We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
After owning my machine for a few years I was never quite happy with it’s performance in aluminum, so I threw a little money at it to see if I could get some satisfactory results.
Upgrades:
8" CNC4Newbies Linear Z-Axis w/ fast screw - direct drive 270oz stepper
9mm belt upgrade (thanks tbd!)
270oz steppers all around
2" Y-Axis lift with braces (thanks tbd!)
Makita RT0701C Router
It’s a very simple set of pockets, 0.20" depth, with each of the three at a progressively deeper depth of cut. The pocket starts at a 0.02" DOC (0.5mm), and moves to 0.03"(0.75mm), and finally 0.04" (1.0mm). This is a roughing 2D Adaptive clearing toolpath without a finishing profile, so the edges will look a little rough.
It should be mentioned this is a specialty bit with an extremely long stick out (~2.0") which probably has some blame in the final finish, as I expect it increases whatever flex and runout my spindle has.
Overall it would seem a DOC of 0.3" seems to be the best looking finish of the bunch. I did notice chatter at 0.4" DOC, not sure if I want to push it any further with this particular bit. I will pick up a much shorter bit for profile and slotting work as this is definitely not ideal. I wanted to get peoples opinions on what I could improve, and how it looks so far.
Ultimately the purpose of these upgrades and this particular bit is to machine a FCG pocket in an AR15 receiver, which is about 1.25".
I am not experienced in adaptive clearing tool paths but the 0.03 doc seemed to be taking smaller bites of the material that the 0.002 doc.
And what is the advantage of adaptive clearing method?
Adaptive will maintain (try to) keep the slice thickness constant, with everything else the same different DoC will cut shorter or longer slices with uniform thickness.
2D Adaptive tool path in F360 try to keep the tool load constant. (Width of Cut, WoC)
That means it will taper in/out in corners so the load is maintained. (Image moving into a corner, the bit will engage both sides of that corner unless tapered in/out)
Another advantage is that you can go deeper per pass using more of the actual cutter length and not only the tip area of your bit. How deep is ultimately governed by the overall rigidity of the particular machine.
One example here:
RPM 17K
Feed rate 4000mm/min (157ipm)
WoC 0.1mm
DoC 8mm (Single full depth pass)
Note that 2D Adaptive is a to be considered a roughing operation, intended to be followed up with a finishing pass or two. For such a pocket cut I usually do the following:
2D Adaptive roughing pass with 0.5mm rest material (radial) and 0mm (axial), multiple depth pass (if required).
2D Contour, full depth with multiple finish passes, say 2-3 incremental passes until the radial 0.5mm of rest material is done. Feed rate for the last pass is 50% of main feed rate.
55IPM feedrate, 25IPM helical plunge. The bit (as I mentioned before) is not ideal for this kind of work as it’s a specialty bit meant for AR15 receiver pockets with a stupid amount of stick-out. The part number of the bit used is Destiny Tool Viper DVH #V21624S.
Yes, I mentioned that in my initial write-up, I did not do a 2d contour on these just for speed sake. My AC pass was with .001 stock remaining, and my final contour is usually .001 to clean up the face. I did go back and do a final contour pass of .001" and chamfer and the pocket, it looked fine. I think the reason the pocket edges are a little rough is the runout of that long bit. Granted, X-carve’s are not the most rigid machine, but I think you could expect better with only 1" of stick-out compared to over 2".
I made a widget, came out okay. I learned a lot from this one. I had to bring down my RPM quite a bit when slotting, I was getting some heinous chatter.
Another thing I learned is when Fusion 360 sets the spindle speed below the $30 value, it shuts off your IOT relay. I lost my zero on the chamfer pass and had to abandon it.
Try to avoid slotting when possible. If you use an adaptive clearing toolpath on your “profile”, you can cut deeper and faster to make up for more motion. The tool will always engage the same amount of material.
I just couldn’t avoid it on that piece. The workpiece was cut to roughly the dimensions you see, but that angled portion and the mouth both had to be slotted, unless I did a AC cut for that entire part. This isn’t the bit for this kind of work, but i reduce my speed, add some ramps, and hope for the best. I also have a router plate to cut soon which will have some slotting as well.
Sorry, that was actually on a stock Shapeoko 3. I was bouncing between forums. That’s why I added the Carvey links. It’s more about the toolpaths.
I’d do most of the work with Adaptive, and then I’d finish with a variety of toolpath strategies, including contour for the profile. If you share the Fusion model, I’ll show what I’d do.
I would use 2D Contour with roughing enabled with 0.5mm material to leave. This means it will carve one single pass, a little wide, around the circumference (CF) then step in tighter for a 2nd pass before stepping down to next depth.
This work very well for me as only one side of the bit is engaging when close to the design shape. This also allow some room for chips to clear.
Once full depth is reached a single full depth finish pass is done.
For a non-rigid machine (like ours are) any chatter will make the bit bounce between the walls if they are too close.
Hey pyrex. I would have done adaptive and made a pocket . Just leave a small piece of material at the edge an 1/8" or 1/4" and then cleaned that piece out after with a zigzag path. Then the likelihood of having a tough spot is much less and it would be only in 1 or 2 small spots
Ah, I see what you mean, basically AC an area both ways about 0.5" around the part? What’s the best way to do that, set the toolpath constraints with a spline?
