3D Finishing Issue

[mgoodwin]

Hello, I am not really sure how to explain my issue. Recently I was cutting the finish pass for a 3D carving. The carve was approximately
3/4 complete when my machine came to a stop, all but the spindle rpm speed. My first thinking was to reload the program and run it again. The machine stopped in the same place again. I remodeled the carving again saved it to the flash drive and when I tried to download it to the machine the name of the file that normally appears on my machine screen showed only dashed lines, no name of a file. I saved the file anyway and did a test of the downloaded code. It stopped testing the code with an error showing a syntax error number Block 100400 Line 1101005 Column 30. I am not sure what that may mean. I Seem to have differing result with each try.
I have tried other flash drives with no positive results. The 3D roughing pass works fine. 2D carving is also fine. I am not sure if this maybe a post processor issue or a migration issue to release 10.505 things seemed to go awry following this update as I have done numerous carvings previous to this update. I am sure that I probably just missed an update step but I am unsure how to proceed to repair this issue. I have a Laguna Smart Shop 2.
Thank You Much

[Adrian]

The usual cause of issues like this is a failing flash drive but you've tried others so that's not it.

3D finish files tend to be very large so can take a few seconds to write completely to flash drives. Are you ejecting the flash drive from Windows via the "Safely Remove Hardware and Eject Media" icon on the Windows taskbar? If not the file can be corrupted.

[mgoodwin]

I do think that it does have something connected with the size of the file. I saved the 3d file with a 20% step over by mistake and that program loaded and did start to run but I stopped it before it completed the carve so I am not sure if it would have run through. I have been safely ejecting the flash drive. I will try the model from my laptop to see if it maybe a computer issue.

Thanks

[SteveNelson46]

What is the capacity of your flash drive?

[dealguy11]

How long have you had the machine, and have you ever run a file this big before? This might not be a useful direction to look, but I have had a problem in the past where the manufacturer put an unlicensed version of the control system on the controller and it would only run up to a certain number of lines before it stopped. It was around 1000 lines, and I just happened to notice that the line number ends in 1005. Just a thought.

[Savannahdan]

Are you using a pendant and if so, have you tried saving the file to it and then running the program. I know that I've had problems with USB flash drives that don't have a brand name on them. I was using one about 3 months ago and it worked just fine in the cnc pendant but showed bad file names after I took it out of the pendant and made some changes. I, too, remove the USB flash drive using the proper ejection process for a save removal. Sorry to hear you're having problem and hope you get it resolved shortly.

[scotttarnor]

I had a similar problem about 6 months ago, I tried different flash drives, reset CNC, it was driving me crazy! Finally I deleted the tool path, re computed, saved to the same flash drive and had no problem.

[mgoodwin]

I think that dealguy is on the right track with this being a memory capacity of my cnc. The 4 years that I have had this machine this appears to be the largest file I have attempted to cut. The cut file is 55,124 mb of data. The only other closest past carve I could find that I have done in the past is only 35,675 mb of information. When I try to load the large carve program it starts to load and does load most of the file but then the name of the file goes blank and that and I think that is when my machine stops. I do have a call in to Laguna support to see if there is a work around or if it is what it is. I guess that this happened just after the update so I was to quick to blame the update. Sorry for that but I do think it is a machine memory problem.

Thanks much for the replies

[Rcnewcomb]

If it is memory another work-around is to use tape-splitting in the post processor. That breaks the job into multiple smaller files which are run sequentially.

[mgoodwin]

Hello I am wondering how one does a tape split in the post processing? That would be great for this as I do have a very large carving to complete following getting this one done.
Thanks Much
Mike G

[Rcnewcomb]

From Help/Post Processor Editing Guide

Tape Splitting Support
A section that describes how a long toolpath output will be split:

TAPE_SPLITTING=MAX_NUM_LINES LINE_TOL "FILENAME_FORMAT" START_INDEX INDEX_ON_FIRST_FILE

For example a command of:

TAPLE_SPLITTING=1000 100 "%s_%s.tap" 1 "YES"

would lead to...

Output will be split into multiple files of a maximum of 1000 lines (+ however many lines in there are within the footer section of the post processor), if a retract move exists after line 900 (1000 – 100), the file will be split at that move. If the file was called "toolpath" the split files would be named toolpath_1.tap, toolpath_2.tap etc. The first toolpath output will be "toolpath_ 1.tap" there will be no file named "toolpath" without an index number, (as INDEX_ON_FIRST_FILE= YES is used), unless the file was less than 1000 lines long, in which case the file would not be split.

Note
Some controllers that require NC files to be split, also have limitations on the number of characters within a filename. For example they may require the file to be named with the MSDOS style 8.3 filename format. This should be considered when naming the output file.

[adze_cnc]

As Adrian pointed out in a similar post the line needs to have spaces around the "=" sign and the 2nd "%s" changed to "%d": see viewtopic.php?p=255118#p255118

Code: Select all

TAPE_SPLITTING = 1000 100 "%s_%d.gcode" 1 "YES"

[bobgu123]

I edited my Post Processor to include the instructions. I applied this at the beginning of the post processor.
I also changed it from 1000 to 75000 lines of code. The problem I have is this procedure is not consistent, it works on some fioles but not others.
For reference this is how mine is installed.
+ =======================================
+ ---
+ Version 1
+ Supplied by Onefinity. Adding new post processor.
+ ---
+ Version 2
+ Consolidated mm and inch configurations
+ =======================================


POST_NAME = "Onefinity (inch) (*.ngc)"

FILE_EXTENSION = "ngc"

UNITS = "INCHES"

LASER_SUPPORT = "YES"

TAPE_SPLITTING = 75000 100 "%s_%d.ngc" 1 "YES"

[Adrian]

What doesn't work? It's not creating multiple files when there are more than 75000 lines?

[bobgu123]

That's correct. Sometimes it works, other times it's like it doesn't exist.