I’m trying to make a tray. My bowl bit is leaving behind a lip. I dont know if this means my settings or wrong or if I need to go deeper with the bowl bit our what. Attached is my c2d file.
I use a 1/2" chip breaker to hog most of it out, then come back with the bowl bit to make the bottom nice and have nice curbed bottom edges. The bowl bit is an UltraShear 3/4" diameter (1/2" shank).
Any advice would be welcome.
24x10.5 charcuterie board.c2d (288 KB)
Looks like the toolpath is offset too far from the sidewall. Or the bit is not going down deep enough. Is the bowl bit cutting the sidewall at all?
At first, I thought it just needed to go deeper. So I ran another pass and it actually seems worse. I didn’t watch for contact with the sidewall, so I guess I’ll have to cut another pass to see if it actually hits the sidewall at all.
edit: analyzing read your post better
This is the bit I’m using:
Ultra-Shear Bowl Bit, 1/2" Shank, 3/4" Diameter, 3-Flute Deep Reach, 5/8" Cut Length, 1/4" Radius, 2-7/8" Overall Length
Only thing I can guess is you are losing steps running those feeds and speeds on that 1/2" compression bit in oak. FS wizard is saying its viable but I’ve seen the S5Pro lose steps on less? but then you’d have the lip on only one side so I’m kinda confused too unless this is another one of those “carbide create is more for artistic purposes use meshcam” type deals where CC just doesn’t understand.
You should be getting a lip in the corner though because your corner rad is .25 vs .375 on your bowl bit!
If the case is you just have an issue in the corners add a .375 radius to all corners and your problem should be solved.
That said I see that is not the case… hm
Good catch on the corners though, I’ll need to adjsut that either way!
The radius is .375 for the bowl bit, that’s what you should have set on the pocket. The .5” bit will cut the .375” radius, most will offset the pocket to leave .1” or less for the finishing pass with the bowl bit.
I’ve not done the “finishing” pass idea yet. I want to make sure I undestand that. Make one pocket with the .5" chipbreaker. Then offset (outwards) someting like .1" and assign the bowl bit? So that would have to start at the top fo the stock again? Feels like I’d have to do something else too with that finishing pass…or I’d cut a lot of air if I started at the top of the stock with the bowl bit again. I think I’m missing something on that concept
Further to this try a small plunge about .2 max into the oak and measure the diameter of the cut maybe you got unlucky with an oversized compression bit.
Well shoot, screwed up. Fat fingered my settings. Going to have to make a new board. Things went south pretty quick there…,.
yeah its nice to create a separate tool in your library for each thing you do. That way you can have easy access to all the profiles without fat fingering
That’s another good idea I’ll be taking advantage of, At least I learned a lot today. Appreciate all the input!
Good point. 20 characters.
This should help you out.
Your rough path has a depth of 0.865, and the finish path is 0.940. That’s only a difference of 0.075
And the radius on the finish tool is 0.250.
If your final depth is 0.940, the rough path should be no more than 0.690
I would follow the rough/finish strategy mentioned.
Offset the curve inward about 0.010" and use that curve to rough to 0.690
Do a contour path on the outer curve with the bowl bit from 0.000 to 0.690 to finish the sides to that depth
Then do a Pocket path with the bowl bit from 0.690 to 0.940 to finish the bottom. Use a reasonable depth per cut, 0.050 - 0.100??
Isn’t it just that the slope on the side of the bit is steeper than the design slope, and you are taking big cut depths. To have a smooth side the bit needs to move over and down along the slope of the side of the bit
John
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
