[Enk1du]

I'm preparing to do a big job for a friend out of Plyboo. Cut my first little practice piece and it looks awful! The bit (compression bit as per the mfg. recommendation) seems to be wandering around all over the place so the edge is rough at best, and in some places its scalloped pretty badly. I'll try to attach a pic . . .

Plyboo recommended a 18k spindle speed with a 200 IPM feedrate using a 3/8" compression bit. That is alot faster than I felt comfortable with on my first try so I ramped that down to 5k spindle and 50 IPM. Also, the only compression bit I had on hand was a 1/4". I have no idea if getting a bigger bit would make the difference. The chips are not clearing the cut at all - it took me awhile to pop the part out when I was done.

Will a bigger bit and/or faster cut fix the problem?

[JerryBurks]

Oh my.....that is my favorite material. Actually my entire CNC machine (frame, gantry and z-plate) is made of bamboo plywood.

I never had trouble cutting it, although I started making the parts on my previous CNC which was a flimsy CNC-Shark.

I like it mostly because it is hard, cuts clean and super precise and leaves little or no fuzz. Normally I use an 1/8" upcut bit bit I used 1/4" as well. Never tried downcut, though and it does not sound like a good idea. Keep in mind, manufacturer's recommendations may or may not reflect practical experience.

Typical speeds were around 80-100 ipm or 150ipm for the bigger bit with 1 bit diameter cutting depth. Spindle usually 12k to 15k rpm. Except the usually smoother surface I find it cuts similar to e.g. maple.

So, I don't know what is wrong with your cuts. Maybe you got chatter with a dull bit? Or overstressed your machine rigidity?

Here is an example of some pretty precise finger joints in bamboo that I did for a bathroom sink cabinet. Even the 1/4" dowel holes are routed with the 1/8" bit.

[Dylwad]

What spindle are you using? 5k is very low for decent torque on a router, or water cooled spindle.

I think your rpm and feed were just too low, and I would try an up cut bit. If the edge finish on both sides isn't up to par, maybe rough with an up cut and finish with a compression.

[ger21]

What kind of machine do you have, and how rigid is it? How securely was the work fastened?

Looks like you had some serious deflection there, either the tool, machine, or the workpiece moving. It looks too much for tool deflection, as I think it would have snapped before the cuts got that bad.
50ipm @5000 rpm is roughly the same chipload as 200ipm @ 18,000, so you were actually cutting with nearly the chipload recommended for the 3/8" bit, which is a lot more rigid than a 1/4" compression.

I need to know more about your machine and it's capabilities to give a good recommendation.

[Enk1du]

Thanks for the responses so far.

My machine is basically a cncrouterparts machine (CRS rails, rack & pinion drive on X and Y, leadscrew on Z) with a ~3' x 5' table. The structure of the table is 80/20. Its driven by a G540 with 4x 380 oz/in steppers (two on the X axis). The spindle is a Makita RF1101 router and its hooked up to a superPID - thats how I was able to get it down to 5k rpm. The readout on the superPID display was about 5200 when I started, though I honestly didn't monitor it throughout the cutting. The table top is MDF and the workpiece is secured by hold-down clamps (from Rockler) attached to threaded inserts in the table. I'm not happy with my fastening system, but thats what I'm working with at the moment.

I'm going to give the machine a once-over to make sure everything is still tight. Upon close inspection of my test piece I noticed that the shallow pocket I cut has slightly different radius's in the two corners which is weird. Maybe its just bit deflection?

[JerryBurks]

For a sturdy 3/8" bit I doubt it is bit deflection. But reading your first post again i now see you used a compression bit not a downcut. Therefore I assume you did the full depth in one pass. Now, given the 3/4" thickness, rather wide 3/8" slot, no easy escape for the chips and the somewhat hard bamboo,...I suspect the machining forces may be pretty high. A massive pro machine will not mind but if your machine has some flexibility or slop such cuts may result and probably would come out with any hardwood.

