-
I noticed there’s an indicator in the toolkit. It would be nice to use in a couple of situations, but I couldn’t figure out how to start the spindle manually from the controller. Is that possible, or would we have to run some gcode directly? Also, what is the slowest possible/acceptable spindle speed?
-
I was trying to test my drag knife, and I ran into the same problem Brian Watt had when working on his CNC plotting/drawing device (https://yo.asmbly.org/t/big-cnc-as-a-plotter/5018/36). I used the drag knife toolpath gadget in VCarve to generate gcode, but it would only run a few steps and then pause (not stop). I compared it to gcode from a normal cut, and it was essentially identical — the only difference in the executed lines was “S0” for the drag knife versus “S18000” for the end mill pocket cut. Which makes perfect sense; you want the spindle off for the drag knife. But the drag knife code pauses on the line just before executing the first plunge. And I noticed that the “AtSpeed” light in LinuxCNC was red then (whereas it was green when making the first plunge on a normal cut). So perhaps the code pauses because it’s waiting for the spindle to get up to speed (even though it is, since the desired speed is zero)? Is that the likely explanation? How would you fix or work around this?
-
I was thinking of cutting some aluminum, and I’m reading online about the necessary adjustments. Does anyone who has actually cut aluminum on this CNC have any advice?
@dannym can answer this. There might be config setup that has a min rpm to run
I would use the air nozzle to clear the chips. I would use an oflute cutter. In your case probably 1/8". Probably 13 ipm and 8k rpm.
If you want the spindle off, S0 is not the way to do it. You want M03, the clockwise spindle start command, removed from the G-code. M05 is also the spindle-off command.
The system literally runs g-code as a script. It will execute anything the codes tell it to do. There are a few higher level limitations- it will not execute a g-code that would move it out of the work box. It will actually evaluate before starting and refuse to start if any g-codes would take it out of bounds.
It will pause and not run any “cut” g-code if the spindle is in the “run” state but not at-speed. The motion command that is not a cut is a G0 rapid move. However, if the spindle is NOT in the “run” state because M03 was never given or has been terminated by M05, all motion commands will execute.
The SPINDLE button on the remote will start and stop it, plus the SPINDLE (clockwise symbol) will start it on the terminal screen.
There was a custom postprocessor on the machine for a drag knife in Inch and Metric flavors. The postprocessor is where the project generates that G-code ASCII file and just like the metric vs inch option, there’s a drag knife one, which will not have any M03 Sxxxx or M05 in it.
However, it appears that VCarve machine was updated and whoever did it didn’t copy the postprocessor directory so the install is incomplete in that regard. There are several things there we needed there. Hopefully the directory is still there with the old install, if not we can just write new postprocessors it’s pretty simple.
Postprocessors only execute in the “save as G-code” step, so they can’t run on users’ Makerspace User editions, only the two Master editions at the space. The postprocessor is stored with the VCarve installation so it stays on the machine you’re at. They’re ASCII files and pretty easy to see what it’s doing and just delete the spindle section.
There is a lower limit to the spindle speed, I recall I have it set to a ridiculously low number but it is above 0. It is not geared down, the motor does not have much torque at low RPM but can still do a light drilling operation at low rpm. It could be prone to overheating if loaded down a lot, since the motor is cooled by a shaft-mounted fan. At low rpm the fan can’t provide significant cooling anymore, but I’ve never seen it used long enough to lead to excessive heat buildup.
What thickness of aluminum, and what grade? Carving a billet (thick stock) is different than cutting a sheet. However, o-flute is often the best choice.
I do have a 3 flute aluminum finishing bit that I’ve been wanting to try with billets on the CNC router.
Machinability is easiest with 6061.
OK, so for the drag knife, I either need to find the possibly MIA special post-processor, or just manually edit the regular gcode file to remove the spindle start M03 commands.
I always get 6061 aluminum for the machinability. I’d be using plate stock, some 3/8” thick, some 1/2” thick, and possibly one piece at 5/8” thick. Some cuts could be done with a 1/4” end mill, but a few details are smaller and would need a 1/8” end mill. Definitely requires some thought about spindle speeds, feed rates, and cut depths.
I’ve done a fair bit of aluminum, but mostly sheet. The bed is mostly meant for wood, so it’s not insanely rigid like the Tormach. I’ve some simple features into 3/8s stock (interpolated holes, basic profiles), and it’s not perfect, but it’s good down to 0.5mm or so. More so if you do a spring pass at the end.
It drills like a champ. Pre-drill everything, it makes a world of difference in the reliability and tool life, especially if you have a lot of through features. I went from regularly breaking endmills to not, and drilling was about 50% of it. Air blown straight on the part for chip clearing was the other half.
