I have an upcoming 3D project. The "roughing toolpath" will take estimated 5 hr. The "Finishing toolpath" is estimated to be 33 hr. I'm using OpenBuilds Control. What I would like to know, would it be ok to run the "Finishing toolpath" for lets say 12hrs, then in Control software "Pause" the job, turn off router and take a break for several hours or even overnight. I will not close Control software. Just leave program open on PC. Get up the next morning, turn router on and in Control just "run or resume" finishing toolpath. The PC has all updates turned off and no screen saver active. The PC will just be idle overnight. Assuming there are no power outages, will this process work for running extended toolpath jobs?
It should but it may be safer to split the job smaller if at all possible (maybe lighter finishing passes, but at faster rates, and run one per day? )
How would one go about performing or setting up "lighter finishing passes" in VCarve Pro? That would be a very doable process.
I am not sure, sorry. Was just offering it as a general advice, that perhaps a mindset change might be safer than pausing, etc. How to actually do that, and if its even possible (did say "if at all possible hehe) I'll leave up to the v-carve pros who may be popping into this thread through the course of the day.
Only solution found was to plan roughing toolpaths early in the morning so they could be monitored. That's the more aggressive process in the project. I then let everything set (computer and control progam) overnight (do not powerdown or close control). That way work zero is still set. Then early the next morning I start my finishing toolpath and let it run till completed. I feel more comfortable letting it run and just checking in on it throughout the day. I'm usually using a 1/8th or 1/116th tapered ball nose bit and it is not an aggressive cutting tool. So I feel comfortable letting it run with out constant supervision. I also have a baby monitor cam set up so I can check in on the project throughout the day without having to walk out into the shop.
Hi; I might be wrong but if you went in and edited your toolbit spec's to a lighter and or faster cut rate would this do it? I know to get better finishes on different species of wood, that's what I do. Might want to try on a piece of scrap.
I'll give that a try. To tell the truth I have thought about it, just never did it. I've read all the literature on "speeds and feeds" and have a grasp on the theory of it. But never took the time to measure my "chips" to see if I should/could increase my speeds. There is no one else in the area with knowledge on the subject to give advise and I'm a little timid to push my machine for fear of breaking something. Just the other day I was thinking of trying "lighter" passes to reduce the amount being removed during a roughing pass. I don't think I'm having any "chatter" when cutting, but It does make a different sound when cutting in the different directions on the wood grain. I did notice on one of my end mills some "darkening". I think that is one of the signs of needing to adjust my parameters.
Do you have homing set up on your machine? If so you can safely turn things off overnight as grbl remembers your workplace offsets. Alex.
Yes Sir, homing is indeed set up. Thanks to the people at Open Builds and Peter Van Der Walt, my machine is fine tuned and running like a fine Swiss watch. I read somewhere that every time you turn the machine off as well as the PC that the first thing you should always do is "Home" your machine. Are you saying if I left a project unfinished (say only the roughing part done), turned off machine as well as the PC and the next morning turned everything on and "Machined Homed" first. That the "Work Home" would still be there as when I left it?
I'm curious as to why so long of a cut time, is the project that large? Maybe we can shave off many hours by optimizing your machine and cam? -Increase acceleration and speed, many people run default acceleration which is low and will slow a system unnecessarily. -decrease your safe retract height to just a few mm, lots of wasted time on z retracts -increase your step-over to a "good enough" finish quality cheers Gary
The files are pretty large. The last project I did was "The Last Supper". The roughing gcode file was 888 KB, and the finishing gcode file was 51.5 MB. The roughing cut time was 01:52:41. While the finishing cut time was 42:39:54. I use a 1/4 in. flat end mill running with a step over = 0.1 inch 40%. Feed rate = 50 inches/min and Plunge rate =20 inches/min. For the Finishing cut I used a 1/16 in. Taper Ball Nose with a Stepover = 0.005 in, (8%). Feed rate = 30 inches/min and Plunge Rate = 15 inches/min. My Rapid Z Gaps above material, Clearance = 0.2 in, Plunge = 0.2 in. Home/Start Position Z Gap above material = 0.8 in.
My machine is the WorkBee 1010 with the Makita router. I also use the X Carve, X Controller to run my system.
Hmm...interesting, i was actually just reading about editing the post processor in what’s called tape splitting. Vectric’s post processor guide has info on it. May give it a go.
That's a great tip @Bigmontel, thank you! Am I right that you can reach that through the help menu in your Vectric software? Alex.
Me again, how about tiling the artwork. Vectric vcarve uses this for big signs (probably works in Aspire), you could reverse it to make them smaller pieces. Here's a you tube it allows over lap of the artwork, so you don't have lines.
Appreciate the video Steve, I’ve thought about tiling and will probably go that route if this whole tape splitting of the post processor doesn’t work. I would love to have a go to post processor set up to just break down large projects into quarters automatically.
So I managed to make my post processor tape split successfully in theory. Had a 36 hour 3d carve save as 10 separate files when i selected my new edited post processor. Now to test on a smaller file with a real carve.
Hi Dlhoulton, Your plunge rates can be double, your feed could be higher as well with such small step-overs. What is your acceleration set in GRBL? this can make a huge difference. I bet with some tuning you can easily knock half the time off. Gary
Gary Caruso, Thanks for the advice. I'm going to try doubling my plunge rates and increasing my feed rates. As for my "acceleration set in GRBL". I'm not sure what this is. I'm using the recommended settings that OpenBuilds provided for the WorkBee 1010. I can report that my settings for $110 through $112 (X,Y and Z) are 2500 max rate, mm/min. It says that it can go up to 7500. I'm not sure if that is what you are talking about. Looking forward for your help.
Dlh, acceleration is setting $120, 121, 122 (x,y,z) the default is a conservative starting point. For example on my ox I have it set for about 600mm/min^2 it really wakes up a machine. If set too low you won’t get up to your feed rate if many direction changes are occurring like in 3D carving. Cheers Gary
So, successfully ran my first tape split file today. I had a single roughing file that I ran and then proceeded to run one of seven finishing files. I plan on running one file every evening this week. The first finishing file was 1.5 hours start to finish.