My recommendation:
- check the machine
- take a smaller upcut bit, 1/4" or 1.8" two flute. Single o-flute is also good but may break earlier
- run faster (at least twice your previous speed)
- do one bit diameter max. depth

To establish an objective measure of rigidity it is pretty simple: install a rod or tube in the collet and clamp a dial indicator on the table with the tip against the rod. Then take a fishing or luggage scale to the collet and apply 20 or 50 pounds of side load in x and y-direction. Divide the load pounds by the indicated deflection.

If you have less than 1000 lbs/inch your machine is on the soft side especially if you have measurable backlash when loading the collet from opposite sides. Between 1000 and 10,000 lbs/inch you have a usable router. If you happen to be better than 10,000lbs/inch you are in good shape to mill some harder metals. If you have more than 100,000 lbs/inch I suspect you have something like a Bridgeport mill.

[johnjblair]

Upon reading your post I was going to tell you to ask Jerry Burks. He built a cool machine out of Bamboo called Big Bamboo. His build log is at:
http://www.cnczone.com/forums/cnc_wo...t_started.html

He has some pictures of the beautiful splinter free cuts he made in Bamboo:
http://www.cnczone.com/forums/cnc_wo...ml#post1052060

Then I saw that his was the first reply.

[Enk1du]

Plyboo recommended a 3/8" bit, but I used a 1/4" bit. Thanks for the suggestion on how to quantify rigidity - I'll see if I can get a setup like that.

edit: The worst of the cuts were at full depth. I ramped in on that main profile cut and the edge it ramped on looks a little better, but I do notice there a bit of a lip on it. I'd say something is definitely awry with my machine mechanically.

[ger21]

I's cut it in at least two passes, at 200-300ipm and 15,000-16,000 rpm. I'd use either a 3/8" downcut, or a mortise compression spiral. You need to make the first pass deeper than the upcut portion of the compression bit. A mortise compression spiral has a very short upcut portion. You can also cut one pass with a downcut, then change to an upcut for the rest of the passes.

[louieatienza]

I'm preparing to do a big job for a friend out of Plyboo. Cut my first little practice piece and it looks awful! The bit (compression bit as per the mfg. recommendation) seems to be wandering around all over the place so the edge is rough at best, and in some places its scalloped pretty badly. I'll try to attach a pic . . .

Plyboo recommended a 18k spindle speed with a 200 IPM feedrate using a 3/8" compression bit. That is alot faster than I felt comfortable with on my first try so I ramped that down to 5k spindle and 50 IPM. Also, the only compression bit I had on hand was a 1/4". I have no idea if getting a bigger bit would make the difference. The chips are not clearing the cut at all - it took me awhile to pop the part out when I was done.

Will a bigger bit and/or faster cut fix the problem?

How many edges do you have on your compression bit? Using Onsrud's charts, they recommend a chipload of .014"-.016" per flute. So with a single-edge compression that equates to 252-288ipm at 1/4" doc. If you have 2 flutes you have to DOUBLE those speeds, or cut the spindle speed in half, both things that may not be too desirable for your machine. Like Gerry mentioned, I'd use a mortise compression spiral (I believe the upcut portion is .180" or so, so 1/4" doc should be fine. If this doesn't help then you may have to either lower the feed (maybe 200ipm) or increase the spindle speed to make the chipload slightly smaller. The shortest 1/4" compression spiral has a 7/8" cut length, and I would use that, as keeping the collet as close to the work is always best.

[nlancaster]

I had an affect like the cut piece in the OP. Happened to me because my machine was moving around ont he bearings. Because I had not tightened them enough on my JoesCNC2006. If your machine is wobbly at all it would do exactly what you are seeing.

