I've got a big project coming up that will require cutting lots of 3/4" plywood. I'd prefer to do full depth cuts because I'm already expecting about 36 hours of cnc run time. However, I haven't made full 3/4" deep single pass cuts before. Could someone recommend an appropriate router or spindle (horsepower), bit type/size and feeds and speeds? I'll be running NEMA 32 steppers on lead screws. Do you think that will be sufficient? Thanks!
Strategy: often, more shallow passes (less deflection, less risk, higher yield, etc) at a much higher feedrate, results in a faster total job, than running slow enough to do full depth cut, even with trochoidal strategies. Experiment and see if you can optimise that way For example: 2 passes at 800mm/min (effectively 400mm/min) Vs 4 passes at half the depth of the other one, but can push it to 2000mm/min (effectively 500mm/min) because the loads are lower Bigger endmills make bigger chips, so go as big as you can
Deep of cut is usually 1/2 the size of bit. Most trim routers can't accept router bits with 1/2" shank. On a scrap piece of plywood, try 1/4" bit with three passes. If it doesn't work, try four passes.
Thanks guys. I'm not running trim routers I currently have a Bosch 1617 2-1/4HP installed, and could easily go up to the MRF23EVS 3-1/2HP router. I would also be willing to consider an inexpensive spindle if that's really what I need to increase speed. Does that change either of your advice?
The simple answer is 'no'. You will not be happy if you will cut the plywood in one pass. Besides the bad finish you may have all what Peter said about the speed.
Nothing to do with the spindle: all about loads on the bit and loads on the frame: How to calculate V-Slot® deflection
Even when the frame can handle it, high speed strategies tend to win out against high torque strategies regardless. At that point it's mostly about spindle top speed to generate true chips vs rubbing and dust.
The short answer on ANY cnc machine is, shallow passes at higher feed rates wins the day. Others have already said this to you here, but I can attest that going too deep, too fast, even with high end bits on a big machine, is always a bad idea. Common rule at our workshop is "the tortoise beats the hare". Stick to not going over 1/3 the diameter of the bit for a pass depth on any project, the feed rate can always be adjusted (faster or slower) as needed while running the cut. To me it boils down to how the cut operation sounds. A high pitch whine isn't usually a good thing and is often followed by the sound of the bit breaking. A low pitch, or heavy "thumping" noise is bad too, you can probably smell the bit burning up if you let it go. Its all about how well the bit itself can clear the chips and material in front of it. Different bits can go faster than others, but all of them should never go deeper than 1/2 their diameter in any material. For 3/4" plywood a spiral "O" flute bit (1/4" diameter) with a pass depth of .12" at 80 to 150 ipm will give a fast cut and keep the bit from burning up.
Thanks for the advice everyone. Hoping to do some sample pieces this week. I'll let you know how it goes.
Hi, I have to disagree with the general flow of replies you've received so far. I routinely cut 19mm (3/4") plywood in a single pass. This is entirely possible if you use Trochoidal milling. I have cut 3/4" plywood with a 3mm (1/8") bit on a standard Makita router, but a 6mm bit clears chips better. My settings: 6mm 2 flute upcut bit Makita speed 4 to 4.5 (listen to the router to find a happy speed) CAM: Estlcam - settings: 20% width, 40% stepover, feedrate 3600mm/min, final pass 1mm The final pass might seem excessive, but all it is doing is cutting away the little "ripples" left by the successive cuts of the bit. The finish is stunning. Estlcam is a $59 CAM program, so if your CAM program of choice doesn't do Trochoidal milling, give it a go. Regards, Duncan
Is that translational linear, or the feedrate that runs the trochoidal? (ie the speed at which it draws the loops, thus proportionally slower linear feedrate) While it is true that trochoidal is better for tool wear, and HSM strategies, that mostly holds true on very rigid machines
Thanks for the opinion Duncan. I still feel that it is possible....with the right set up. This is exclusively how professional millwork shops cut out cabinet parts. However, they definitely use larger/stronger machines that I currently have. I want to cut parts out of a sheet of plywood. So I'm hoping for full width cuts, following a profile. Do you have experience with that? Correct me if I'm wrong, but isn't trochoidal milling mainly for pocketing? I'm using cambam and would prefer to stick with it. There is a beta trochoidal mode, but I haven't really tested it out yet.
