New owner of a journeyman x50 and first cnc and first post, ouch.
I calibrate my cnc using the probe block. works fine. Using GO GCode to move, I have about 0.1% tolerance in excess (60.07mm mesured for 60mm move). I can live with that.
But, when I send a toolpath done in fusion 360 of a 20x20mm pocket, I end up with a ~19.74X~19.74 pocket.
First tought I forget to uncheck ‘stock to leave’ but no, it IS unchecked.
I tried different types of pockets, same results (at least it’s consitant)
Any ones knows what it is ? or have some pointers ?
The 0.1% travel error is easy to fix. Just go into the motor setup pages on the controller, and scale the “travel-per-rev” gains to compensate for any slight ball screw lead errors.
Your undersized pockets are most likely due to slight machine and tool deflections from cutting pressure, as nothing is perfectly rigid. If I need a highly accurate cut, I’ll first rough it out with a climb cut (to minimize tear-out), leaving about 0.010" of material for the finishing pass. Then on the finishing pass, I’ll use a conventional cut, which minimizes fuzziness.
On many toolpaths, Fusion has a “Repeat Finishing Pass” check box to add a “spring pass”, which simply traces the exact same path again, to remove a little bit more material.
Even after all that, I find that I still need to specify a “Stock to leave” of about -0.003" on my finish passes, to get pocket dimensions dialed in just right. By way of comparison, your 0.24 mm error equates to about 0.005" of error on each side of the pocket.
I understand what you said I it makes sens. but if it were bit deflection I would imagine that a ¼ bit would deflect less than a ⅛ and so the mesurements should be slightly different but my results are consistant…
Gonna do more tests based on you’re reply tough. thanks a lot
any possibility that there’s a probleme in the postprocess ?
I’ve never seen nor heard of a post processor causing a scaling error.
But like I said, nothing is perfectly rigid. The machine (especially the tubes), the bit, and the material will all deflect a little bit under load. And depending on the preloads on the various bearing in the machine & spindle, you could have a little backlash in the mix as well.
Since you are willing to do more testing, perhaps try a 10X10mm, and 30X30mm pocket.
Also try making a 10X10mm, 20X20mm, and 30X30mm square.
Using the same endmill, I would be curious as to the results you see.
I also recommend trying something other than MDF. I don’t know what it is about MDF, but I always get spotty results and it dulls my end mills rather quickly for some reason – maybe all the glue?
My experiences are similar to BuckeyeDennis. Bits themselves are rarely off by very much.
I generally find that a Stock to Leave of -0.1mm (-0.004") results in a tight fit. If a clearance is needed, then more negative Stock to Leave is added. With Fusion, this can be specified with a parameter so that adjustments can be made without changing the 3D design model. I usually use a finishing pass of 0.1mm to clean up cuts and improve dimensional accuracy.
It’s been my experience that the precision of CNC fools me into attempting to make things fit much tighter than I would using traditional tools. Penance time with rasps, chisels, and sandpaper eventually smartens me up.
Ok… I’m not going to bother you with all the tests I’ve been doing these last few days.
I think as said by others I was expecting to much of the CNC idea. After adjusting my calibration and my expectations I have coherent and quite good results.
I’m still a noob so there’s a lot of room for progression but at least I’m at an acceptable starting point.
Thanks all for the reality check and all your advices and experience feedback.
I will be back with a lot more questions for sure but this one is closed.
I would recommend searching this forum for discussion of step motor resolution. I have an elite, and they arrive with the motor resolution set to 400, which is very corse. I don’t have the math in front of me, but that 400 resolution, run through the pitch of the ball screw translates to a not-super-accurate tolerance. Something like a dozen 1/1000" per step I think, but don’t quote me there. First thing I did when I got my machine setup was adjust my motors up to 2000. There are dipswitches on the motors and software settings. Might be worth looking at.
