Or even a touch faster, not sure which one you need, but a larger chip (if it can handle it) should take more heat with it.
That looks amazing!
I’m quite a bit jealous. 
Keep on going and posting photos!
Thanks guys…
Did a couple more tests at full depth. One at 7mm/s and the other at 9mm/s feedrate. Only did about 3/4" long cuts. At 7mm/s the collet and bit got significantly hotter (no measurements, just using a calibrated finger). I let the router cool down for over an hour, then tried the cut at 9mm/s - the bit was cold, but the collet was warm (and I would say warmer than the 8mm/s cut I did last night).
I decided to cut my next part using 8.5mm/s feedrate at full (7mm) depth, with 0.15mm finishing cut:
The completed part:
I had something go weird on my first attempt - almost seemed like Repetier and Marlin disagreed on where they each thought the coordinates were? This led to the drill-spot in the upper left being miss-located and drilled through. I killed that reset everything and on the second attempt everything worked as expected. I’ll just drill that hole out on the mill and oversize it a bit if I have too.
Apart from that, this cut was smooth and uneventful. At the end both the bit and the collet were stone-cold. Kinda confused how my shorter test cuts are generating heat, but the longer cut isn’t. Not going to complain about it though, these feeds seem stable enough. This part took about 50 minutes to carve out (while the previous part which is comparable in size) took an hour and 45 minutes - so happy with the decreased cut time.
This part wasn’t as spot-on dimensionally as the last. The hole is about .015" under, and the outside is about .010" undersized. Those are reasonable as far as I’m concerned, and IMO a reasonable trade for the decreased cut time.
Oh, almost forgot – chip evacuation at full depth was significantly reduced. The longer chips were still moving away from the cutter, but whenever there was a bend or curve in the slot behind the cutter the chips would tend to start stacking up and the vacuum by itself wasn’t dislodging them - so I had to keep a fairly close eye on what was going on and give air blasts (from a compressor) more often than on the previous (half depth) cut.
1 Like
How much of a finishing pass did you use? This should solve the problem if you dial it in correctly. (I think).
Trichodial is great and makes it possible for way more people to machine metal but the trade off is time. Once you dial in your settings slotting does work, but it does take a lot of experience to get there.
I used a .20mm (~ 0.008") allowance for the finishing cut on the first one, and .15mm (~0.006") on the second. As the cutter moves around the part you can definitely hear where it’s taking more of a bite on some edges than on others. I wish that estlcam allowed for multiple finished passes, but if it exists I haven’t found that setting yet.
I’m not a fan of slot cuts even on a ‘real’ mill, especially with small diameter end mills. So I think the troch cuts for slots are a great way of taking advantage of the strengths of the CNC machines (making sinusoidal cuts you could never make on a manual mill).
1 Like
I’ve been thinking about how to nail tool changes and decided in order to do it “right” I really need to be able to home in X an Y. For some reason I have a pile of this style end-stop, so I wanted to use them:
Of course if I’m making metal chips they need to be somewhat enclosed to avoid shorts. I looked around thingiverse and didn’t find anything appropriate, but did find a mounting style I liked, so I whipped up a couple of enclosed mounts. Kinda difficult to get a good pic, but hopefully it makes sense:
Had to make different versions for X vs Y axis, oh well…
My plan is to use one of those cheap Z-probes to set Z-zero. But I’m thinking that having a Z-Max end-stop would be good (to be able to lift the router for bit change access, but not run it off the Z-rails). I saw some Z-Max mounts, but most seemed to mount under the Z-tubes (which would technically, although probably not a problem in practice, eat into my already minimal Z space). I ended up with this:
It mounts to my (no longer needed) dust shoe rod holder, which is part of my bracket to hold the vacuum exhaust tube. The top edge of the tool holder activates the switch (also fully enclosed). It can also be easily removed if I want to pull the whole Z assembly out of the gantry.
I had to reconfigure marlin to recognize the limit switches and to get the proper polarity on them. X-min and Y-min work great. I haven’t hooked up the Z-probe yet, so I haven’t tested Z-min. However, Z-max has an issue I don’t understand… M119 confirms that the Z-max switch is recognized by marlin, and it reports back the correct status (activated or open) - BUT when the Z-max switch activates it does not act like an end-stop (meaning I can continue to move in the +Z direction). I’m sure this is some kind of config issue, but if anyone knows what it is - please let me know. Thanks!
