3d Carving help

Hi All!

So I'm cutting a deer scene piece in some basswood for a charity thing and not long into my finishing toolpath my tapered 1/8" ballnose bit snapped towards the top of the cutting threads. I haven't really cut anything 3d other than a few tests over the years in foam board so as far as feed rates and settings I'm no expert. Hell, I don't even have Aspire (yet)! I did my rough pass with a 1/4" endmill.

Attached is a screenshot of my toolpath setings in Partworks 3d, as well as a picture of the piece being cut and my broken bit. Looking at my settings, am I cutting this too fast?

Do I need to get rid of some of the excess wood around the long edge of my carve? It seems as if when it hits the edge of the cut it wants to take more of the boarder around the carving out with the ballnose bit and maybe because its a deeper cut it is putting too much stress on the ballnose bit? Any advice would be greatly appreciated! TIA.

Attachment 28962
Attachment 28961

Nate, What VCP are you running?
Only done a PW3D a few times,is there an offset/allowance in the roughing path to remove some of the border material?
Speeds/feeds if anything seem a bit slow( maybe 1,1,16K? at least), and speeding up will allow a lower stepover (like 8%)for less sanding and a better finish?
Bass Wood is a hand carvers delight, but may not be best for a CNC cut. Never cut, but they say it's a lot like Butternut which wasn't that hot for 3D.
Listen to other people instead of me, but just my first thoughts from my couple of dozen cuts.
scott
I would NOT have expected a .125"TBN to break on that cut:(

I am not going to touch basswood again on the CNC. Way too fibrous and tough fuzz.

Depending on your roughing path setup (skin thickness or work envelope), the finishing bit may have run full length into the roughed-out side wall and snapped. You must make sure the finishing tool touches only with the very tip.

I think it did break because it hit the sidewall just from what I could see and hear when it started finish tool path. Maybe I can try to take a router and clear some of it out before. I think part of my problem is that Partworks 3D is pretty limited. Might be time to invest in some more software. Most of the time I'm only cutting 2d parts for cabinets and countertops.

Do you think if I change my speed and stopover settings and re run my file I'll be able to salvage my initial roughed piece without seeing a line where the first cut quit when my bit broke? I am also really hoping my local rep has a replacement bit so I don't have to tie up my bit waiting to finish a project I started.

Nate,

I would draw a rectangle around the 3d (maybe offset by .0125) and have that cut to the finish depth during the roughing stage or separate between the rough and finish stage. That will save the finish bit from hitting the side wall and add some relief to the appearance.

Also, note that Scott is talking inches per second when he suggested 1,1,16k.

Joe

Also, what do you mean by "what VCP?"

VCarvePro.....VCP8 and 8.5 has a much easier 3D format that is almost like Aspire as far as carving goes.
Tapered Ball Nose category in the tool database eliminates some problems, and toolpaths can be mod'd without having to go back into PW3D. Also has an automatic 3D border icon, so that you could run a profile toolpath to clear that side waste, OR profile/VCarve ON the 3D itself.
It also has an offset on the roughing toolpath to prevent what you ran into.
Once you clear the side walls a bit so the TBN doesn't contact it, you can trick your Z down -.005 to -.01" and resetZ and you won't have any lines.
A lot of new tools,3d library, plus the moulding toolpath might make it worth you while to upgrade.
The integral 3D modeling tools make it a LOT easier to change things on the fly after preview.
On your roughing pass,perhaps change to a downcut bit? Looks like a lot of tearout with the bit you used?
Good luck
scott

in vcp in the roughing toolpath it asks how much material you want left for finishing toolpath(machining allowance). I leave a few hundredths for the finishing toolpath, so most of the material is removed during the roughing toolpath, next is what strategy did you use for the roughing toolpath? There are two,a z level and a raster. I usually have better luck with the raster.

Bob

I replied once and lost it (I think). So, hopefully this is not a duplicate.
I am no expert, but I do use my BT32 for carving. I use a .25 diameter roughing bit when I can and I believe it is a down spiral. I leave .020 stock for cleanup. I use the .125 ball nose to finish. I have not broken one yet, but it is bound to happen sometime. For the finishing cut with the ball nose I set the spindle speed to 17,000, the feed and plunge rate equal at 40 (sometimes 60), set the step over to 8%, and then set it the passes at a 60 degree angle away from the direction of the grain. I do end up sanding. I use a sand mop where I can and then a dremel in tight spaces. If anyone has any comments or suggestions on my methods, I would love to hear them.

So I did get a lot of strings because I roughed out with a spiral upcut bit. Next time I'll go with the down cut bit. I'm not sure what version of VCP I have. I know I have Partworks 3.5 so whatever came with the upgrade when I changed the software licenses from the guy I bought my machine from. I will look tomorrow morning when I get to the shop in the morning.