December 21, 2017 at 8:47 am #49845
General thread for the stuff I’m making on my ~17″ sq. cut area 525.December 21, 2017 at 8:53 am #49848
1st up- a sign for a secret santa exchange with my endurance racing team. This was a bit of a toughie- first time doing multiple setups on the same workpiece. Had to do three operations on the front side, maintained tool position by keeping the steppers locked after the cuts and using locating holes on the workpiece to shift the stock. On the rear there were two operations, maintaining Y location and getting the X close enough that the nails go into the thick parts of the workpiece (they would have poked through if I messed the X up). I ended up scrapping three parts out due to stupid errors, but finally got a good one off. I was going to paint it up, but ran out of time with all the scrapping so I just sanded it and am leaving it to the giftee’s discretion to stain or paint.
I had some slight Z inconsistencies between the front operations, probably either variation in the stock or my clamping (screwed into the spoilboard)
All done with a 1/8″ e-mill, .25″ DOC .05 stepover adaptive clearing with contours to finish, all at about 40 IPM.
done section by section like this
As machined, after the third op.
Nailed the alignment pretty good on the X/Y, no discernible irregularities There was about a half inch overlap from the corner on the contour between the two operations.
Now that I’ve got the multi setup thing figured out, the door is open for some interesting larger projects.December 21, 2017 at 10:09 am #49853
Damn it, my post didn’t go through…
First major project- a sign for a secret santa my endurance racing team is doing:
Bit of a tough one, some personal firsts. Three workpiece shifts to do the front, then two on the backside to make pockets for the hanging hardware. I added positioning holes on the stock outside of the part and kept the steppers locked up between operations to maintain tool position. I got the XY alignment pretty bang on, had some small Z variance, likely due to the stock or my workholding (screwed down into spoilboard). The logo was taken from another format, converted to DXF and scaled up a lot, so the curves aren’t very smooth.
Cut settings: 1/8″ 2 flute flat end mill, .25″ DOC, .05″ stepover at 40 IPM. Roughed with adaptive clearing at finish depth, used contours to finish around the lettering. Ran pretty well, a little chatter when starting slots with the cutter at full 180 deg. engagement. I used .125 DOC when I scrapped the first two out in poplar, moved to .25″ in pine.
I ended up scrapping three out for stupid reasons, was pretty frustrating but I finally got it. 2.5 hours machine time with the final version of my CAM settings, was around 6 hours on the first poplar part.
I intended to paint it two tone, but ran out of time with my poor time management skills and scrapped parts.
Now that I’ve got the multi setup workflow down, I’ve got some neat ideas for future projects and better alignment processes. Infinite X axis!December 21, 2017 at 10:14 am #49855
after first operation
after 3rd operation, as machined
XY alignment, no visible defects due to XY positioning. The contour tool paths overlapped about a half inch on each side of this cornerDecember 21, 2017 at 10:49 am #49860
That came out great! Nice job stepping out of the comfort zone.December 21, 2017 at 11:25 am #49872
Thanks! The multi setup work isn’t too scary once you do it. Opens the door for some neat projects. I’m probably going to make a super sized (use full Y axis, 4 ft X) version for my garage at some point. I want to design/make my own carbon fiber or fiberglass wing for my personal track car and our endurance car, so I’m hoping to make all the molds/forms for composite layups on the CNC.February 3, 2018 at 9:46 am #52133
Did 3 tap handles for a local bar recently in Maple, really pleased with them. Roughed letters and symbol w/ 1/8″ e-mill, finished with 1/16″ and engraved top with 90 deg V bit.
Did a little test to make sure my tool changes were OK first. I got the Z a touch off with the 1/16″, but nailed it on the actual parts, can’t feel the transition at all.February 3, 2018 at 10:39 am #52139
So nice!October 6, 2018 at 8:01 pm #71207
Got back to the MPCNC after a dormancy & partial rebuild. Running better than ever, got it tuned in on plywood & then went to work on aluminum. The machine has been killing it, just plugged Kevin’s settings into Fusion and have had very little trouble tweaking it in. I made a couple keychains for my Miatas. One current Mazda emblem with 1/8″ 1fl in 1/4″ alu, the other is my endurance racing team’s logo with 1/16″ 2fl in 1/8″ alu. I’m really particularly happy with how the smaller one came out.
