First off, I'm a machinist and usually work in metal and both dislike and don't have much experience with woodworking...no flames please, just a personal preference!
I have a CNC table that I use extensively for metalworking. I got dragged into a project and volunteered to cut out some plywood countertops, no big deal I thought.
I got one sheet of plywood and cut out a few pieces, no problem, using a
1/4" x 1" wood bit, cut through 3/4" plywood at 32 inches per minute running at 18,000 rpm (5 hp motor). Must have made cuts totalling about 16 linear feet. Cuts looked beautiful.
Then I went back to home depot and got another sheet of what appears to be identical plywood (finished one side exterior) and immediately broke my bit. I put in another bit, slowed down the feed rate to 22 ipm and almost immediately broke that bit. Then I set up the machine to take 3x 1/4" depth cuts, got about 4 feet cut and broke a fourth bit.
Can somebody tell me what the heck is going one? I don't see any difference between the two sheets of plywood.
I don't have a clue why you are having problems, but a couple of observations:
1) Don't know what you are using, but you will get better results with carbide rather than HSS bits.
2) 1/4" dia is a bit skinny for this job IMHO. I'd probably use at least
1/2" dia, probably 3/4" dia bit for this job.
On Fri, 05 Dec 2003 03:28:00 GMT, "Tom Kreyche" scribbled
No flames, just some heartfelt sympathy from us generous and considerate woodworkers for your unfortunate serious affliction. :)
Don't know what could be wrong, but the tool of choice for cutting through plywood is a saw, not a router bit. What surprises me is that you managed to cut 16' without breaking the bit or burning the edge. Routers are used for edging or for short plunge cuts such as mortises. Remember that wood has different properties depending along which axis you're cutting, and different pieces of wood have different machining properties, even when they come from the same tree. Most of us have no idea at which speed we feed materials, we work by feel.
Maybe cut it out slightly oversized (1/16" or so) with any kind of saw you might have access to (hand saw, jigsaw, circular saw) and then use your CNC to clean up the cuts.
Luigi Replace "no" with "yk" for real email address
Wood isn't metal. You're used to working with materials where everything is consistent, and has very predictable characteristics.
Programming a depth of cut and a feed rate into a CNC machine is a pretty alien concept to the average woodworker. You're trying to bring digital precision to an analog world, my friend. You need to *feel* the wood.
Plywood is remarkably consistent as wood goes, but it's still wood. Those two sheets could be made from completely different trees with different growth rates, and different densities. The moisture content might vary. They might even be made of different species entirely, perhaps only on the inner plies, and you'd not likely notice the difference. Then there's all the stuff on the inside that you can only imagine. Knots, voids, wood filler, pockets of glue. It has to look good where people can see it, but utilitarian grades of plywood are not meant for making fine furniture, and they're not manufactured to the same standards.
The bottom line is if you're breaking that many bits, you're pushing them too hard.
Consider that routers normally run at 25,000 RPM or higher. Consider that you're using 1/4" bits, which are intended for the low end of the router spectrum, where 1.5 hp is a big motor.
I suspect you're turning the bit too slowly, with way too much motor behind it, and feeding too fast. Your first piece of plywood was relatively uniform, and your second one has a bunch of knots or other hidden variables buried in the plies. Maybe they're from different lots, which would increase the chance of variability between them considerably.
Maybe try punching in a much slower feed rate and/or higher RPMs the next time you program your Big Trak, depending on what you can control with that gadget.
Good thoughts and comments Silvan... As someone else mentioned, a 1/4" diameter bit is pretty fragile - a 1/2" or 3/4" diameter would be stiffer and likely longer lasting. Also a 1/2" shank over a 1/4" would be advised. His 22 inch per min feed rate seems pretty slow and a non-issue, just by pretend routing a 22" edge on my desk. I agree on speeding up the rpm's - 25K, which, with a larger diameter bit would yield a faster cutting edge speed and may help power through knots or other tough stuff in the plies.