[Enk1du]

Hey folks, just an update. I reset the bearing blocks on my x-axis (and realigned the x-axis rails at the same time), and also tightened the z-axis blocks. I had found both to be slightly loose. The y-axis seemed fine. Using JerryBurks suggestion for measuring rigidity, I got ~2500 lb/in before and ~3000 lb/in after so that was some improvement. I also switched to trying 2 and 3 passes for subsequent tests and that seems to have been what I needed to get a good finish. All this extra scrutiny has uncovered another issue though, which is a slight sagging of the router head which causes a slight lip on the gantry side of the cut. I'm assuming that I just need to find a way to shim the bottom of the spindle mount out a little. Alignment of the z-axis is otherwise perfect - its sagging in the x direction but is straight in the y direction, if that makes sense.

Anyway I want to thank everyone for the good advice.

Oh one last thing. Given what I've seen using this 1/4" shank compression bit, would it be better or worse for me to try a 3/8" instead? I'm inclined to stick with the 1/4" when I order up some extras, but I'm interested if anyone has an opinion on the pros/cons of switching. Thanks!

[louieatienza]

Hey folks, just an update. I reset the bearing blocks on my x-axis (and realigned the x-axis rails at the same time), and also tightened the z-axis blocks. I had found both to be slightly loose. The y-axis seemed fine. Using JerryBurks suggestion for measuring rigidity, I got ~2500 lb/in before and ~3000 lb/in after so that was some improvement. I also switched to trying 2 and 3 passes for subsequent tests and that seems to have been what I needed to get a good finish. All this extra scrutiny has uncovered another issue though, which is a slight sagging of the router head which causes a slight lip on the gantry side of the cut. I'm assuming that I just need to find a way to shim the bottom of the spindle mount out a little. Alignment of the z-axis is otherwise perfect - its sagging in the x direction but is straight in the y direction, if that makes sense.

Anyway I want to thank everyone for the good advice.

Oh one last thing. Given what I've seen using this 1/4" shank compression bit, would it be better or worse for me to try a 3/8" instead? I'm inclined to stick with the 1/4" when I order up some extras, but I'm interested if anyone has an opinion on the pros/cons of switching. Thanks!

The 3/8" may require a higher chipload, and your spindle would need to able to handle it. There are calculations in Onsrud's catalogs (check the metal tools one) for calculating the horsepower needed for a certain material removal rate. Routers are rated for peak HP so the actual HP can be a lot less. You may find you need to take shallower passes with the 3/8" and if the upcut portion is not below the suurface youu may end up splintering the top edge. I would use a single flute compression 1/4"...

[JerryBurks]

.......Oh one last thing. Given what I've seen using this 1/4" shank compression bit, would it be better or worse for me to try a 3/8" instead? I'm inclined to stick with the 1/4" when I order up some extras, but I'm interested if anyone has an opinion on the pros/cons of switching. Thanks!

I would keep the 1/4" bit. The forces of the 3/8" bit will be higher and you may get some of the waviness back.

However, I use 1/4" or bigger only for pockets. I cut slots in bamboo usually with a small 1/8" upcut bit and prefer a Kyocera with 22mm long 2-flute and fishtail end (100-120ipm and 12-15krpm, 1/8" deep). In spite of the upcut flutes, it does not make a lot of tear-out. The little fuzz can usually be scraped off with a fingernail or a sanding sponge. That said, the heat treated brownish bamboo is more finicky and weaker than straw colored natural bamboo sheet. I tried downcut bits lately and, while it cut about as well as the upcut one I needed an awl to scrape the compressed chips out of the corners.

[Enk1du]

I just wanted to post an update on the Plyboo cutting job I've been working on. The last two sheets will be going through the machine today. Its been an epic project: 20+ sheets of plyboo and 15+ sheets of baltic birch. Since my cutting bed isn't big enough for a full sheet (who's is though) each one has to be ripped lengthwise, and then run in two sections with a couple feet hanging out over the edge of the table. I might post some pics if I find any good ones.

The compression bits wore pretty well IMO, especially since we weren't cutting full depth - the first 0.27" of the cutter was doing almost all of the work. I ended up increasing the spindle/IPM ratio from the recommended speeds because there seemed to be some chatter or something going on, but the 10k RPM 70 IPM setting we settled on worked well. In the end we only used 4 bits.