The Mazda emblem cut fantastically using Kevin’s settings.
1/8″ 1fl e-mill
Adaptive roughing (.125 DOC 23 IPM, 15% cutter engagement)->finish contour at full depth with tool dia adjusted for for deflection->bore->contour OD (triangular tabs, .030 DOC ramped gently at 17 IPM & finish pass at full depth. Ran ~16 minutes, I haven’t experimented with DOC beyond .125 but if I keep the engagement low I think it will go further.
The HJ logo was a bit trickier with the 1/16″ 2fl. I wadded up my first ever tool on the first cut trying to profile. I took the settings right off my 1/8″ toolpaths & slowed it down a few IPM. Wasn’t enough on the slot, so I adaptive roughed it .125 wide at tab depth (.025″) & ran a contour starting just above that with tabs to clear the rest of the material. The middle attempt I didn’t have my radial stock set high enough & it tried to make some travel moves down in the adaptive cut which lost it’s position. Ran fine after I fixed that, but the cutter is a little gunked up from the accidental travel moves so you can see the top half of the finish pass looks good like the 1/8″ but the bottom is a bit fuzzy looking. I only had two 1/16″ flat end mills so I’ll have to pick some more up, one is probably shot and the other is giving what you see on these pictures. It still cut great, roughed .125 DOC at 40% engagement & sounded just as happy as the 1/8″ at similar parameters.October 6, 2018 at 8:12 pm #71208
Video of most of the cut on the smaller one. I am pretty happy with the CAM on this cut, effective material removal & minimized air cutting/slow ramping. About a 9 minute cut on this one.October 6, 2018 at 8:47 pm #71212
Awesome, I have been a bit nervous to try the 1/16″ in aluminum. Not anymore. I am getting a similar surface finish and I am not sure what to do, I get the feeling maybe we should really slow down the finishing pass, I keep going faster and it doesn’t seem to change it so next time I cut something it will be really slow to see what happens. The rest of your settings look spot on, motivational for sure. Thanks!October 6, 2018 at 9:10 pm #71215
With good CAM it hums along just like the 1/8″ though I haven’t pushed either to their limits on DOC yet. With how hard it was ripping through the adaptive cut I was a little surprised to see it bog down so bad/go to shit on the slot, I think it was around .03 DOC 15 IPM. I may experiment more when I get some more 1/16″ cutters in, but for now adaptive slotting with a finish contour to get tabs & a finish pass seems to be the way to for for me. Slot ran great at same settings with 1/8″ 1fl. Watching it happily fire .125 DOC chips out of an adaptive cut is just tremendous, I’m so happy with how this thing is cutting for what it is. I’m looking forward to trying some steel once I do some more aluminum work.
On the surface finish I was wondering whereabouts you/Kevin/other good metal cutters are at. I’ve made maybe 7 or so small cuts in aluminum so far and have been experimenting slightly on each, I am getting about the same finish on walls for everything so far. I haven’t tried anything lower than 15 IPM on the finish pass. Most of them have been .005 stepover with a spring pass. The first pass it spits a pretty good amount of chips & the spring pass sees a bit more flying out, especially in inner corners which I can improve further. I’ll experiment with some slow & varied stepover finish cuts tomorrow.October 7, 2018 at 2:48 pm #71283
OK, pretty excited about this one. Tow hook to replace the factory hold down point on the track car. I need better chip clearing, I accidentally lost position and chipped a cutter while raking chips out of the groove around the part. Didn’t realize it lost position, so the outside of the part got shifted maybe .1″ left. Sanded down the step on the front of it, still usable. Going to be making one for the rear, another set for my street car and a license plate bracket based on the same mounting holes on the other side. Full DOC adaptive roughing the pockets, .025 stepdown slotting around the part. The holes are within .005″ (only easily measurable feature with the x shift accident),
Super quick and dirty FEA says it’s probably maybe fine (500lb load at slight angle on big circle, three bolt holes fixed). First time trying the simulation package in Fusion 360. Easy to use, I did no verification on this though, ha.October 7, 2018 at 3:29 pm #71296
I’m going to have to go back and bore the third bolt hole out again, I forgot to put the finishing pass on that one… The rear bolt hole was supposed to be oversize to allow for slop in my positional tolerances as designed against the old part. I think I may need to look into home anodizing, this metal is fun…
155g vs 666g original steel part, plug I’m taking the other side off so that’s 1/4 the weight part to part & 2.6lb off the very front of the car.