Q for the OP: Did you notice if the breaks were happening at any consistent point with respect to area on the sheet or direction in relation to the length/width? Did you examine the sheet where the breakage occurred to see if there was any sort of internal anomoly with the material? What is the source of the bits and their configuration - one, two, four flute - solid spiral, brazed carbide - etc.?
Because you had success with the first sheet, and lacking personal experience with CNC routing of plywood, I'm hesitant to offer up commentary, but... plywood is tough on cutting edges. The glues will dull an edge much faster than solid wood as well as cause greater heat buildup of the cutter. Light passes at 1/4" max per pass at 25K rpm with a larger bit may help.
Most likely the bit is breaking because it is loading up. Increase bit speed, decrease feed rate and keep the cut area free of sawdust with good airflow. 1/4" bit is not too small for what you are doing. There can different cut characteristic from sheet to sheet in plywood.
I have a ShopBot CNC router in my garage that gets used on both plywood and HDPE plastic. I also use it to engrave equipment labels (text down to 14 point) and mill printed circuit boards, but that's another story.
I'm cutting at 21,000 RPM (nominal) with a Porter Cable 3-1/2 HP (yea ... another story there) router using both 1/4" and 1/2" inch bits. Cut speed is
3 inches per second (180 inches per minute) ... but I don't make the entire cut in one pass. Rule of thumb is to cut no more than 1.5 times bit diameter, but I seldom go over .66 times bit diameter (0.166 inch depth of cut on a 1/4" diameter bit). Yes, it takes a few more passes, but the only bit I've ever broken was the one I ran sideways into the material with the router off (oops!). I get a nice clean edge, and since the repeatability on the ShopBot is on the order of 0.005 over the entire 4' x 8' bed, I don't worry about the multiple passes. In fact, once you make the first pass, you can walk away knowing the rest will miss the clampdown bolts, parts of the machine, etc.
I get the smoothest cuts with a two-flutie, O-flute with no spiral. Up spiral really keeps the chips clear, but lifts the work off the table, and a down spiral packs chips into the cut so tightly that you're recutting the same path again and again (loading the spindle down in the process).
Sounds like you have a heavy duty spindle motor (Columbo?). Listen to determine if you're loading the spindle down when you start cutting. If you have any means of monitoring motor current, that would be more accurate than by ear. You don't want to push the bit to the point where it can't cut fast enough. Rule of thumb I was given when I started out was to achieve chip thickness of around 0.007" to 0.009"; any thicker and you're going too fast. Thinner is ok, but it just takes up more machine time.
I also have a dust collector pickup that surrounds the bit and pulls most of the waste away from the working surface. Chip clearance is important ... lacking a pickup, you could use compressed air to keep the path clear.
The ONLY burning I've ever experienced was when I tried using a "high speed steel" bit to countersink some holes in the waste board. Switched back to Carbide bits and have not had any burning. I found that Onsrud bits are pretty good ... they design the bits around the material being cut ... getting a bit specifically ground for CNC plywood cutting will help.
From a former machinist: It's not the material you're trying to cut, it's the junk bit you're cutting with.
Don't use "wood" bits. Use a quality HSS 2-flute center-cutting spiral endmill, 4-flute mills tend to clog up with sawdust. Use all the spindle speed you've got (18000RPM is way too slow) and feed at about
0.0007 per flute per rev. That would be 56 IPM @ 40000 RPM or 140 IPM @ 100000 RPM.
18000 rpms is fine, your feed rate may be too fast and the depth of cut should be no more than 3/16" deep. Use carbide tips ,or put an end mill in the machine instead of a router bit. The glue in the laminations wears out highspeed steel and carbide quickly.I am not familiar with Cnc routing although I did see it once. Is it possible that you are routing in the wrong direction? I imagine with metal it makes no difference ,but wood the cutter should chop into the wood.If you go the wrong direction ( climb cutting ) the bit will heat up quicker.
HomeOwnersHub website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.