First experiments in CNC

[Zekromtor]

Hmm that might be pretty useful then. Apparently you can melt up your own machinable wax with just paraffin and plastic bags/LDPE. I feel like my IQ decreases every time I get a sniff of melting plastic though, so I won't be trying that.

[matt3o]

Hmm that might be pretty useful then. Apparently you can melt up your own machinable wax with just paraffin and plastic bags/LDPE. I feel like my IQ decreases every time I get a sniff of melting plastic though, so I won't be trying that.

I tried that, it's not something I can regularly do at my place (ie: fumes and angry neighbors)

[Muirium]

Neighbours fumes sure make me angry…

[jacobolus]

the bit is 2 flute.

as you probably know each machine requires different values.

1000mmpm is approx 40 IPM. I believe 90 IPM is too fast if you need to do small details, but good enough for large areas. My spindle is 800w/24k and I tend to always keep it under 18k.

1.5mm is probably too much as depth of cut but the bit was brand new and sharp as it could be. 0.5mm (0.02") is really too small imho, I cut aluminum at 0.5mm, but you run your mill way faster so it makes sense.

The spindle speed/feed rate to use depends dramatically on the cutter you’re using, the material, the horsepower of your machine and how rigid it is, what kind of surface finish you’re looking for (vs. how fast you want to push things vs. how long you want your cutters to last; go too fast or too slow and tool life is greatly reduced), how deep your cut is, and how much stepover you have.

“High speed machining” has really changed CNC milling in the last 15–20 years, as far as I can tell.. basically by avoiding any sharp corners and using a small stepover (like 15% of the cutter diameter or something) but full depth (even 2–3x the cutter diameter), you can cut much faster overall than if you run the cutter with a large stepover and do many shallow layers of cut. The only thing is you need fancier software to calculate the proper cut paths.

Even with a more “traditional” cut path though, it’s a bit tricky to calculate the proper “feeds and speeds”. I recommend trying out one of the feed/speed calculator programs floating around, e.g. http://www.cnccookbook.com.

(Take this all with a grain of salt: I’m still also a newbie here.)

[matt3o]

so far I'm trusting my guts and my ear. I've seen those guides but most don't take into account the fact that I have a hobby machine. I can't run my spindle at 25k and if I push the motors too hard I lose precision. So I mostly trust my gut and do a lot of trial and error

[jacobolus]

That software actually lets you dial in the horsepower and range of spindle speeds of your machine, and gives you some idea of the deflection the cutter will experience under particular conditions. It even lets you pick a maximum acceptable deflection and then optimize other parameters based on that.

Anyway, do try to make sure that each flute of your cutter is getting enough material to be making chips and not just rubbing. If your feed rate is too low for a particular spindle speed you’ll dramatically reduce the life of the cutter. (One way to find this out is by feeling the bit after making a cut [and stopping the spindle of course]; it shouldn’t get hot.)

Trial and error sounds good too.

[matt3o]

don't get me wrong. I know nothing about CNC, you shouldn't follow my suggestions and I appreciate your input, I really do. I wish someone guided me the first days. I followed some threads on CNCZone but it seems you get 11 different opinions by 10 different people. The idea is that the pro-machinists hates you (hobbyist). They don't want you around, you are not worthy... but I might be wrong.

There seems to be so many variables. The bit quality also. I have bits bought at $10 for 10 and I have a bit that alone costs $30. I can probably cut at double the speed with the good one.

[Zekromtor]

If you want to post on CNCzone and not get snubbed, you better quit calling them bits

I've had good luck with Niagara, YG, and Precision Twist end mills. I'm still in the process of evaluating Richards Micro and Lakeshore carbide to see if they are any better/worse. I've had some really bad chinese end mills that you wouldn't want to cut a piece of scrap with.