EDIT - I think I’ve figured out the Z-max issue… Seems the default marlin behavior is to ignore endstops except when homing (ENDSTOPS_ALWAYS_ON_DEFAULT not defined). M120 enables them, M121 disables them. Since my use case is to lift the router all the way up during a tool-change I should be able to do something like:
M120 //enable zmax detection
G0 Z100 F280 //move router all-the-way up (stop when zmax activates)
M121 //back to default setting for zmax detection
Haven’t verified this on the machine yet, but from what I’ve read this seems like a viable approach for me.
Interesting use of soft stops. I like that.
I had my other machine set up to home upwards, similar to yours but uglier, and I would home upwards and probe downwards. I think your solution might be better, where you can home downwards and reset zero, or probe downwards and not reset zero, and it’s still handy to move up to the endstop.
I am not sure if it’s possible to use zmin for both G28 and G38.2 but worst case you could wire the same signal to zmin and xmax and use xmax for probe and zmin for home.
Looks like dual endstops and auto-squaring are probably in this machine’s future…
Today I completed the two parts I cut out above and discovered that the second one is just slightly trapazoidal in shape (vs square). It wasn’t off by much, but maybe 10 to 20 thou over 3 inches - enough to be noticeable when fitting to mating parts.
The first part I cut out was closer to square, but still just ever so slightly off.
I did a quick inventory and I should have all the necessary cables - just not looking forward to unbundling the existing wires and including the extra set of motor cables…
Before tearing all the wiring apart I decided it might be fun to try a little project (where being slightly out of square isn’t an issue). We’re having our family christmas get-together this weekend, so I tried making a trinket for one of my cousins. Used some of her original art for the design. I’m happy enough with the result.
Unfinished:
Finished:
4 Likes
Spent the last couple of days rewiring the machine for dual endstops and separate motor drivers. The worst part of the whole exercise was de-looming (then re-looming) the existing wiring to make the motor wiring changes (from serial driven to separately driven).
A hint for anyone who does this in future – if you reuse the existing (serial) motor cables for one of the motors you MUST jumper wires 1-and-2 and 3-and-4 on the unused motor connector! In hindsight it’s obvious, but I missed it first go around and had one undriven motor on each axis. Guess what that leads to - yep another de-looming/re-looming session… sigh…
After making sure I could drive all 4 motors again I carefully made certain that I had all the endstops plugged into the correct spots on the Ramps board and they were being recognized (using M119). Everything seemed good, so I tried an X-home and it seemed to work. Then I tried a Y-home and all hell broke loose (lots of trying to drive the axis into the wall, motor skipping, cursing, swearing, throwing things, etc). Eventually I figured out that I had Y1 and Y2 motors ‘reversed’ (plugged into the opposite drivers on the Ramps). So one endstop was triggering, that would cause the other motor to stop, and the motor that just hit the endstop just kept on going (and going, and going…)
Once I figured that out and fixed it (which did not require re-looming - yay!) I was able to begin configuring it for square. My endstops can be moved, so I opted to go for squaring it without using the M666 offsets - instead I adjusted the endstop positions until I got it square.
I used a piece of printer paper taped to the bed, then just lightly touched a v-carving bit to the paper to make a small mark, then lifted Z, moved 179.6mm in X, touched down again, then 179.6mm in Y, touch, repeat for the fourth corner. Then used a scale to measure the diagonals (should be 10 inches). First measurement was off by 1/16th of an inch (total). By the 4th iteration I had it to about 1/128th of an inch (.008", .2mm) off. On the final iteration it appeared dead-on. Since the 1/128th inch was quite discernible with the scale, I would estimate my final error is probably less than (or about) .003".
Now, how repeatable and how stable will that be? Probably not that good. I know I will accidentally hit at least one of the endstops at some point, so I tried to be proactive and super-glued, and hot-glued them in place. I doubt either of those will work long term though. But I can at least sleep well tonight knowing that it was once quite square!
