I haven’t cut the holding tabs yet, so outer dimension measurements are a bit more difficult to get accurately (was able to use pin gauges on the hole). But the outer dims seem a little oversize (measuring from flat to ‘point’ of the curve). It’s pretty good in the Y direction at .003 oversize, but the other two directions (which are mostly X, some Y) look to be about .010 (~ 0.2mm) over. As I said though, not sure I really trust those numbers yet as it’s hard to get good measurements with it still attached to the source plate.
I received the real carving bits and that 5 now carves out nicely:
Except - the center of the character isn’t being removed? I’m using estlcam and must be missing some setting? I’ve tried setting it up to use a 1/8" flat bit as the carve pocketing tool, but that didn’t add anything to the resulting program?
Are you sure? Did it just pause for a tool change and you stopped it? You should be able to tell from the preview.
I had this problem when I started. Then I figured out the one setting I wasn’t using:
Set that higher, and it will carve the whole thing with the one tool. Just make sure the stepover on that tool is set low.
Hmm… can’t seem to figure out quoting in the new forum s/w either… 
Jeffeb3 - Yep, positive. Checking preview often now (it’s my new go-to tool in estlcam).
Chris - That was the problem! If I bump up that setting on the carve it will fill-in the letters. And, if I specify a pocketing tool it’ll use that for everything it can other than the edges.
I knew it had to be sitting there staring me in the face, but just couldn’t see it.
Thanks!
1 Like
No problem. I don’t even add a pocketting tool to mine. This was done with an 1/8" 45* v-bit, set to 10% stepover.
3 Likes
Hmm… tried cutting my first real part out of aluminum this evening and met with utter failure 
First had issues with a tool change (can’t believe I didn’t test that out in foam before trying it for real!) Was trying to use a drill bit to spot drilled holes, then switch over to a single-flute cutter to cut out a motor mount plate with a large hole and a curved slot in it. The spotting of the holes worked ok, but when it came time to switch bits I managed to loose XY positioning. So I ended up trying to restart the part, just using the single flute cutter for everything - tried re-zeroing and got close, but apparently not close enough. Some of the holes recut fine (just a little off) but a couple got very squirrely augured out some nasty looking oversized holes. Then the real horror story began… Cutting out the large hole (using trochoidal cuts) completely went to crap…
I eventually had to kill it. The cut was completely packing up with still attached chips. The cutter got trashed of course. But what surprised me was the path that it was trying to cut was significantly smaller in width than my previous test cuts. I now suspect that the cutter may have lost it’s tooth in one of those messed up holes and the other cuts didn’t stand a chance…
Gonna have to order me a supply of new bits…
I was wondering if the aluminum plate I was using now may have been a different alloy than the one I was practicing on, so I tried my test part again on this plate (I did bump the troch width up to 50%, was at 30% before):
The (new) bit seemed to cut well and chips were evacuating fine, BUT I’m seeing some very disturbing things on this cut:
- When the cutting path made it back around to where it started, there was a visible shift in X (probably .5 to .7 mm).
- The center hole (which was cut first and should be in the middle of the part) is shifted significantly ‘downward’ (in Y) - so I guess actually it’s the outline which is shifted ‘upward’ in Y…
Now that I write that and look at the pics I’m suspecting that I may not have left enough room in the Y axis for the part to fit (meaning I ran out of -Y room, lost steps as it was moving into the lower left corner and that ends up shifting the outline in +Y, which would also explain not lining up when it got back around to the starting point (which was about middle of left side).
Ok, maybe I’ve figured out what’s going on… just had to write it down to have it all click. Going to go ahead and post this anyway, just in case it may help someone in the future…
Thanks for listening 
2 Likes
Much better results today…
No tool changing, just used the single-flute mill to mark the drill holes. Bumped the trochoidal width up to 50%. Finishing cut, with 0.2mm allowance (will probably bump that down to 0.15 in next part). New bit, and made sure I didn’t run outside the working area…
Very pleased with the results. Dimensional accuracy is spot on:
In that last pic it looks like the hole is undersized, but that’s misleading. The hole is spot on at 2" diameter. The calipers are just sitting on the part for the pic after taking the measurement.
Only thing I didn’t really care for was the amount of time it took carve out - an hour and 45 minutes. I did two passes (@4mm DOC then 3mm DOC). I’m going to try a test with the troch cuts at full depth and see if that’s feasible. it would only be 2X bit diameter, so it’s possible it could work. If so, that would basically cut the time in half. Overall I have to say I’m pretty pleased with it.
I do want to get tool changes figured out though, cause I really want to be able to accurately spot drill for simple holes to be drilled out later in a separate operation (just using a drill press).
Just a bit of info on the tolerance of the Dewalt 1/8 collet – I have a bunch of #30 drill bits (0.128") and I figured they would be good for doing the spot drilling… Nope, they wont fit in the collet. This really surprised me, I figured .003" over wouldn’t be an issue – totally wrong on that account.
4 Likes
AWESOME!
Now that you have a part and got some metal under your belt. There are tons of things to try to speed that up. I have never actually used trichodial on a part, slotting works but you need to make some test cuts to figure out if it saves you time and all the settings you should use.
In the end it is not super horrible of a time for that, difficult to do that by hand in that amount of time and accuracy, but you are right I think you can cut that way down.
I just did a test cut (my small triangle again) at full depth (7mm) using Trochoidal with an 8mm/s F(xy) (which was the same rate I was running earlier on the motor plate), 50% Troch-width. There was no noticeable difference in the cut other than it completes in one pass instead of two. It sounded good, looked good and chips evacuate well (mostly with just the vac and the router exhaust, only a very occasional build up that needs a squirt of air to go away) - . However, I did notice that the bit got noticeably warmer than it did in the previous cut (which was about 105 minutes long, this one was 7 minutes). It wasn’t “hot” just warm - but of course that would indicate that the chips are no longer carrying away all of the heat. In the motor plate cut the bit was stone-cold at the end of the cut.
I might try dropping the feedrate just a little (maybe to 7mm/s) to see if it stays cooler at that speed…
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