I run a Makerspace and am a long time mentor for FRC1296. A maker joined who is a parent of students from another team. I just bought a OMIO X8 and other makers are using it for wood with no problems.
I’m trying to get a part cut (to show them how to do it themselves) - happy to do it. It looks good but the Z is screwy. It is 0.250 polycarb and the students have the depth of cut at 0.290. Z0 is set on the face of the part I think. But it is not cutting all the way through, not even close only 0.150 deep or so.
I’m trying a 3/16 2-flute mill with 8000RPM and 20 feed rate. I’m looking for things to try. Any wise mentors or students out there who can help a guy/team?
My spoil board is kinda rough, simple plywood. I think I should cut some MDF that would be way flatter. But the part perimeter is pretty uniformly cut shallow. I doubt the spoil board is so untrue it is the problem.
The bit is pretty tight. I doubt it is slipping
Are my feed rates and plunging rates too high? Maybe I’m losing steps in X because it is too difficult? But it seems to cut like butter as one would expect.
I do not know Fusion360 very well. Are there some magic offsets that could be doing this?
3 things. Look at the actual G code to see how deep you are commanding it to go in Z. Check your Z offset and/or tool length offset on the machine. Check that your Z axis scale factor is correct on the machine, in Mach or whatever runs it.
The G-Code looks right, typical depth is right. For example:
X1.7245 Y-0.1448 Z-0.2897
I can’t see anything in Fusion 360 that might hurt. I’ll check Mach3 but others are cutting wooden parts that look nice. I’m, thinking it has to be in this Fusion 360 file. Arghhh
We had similar problems when first starting out with our CNC.
Some of the problems came from a loose collet and the tool slipping upwards. However that doesn’t seem to be your problem.
Another one of the problems we had when self-teaching CAM/CNC was we selected the top contour instead of the bottom contour and our bottom height (in heights tab) was set to x below the contour. The X was less than the thickness of the material. However, its hard to say exactly what is wrong without looking at the CAM itself.
If you share an archive file I can see if I see anything.
our 0.25 polycarb recipe
600 ft/min surface speed with a 2 flute 1/4 inch endmill. 55 IPM 0.003 feed per tooth
27 ft/min plunge rate at 0.003 feed per rev
we also use a maximum roughing stepdown of 0.1
Edit: If you simulate the operation does it show the endmill going through the stock?
There’s a set screw coupling the motor to each axis on the Omios. I’ve sometimes lost steps due to a loose set screw. Worth checking while you’re at it for all axes.
great suggestion! will do! Another maker milled an absolutely beautiful walnut stock for an antique rifle a couple days ago. So I’m leaning towards Fusion360 error since it is these students first effort and I’m a flailing SolidWorks guy. But I’ll go check the set screws now!
As for your feedrates, they sound a bit slow for thin polycarbonate I think (I’m no expert, but you’re also using a 2 flute bit), which probably accounts for why the cut in the photo on the facebook page looks a little messy/gummy. I have used 1678’s spreadsheet extensively with great results. I’m unable to find it at the moment but will link it in a bit.
Thanks! If I simply run my finger along a cut it cleans up pretty nice. But I definitely need to get the best practices down for polycarb. 1296 will want to make some parts sooner or later!
It would depend on how you have the bottom height set up in the heights tab. If you want to use the contour to determine the bottom height, then selecting the bottom contour is important. We do this, but we might go ahead and change it to stock bottom in our template. If you use model bottom or stock bottom then the contour’s height would not matter.
If your “stock” is being generated with it’s middle centered at z=0 rather than it’s top starting from zero, that would explain the ~half thickness cut. (or if your “stock” is being generated at half thickness… but thats much less likely)
I encourage my students to avoid “from stock” settings. They’re great for doing the same contour in multiple thicknesses of work pieces, but can bite you if the stock is set up incorrectly and is difficult to diagnose. We usually run bottom height at “Selected Contour” like jago is showing in the screenshot.
The other use case for “from stock” is adopting a customer part to your stock without modifying the customer data. The team owns our own part data & can adjust the part data to match our stock, rather than needing to treat customer drawing data as sancrosect.
I think they did just that. The green line in design mode goes through the middle of the thickness of the part (what would be Z if it were drawn optimally)