You obviously have a good grip on it already, but there's one concept I wish I learned earlier, SFM. There are two factors that are incredibly important: Surface speed (often SFM) and tooth feed (ipt/fpt/ipr). Tooth feed is obvious, it's how much each flute cuts and can be determined by your number of flutes, RPM, and rate of feed. SFM is often misunderstood. It's the speed of the tooth when it actually makes contact with the material and is based on cutter diameter * RPM. Different materials and cutters want different SFM. Things get less than perfect when your using more than the outside edge of your cutter, such as when drilling or chamfering, because the SFM decreases dramatically as you move toward the center axis of the cutter, effectively reducing the diameter to near 0 in some cases. For this reason, if you decide to chamfer, especially plastics, try to use the portion of the cutter as close to the outer diameter as possible, since the tip's SFM is so low and can ruin your finish.

[Zekromtor]

Here's a visual


The very same thing obviously applies to ball mills, which is why I try to avoid them when working in soft materials like acrylic. You are likely to get a better finish doing small steps with a square end mill like I did with the sharkskin key caps than with a ball mill.

[matt3o]

first experiment with keycaps



I made (again) some little errors but I'm getting there. The surface needs to be hand sanded (Zekromtor, any suggestion to get a smooth surface?)

Thanks Zekromtor for all the info. I have a vague understanding of the SFM concept, but I really need to dig deeper into the theory. So far I'm just learning by trial and error.

Can I ask you what CAM software you use? (ps: I call them drill bits so people here understand what we are talking about)

PS: also poplar is not probably the best wood for CNC, have to try others.

[Muirium]

Not bad for a first shot. How did you model the DSA profile? Did you use your work on the Granite renders or did you use the machine to measure a real cap?

[Nuum]

Looks nice, have you sanded it or is this directly out of the machine. I reckon you sanded it, the surface looks good. Does it fit well on a MX stem?

[matt3o]

Not bad for a first shot. How did you model the DSA profile? Did you use your work on the Granite renders or did you use the machine to measure a real cap?

no the model is new. this one is (almost) a 1:1 replica of a DSA cap.

Looks nice, have you sanded it or is this directly out of the machine. I reckon you sanded it, the surface looks good. Does it fit well on a MX stem?

no this is not post-processed in any way. I just removed some wood filaments/left overs. The key fits very well but maybe the wood stem is a bit fragile, I have to find a way to make it stronger.

[Zekromtor]

Most people use the top edge of a ball mill to do the stepped profiles to get closer to the desired shape and have less to hand sand. It can work well with wood since it's a bit more forgiving than plastic. What did you do? It looks incredibly smooth already for not having been sanded.

I use Sprutcam which is the best bang for your buck when doing live 4th axis stuff, but even that is rather pricey at $1k and it has it's fair share of issues that will make you want to pull your hair out. I don't recommend it for a 3 axis machine due to the bugs. What CAM are you using now?

[matt3o]

Most people use the top edge of a ball mill to do the stepped profiles to get closer to the desired shape and have less to hand sand. It can work well with wood since it's a bit more forgiving than plastic. What did you do? It looks incredibly smooth already for not having been sanded.

I used a 3mm end mill for roughing and a 2.5mm ball mill for finishing (there are no details I could have used a 3mm ball mill probably). I believe I can get a better result playing with step-overs. Also probably I could leave a little more stock from the roughing phase.

I use Sprutcam which is the best bang for your buck when doing live 4th axis stuff, but even that is rather pricey at $1k and it has it's fair share of issues that will make you want to pull your hair out. I don't recommend it for a 3 axis machine due to the bugs. What CAM are you using now?

I'm still trying cambam and meshcam. They are the few CAM softwares I can afford at the moment This keycap comes from meshcam. Since I use Rhino I also tried Madcam which doesn't seem too bad, but a bit pricey for my pockets. I'll also give pyCAM and heekscnc a shot, they are open source but they look pretty nice.

[jacobolus]

I used a 3mm end mill for roughing and a 2.5mm ball mill for finishing (there are no details I could have used a 3mm ball mill probably). I believe I can get a better result playing with step-overs. Also probably I could leave a little more stock from the roughing phase.

How long does it take to cut one keycap with that 2.5mm ball for finishing?

(I plan to use a 1/4" ball = 6.35mm for sculpting keycaps, because there are no sharply concave features, so it should hopefully result in better finish and a much faster cut)

[Eszett]

@matt30 Ever considered to get advice from the element14 community and Mr. Heck:

[matt3o]

I used a 3mm end mill for roughing and a 2.5mm ball mill for finishing (there are no details I could have used a 3mm ball mill probably). I believe I can get a better result playing with step-overs. Also probably I could leave a little more stock from the roughing phase.