High-speed strategies don't preclude high-DOC operations- more to do with WOC/chipload than anything- but having done trochoidal slotting (as I'm assuming is the case here for outlining plywood panel sections) in aluminum to protect 1/16" end mills, I don't know that forward progress is fast enough to significantly differ from multi-depth operations overall, and the higher MRR you can usually get with by putting more power into short cutting edge/stubby cutters may tilt the scale the other way. It'd be interesting to see an A/B test on the same machine though, that's for sure.
Hi guys I'm new here but not brand new to CNC (hi Duncan!) but to the op's question why is it that you want full depth cuts? Is it just to say I did full depth passes or are you trying to save time, improve cutting results or something like that. If you're just trying to cut down time then you should be indifferent to feedrates and DOC and be objectively looking at the outputs of the machine, and the machining time. I think you're on the right path with the idea of reducing passes but like other's mentioned it's the combination of feedrates and doc that determines the total. Mock it up in your cam, it'll get you most of the way there without actual cutting.
Hi Banjopete, I'm cutting half sheets of 19mm ply in order to get a one-piece fuselage airframe (well, actually two pieces, because I join the front and back halves). Doing it this way gets rid of every epoxy join (except the join in the middle), so it looks great and there is no danger of poor bonds. It also results in extremely accurate dimensions and it cuts down build time hugely for any prospective builder. The problem is, I can't easily get to the rear of the table to clear out the chips. Even though I have a Makita router which blows downwards quite strongly, and a shop vac trying to clear the debris, I have to clear the chips by hand. Multiple passes compounds the issue. My "solution" was to cut the plywood in a single pass with Trochoidal milling and simply ignore the debris. Works well. Question: I was taught that cutting through the previous pass' debris was extremely bad practise, and could result in the bit loosening and coming out of the chuck. I never understood this, but I live in fear of my bit working loose and ruining my job (and a $270 piece of plywood). Any comments on this? If ploughing through previous passes' chips is only inefficient and the "working the bit loose" is an urban myth, I might give straight milling a go with multiple passes. Duncan
Nearly all jobs save the thinner stuff will be multiple pass jobs, it's nearly unavoidable and for 19mm ply I wouldn't be trying to do it in one shot anyways. I've not heard of bit loosening because of sawdust in the tool path but I'd be very surprised if this was the only cause of such a problem. Upcut bits will certainly help clear those chips out, and perhaps a modified vacuum setup would improve things at the hard to reach end of your table too. You can certainly to a dull depth finishing pass on your pieces to clean up the edges but it sound like a doc in the 5-7mm might get you farther. Like you I'm coming out of the v1 lr2 so don't have a good grasp on the feedrates for these openbuilds machines yet as I don't have one (any day now once ups gets here!).
Hi Banjopete, (Do you play banjo, BYW?) Well, I took your advice, and cut the 2nd side of the airframe as follows: Six passes, but at 2540mm/min, it didn't take too long! Cut beautifully. I have to say, I was very nervous, and ready with choice expletives directed in your direction if it went pear-shaped. But I was really impressed. I honestly think I was fed a bum steer about the bit working loose if it cut through previous passes junk. The downdraft of the Makita does a reasonably good job of clearing out the channel anyway. I don't currently have a single flute bit, but have a few on order. I bought one of those fancy clear perspex dust boots, but didn't specify the diameter of the spindle, so I gor the 85mm diam version, and I can't use it. The Makita is 65mm. I have to work out a way to shim the Makita to fir the dust boot. Bugger. I have more sawdust and wood chips on my desk than I can keep up with, so I need to find a suitable dust shoes. Quickly. Thanks for the advice. Duncan
Great to hear, and happy no expletives my way were necessary. Should be easy enough to create a shim for the dust boot with your cnc I imagine a flanged spacer and a hose clamp or something would cover the job well. Good luck, and no, no banjo, it's just a play on my initials for a long running username.
