Finally finished moving the machine into a garage. Had to make a new desk and clear out a ton of stuff. This build is primarily for milling aluminum. I took the size advice and lowered the z axis about as low as you can build it. I only have about 3cm of z travel. Still need to come up with a good clamping system. Everything is sitting on some osb particle board which I don’t want to use as a wasteboard just yet. I am probably going to put another board on top to move the workpiece closer to the gantry.
There are some really early stage pics taken at night just now…kind of rushed. I am seeking advice from people who have had success with aluminum, particularly the feed rates.
The 2 circle cuts are really basic test gcodes. They’re 20mm diameter circles with .2mm left over until I find a way to use the cut outs they have on estlcam. Currently I am using fusion360 w/ v10 post processor. I need a lot more learning of the cam, but I like the workflow from model to cam on autodesk.
Currently I have tested with carbide 1/8 inch single flute endmills, the same ones Ryan sells on the site. I also ordered a double flute of the same type. My feedrate is 10mm/s and 2mm/s plunge. The DOC was .5mm. A little on the aggressive side compared to what I am seeing.
As you can maybe see from the blurry picture of the test cuts, the edges are pretty burred. Is that normal to expect? The diameter was nominally 20mm but came out as 19.5mm. Little disappointed, I suspect it is from the really crummy surface finish. They were done conventional milling which from what I have read, seems pretty much worse in every way compared to climb milling. Does anybody ever climb mill aluminum? I tried climb milling and it was a complete disaster! The work came unclamped as the bit started burring itself into the workpiece, a common issue with climb milling. I don’t think I want to try it again seeing as it probably almost broke the bit. Then again I am curious to see if I can pull off a climb milling light finish pass.
I used adaptive clearing on fusion. The bit spirals from the middle initially. I am going to try a lot more tests tomorrow. I have 72 of those sheets I picked up on ebay for this very reason so I have lots of test material. This has got me curious though on higher feeds https://www.youtube.com/watch?v=_o5sBvN_VF8
Stepover %? Less than 45 is a good place to start, yours looks like 80%. What kind of aluminum is it?
Not saying you can’t cut fast but metal has very ideal settings once you find them, the only thing to vary is the depth usually. Depth will vary on the mpcnc depending on your builds rigidity. Wood is extremely forgiving, metal will eat your bits and crack parts.
Adaptive and tricoidal help push this further. Start light, shallow, low step over and get a clean cut, good surface and edge finish then work your way up.
I can’t find the percent, but there is an option for maximum engagement which seems to be stepover. I just started cam today so I am still a huge noob. It is 1.27mm, which out of 3.175mm is a 40% stepover. On the simulation it looks 40%. They are 6061 T6 plates, 1.55mm thick. I think I will keep a +5mm/s feedrate as I keep reading everywhere how these endmills especially at this speed will more rub that actually cut. What I will experiment with tomorrow is a finishing climb pass unless. First though I am taking your advice and doing some shallow depths and stepovers.
Just did a second run today with brand new bits I ordered. Same Kyocera brand and size, but I also have a 2 flute I have not tried yet.
The results are significantly better! My other endmill must of been really dull because the burring on my cuts are totally gone even though they’re the same bit and gcode. My tolerances are still a bit off. The ID of the big pocket on the Y was 19.7mm, the actual is 20mm. .3mm is pretty good but I know I can get better with more refining.
Look at the chips They’re no longer dust but actual flakes. The aluminum sheet was only slightly warm after the cut so the chips are definitely carrying the heat and not being recut.
From what I have seen on youtube, some people seem to be feeding too slow. Don’t want to jump to conclusions because I don’t know their settings but from my research and results, you want to feed faster than what I see on the MPCNC. With the 30,000rpm of the router, either you go single flute or you have to really amp up the feeds, otherwise you are rubbing and not cutting which worsens tool life and surface finish.
I will do more tests later but I am feeling pretty confident in the rigidity. I accidentally plunged 1mm DOC 40% stepover at 8mm/s and I noticed no chatter even on my rubbish setup.
The cuts look great. There are always little things you can change, that’s the fun part. 0.3mm is pretty good, I would guess with aluminum you can make a much smaller finishing pass than wood and get that a little closer. At the same time if you’re outside cuts are a bit big and your inside cuts are a bit small it count just be the diameter of the bit is a little off, if that makes sense.