How long does it take to cut one keycap with that 2.5mm ball for finishing?

(I plan to use a 1/4" ball = 6.35mm for sculpting keycaps, because there are no sharply concave features, so it should hopefully result in better finish and a much faster cut)

from the simulator 6mm was not working very well, so I went for 3mm (but probably your cam software is better than mine). It just takes 12 minutes overall so not a big deal. Like I said I should have used a bigger head for finishing, but I'm still learning and it didn't come out that bad after all.

[jacobolus]

It takes 12 minutes to do one 1x1 keycap? Eek. We should definitely be able to do it faster than that. I’d hope at least 10x faster.

I am not planning to use any CAM software [too steep a learning curve to make them do anything interesting; too inflexible; too expensive], but just making the cut paths with a python script.

Having read a bit more about this online and thought about it a bit, I think the best bet for cutting the very top part of keycaps (whether cylindrical or spherical, the tops are still fairly flat) is to cut them at an angle (30° is probably enough I think). Otherwise, the problem is that the very tip of a ball end cutter near the axis doesn’t have much motion in its rotation: it’s spinning in place. Which prevents it from working super well. But if the part of the cutter contacting the surface is at a 30° angle, then that gets us all the way to 1/2 the diameter of the ball [because sin(30°) = 1/2].

Cutting the sides of the keycap will then have to be done in a standard flat orientation, so this gets slightly more complicated, because it requires moving and re-fixing the material to the table. But I think there’ll be enough advantage in cutting speed, tool life, and surface finish to be worth it. And anyway, one change of orientation is already necessary to cut both the top and the bottom of the keycap.

I’m going to try to build a little jig to securely a piece of wood down to the router table at an angle.

I think the best way might be to cut the wood to be turned into keycaps into several thin strips, like 3/4" wide by 1/2" tall by however long (12"?). Then make two jigs to hold all the strips: one that holds them each at a 30° (or maybe 45°) angle for sculpting the tops, and another that holds them all flat for sculpting the sides / cutting out the bottoms.

I think it can be done with 3 changes of work holding, plus one additional tool change, at least for Alps keycaps. Might take one additional tool change for MX caps, since their stems are much sillier complicated shape.

1. put material in flat jig upside-down, cut out keycap bottoms using a 1/8" end mill. (this takes a deeper-than-standard cutter, maybe 1/2" long?)
2. flip the material over still in the flat jig, and do the 'roughing' pass for the sculpted top of the keycap. Could use the same 1/8" end mill probably.
3. change to a 1/4" ball end bit and do a finish pass for the sides of the keycaps and the outside edge of the top; Depending on the keycap geometry it might be a lot faster (even with the additional tool change) to use a chamfer cutter to finish the sides here
4. put the material into the angled jig, and still using the 1/4" ball end bit do a finish pass for the keycap top

It might be easiest even to build both the flat jig and the tilted jig into one unit, assuming it could be made accurate/precise enough. Then it could be fixed down to the table, and some unmoving part of it could be used for zeroing the Z axis on each tool change.

[matt3o]

It takes 12 minutes to do one 1x1 keycap? Eek. We should definitely be able to do it faster than that. I’d hope at least 10x faster.

if you do more than one at a time it takes less time.

I am not planning to use any CAM software [too steep a learning curve to make them do anything interesting; too inflexible; too expensive], but just making the cut paths with a python script.

you are flying way over my head I do not intend to do mass production. If I can make 20 keycaps in an hour I would be quite happy.

The finishing in the inside of the keycap must be very slow because the end mill is small (<1mm) and the stem fragile. I will probably push the CNC faster on the top, but I don't think with my hardware I can go faster than 6-9 minutes (for 1 keycap; 4-5 minutes inside, 2-3 minutes for the top without legend).

My setup is:

1) carve just the inside of the keycap with 3mm end mill.
2) carve the stem with a 1mm bit
3) flip the stock and do a roughing with 3mm
4) change bit with ball mill and finish

maybe you can merge 3 and 4 and just to the finishing with a 3mm ball mill. I don't know. Have to try

Again if you make say 10-20 keycaps at a time of course it would be way faster.

