Greetings everyone, I have read all previous post regarding this issues, but they are all over a year old. I am posting this to see if there has been any new solutions that I might have missed. The issue: When working with STL files it seems that large files are not able to process completely. The machine stops at around 20-30%, but the controller or computer (I have tried both) states that the job is complete. I use V-carve pro and/or Aspire to run my toolpaths. I have tried Open builds, GRBL, Linux CNC, NC Easy and a few more postprocessor's all with the same or similar result. I have also tried disabling the 3D viewer when using the laptop. No change My laptop and computer both have 16G RAM. As of today Aug 7 2021, I am running OBC 1.0.304 and V1.47 interface flash. Any help and/or suggestions will be greatly appreciated. Respectfully Javier VG SFC US ARMY (Ret) Manufacturing HS Teacher Central Florida
Make sure all chipset and other drivers are up to date. Make sure sections 4.1 and 4.2 of docs.openbuilds.com/blackbox has been applied
Thank you for the fast response. Will let you know how that goes. Respectfully Javier VG SFC US ARMY (Ret) Manufacturing HS Teacher Central Florida
The only correct one is OpenbuildsGRBL postprocessor (-: Linuxcc and others support Gcodes that GRBL does not support and will cause error stops. STL files tend have many facets, and each one will cause at least one line of Gcode to be output. Can you simplify the STL files? Then you also want to mess with the smoothing settings, this reduces the number of lines in the Gcode, also do a roughing pass with a big bit, then a smoothing pass with a smaller bit for the details. What happens in you feed the gcode direct from OBControl? Then you are not relying on the Interface memory, instead Control will only send as much as the Blackbox can handle. Any error messages in the Serial console? and make sure your USB port is not turning off due to power saving by Windows.
David, Thanks for your response. Yes, I understand that OB GRBL is the correct processor, I just tried the others just incase. The smoothing of the STL in V-carve / Aspire diminishes and or delete some of the fine details of the STLs. Although the program states that they stay intact, I can assure you that they do not. The changes are clearly visible in both: the computer program as well as the finish product. Triangulating and exporting a new STL does the same. It actually shows the triangulation of the new faces regardless of the settings (Leave Open, inverted front, flat plane). Another issue that I did not mention earlier is the diagonal lines that it leaves when using the Offset/Climb or Conventional option. Now, these are not clearly visible when looking at them in V-Carve or Aspire, but they do show up in in the final product. Also, If I export the file and try running it in Estlcam, then they are visible in the computer as well as the final cut. The reason I did not mentioned that last part earlier is because I believe these are issues related to the software and not Openbuilds equipment. (maybe I am wrong of course) Attached is the Gcode file that I am currently trying to work with. If you have a copy of ESTLCAM open it so that you can clearly see the diagonal white lines that I am referring too. All power/USB settings are good as per OpenBuilds documentation. As Always all help and sugestions are greatly appreciated. Respectfully Javier VG SFC US ARMY (Ret) Manufacturing HS Teacher Central Florida
This is probably due to the grain in the wood interacting with the direction of cut, as well as the cut direction interacting with the backlash in the system. which indicates that the gcode is generated with some cuts being further apart than others. there is probably a setting for that (-: Attached is the Gcode file that I am currently trying to work with. If you have a copy of ESTLCAM open it so that you can clearly see the diagonal white lines that I am referring too. Respectfully Javier VG SFC US ARMY (Ret) Manufacturing HS Teacher Central Florida[/QUOTE] I see more than 1.2 million lines of code with a max line of 519.718mm and min cut length of 0.0042mm (which is uselessly small, your minimum step is bigger than that). and avg cut length of 0.715mm. So this is quite detailed and will take quite some time to cut. I highly recommend a roughing cut to remove most of the material with a 1/4" 2 flute carbide router bit. This will preserve the life of your final cut bit. (Tapered ball end mill?) As to the feed stopping, if there is a problem there is an error message in the serial console. I would remove the Interface from the tool chain and run direct USB from laptop to Blackbox. Make sure the laptop is set to never sleep, never power save, max performance power profile, and USB will never power off, aaand stand by and move the mouse every 5 minutes. While the ultimate goal is to be able to walk away for hours while it runs, right now you need to stand and watch and interact to figure out what is going on.
David, which indicates that the gcode is generated with some cuts being further apart than others. there is probably a setting for that (-: Sorry, lost me there. What setting would that be? I see more than 1.2 million lines of code with a max line of 519.718mm and min cut length of 0.0042mm (which is uselessly small, your minimum step is bigger than that). and avg cut length of 0.715mm. So this is quite detailed and will take quite some time to cut. I highly recommend a roughing cut to remove most of the material with a 1/4" 2 flute carbide router bit. This will preserve the life of your final cut bit. (Tapered ball end mill?) Yes, the final is a Tapered ball end mill with a 1/16 diameter 6.2* 1/4 shank (Amana tool) I normally use a 10% stepover for final cut and sometimes 8% if the job is small and has lots of details. That file takes approximately 23 hours to complete. I do not mind, since I don't sell my work. I use it to decorate my house or give as gifts to close friends and family. As to the feed stopping, if there is a problem there is an error message in the serial console. Negative. The interface actually reads JOB COMPLETE in green letters! Some times it does this after 30 minutes other times after 3-4 hours. Yesterday it did it with that large file as well as a smaller file with around 450K lines of code. At this time I am switching back to laptop and USB direct to Blackbox I will keep the Interface for my next plasma table build. I would remove the Interface from the tool chain and run direct USB from laptop to Blackbox. Did it this morning. It ran a job from start to finish without an issue. Just the darn diagonal lines! Make sure the laptop is set to never sleep, never power save, max performance power profile, and USB will never power off, aaand stand by and move the mouse every 5 minutes. While the ultimate goal is to be able to walk away for hours while it runs, right now you need to stand and watch and interact to figure out what is going on.[/QUOTE] The computer is set as advised. Respectfully Javier VG SFC US ARMY (Ret) Manufacturing HS Teacher Central Florida
Per se, there is no File size limit (well, FAT32 file system has a 4Gb per file limit. Very unlikely to ever have gcode that big) , but the COMPLETE message does indicate the end of the file was reached (no more bytes to read) Could happen if you copy it to USB and not do the "safely eject" thing for example (file not copied completely) - or it could be an issue with the drive itself (try a different one, and format as FAT32) An EMI related reset can also not be ruled out. Do you have Dust extraction? But, yes, first of all get it running reliably using the PC (more logging makes troubleshooting easier). Once that's running perfectly, you can try Interface again. Next time it has issues on the PC side, check the Serial Terminal tab - serial log will have clues
I don't know exactly as i don't have that software. I see the tool is moving in expanding rectangles with sharp corners. Do the diagonals occur along one of those sharp corners? Can you change the sharp corners into arcs? ('roll around corners' is common language for that) Can you change to a raster toolpath that starts one end and moves to the other, then there are no corners inside the toolpath. Have you googled for something like 'aspire diagonal mark on carving'? Someone else has had this problem, asked in a forum, and found solutions, you just need to ask google the right question (-:
