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.

With regard to tricking the z down and re setting, where might one do that? Is that just in my Shopbot control software?

Nate, I started in 2013 with VCP7 Shopbot edition, but I THINK your Partworks may be upgradeable by Shopbot to VCP8 and you may want to check it out.
Only seen 3 upgrades, but Version 8 was a Major one and just the 3D model library alone is worth the cost.
I think the choice of wood had a lot to do with your fibers ripping up, but I just did a Lacewood 3D and used a 3/16"upcut, and everything cut fine until it hit the first "Peak" of a mountain...It tore the fibers up so much it looked like a Chia Pet:( I only had a .02" skin programmed and it blew right through that. Wish I had taken a pic of it.
I swapped to my .25" downcut/ Z'd to my spoilboard like the first time/ Moved to a spot with a hole in it/moved Z to -.01/ and then Zeroed Z axis in Keypad.
That dropped my cut down .01" and cleaned off the tearout. It was the Lacewood fibers that made it so bad I think, but Butternut was the same way, and from what Gert said, Basswood is similar. Denser woods seem to cut cleaner.
There are other ways to trick/nudge Z down, but I like simple when I'm tired.
Just do the same thing with your finishing toolpath Z.
Seeing as you can't specify a Tapered Ball Nosed in PW3D, I like Joe's idea of cutting a relief so your finishing bit won't touch.
May want to decrease your stepover to reduce the ridges unless you like sanding more than I do.
Here's the downcut roughing in Lacewood....it's a World of difference from the upcut 2F disaster.
scott

I'll give that a try. I roughed out around my carving with an endmill and no more issues with my 77-102 hitting sidewalls. Still made about breaking that damn bit. Feel like I just lit 60 bucks on fire 🙈. At any rate, here is a follow up picture. I changed the feedrate to 1,1,16k and man it's looking nice!Attachment 28964

As it turns out I don't have VCP. I set up my bot to carve overnight and about 60% through my file I got a missing comm error. I'm so bummed out. I normally don't have issues with that since I grounded inside my dust tubing. I got back to the shop early this morning and my spindle was still running sitting in one spot and very warm. Maybe I'm just destined to be a 2d part cutter. It's a bit frustrating so I have to walk away from it for a while and go back to this project later this week

Might be a good time to try this?
https://www.youtube.com/watch?v=OLY1...de=transparent
Hopefully you had your log file active, or noted on the control panel what line of code you were on.
Bummer, but it could have been a fire, so look on the bright side.
How did the cut area look?
scott

Nate,
When I first started with VCP7, I think I remember TJ and others saying Partworks and VCP were the same thing, so they decided to call it VCP Shopbot Edition.
I may be wrong with your version, but if your screen looks like these(but with less icons) then you can probably upgrade through Shopbot, and only have to learn the new tools they added that add more options for ease of drawing and 3D.
I had to struggle with PW3D, but 3D's are WAY easier now.
Somebody correct me if I'm wrong please.
scott

I just have to say thanks again everyone for all the input! This forum has been so great over the last few years getting to know my Bot.

At some points I get so frustrated when I get comm errors, or a part doesn't run correctly (usually because I've told it not to). The comm error I know is usually attributed to grounding and I'm baffled, maybe there's something I'm missing. Maybe its a computer issue. I've been playing phone tag with Shopbot as I've got a couple technical questions as well as to inquire about software upgrade availability.

In the mean time, those feed rates worked out really nice.

How fast would any of you guys recommend pushing that ballnose bit while carving? I know it varies depending on the product being cut, but do any of you cut faster than 1,1,16k? Specifically talking, faster feed rates on a PRT Alpha or do you start to run into cut quality issues?

Just Desktop doing small stuff, but 1,1,16K....1.5,1.5,17K....2,2,18K have worked well for me depending on size and material...remember though I'm using a spade type Onsrud engraving bit with.005-.01 flats for tiny details on the Desktop in Maple,Cherry,Black Walnut,Bloodwood and Lacewood.

Scott,

So I think I accidentally deleted the information file that told me what line to attempt to run from because I actually had those values set to record.

My file has 1.4 million lines of code so by looking at the amount of carving completed I figured starting somewhere around 795,000 would get me close to where it quit.

I went through his video tutorial and tried to run from line 795,000 and hit "Go to" and it lags for a few seconds, and then gives me a "Run Time Error 9; Subscript out of range". Click okay. Shopbot 3 software closes, spindle turns back off. Strange huh?

Not sure Nate, as I never had to use that yet luckily.
Does sound odd if you followed all the steps correctly:(
Log file should be in the same folder as the .sbp folder in the control computer?
I'm computer illiterate, but thought most "Run time" errors were windows/computer related.
Sorry it didn't work, maybe someone who knows computers/SB3 version you're using will chime in?
What SB3 version are you running?
No internet for for a few days...hope it works out for you!
scott

I'm just also going to throw this out there for what its worth...

My computer running my bot is older. AMD Athlon X2 Dual Core Processor 4600+ 986MHz. Ram is just under 2 gigs. Running SB3 on Windows Media Center Edition 2002. I don't connect it to the internet. And I don't have any programs on it other than Cabinet Parts Pro, PartWorks 3.5, and Partworks 3D. All of which are closed when running parts.

I've never heard of the Window version you mention but that's just me. The favorite for years was XP and probably hard to find now. Some people on the forum have reported using Windows 7 and 8 with good luck.