Getting straight into the specifics now I see
I would recommend reading this article about the chip-load from CNC cookbook for more background on the concept of chip-load when you have some time, then consult this article about end-mills from Make magazine if you want more helpful diagrams and descriptions, and lastly when you’ve got some serious reading time, dig into Michal Zalewski’s excellent treatment on hobby CNC and resin casting.
You’ll have many questions answered you didn’t even know you would have, as you go about learning this stuff
Ok, to answer your questions:
- Should you try slower speeds? Possibly. More importantly, the “tollbooth” wizard probably isn’t optimized for your material and the stiffness limitations of the Nomad, just some fine-tuning to do there probably. Also, there’s a fair bit of difference between different woods, and as soon as you hit a knot all bets are off. Check out the Janka hardness scale, and also this bit about guesstimating feeds based on it, as well as running your own sweet-spot tests based on the wood you’re trying to cut with a given tool.
In your case, instead of just reducing speed as a first-step, I’d be inclined to reduce your step-over. When you have the tool trying to turn a corner and then “plough-cut” through that much material without any momentum, that’s more likely to overload the steppers than if you keep a greater depth and maximum speed, and just take 1/2 to 2/3 of your tool’s width per pass. Try it, and see if it works better for you.
As one tertiary thought, you may want to try setting it only to climb milling rather than “use parallel path” for your roughing pass if you’re cutting soft wood, or just conventional milling if you’re in a particularly hard wood. I say this because in climb milling the tooth is engaging the most material at the beginning (which will take a bite out of softer wood that would otherwise want to yield and rub instead of getting cut) and conventional milling engages the most material at the end of the cut, so it induces less vibration in the tool and work piece as it cuts. Your mileage may vary, it may help or may not matter depending on your wood, fixturing, etc.
- Should you set up your own custom tools with suggested settings instead of using the wizard? Yes, and no. You should be figuring out what works with your available tooling in your available materials, and making note of it, but you may not want to make different “tools” for each different material, instead just get used to entering different values into MeshCAM to get the desired results in each material with the base tool definitions you have.
So basically, create a spreadsheet that is divided up per tool and per material, and note what’s working well and what needs tweaking, after you look online and find good starting points like these Onsrud tables for their tooling.
I use Fusion360 which has HSMworks embedded in it for much of my work, so my tool library looks like this:
Individual tools have a lot of different details that I’ve programmed in:
And I’ve created a holder profile to approximate the ER11 collet nut, so when it simulates toolpaths it takes into account the holder so I don’t bottom it out into anything:
But, even with all that pre-programmed in, I still end up adjusting feeds and speeds based on the ideal chip-load in the material with a given cutter. If you dig around on the internet you’ll find tables like this one that give general recommendations for starting points on different materials.
Acrylic, Aluminum, and Hardwoods are all within-range with 0.004" chip-loads, which at 5krpm and a 2-flute cutter works out to 40 ipm feedrate.
The settings given in the toolpath wizard would put the chip load at 0.0068" per tooth, assuming 5krpm. That’s a bit high for all three of those materials with a 1/8" tool, but would be better (but not quite enough) for a 1/4" tool.
As for depth per pass, machinists with bigger equipment generally try to get a 1x diameter depth when plough-cutting at rated chip-load, and feed is reduced by 25% for 2x diameter, or reduced by 50% for 3x diameter.
Since our machine is belt-driven and isn’t that rigid, I would recommend starting at 0.5x diameter for depth in most materials, with 1x diameter being the goal for roughing passes. I generally leave 0.005" to 0.01" of material to remove with the finish-passes—more for softer materials (Poplar, Acetal), and less on harder ones (aluminum).
I’ve used both tape and glue, and the tape works well as long as the materials are non-porous/minimally porous and clean—free from oils/moisture and dust, and you’re not cutting too aggressively where you’re going to pull the work-piece up.
In order to ease part removal when working with the glue, you want to apply a thin bead around the edge of your block of stock material, not under the middle, because you want to be able to apply a bit of rubbing alcohol after a job to it to get it to release—I haven’t looked into why rubbing alcohol makes the hot-glue release, but it does as long as it’s wetted. Once the alcohol evaporates the glue returns to full-tack strength if you haven’t removed the piece fully yet.
Tape should work well for plexiglass, especially if you’ve got a nice clean spoil-board to tape to, and don’t make your cut-depth to great. Try pressing and holding the tape for 10-15 seconds before letting up, to make sure you’ve really make a good connection between the tape, work-piece, and spoil board.
Alright, I have to get back to some actual work, so good luck!