Success and a bit of failure, bad cut files from V-Carve

OK, finally got a chance to spend learning the software side of this and try some cuts yesterday. Engrave, success!



Next was to cut some pieces from that, and now we have a problem.



The bottom cut was supposed to be 5.5" wide by 3" high. I can't remember the dimensions of the top one, but it was supposed to be higher, same width. At least I got to test the emergency stop.

Both those cuts previewed as expected so I have no idea what happened here. I'd attach the design and output files, but I'm not seeing a way how to do that in the forum.

OK here is a first guess try. Looking at your engraving it appears the wood has high center bow in it (left to right). The engraving on the left is very light while the engraving on the right is pretty consistant. So when you did the cutouts the Handi might not have stayed in position since the base did not have a solid / flat level to stick to, Just a guess. You might try a simple c-clamp test, by clamping the Handi in place to insure no movement. Russ

No, the handibot and the wood did not move. The dimensions are way, way off for what it is cutting. Movement would not account for it.

And yeah, the wood is rough scrap play to learn with. I just need to get some good straight cuts and I'm going to move on to nice stock. I was shocked at how well the first engraving went. I thought my rough stuff would be learning material, I'm looking at it as backer board now.

Hi Marc,

Please do share your file. Should be a faily straight-forward diagnosis.

Best,
David

So offline conversation is my speeds were too fast. I copied a similar upcut bit, but it was defined for a bigger machine. I missed David's comment in the other thread that speed shouldn't be above 2" per second. The settings I copied were 6. Turns out that can impact dimension. I haven't had a chance to rerun a cut file. Somehow the last four nights have all been booked, and for some reason I'm not supposed to run a router after the kids go to bed. If I don't get to this tomorrow it will be this weekend and I'll post back results.

Marc only the Alpha ShopBots have feedback from the servo motors, so the speed issue may be the problem. If the servos are driven to hard they MAY skip a pulse and then be out of sync with the file. I always make several thin cuts when starting out with a new material. If it cuts good then I can always make a new toolpath with slightly deeper cuts. When I was playing with the HandiBot in the ShopBot booth at Maker Faire we were cutting 2x8's! So I know the little beastie can make some impressive cuts. Try the same test cuts but shallow up the cuts and slow down the feed slightly and see if you get better results. Russ

I forgot to come back and update. Yes, slowed down to 2 and it cut well. 2 on some 2x4s was too fast though, had to go shallower and slower. Backed it all the way down to 1. Still need more experimentation.

Hi Marc,

What cut depth per pass are you trying for on 2x4s? What setting do you have the DeWalt router at?

Make sure your jog speed is around 2-3"/second for rapid moves above the material. If you have slow comm between your tool and computer, fast moves can lead to lost steps when jogging.

David

I have the router set to it's slowest setting, which per the manual with it is 16000 RPM. All other speeds were higher than anything I saw in the existing tools database in Vectric so I decided it made since to put it there and leave it.

Shouldn't be slow speed with the PC. I'm using a USB3 port on a laptop that has an I7, an SSD and a 16GB of ram.

Marc,

The default values in V-Carve's database are just place holders. If you watch the video tutorials on Vectric's site, you'll hear them say that over and over.

You need to either know the recommended chip load for your bit or be able to figure it out experimentally. The better bit vendors post chip loads but even then it's usually a range where the upper limit can be 2x to 3x the lower limit. That translates into a 2x-3x difference in feedrate depending on where in the range you pick a chip load.

You can chance the feedrate on the fly with a key equivalent. That should let you pick a reasonable starting value, set up a test cut, and increase/decrease the feedrate as you observe the cut in progress. Or, stop it periodically, inspect the dust/shavings you're making, check the bit/collet's temperature, adjust feedrate as indicated, and resume the test cut until you've figured out what YOUR bit in YOUR material need.

The collet should not be hot to the touch at the end of a cut. If it is, you're spinning too fast or cutting too slow…heat comes from excess friction…heat means lost bit life.

Pocket cuts typically have 20% of the bit's cutting surface in contact with the material. Profile cuts have 50%. So you'll need to figure out the proper feed rate for both types of cuts instead of using the same values for both…there's a 2.5x difference in the load on the bit (based on comparing contact patches) which is a lot of extra drag on the system.

My amateur two cents (but they're really fancy wooden cents at least),
Tim S.

Tim has it right on.

Marc, for pine 2x4 cutting, I typically run the router at 5 with a 1/4" bit with 1/4" pass depth at 1.5-2" per second. That is a good starting place. The bit screams, but the chipload is good. If you post up images of your cuts, we can probably help diagnose your issue.

David

Wow, thanks guys. Great advice. I clearly need to dedicate some time to just figuring this stuff out without a project in mind. Just test materials.

Tim Swihart,

You wrote, "You can chance the feedrate on the fly with a key equivalent." I did not know that was possible! Can you explain this in more detail? On several occasions I would have liked to have done that. Thanks in advance.

Also, is it possible after you have interrupted the cutting to restart at a specific line? I am new to shopbots and do not know how to do this. Again, thanks.

Tim Flugum,

ShopBot has a help file posted on their site with a list of key equivalents. I stumbled onto the ability to change the feed rate on the fly while browsing that list. You can also change the RPM on the bigger bots with a different key equivalent (assuming the bigger bot in question has the right controller).

You can find the full list at:

ShopBot Keyboard shortcuts

I'll defer the question about restarting at a specific line number to one of the ShopBot admins here. Worst case, it can be done with a text editor, but hopefully there's a cleaner solution that I haven't yet needed to learn.

Very nice. Thanks.

Hi Tim,

You can start at a specific line by going to File-Goto line/single step. That will walk you through the process.

David

Thanks David.