second pass:
12000 RPM
4" per second feed rate

I've never had a bit break and my cuts are very clean. I can go directly from Shopbot to automatic edgebander to veneer the edges. Like Dave said, 30-50 sheets between bit changes and life is good.

Don
www.dlwoodworks.com (http://www.dlwoodworks.com)