[jacobolus]

If you’re doing a bunch of keycaps at once, maybe using a 1.5mm (or 1/16") drill bit to drill the center of the cross for each stem would speed you up somewhat. You should be able to plunge a lot better with a drill than with a very skinny end mill.

[matt3o]

yeah if you do many caps at a time it might be worth. have to check what's the max bit diameter I can use.

[jacobolus]

yeah if you do many caps at a time it might be worth. have to check what's the max bit diameter I can use.

Max diameter you can use in the center would be the width of one of the cross arms * sqrt(2). So up to about 1.6mm or 1/16".

I have no idea how accurate it is, but this feed rate calculator suggests that for a 1mm thick end mill, cutting a slot (i.e. maximum possible tool engagement) at a full depth of 4mm, you can set the spindle speed as high as you’re able (18000 RPM or whatever) and then do something like .0002 IPT ("inches per tooth"; or .005 mm/tooth), so at 18k RPM that would be 182.9 mm/min.. go any faster and you start getting a lot of cutter deflection. (I’d probably test starting a bit more conservatively than that and then work up.)

At that speed, it shouldn’t take *too* long to cut out a little cruciform with four 2mm long arms. Like 10 seconds or something, assuming each arm of the cross requires moving out to the end and back.

[matt3o]

rhino says that indeed the clearance in the middle of the stem is 1.5mm. now the problem is that I don't have a 1.5mm collet, neither a 1.5mm drill bit with a bigger shank size

but now that I think of it, maybe it is better to have the stem done alone (not together with the finishing phase)... so the bit never exits the stem area. More testing's required.

[Zekromtor]

If you’re doing a bunch of keycaps at once, maybe using a 1.5mm (or 1/16") drill bit to drill the center of the cross for each stem would speed you up somewhat. You should be able to plunge a lot better with a drill than with a very skinny end mill.

This is something that people like to do with metal, but for wood I'd avoid it like the plague. Any natural stock with variations in hardness absolutely plays havoc with thin diameter drill bits. They end up following grain patterns and walking way off target. Anything <1/4" you should use end mills over drill bits when it comes to wood. Even in metal it may not be advisable at the smallest diameters.

[matt3o]

like I said: nobody agrees on CNC setups

[matt3o]

I made a second test with documentary video

This is the RAW top, still not finished!



I believe that is the kanji for "wood".

Unfortunately I made an error in the bottom set up and it came out pretty rough. Final version will be polished.

So, what I've learned so far:

- you can go pretty fast on wood and also use incredibly small bits (0.2mm), but if you want a nice surface you need a lot of finishing passes.
- poplar is not probably good for small detailed pieces
- I can probably make 50 keycaps in approx 30 minutes, the most time is spent changing bits and and fixing the stock to the table
- the finishing phase (sanding, varnishing, ...) takes quite some time but it's pretty enjoyable.
- you can carve basically anything (both depressed and embossed)

[acolombo]

Finally a video of the machine in action That's awesome.

Also, to me, it's surprisingly fast. The video looked like it was speed up.

And the result keycap is really really cool!

[beltet]

I made a second test with documentary video

Spoiler:

This is the RAW top, still not finished!

Spoiler:

I believe that is the kanji for "wood".

Unfortunately I made an error in the bottom set up and it came out pretty rough. Final version will be polished.

So, what I've learned so far:

- you can go pretty fast on wood and also use incredibly small bits (0.2mm), but if you want a nice surface you need a lot of finishing passes.
- poplar is not probably good for small detailed pieces
- I can probably make 50 keycaps in approx 30 minutes, the most time is spent changing bits and and fixing the stock to the table
- the finishing phase (sanding, varnishing, ...) takes quite some time but it's pretty enjoyable.
- you can carve basically anything (both depressed and embossed)

Beautiful machine, its impressive that a machine at home can be that precise. It's good to live in the future!

[pyrelink]

That is so damn cool. Were you having to manually flip that block of wood over to get it to mill the underside? Amazing how fast it was able to tear through that wood.