1 user thanked author for this post.October 7, 2018 at 3:33 pm #71298
Heck yeah!November 4, 2018 at 5:43 pm #74537
So turns out what I made is absolutely useless for the DW660 collet on a MPCNC, but it’s still the sexiest thing I’ve made so far and I’m super happy with it/the processes I’m working out.
Double chamfered lightweighted goodness.. BECAUSE I CAN!! Cut really well for the most part, I could stand to control the tool a little better in tight corners on my finishing passes (I think due to deflection these are not clearing out as much in my roughing) and the only real issue with the cut was I didn’t notice a little chip in the flute of my e-mill which left an annoying little line around the wall. All my tolerances I’ve checked out within .005″, most at .003″ or better which is just incredible.
Main cutting 1/8″ single flute adaptive/contour, held down with tabs. Cut a fixture in plywood to do the chamfering ops, part sat nicely with a quick tap of a hammer. Chamfered with a 2 flute 1/8″ 90 deg tool.
nasty little bump 🙁
I forgot to drain my compressor recently, got some free MQL going… Garage got really foggy, gross.
Fixture, held the part perfectly when I tapped it into place. didn’t end up needing the holes I put in.
Made my chamfers a little bigger than the tabs to cut them right off, unfortunately that line gives them away plain as day, also still have the two telltale marks where it aggressively ramps on triangular tabs. Better than straight ones, but still could be improved.November 4, 2018 at 6:21 pm #74543
Useless or not that is one really nice looking part!
That fog sounds nasty though, I hope you had a mask on. I don’t want to hear any stories of minor’s lung or anything.November 4, 2018 at 6:28 pm #74544
It doesn’t work on the dw660? Because there’s not enough clearance behind the tool because of the z? Probably best to just go ahead and design something to use it for. Door handle, light switch, socket set, computer mouse… Something. That thing is gorgeous.November 4, 2018 at 6:34 pm #74545
Dui, ni shuo de duiParticipant
WoW, absolutely beautiful work!
Keep the pictures coming, those projects are amazing.November 4, 2018 at 7:27 pm #74547
That fog sounds nasty though, I hope you had a mask on. I don’t want to hear any stories of minor’s lung or anything.
Well I’m 23 now, so no worries there! I didn’t notice how nasty it was until I went upstairs and came back down to notice a nice haze in the air… Just need to purge the compressor, it was spitting an oily emulsion. I would love to rig up some non fogging coolant mist with the way Kevin is taking it up… One thing at a time.
It doesn’t work on the dw660? Because there’s not enough clearance behind the tool because of the z? Probably best to just go ahead and design something to use it for. Door handle, light switch, socket set, computer mouse… Something. That thing is gorgeous.
Yeah, exactly that. I spent so much time on the CAD/CAM and didn’t notice until I was already cutting it, lol… So now I have a super cool custom 16mm wrench, which is never used on my cars and doesn’t fit the router.
Oh well, I learned a lot of good stuff and am refining my settings nicely to make future jobs go a lot quicker. It’s quite satisfying to spin on your finger, so it will likely be a desk fidget thing for a while, maybe I’ll use it for a valve or some kind of knob eventually. I’m so excited to make more sweet aluminum stuff. I COULD try another setup and just cut one of the arms off.. Right now, for lack of probing ability cutting fixtures for known features & holding position between the fixture & secondary op is getting the job done. It would be awesome to get XYZ probing going like Shapeoko is doing.