I have been doing tons of cuts lately trying to keep up with the lowrider flat parts, so I keep testing lots of settings and bits. The single flute seem to work significantly better on all materials I have tried, they even drill/plunge better, they might be giving me odd shaped small holes though, or maybe it is something else. Next I want to try the single flat flute but they have not been delivered yet.
How perpendicular is enough would you say? Along a 100mm span from my collet, I raise about 1/16 inch on one side vs barely skinning the bed on the other. I tried putting tape on the mount and nothing seems to do much. I think I will just leave it as it is because I am getting .1mm tolerances with 1mm DOC 8.3mm/s just fine.
Remember I am talking about the z axis perpendicularity. I don’t believe my feet are off as if you see from my pic, they’re all as short as you can make them. That makes their overall length irrelevant from the conduit length which is often what varies. I can tell I need to change something about the perpendicularity because my bottom finishes all have end mill marks. They’re facing the x axis, and look like a ton of tiny crescent moons. I also get chatter at certain points How do I shim properly?
Possibly, when I test it all the z axis height varies by about 1mm. It only chatters lightly on certain parts of the circle. My feed is aggressive and it just slices through, just need to fix this one issue and I am perfect.
I notied something with my machine that may or may not be the same for others. When I lock the steppers and try to flex my gantry by pushing the bit, most of the flex is coming from my zip ties. This leads me to believe that I need to secure my belt more.
My belt isn’t loose, it may even be too tight but I am convinced that I am losing rigidity due to the lack of hold my zip ties are giving to the belt. It is allowing the gantry some linear “allowance” due to the elasticity of the zip ties giving it. Maybe I need thicker/shorter zip ties but it is just something I noticed. I suppose this is somewhat of a downside of using belts vs ballscrews but they are a LOT cheaper and have very little backlash.
Edit: I just tried to move the bit even more, and it is more severe than I thought. I would say around 80% of the deflection is caused by the whole gantry moving in respect to the outer rails due to the belt actually moving with it. Hardly any of it is z axis flex or conduit flex.
one end of your belt should be basically zip tied directly to the mount, zero flex. The other end should be as close as possible and this will give extremely minimal flex. Sounds like you might have some big zip tie loops.
Also see that you have them oriented like in the instructions, that helps as well. you should not be able to notice any movement do to the cable ties.
Yeah those were my thoughts too. One end is tied like the instructions, but yes I would agree that the adjusting side is far too big…whoops. Now I gotta buy new belt, darn. At least now I know that I have still not maxed out the machine just yet, it’s got more rigidity in her
If you get the tension right it should be too bad, you can also try zip tie to close the loop, around it perpendicular. The size shouldnt matter too much don’t buy new belt.
Lol, the order was just placed. There goes my $8. 5m of 6mm wide. I am just gonna cut the belt a little too long on each axis on purpose, then trial and error the length until the tension is proper and each side looks like the fully locked down side. With such a short z axis combined with all my cutter load being pretty much radial, this new arrangement should hep immensely.
I am thinking about getting an air compressor type thing to put on the gantry to maybe add some air cooling. My endmills are not lasting very long I have went through about 5, thing is only 1 has snapped and only because of a crash. My Kyocera single flutes keep chipping. My only double flute died in a collision, poor guy didn’t even have a chance
I think the issue mostly due to our machines only being able to be rigid enough to do a DOC on 100% full radial engagement (like a slot) of the very tips. The rest of the flute length is totally wasted, I feel like I am just wasting endmills I shouldn’t be.
Also, they tend to get molten aluminum coated on them, but only a very thin coat. Perhaps cooling is the answer, didn’t think it was needed since my MRR is so low.
Whatever, video up soon. I am beginning to mill up some electric longboard motor mounts.
I suppose so, but adaptive clearing only works when the slot is above the cutter diameter. My way of cutting out parts is to do a contour around them, so I guess now I have to sort of make an oversized pocket around it, maybe 4 or 5mm wide and try that. Kind of a weird way of doing things imo, but I have adaptive cleared at 2mm doc with no chatter at all. I’ll try this out
They’re no longer dust but actual flakes. The aluminum sheet was only slightly warm after the cut so the chips are definitely carrying the heat and not being recut.
How do I shim properly?