Cutting balsa and ply

[markdib]

I am having trouble getting my homemade cnc router to make clean cuts in soft balsa and ply.

Soft balsa sometimes seems to tear itself apart along the grain as the cutter goes past. Harder balsa is OK, maybe the batch of wood that I'm using is particulaly soft?

Ply gets burned away rather than cut, so this fills the room with smoke - not nice!

My question is what type of cutter, router speed and feed rate should I be using and what does everyone else use?

At the moment I am using a 1/16" end mill in a 500W router running at 27000rpm. Feed rates are approx 6"/minute for balsa, and approx 3"/minute for 1/4" ply. I've tried a brand new cutter which did exactly the same thing.

Any suggestions?

Mark.

[balsaman]

Cut faster. Burning wood means the cut is too slow. Go 6 inches a minute in the ply and see what happens. Also a little larger endmill is a good idea. You could try 1/8". Use carbide endmills is you can. They stay sharper. If you cant go faster slow the spindle down a bunch.

If your machine cant can't the ply that fast take a 1/8" deep cut twice.

Eric

[markdib]

Thanks Eric,

The reason I was going that slowly was that at faster speeds the tool breaks. I wanted the smallest tool possible to allow for cutting smaller slots etc, but in reality I haven't needed it so I'll try a 1/8" tool. At the moment 6"/min is the fastest I can go (need more voltage!)

I may try to slow the router down, but will need to build a speed control for it as it is fixed speed.

It's interesting that the problem is too slow a speed, I had been assuming that I was going too fast and was slowing the cut down.

Thanks again for the help.

Mark.

[balsaman]

Rule of thumb is don't take a deeper cut than the tool diameter, especially for a 1/16" cutter.

I don't usually obey that rule. With a 1/8" endmill I take up to 3/8" at a time..

Soft balsa is hard to get a good edge.

I save the 1/16" bit for the stuff that NEEDS such a little cutter. 1/8 is much sturdier.

Eric

[mikeschn]

Would any un-coated end mill do for cutting in wood? Plywood, MDF etc...

There are myraid choices. 2 fluted, 3 fluted, 4 fluted, uncoated, TiN coated, TiNC coated.

My thought was just to get some long 2 fluted uncoated endmills... I like to be able to clean up the entire 3/4" deep cut with one pass. I'm probably only taking off .005" when I clean up.

What do you think?

And as long as your suggesting an endmill, can you suggest a good place to buy them?

TIA,

Mike...

[Jcadwell]

I've bought tools from www.discount-tools.com with good results. Good prices, reasonable shipping time, no problems or errors.

[balsaman]

I use solid Carbide endmills, two flute. The HSS endmills last longer cutting steel than wood....do I smell something burning?

Long endmills are great but the trick is to get the chips out of the way. Making deep cuts doesn't let the endmill clean out.
www3.sympatico.ca/robert.tisdale/websales_files/page0009.htm

Canadian prices.

Eric

[mikeschn]

Hey Balsaman,

The longest cutting length I could find on a 1/8" bit is 3/4".
Doesn't anyone have something longer like 7/8"?

Thanks,

Mike...

[balsaman]

You can cut 7/8" with a 3/4" bit just take 3 passes. A rotozip bit is 2" long or so....

Eric

[ger21]

Would any un-coated end mill do for cutting in wood? Plywood, MDF etc...

If your talking 3/4" thick materials, I would recommend carbide wood spiral bits. Wood router bits have different cutting flute geometries than endmills and will cut better. Unless you need 1/8" bit, I'd use 1/4" or bigger spirals. You can get some really good ones from http://www.vortextool.com. If you want to do a 3/4" clean up pass, I'd probably use a 3/8" or 1/2" instead of the 1/4". You can also try here:

http://www.eagle-america.com/html/ca...p.asp?id=87693
and another good choice with a huge selection is

http://www.onsrud.com

None of these are really cheap if that's what your looking for, but I use Vortex at work and they're great bits.

Gerry

[whiteriver]

As for a speed control to slow the spindle down. Go to harbor freight. You can pick one up for $20 or $10 on sale. I use one on my 3 1/4 hp Portor cable and they work pretty good.

Donny

[ballendo]

Hello,

Slow down your router rpms! Run your machine as fast as you can (6IPM).

You're burning your bits up, which makes them dull. Then they break. Never forget that heat is the QUICKEST and MOST RELIABLE way to dull a cutting edge...

You need to be making CHIPS, not dust. Each chip will carry away some of the heat of the cutting. Dust won't.

Let's look at the numbers: At 6IPM, you're moving .1" per second. At 26000 RPMs, you're turning the cutter 450 times in that same second, over the distance of that .1". Which means your chip thickness is... .00022 (Two-tenthousandths isn't much of a heat carrier!)

Even at a spindle speed of 10K rpm, your chip thickness is still only .0006" And your taking 166.6 cuts per .1", or nearly 1700!!cuts per inch! (for comparison, what many would call a high quality wood planer finish might have 50-85 cuts per inch... And most folks using a hand held wood router cut at about 50-70 IPM. This means they have about 285-400 cuts per inch )

So slow the spindle to match the slow travel of your machine. Your cutters will actually be cutting, and your results will improve.

Dramatically.

Also, for ply the carbide is a good idea--because of the glue in the ply; but for balsa, use HSS. It's sharper, and will stay sharp longer as long as you're not beating it to death<G>

Carbide starts out "duller", but handles the heat better, so that may be why you've received advice for carbide on balsa.

You're not the only one who needs to slow the spindle down...

Get into the habit of figuring your chip thickness, and CUTTING speed. Which is NOT the travel rate of the machine, but the actual "distance" the cutter travels through the cut. Most texts will call this SFPM (Surface Feet Per Minute),or SFM.

If you've got a 1/16 cutter, making a full width cut, as soon as it is in the material up to its diameter, you're cutting .098" with each rev. of the spindle (PI times diameter, divided by 2, because only the leading side of the cutter is actually cutting). Now if the spindle is turning at 10K rpms, you'll have a Cutting speed of 81.8 SFPM.

Note that if you were making successive passes around an outline, or milling a pocket, the CS-Cutting Speed-- would become 40.9. Because now the cutting edge is only being used for 1/4 of each revolution of the spindle

There are tables prepared by people like the Forest Products Laboratory in Madison, WI, USA; which will tell you the "correct" cutting speed for many types of wood. And machinery's handbook will have the values for metals. (Cutting tool mfrs. and distributors also have this info.) Use it...

By getting into the habit of knowing your numbers, you will discover the best rates for YOUR machine and YOUR materials. By STARTING with the "table" value-- or as close as you can get, since your machine speed may not let you hit the numbers exactly-- you will avoid the common mistake of misinterpreting the empirical results. (As you did when you slowed down because bits were breaking...)

Hope this helps,

Ballendo

P.S. Blowing air at the cut will help tremendously. You can do this with a small vacuum set to BLOW through a drinking straw. This will get the chips out of the cut area, and help the OTHER vacuum (dust collector) do its job. It will also do some direct cooling. HEAT is your biggest enemy, when cut quality is being considered... BTW, Remember that most vacs need a steady movement of air to keep THEIR motors cool. (Which means you may want to divert some of the air before it gets to the straw, to keep the flow rate through the vac up.

A better choice might be one of the hobby air brush diaphragm compressors... Try it, you'll like it!

P.P.S. One more thing. Using a spiral flute cutter will also help.