Ok, I've got a C-Beam XL that is fairly stock, except for I did opt for the high torque motors when I bought it and have a BlackBox controller. I'm using a dewalt router (DW618) for a bit more power, especially at lower speeds (unloaded low end about 8400RPM). In addition to the 1/2 and 1/4 inch collets I also have 1/8" and 6mm to give some more flexibility (and a stock of 1/8" single flute cheap chinese carbide cutters). A spindle might be in the future, but this is located in an unheated garage so I'd need to set up an antifreeze based cooling system. This has been a tinker project for awhile but was put aside and now I'm getting back to it in a big way as I have some immediate needs supporting a high school robotics team. As such, I'd really appreciate some basic guidance on feeds and speeds people are using to cut down on my development time in different materials. We're using Fusion 360 to handle the CAM, and using the OpenCAM sender for blackbox. Our need is to identify max travel/cut speeds for each material to populate Fusion, plus specific recommendations for different types of cuts in the following materials. I'm assuming the polycarbonate and aluminum will all be using 1/8" bits. 1. 3mm and 6mm hobby plywood (prototyping) 2. 2mm and 3mm polycarbonate 3. 0.125in 6061 aluminum sheet 4. General thoughts on wood 3D cutting with a tapered ballnose (just for fun/decorations). For most of the above, its for making flat parts so basically cutouts and through-holes for screws (basically for 4mm bolts). But getting into Fusion, it's all about stepdown, stepover, plunge rate, ramp rate, RPM, etc and it's a bit of a steep learning curve. So I'm hoping the community can give me some reasonable starting points. Heck, even giving me profiles you're already using or exported tool libraries would be greatly appreciated BTW: I've watched a ton of the NYC-CNC videos, Shapoko stuff, reading threads here, so I'm familiar with how to approach the problem, but I'm drowning in options and looking for a safe starting point from wiser people. Edit 2: One item I forgot to ask. We might be interested in making a steel flywheel (100mm diameter). Any chance of cutting a 1/2" thick round out of flat stock, even if it takes hours? I could set up a mister. What type of steel would be best? 303SS? Hot rolled? Too many alloys. Thanks in advance!
For reference I use the 1 1/4 HP Makita. I do not cut a lot of polycarbonate, so I am not of much help there. Plywood and other woods are pretty easy. My depth of cut is usually 1/2 the diameter of the endmill at 2500mm/min feed speed. I plunge into wood at 1000mm/min. For 3D reliefs in wood, I am using a 1/4" 2 flute ball end mill for roughing at 5000mm/min, 1000mm/min plunge, 3.5mm DOC and a 40% stepover. I use a 2 flute 1/8" ball end mill at 10% stepover with 1.587mm DOC, 4500 mm/min and plunge of 1500mm/min. For the rpms of my router, I manually set it depending on how the cut "sounds" between 18000 and 22000 range. For aluminum, unless you need to use a 1/8" endmill I would not. You can cut deeper, faster, and with a better finish with a 6mm or 6.35mm. Using a 2 flute 6.35 mm endmill I can easily cut aluminum at 900mm/min with a 500mm plunge rate and 6 degree ramp. My depth of cut is 1mm. I have accidentally cut the full 1/4 full depth plus some of the spoil board of aluminum when I forgot to re-zero the Z between tool changes. This is not recommended. The cut was not accurate due to machine flex. I may try pushing it to 2 mm depth of cut to see, but on the hobby grade machines, you start getting inaccurate cuts due to the flexing of the frame. Although, not perfect, I get a decent clean cut with these settings. If the holes are smaller than 7mm in aluminum, I do a helical drilling tool path with either a 3/16" or a 4 mm endmill. The feed rate is 800mm/min and a plunge of about 300m/min with a 6 degree ramp. As you can see, I avoid a 1/8" end mill if at all possible. The flex too much and I have to cut too slow. I started with this resource then dialed it in for my machine: Speeds and feeds
Thanks, what machine are you using for these? What about travel speeds? Basically anything that doesn't skip steps (e.g., dial it up to 11 then back off until reliable)? Also thanks for the pointer to the table. I had seen that a long time ago and was a bit confused about it since it didn't reference anything about the cutter geometry. I see now he's referring to a 1/4" cutter although he doesn't mention type or flute count. I definitely appreciate the speeds for aluminum. I'll give it a shot tomorrow and see what I can get. I might have to order a 1/4" endmill as all my other 1/4" stuff are more wood router type bits, not endmills, so wrong geometry. What about drilling for smaller holes? Just use a spotting bit to divot the right places and then finish on the drill press? For the 4mm holes I wonder if a spiral with a 1/8" bit would work? I wouldn't be able to leave any stock so it would be a single pass cut with no cleanup.
The machine I am using is one I made based on the Ox before all the kits came out. ACME OX (A Lead Screw Driven Ox Derivative (850x1500)) For smaller holes I do use a 1/8" inch endmill. As for travel speeds, I do not know and have not looked at my settings in quite some time. I believe it may be 5000mm/min, but most stuff I cut is not very large so it is never getting up to that speed.
