Hi all, this is my “Concept 1” for a Salad Bowl design. I was focusing mainly on the inlay, and not the real shape of the bowl. It took a lot of trial test cuts to get it just right. I also trimmed my z-gantry mount a bit to get it to fit under my machine! Video of making it: CNC Salad Bowl - 5" DEEP INLAY Failure. With so many mistakes and test cuts... - YouTube
Free Fusion 360 download for it:
On the topic of deep cuts, check out this bathtub carve out from elsewhere on the forum:
Thanks! That is definitely a nice tub!
I’m grappling with the layers-vs-deep-cutting choice, too.
I only did layers because I had to do a vertical cut so the inlay would line up. Otherwise, I really prefer to do as deep a cut as I can, assuming the bit and collet don’t hit anything. I usually design things to avoid collisions - Fusion 360 is great for testing out theories and seeing what will happen in Simulation.
As they say where I come from, … Spec-freaking-tacular! I quite enjoyed the video!
I recently did a project where I really needed to minimize chipping and tear out. I ended up using multiple finishing passes, with down-spiral bits, and always climb cutting. Woodworkers like to “conventional” cut because it’s safer for hand routers, but climb cutting pushes the fibers together instead of pulling them apart.
Even doing a final surfacing pass, it mattered if the bit was pushing fibers towards the uncut area, or the cut area. And yes, this was with brand new name brand bits.
Also, many years ago some local woodworkers who were also machinists reported that they needed to leave 0.007" clearance for glue for their projects (er, that might have been diameter, or 0.0035 per edge). If you’re hammering it together dry then you aren’t leaving enough clearance. Also, switch to a non-water-based glue so the wood doesn’t swell from the glue itself! I use a slow set epoxy.
These are all great ideas!
I know the majority of the chip out happened on my roughing pass. I took a look at my tool path, and I was doing a climb cut, but I was using a spiral up cut bit. You now have me wondering if I would have had better success by doing the roughing pass with a down cut bit! I usually use an upcut bit on bowl middles to better evacuate chips, but with a small step down it shouldn’t matter too much.
RE glue: those are some good ideas. I did experiment with tolerance – I know my bit isn’t exactly 3/8" in diameter, so it took some tweaking to get it dialed in. I’ll have to experiment with using epoxy instead of a water based glue; I actually was thinking the water based glue might help prevent gaps due to swelling, but maybe it was hindering me more than helping.
When you did your multiple finishing passes: how much were you taking off in each pass?
/me checks FreeCAD job… these are all 1/4" square-ended bits, 21000 RPM. The “finish” bits are just newer (sharper). The job was basically cutting in inset into an oak panel, and shaping one edge. A simple pattern but oak chips pretty easily.
Looks like the adaptive roughing (300 IPM up-spiral) leave 0.066 on the sides and 0.040 on the bottom. The bottom (100 IPM up-spiral) is finished with a straight pattern in line with the grain. The sides are finished with a 30 IPM down-spiral; first pass removes 0.050", the second removes the last 0.015". For the one edge the final passes were 0.060, 0.025, and 0.015 as I had more tear-out problems with that as it was curved and the bit was guaranteed to cut the grain in the worst possible way 
For chip evacuations, I have two ideas: (1) up-cut but leave 0.5" or so for a down-cutting 2nd roughing pass, or (2) all down-cut and run an air hose to the spindle to blow the chips out. Messy, but effective.
Also, a hint from the woodturning arena - before you do the pass that might chip out, spray the wood with water to make it swell and pack the fibers together.
Awesome…I’ll make some notes of all these things for some of my future projects!
That certainly is a STUNNING bowl! Well done. Not something that I wish to try though
