After a year of working with the MPCNC I’ve reached a state of general hapiness! Hooray!
My machine is fairly small footprint (200mm travel) and about 70mm Z travel (I usually work with a vice). This week I’ve built a fogbuster style mist-cooling system which has also helped loads (primarily the air to clear chips). Lastly, running dual endstop firmware and I do most of my CAM in Fusion360.
I took some time this week to calibrate squareness, tram the spindle, flatten my MDF base and square up my vice.
I did some verification parts working with Delrin and the results were very good.
I know the following might sound stupid, but I would like to push this machine to its limits and get to a general dimensional tolerance level of +/- 0.1mm.
Currently on my test parts the accurancy is bound to +/- ~0.3mm levels.
Any thoughts on this ? has anyone been systematically achieving these tolerance levels on hard plastics / aluminium / brass?
Here are the general settings I used for my verification parts:
My steps/mm are still from the theoretical calculation and have not been calibrated in practise. Any methods for doing this calibration with an accurate setup ?
I’ll post some pictures of my machine tomorrow just in case.
I’ve done a calibration of the X,Y,Z steps/mm. X and Y were over-travelling a tad bit.
X was 0.25mm off in 90mm travel.
Y was 0.13mm off in 90mm travel.
X,Y setup like this:
Z setup with a dial indicator (plunger style).
I also performed some tool runout measurement with a dial indicator.
I was hand turning the spindle. I imagine the runouts get a lot worse when spinning at 5-10krpm…
These are the results.
Looks like my tool has a lot of runout (63.5um), but the spindle collet holder has significantly less. Bad collet? or bad interface between collet and the adaptor ?
Anyhow, will re-cut some POM this evening and check with my best calipers to see if the situation has improved
I’ve got a lowrider with the dewalt router but I was able to get within 0.1mm accuracy cutting small parts on aluminum with a single flute mill maybe I got lucky. It might have been more accurate but I know it was at worst 0.1mm. I didn’t try super aggressive cuts but if the finishing passes are setup correctly it shouldn’t matter unless you go crazy. A few things that come to mind are making sure the belts are tensioned, using an endmill no longer than necessary, and using a spring pass in fusion.
That does seem like a fair amount of runout but I’ve never measured mine. If it’s the same on all your bits might be worth trying a new collet? Also check your bit against the collet… I heard it causes problems if you use a 3.185mm collet with a 3mm bit.
I think we need to add some sort of disclaimer about those spindles. The ones with the add on collet thing (grub screws on the shaft) are never going to be good. There are some with a integrated collet, they might be okay (I have one but no test yet).
You are using screws on your belt tension, are you sure you did not over tighten and stretch your belts, there is no other way to over travel, if anything you should be under (kind offsets the runnout this way)…
Odd…The one I have linked, http://s.click.aliexpress.com/e/DetyilFa
The first picture shows the bad kind, the one that ships is shown in the second picture and seems much better.
Yes the spindle is one of those cheap ones with the grub screw collet holder. I guess that kind of explains the run-out issue…
With regards to the belts I’ve got them quite tensioned (no way to quantify though…) Any suggestions on belt tension in general ?
It’s hard to do a “how tight” because everyone’s machine is slightly different, or a lot different. Like Tim said, if you can play musical notes, it’s too tight.
It depends on the length of the belt… my 3D printer is a higher pitch than my low rider. There is a phone app called easy tension that lets you input the belt length and then use your microphone on your phone to measure the tension.
Aight, so I relaxed the belts a bit (used a small torque drive to make sure they are consistent). Results start looking better now. Tried a project with Acrylic today and dimensions were +/- 0.2mm.
What I noticed was that in general external dimensions are oversize and internal (pocket) dimensions are undersized.
For example my part today had:
Nominal external width dimension 50mm, was measured 50.2mm
Nominal internal pocket width dimension 20mm, was measured 19.8mm
That suggests that there is flex in the whole gantry system? then again I am using a repeated finish pass option on Fusion 360, which in theory should take care of that right ?.. these are my assumptions… feel free to point out where I’m wrong
I am having a hard time thinking of what it could be if not the fusion settings. You could also try configuring probing and measure the accuracy against a 1-2-3 block using the bit as a probe with the router off. There is a backlash compensation feature that uses this m425/g425
Thanks guys!
I can confirm Stock to leave is definitely turned off during the finishing pass.
Blockquote
You could also try configuring probing and measure the accuracy against a 1-2-3 block using the bit as a probe with the router off. There is a backlash compensation feature that uses this m425/g425
I am not 100% sure what you mean here my friend… can you give me a bit more detail please ?
Being slightly over on an outside dimension is a new one, if anything it should be slightly under. Double check your bit diameter maybe. how are the diagonals, holes round? Spindle trammed?
Thanks for the suggestions Ryan! (btw your machine rocks! full stop!)
Bit diameter is questionable yes - I need to find a reliable way to measure.
Spindle is trammed indeed. Got 2.5 thau “out of vertical” over ~200mm diameter circle.
The machine is pretty square (using the dual endstops to compensate for hardware out-of-squareness). Using a 250mm pen drawn square, I cannot tell a difference in the diagonals using a standard ruler.
I’m machining another part now. Will let you know of the dimensions.
Measuring “truth” can be a real rabbit hole if you are not sure if the bit diameter and spindle runout, and a single flute is tricky to measure separately.
At a certain point you could just modify the bit diameter in CAM to reflect the effective diameter which in your case is 0.2mm undersize, and as long as it is repeatable you will get good results. Nevermind whether it’s runout or diameter.
To this end, I considered just running a single slot path in some material and measuring it, then calling that my tool diameter. Would that basically be the same thing for practical purposes?
interesting stuff! so I was cutting with (what I thought was) a 6mm single flute.
I set my calipers to 6mm and the cutter was easily free to rotate within the jaws. I tried to measure exactly and it must be close to 5.8-5.9mm.
I guess that explains more the problems I’m seeing!
