April 27, 2019 at 1:30 pm #98321
Second project in aluminum and I wanted to do something a little more fun than the speed plate for my MP3DP. The Turners Cube is a great exercise in squaring things up after rough cutting on the band saw. Also excellent practice in getting a repeatable setup as this requires making the exact same cut on all 6 faces of the cube. Even with using the end mill as an X, Y, and Z probe with G38s I am off by a tenth of a mm or two on at least one of the cuts 🙁 I’ll just hide that side!
Final dims are 30.5mm all around. I did manage all ~7h of cutting with a single end mill! Not bad for a $3 cutter.
On my 25.4mm 16″ x 16″ work area machine I used the following cutting parameters:
(no plunging into material here)
12mm/s feed (make sure your accelerations let you get up to this speed)
3.5% trochoidal step
50% trochoidal width
Finishing Pocket Faces:
Plunge 3mm/s (peel pocket strategy uses a helical plunge)
I could have likely cut down the cut time significantly with a more aggressive trochoidal step but these settings gave me decent chips and I’d screwed up a couple of times already by getting too impatient 😉
Attachments:April 27, 2019 at 1:37 pm #98328JMSParticipant
Very coolApril 27, 2019 at 1:38 pm #98330
Please tell me you have a video of this?!April 27, 2019 at 2:56 pm #98345
These aren’t all necessarily from the finished piece in the first post. The feeds/speeds and final setup changed a a lot. I beefed this a few times more than I care to admit.
First successful G38 X, Y, and Z probes: https://imgur.com/n90gSV8
Skim cuts to square up the stock: https://imgur.com/cge0utf
Finished squaring: https://imgur.com/lqUBP1e
Making garage glitter: https://imgur.com/VZOgSjN
No really, this took a few tries: https://imgur.com/lC0nPgo
1 user thanked author for this post.April 27, 2019 at 3:16 pm #98351April 27, 2019 at 4:52 pm #98361
That is awesome. The project did it’s job. From what I understand it is a test in many machining classes, so you get an A+ (the plus is for not giving up).
Also thank you for posting all the specs. I should link this to a main page somewhere.April 28, 2019 at 6:49 am #98449
A couple of takeaways that some of you may find useful:
Use an air blast to clear chips and help keep the tool cool. I use an air blast that’s built into the lower mount. I’m sure it’s a bit overkill but I’m running 40PSI through the air blast with a 25 gal compressor.
Measure the diameter of your end mill with a set of calipers. I’m not sure if this is unique to the stuff I buy from aliexpress but some of mine came out to 2.9mm instead of the advertised 3.18mm. It looks like the shank is 3.18mm prior to being ground but the flutes are a bit smaller. I had to kind of “spin” the end mill in the calipers to find the largest diameter of the flute. I was initially using very high stepover for roughing the block into shape and I couldn’t figure out why it was leaving ridges between passes. Turns out that if your tool diameter is ~9% less that what you tell your CAM software then this sort of thing happens /s.
Never plunge straight into the material and avoid plunging altogether if you can. Id you must plunge into the material take if very slow. I still got some chatter during plunges using trochoidal milling’s helical pecking plunges.
Make a ton of test cuts to get things dialed in first. the majority of the time spent on this project finding the right settings for this machine. Christian’s advice is a great starting point for trochoidal cuts.
Spend the time to get your machine set up as square as possible. Foot height, rail squareness, gantry squareness, z axis, all of it. I used Ryan’s tool and shimmed the router as best I could but still got the slightest of ridges on my finishing passes. I, regrettably, didn’t set up dual end stops from the beginning so I use clamps on my rails and lock steppers to keep the gantry square before every cut.
Take care to get the vise mounted properly. I locked a new spoil board on to the table and surfaced it prior to mounting the vise. Fingers crossed that the base of the vise is perpendicular to the fixed jaw and parallel to the flats. I didn’t have the proper tools to check. Jogging the machine around probing things proved good enough.
The last piece of the puzzle was getting the fixed jaw parallel to the X axis on the machine. You could get this close enough for most work by jogging the machine around and making sure that the end mill just makes contact with the jaw at either end. I cheated by 3d printing PLA soft jaws (100% infill for sure) and getting things close. I then took a skim cut across the length of the fixed jaw. You’re more or less guaranteed to have the fixed jaw and machine parallel to each other that way. I’ll have to get a clip of this… Machining PLA without turning it into a gummy mess was a challenge and, if I’m being honest, I probably didn’t need to go through the trouble here. Oh, and never trust the movable jaw on cheap vises. Jaw lift sucks.
Hopefully some of you will find bits and pieces of this info useful 🙂
Attachments:April 28, 2019 at 8:39 am #98471
The end mill diameter thing has me wondering. Turns out that using calipers to measure the diameter of a single flute end mill isn’t very accurate. A better way to measure end mill diameter would be to note the diameter of the shank and then put the end mill in a v block. You can then reference the difference in shank/cutting edge to using an indicator to find the true diameter of the end mill.
Having said all of that… A lot of things other than end mill diameter could have contributed to the issues that I had. Easy fix was to surface things with a <=90% stepover.
Attachments:April 28, 2019 at 9:03 am #98477
Awesome info, I can not wait to try some of your settings. I have this linked in the gallery, So at least I can easily find it again, I might add it to the milling basics page, or maybe advanced.May 4, 2019 at 10:43 am #99259
The high step over issues that I saw bug me. I mostly ruled out the end mills cutting diameter, however. In hindsight it was silly to guess that this was ever the issue!
I started by measuring shank diameter as best I could. I don’t have a set of mics but my cheap calipers read 3.17mm so we’ll assume they’re right on 1/8″.
Kyocera cutters that Ryan sells:
No-name Chinese cutters that I used for this project:
The largest difference in shank to cutting edge that I saw was between 0.02mm and 0.03mm. Note that the effect on the effective cutting diameter is 2x this.
If we assume the shank is truly 3.17mm that puts the effective cutting diameter at about 3.12mm. Not the nearly 0.2mm of error that I saw when making my surface cuts. The slop comes from somewhere else. I realize I’m chasing my tail here and that I have no real need for the accuracy. I also don’t intend to try and get this level of accuracy out of the MPCNC. This is mostly out of curiosity. If I understand things correctly 0.2mm resolution in X and Y for our machines is pretty good for the steppers, pulleys, and belts that we use.
Fun fact: I measured cutter that I used for the turners cube and after about 7 hours of cutting time the effective cutting diameter was 3.09mm.
Attachments:May 6, 2019 at 2:21 am #99474Thymen van RuitenParticipant
Very cool project!
Thanks for the detailed information and pictures!
- You must be logged in to reply to this topic.