It’s incredible what this machine is accomplishing with good CAM, now that I’m getting tool/fixture changes down I can do some awesome stuff… Gotta try some 3D soon, haven’t given a ball mill a go yet on the MPCNC. Still chasing surface finish & MRR, but tolerance wise I’m impressed with what this thing is pumping out.November 5, 2018 at 6:28 pm #74693
Spent all evening making the STL file usable & doing CAM, hopefully have time to cut it tomorrow. First time in 1/2″, but am facing the part and OD contour area so max DOC is only .391. Still need to do the fixture/back chamfer CAM. Looks like I’ll get to bust out the ball mill for the other side!November 10, 2018 at 5:43 pm #75223
I haven’t done any serious aluminum cutting since I want to do a mist system and haven’t gotten around to that yet, but you can add me to the steel club in the meantime! 3/16″ steel from Lowes, not sure exactly what.
Used the settings out of Ryan’s video, .125 DOC .012 stepover adaptive rough. I spot drilled entries for all the pockets with a 90 deg v bit & then drilled them out with a 3/16″ in a hand drill. I’d like to get a 1/4″ shank stub drill to do this with the machine. The hex wasn’t quite large enough on my first cut (didn’t test…) so when I flipped the part I opened that up a little before I chamfered that side.
First spot drill, messed this up.
Most of the way through first setup.
First side done.
Fixing my hex dimension.
Done!November 10, 2018 at 6:28 pm #75230
OMG!!!!!!! YESSSSS!!! You have just made my night!
That is sexy!November 10, 2018 at 7:02 pm #75233
BeautifulNovember 10, 2018 at 7:25 pm #75234
3/16″?!? Wow.November 11, 2018 at 9:08 am #75281
Thanks guys! I think she’ll suffer more, that piece was the only scrap steel I had laying around.November 11, 2018 at 5:13 pm #75331
Wood dust, yuck.
First serious engraving run, came out pretty well. I have had the CAM & stock for this laying around for a while. Used a 30 deg v bit to minimize the effect of stock height variation on trace width. My outer contour was too close to the ring around the whole outside which is also supposed to be engraved, so I negative offset a finish contour a bit to get rid of it. Still needs a little cleanup, later. I think this would be cool in side lit acrylic.December 6, 2018 at 8:44 am #78305
Making parts for an AEROSPACE company on my $500 CNC!!!
(that’s what I’d title my video if I were a clickbait Youtuber)
Situation came up at work where we needed a piece for some tooling done ASAP and it takes forever to work through the correct bureaucratic channels and have it done in our tool room, I probably wouldn’t have had it for a couple weeks. So I went home and made it on my MPCNC instead J. Two hours later, a solution was designed, programmed & cut. I wish I were allowed to make more neat stuff, problem solving quick turnaround engineering/machining would be a dream job… Cut dry without air blast, chip clearing was no problem on this part and my air blast was dismantled while I turn it into a misting system
Aluminum plate for a handle used to pick up fixtures that go in something akin to an oven (won’t elaborate further). They get hot enough that the straight 3D printed version I tried was melting, so some metal was needed. Works great! The handle was printed on a Markforged Mark Two & reinforced with carbon fiber, it’s crazy stiff for a plastic part.
A little close for comfort, that was lucky!!
Hooks nicely on the fixtureDecember 6, 2018 at 8:56 am #78307
Great design and execution! If it’s anything like the place I used to work, you’ve got some “Cinderella money” coming at the end of the year. Probably a good time to request some new capital equipment in the form of a CNC machine and some spare parts :).December 6, 2018 at 9:05 am #78311
Great design and execution! If it’s anything like the place I used to work, you’ve got some “Cinderella money” coming at the end of the year. Probably a good time to request some new capital equipment in the form of a CNC machine and some spare parts :).
I just counted it as two hours of overtime and am moving on. I’d love to do stuff like this full time, but we are a union shop (I am salaried) and they are extremely protective of their work. I have a tiny Taig lathe in a storage room & even that is getting a lot of kickback.
It really sucks that we outsource a ton of production and tooling (industry is insanely busy right now and we don’t have the manpower/machines to keep up) and all that money goes to companies we have relation to but the moment I want to do something useful and help out I could get in trouble for it. I am the major proponent of 3D printing at my work & even that is becoming a gray area as I’m working printed fixtures/etc. into production areas.
/ranting, I just want to make stuff and be happy 🙂
You must be logged in to reply to this topic.