[Crushmonkey]

Does anyone CNC-Route hard and exotic woods like wenge or coconut?

If so, what feeds and speeds do you use for your range of bits ?

[ger21]

It depends on a few things. Type of tooling, power of spindle, and rigidity of machine. On a commercial machine, using spiral chipbreaker tooling, you should be able to cut as fast as any other hardwoods. I cut a lot of maple, and I've cut hickory on our CNC. Based on using hand tools on exotic woods, I'd say they should cut very similarly to other hardwoods.

[fyffe555]

Can't talk about coconut but I did a large project with wenge last year. Lots of routing by hand mostly though. It has resin depending on the sample and seasoning which will cause the burn marks, clog cutters and also cause glue and finish problems. Apart from that it machines easily and moderate blunting on the cutters.

As Gerry says its much like any other hardwood. Best finish, by hand or in the machine was with the 7518 at 21k, a spiral Onsrud carbide and about about 4ins second and loads of vacuum to clear the cut.

Had some problems with tearout and poor finish when climbcutting in the cnc, though that's because my machine isn't ridgid enough to do what I wanted.

[ger21]

fyffe, I've found that climb cutting will usually give a poorer finish cut than conventional cutting in wood. But the tool must be supported on both sides (cutting through material, not along an edge), or you'll get tearout most of the time. I only climb cut when I know it will tearout if i don't.

If your getting burning, slow down the spindle speed. And if there is a lot of resin, clean the bit often. I've found that cherry has a lot of resin in it, and new bits will be covered in a very short time.

[Crushmonkey]

how often is often when cleaning the bit? a few feet of cut travel?

[ger21]

It depends on the wood. Id say every hour if it's bad.

[earlywood]

How about the real hard exotics?

Wenge is about 1600 Janka and hard Maple is less than 1500.

Has anyone cut anything up in the 3000 Janka range like Bloodwood, Jatoba, Ipe, Teak?

[jm82792]

I cut up some Cumaru(3000+ plus Janka) and it came out well. I used some sort of generic 1/4" 4 flute carbide bit at 40 IPM at 35K RPM for(full passes at 1/4" deep) roughing and for finishing I used a 1/8" (.01 stepover) ballmill at 35K RPM at 35 IPM.

For the smaller piece I used a 1/8" fishtail(1/8" deep and full width) at 35 K RPM at 38 IPM then a 1/16" (like .008" stepover) ball at 40 IPM.
I sanded both pieces shown below with 320 grit and they cleaned up nicely for being tests.
That being said I'm new to all of this(wood working, CNC machines... Etc) these figures are probably poor, but they seemed to work decently.

[louieatienza]

I cut a lot of hardwoods like ebony, rosewoods (brazilian, cocobolo, honduran), jatoba, wenge, and have not had problems. Usually, you can run yor feeds faster than you think; a bit (no pun) of experimentation will get you there.

In fact I slot fretboards with an .024" bit at over 70ipm, and profile cut them with a spiral-o-flute 1/8" bit at 75ipm and .125" doc, climb cutting with no problems. I also use a 1/16" spiral-o-flute with a 1/4" flute length at 75ipm and .063" doc.

Point is, use CNC specific bits, as they have larger gulleys and can clear chips easier.

[earlywood]

Thanks guys. All great info.

What I really want to use is a 1/2" ball nose to cut these very hard woods. It's a 3D contour situation, but I don't have any fine detail (imagine cutting a small bowl out of a blank). Therefore, I would like to use something in the 1/2" range. Have you ever cut them with a bit that big?

[louieatienza]

Thanks guys. All great info.

What I really want to use is a 1/2" ball nose to cut these very hard woods. It's a 3D contour situation, but I don't have any fine detail (imagine cutting a small bowl out of a blank). Therefore, I would like to use something in the 1/2" range. Have you ever cut them with a bit that big?

That's fine, but what you want to do is use a 1/2" straight bit for the roughing pass and leave .02" or such for the finish pass. The job will go way faster.

[earlywood]

Is that because the straight bit doesn't have the cutting surfaces that the ball end does that are near the center of the tool axis and therefore travelling at a slower speed?

[louieatienza]

That's partially it, but mainly because a straight bit has about 30% or so more cross sectional area than a ballnose at 1xD depth. But related to your comment, with a ballnose, your stepovers are going to be a lot less vs. a straight bit for the reason you state.

[ger21]

With a larger bit like that, if you use a small stepover, you don't really need a roughing pass, as the first pass is the only full width pass, and after that, you're only removing the stepover amount.

[louieatienza]

With a larger bit like that, if you use a small stepover, you don't really need a roughing pass, as the first pass is the only full width pass, and after that, you're only removing the stepover amount.

It depends if you're machine is capable of going the full depth of the "bowl" in one pass. If you need to take multiple passes to get to depth then it's probably better to rough with the straight bit.

If your machine can handle a full depth cut then you could probably helix in and do a 3D spiral out. But I think you'd have to lower the feedrate quite a bit as well.