2 Likes
That is far more square than I have ever taken the time to do! Nice job.
+1 for Maryland! Nice job! Where abouts in MD? Howard County here…
also HoCo…
Wow its a small freaking world!
Did some testing this afternoon with a 1/4" 4-flute endmill on 1/2" aluminum plate…
First I picked up one of the Harbor Freight Router Speed controllers because I suspected I would need it to get my SFM into a reasonable range (with the 4 flute bit). I actually wasn’t too thrilled with how it worked. It did reduce the router speed, but also seemed to introduce an almost sinusoidal variation in the speed - it also seemed to bog-down on cuts pretty significantly (presumably due to loss of working torque).
I did quite a few test cuts using estlcam’s trochoidal path (5% step length, 30% width) varying cut depth from .5mm up to 6mm. Adjusted feedrate as well, generally going slower as I went for a deeper cut.
Bottom line is that it cut fine with the larger bit at shallow depth of cut (to about 2mm DOC). Any deeper than that and I started to get flex in the tool holder (router was moving relative to the Z-axis components). At 6mm DOC is was still cutting, but tool movement was pretty sever and worrisome.
I never had any issues with the cutting edges galling up, even when running the router without the speed control (at the router’s lowest speed setting - which I assume is about 10K RPM). Never noticed any issues with the bit heating up, but on the last test cut I did (at 3.18mm DOC) the work piece did start to get hot - in fact, hot enough that the blue-tape adhesive I was using to hold it down began to fail. This just introduced more movement (now the work piece was moving relative to the router, as well as the router relative to the Z-axis) - so I killed it.
So - my conclusions:
- Can I use these bits - Yes, if DOC is kept below about 2mm/pass
- Does it make sense to use them - Probably not, I can do a 7mm DOC with the single flute 1/8" bit, so using the 1/4" bit actually would take longer to achieve a similar cut. It may make sense if I need to do a deeper overall cut than the 1/8 bit would allow (I think its flute length is either .4 or .5 inches, so if I needed a 5/8" pocket for example the 1/4" bit might make sense).
- Is the Router Speed Controller necessary - I don’t believe it is.
1 Like
So far this is the one I would recommend:
The only issue I have with it is that it’s flute length is .400" so it’s should be good for aluminum up to a depth of about 3/8" (not in a single pass!). I’ve had good performance using estlcam’s trochoidal cutting at a 1/4" depth of cut.
I played around with a 1/4" 4 flute end mill because I wanted to cut parts out of 1/2" aluminum plate. That worked as well, but I had to keep the DOC down at about 2mm - so many more passes would be necessary compared to the 1/8" bit.
I suspect a single flute 1/4" bit would likely be the sweet-spot for cutting out parts from aluminum that was thicker than 3/8" - but I haven’t given one of those a try (all the one’s I’ve found are fairly spendy at ~$25/bit).
FYI - I don’t use any cutting fluid and don’t believe it is necessary.
This is where I get my endmills if I don’t get them from Ryan.
Yeah, I’ve also bought some end mills from him (Drillman1)… I suspect I’ll end up buying one of those 1/4" end mills at some point, but even his price is $17 + $4 shipping, so it’s in the range I hate dropping unless I have a real need (I may have mentioned this before - but I’m basically a cheapskate). Besides, I know that if I decide to buy one, I’ll probably end up with 2 or more, just because I will hate it if toast a bit in the middle of a part, then have to wait for snail-mail to deliver another…
I’m actually working on some parts for a CNC conversion of a mini-mill. For some of the mounting blocks I need to mill a .450" pocket into a 1" think aluminum block. Obviously the bit you linked would be good for this, but I’m considering seeing if I can push the 1/8" end mill to that depth (just on the final pass). In theory, if the shaft is no wider than the cutting flute it should work, but I don’t know I may end up just going with the 4 flute cutters I already have a ton of… Or just drop the $21 on the 1/4" single flute – oh, decisions, decisions…
It they’re the 1/8" bits Ryan sells, the shaft is the same diameter as the flutes, so as long as your straight, it shouldn’t rub too bad. I mean, it’s going to rub, but shouldn’t hurt anything.