Tool length is a big factor. I have my own 1/8" collet, so I can do something that’s bad for the collet (but good for my product). I use my own collet, and put a 1/8" drill bit in, but chuck it with about 1/2" extended out of the collet. That means I’m chucking the flutes of bit on the collet (which is why I need my own). It’s terrible for the collet, so get your own if you’re doing this. OTOH, the rigidity of this super-short drillbit setup is amazing. Holes are spot on in location. Did I mention you should use your own collet for this?
The Z-depth is much better then it was earlier this year, but it’s not perfect. How big is the item you’re wanting to mill? Z is always my biggest challenge, and I’m just doing through cuts.
What spindle speed and feed rate were you using on the 3/8” material?
I use the a zrn coated oflute 3/16" shank for 1/8’ up to 3/8" thick plate
I don’t know the numbers exactly, I ran at 35% of the feed and speed suggested by solidworks.
If you’re doing a lot of drilling like that, it’s probably worth getting some stub/screw-machine length drills. It’ll help even more with rigidity and you won’t have to stick the flutes into the collet. For example here’s a cobalt 1/8” one. Stub-length 1/8” cobalt drill
Oooh. I knew things like this existed, but I didn’t know what they were called/where to find them/that they were reasonably priced. Thanks for the link!
I was looking at the air cooling / chip clearing system, and there are a couple of issues. First, it seems to be connected into the old, nonfunctioning compressor, and I didn’t immediately see any way to connect into the new one. Then, the nozzle device attaches with a magnet, but I couldn’t find anywhere to put it that would let you position the nozzle end anywhere near the bit. This was further constrained by the tube to the compressor being a bit short at that end. Assuming we can connect to the new compressor, where does that go?
I sacrificed a couple of really cheap bits to the aluminum spirits today, aiming compressed air by hand. They didn’t get far, though I wasn’t too surprised. I will give Zack’s pre-drilling method a try; in fact, I can pre-mill most of it, leaving just a bit of material to remove to get the final shape and size.
(I would note that what I’m doing right now would be trivial to do on the manual mill if we had a rotary vise.)
And there’s always an intermediate (between wood and metal) that could be made out of plastic on a 3D printer that I’m offering assistance if that would help.
Not sure what you’re trying to do with the aluminum, but it sounds like it could probably be done pretty easily on the Tormach if it’s small enough to fit on the manual mill. Happy to help with that if you want.
What problem were you having? If you were having the bit get clogged with melted aluminum (galling), you need to lower the spindle speed. If the bit was flat out breaking, you need a shallower DOC or a lower feed & speed. I could do about .03 or .04" DOC pretty reliably.
I’m running the spindle at super slow speeds for the large CNC. I think I used 6000 RPMs, 10 IPM. Any time you lower the feed rate, you must to lower the spindle speed accordingly. There’s a sweet spot that’s a ratio between the two, and it’s a pretty narrow band.
Feed rate too low or spindle too fast? You rub instead of cutting, the bit quickly galls up, and results in terrible cutting, eventually leading to bit breakage.
Feed rate too high or DOC too big? The bit can’t take the torque, and it’ll just snap.
DOC too low? The bit will dance across the top of the metal, start rubbing, and break.
The compressed air only helps once it’s actually been cutting for a few seconds. If it’s breaking well before then, your F&S are really off. Also watch for the bit to gall up. It’ll get a deposit of solid aluminum, filling up the inside of the cutting area. If that happens, throw the bit out, a galled up bit will just rub the material away, not cut it.
I got through the first pass and the ramp into the second. I used a spindle speed of 5,000 rpm, a feed rate of 10 ipm, plunge rate was 5 ipm I think, and the cut depth and offset was 0.05 in. The problem could be those settings need tweaking … or that I’m using 1/8” coated end mills from a 10 for $12 pack. 
There’s a reason I was willing to sacrifice a couple.
All of this would be better done on the Tormach, but I haven’t learned to use it yet. I have several projects; I was trying the simplest, but it’s time limited and I’ve moved on to a different method of doing something.
For the other project, there are many ways to proceed, but first I think I need to be more certain it is worth proceeding. @JoeN, could I perhaps borrow your drag knife briefly sometime? I would just need to do a few cuts to see if a drag knife would do what I need or not. Then I can decide whether to invest more time/money in making/buying my own.
Let me know when is good for you? I’m leaving in week. I won’t need when I’m gone
In machining aluminum, you need to maintain .001 in per tooth. that is how much material engages with each flute of your endmill as its going along.
There is a little spreadsheet on this page for reference.
Getting Started with Feeds & Speeds - NYC CNC
The old compressor is functioning you just turn it on (it should be left on)
We need a T on the max line fitting to plumb it into the new system ( I will order T)
@JoeN I’ll be in the shop most of the day today (Monday, 6/13), though you can also leave it like we discussed if that’s more convenient.
Will do