I’ve been using the OF for a few months now but I’m now seeing that when I call for a certain size, I’m always off by a fraction. I designed a small tray in F360, 95x65mm outside with 3mm wall thickness, machined today with expensive tooling, multiple toolpaths, no stock to leave etc etc and I’m oversize on the outer dims but nearly 0.2mm and under on the inside by a similar amount.
See photos for full info.
Is anyone else experiencing the same? Or am I doing something wrong?
Regards
Andrew
Most people need to calibrate their machine to be accurate. The Onefinity is very precise, but isn’t often perfectly accurate out of the box. Search the forum for adjusting the motor motion settings.
I often find that when milling Aluminum you really have to go slow, or the bit deflects slightly and tolerances suffer. It is not really a machine issue vs a bit issue… with that said while the OF can clearly carve and cut aluminum it is not going to compete with $50K+ metal CNC’s when doing harder materials.
-Alex
I tested my machine for accuracy and I had to adjust a fraction of a mm in my travel per revolution setting. Stock was 10mm and I think my one axis I had to adjust it to like 10.09 or something like that. There is a thread in here and one of the members wrote up an excellent method for testing each axis.
Yeah Im generally keeping with in 0.002"-0.001" (0.05mm-0.02mm).
Also you didn’t mention it above so Ill ask, are you finishing your walls with a contour and spring pass? Or just running and adaptive strategy?
In addition to the above, also check out the dimensions of your bit. Just because it says it’s a qtr inch doesn’t mean it is. Also, if you set the X/Y you may touch inside a flute vs on the solid part of the bit and be fractionally off.
Hey Andrew,
may I ask, are you milling this with the makita trim router?
Hi all, to clear up a few points.
Yes, I’m using the Makita router and finishing contour passes with a very light cut. My tooling was very expensive and is definitely the size it states:)
I have a Faro arm in my lab and did some checking on the calibration today. Over 800mm I’m around 0.15mm under on the X travel and I’m almost dead on on the Y travel.
So I’m still a bit confused as to why I’m almost 0.2mm oversize over 95mm on the X dimension of my part…??
Don’t forget about the runout on your Makita, not a precision tool. When I went from Makita to spindle I noticed a large improvement in accuracy, quality of cut, surface finish etc. I will never run a trim router again.
I checked the runout on the router and it was around 0.01mm.
0.2mm is a large enough amount of runout that I would be expecting a poor surface finish on the walls and floors and I’m not seeing that… 
Only other thing I can think of is checking your programming then. Did you have stock to leave selected? If you derived you contour operation from your adaptive operation and forgot about this it could have been selected mistakenly. You mentioned expensive tooling but have you actually measured it? Also could be in other parts of you CAM program, speeds feeds etc. If you are running too hard then tool deflection is a good possibility. Single, 2 flute, 3 flute? Different tools on different operations? Brand new tooling or used tooling? Tool length out of holder etc. Holding .002" shouldn’t be an issue with this machine from my experience. Just remember that while these machines are quite rigid, your’e not running a proper VFC and need to program accordingly. Also the rigidity of your work holding is massive with aluminum also. I’m attaching a photo to give you an idea of how I’ve set mine up. Hope this helps.
Hi alldaysammyj I’m just receiving my machine today and I wasn’t sure if I would go with the Makita or with a Spindle/VFD but, after reading your post, I think I’m clear now. Do you mind providing some details about your spindle/VFD choice in order to create my shopping list? Thanks in advance for your help with this matter.
Yeah no worries. My personal opinion is go spindle, period. I have both an 800 watt and 2.2 KW spindles. Both work well and have their purpose. The 2.2 kw spindle has an ER-20 collet so I can run tooling up 1/2 inch diameter. The 2.2 kw will be mounted to my Joyrneyman model when it arrives and I will just be milling wood with that machine. The 800 watt will be remounted this machinist model and will do both wood and aluminum.
Hi. Thanks again for the input.
The part was programmed with separate toolpath and tools for each operation, facing, adaptive clearing, pocketing, contouring, chamfering. The interior pocketing and exterior contouring toolpaths were not derived and the “stock to leave” was off. The facing was done with a Datron 12mm steppes 2 flute, roughing was done with a 6mm Datron 4in1 single flute and the contouring with a 6mm DLC Cerazit 3 flute bullnose . The final cut was 0.2mm radial, full depth, 29000rpm and 0.05mm fz.
Workholding is via a SMW modvice on an aluminium fixture plate, which is bolted to aluminium bosses glued into the enclosure table floor, which is TRESPA, a really dense composite work surface.
I’m really not convinced it’s deflection, some of the cuts I’ve made in aluminium are mirror finish, just the wrong size…
I would look at this post: Testing and tuning OF for accuracy - #15 by cyberreefguru - but instead of using “eyeballs” on a ruler to see if the movement is correct, machine a pocket the largest size your accurate caliper can measure, and make adjustments from there. You should be able to adjust the distance/step setting to get this dialed in a little closer.
I checked this yesterday with a Faro arm and don’t see any cause for concern, maybe 0.15mm over 800mm of travel. Certainly not 0.2mm over 65mm of travel anyway.
Very strange. Looking at your pictures a little closer, it looks to me like it’s behaving as if your bit is too small or “stock to leave” is on. The router went to the right spot, but it didn’t cut “far enough” on both the inside and outside cuts. That it is off by the same amount in the X and Y dimensions also points to the bit, rather than the steppers being off in their motion. Also, if the steppers were moving the wrong distance the wall width would be closer to the right width - it wouldn’t be off in width .2mm over 3mm - it would just be in the wrong place.
Can you try a test cut with a new/different bit? Maybe the bit you’re using for this part is off or worn?
Are you using 6mm end mills in .25” collets? And if you are using the touch probe to find zero have you adjusted your tool diameter in your controller to 6mm from 6.35?
Hi all.
So I just did a sanity check on the final pass toolpaths and I can confirm “stock to leave” is definitely off.
I also just mic’d the tools using a Mitytoyo digital mic and it is 5.998mm.
I am using a 6mm collet and the touch probe with a 6mm solid carbide rod to zero the machine, and the probe tool size is 6mm, I’m all about the metric 
Does anyone have any experience with cutter compensation in F360?
