Radius to end of arc error

More
12 Apr 2018 17:32 #108891 by aosowski
Hi everyone, I've come across an error that I have not been able to figure out.

The error reads
"Radius to end of arc differs from radius to start: start=(X7.5183,Y5.6580) center=(X7.6296,Y5.6219)r1=0.1171 r2=0.0753 abs err=0.04179 rel_err=35.6966%"

I have adjusted the amount of decimal places in the post processor from 4 to 9. This ended up fixing this error on a previous file but did not work for this file. I have also tried adjusting the CENTER_ARC_RADIUS_TOLERANCE_INCH variable in the INI file. I have also made sure the tool table offsets are correct.

Any suggestions to help fix this issue would be appreciated! Thanks!

Please Log in or Create an account to join the conversation.

More
12 Apr 2018 18:07 #108892 by DanMN
Replied by DanMN on topic Radius to end of arc error
I encountered this in Fusion360 (in some cases) when using helical moves. In my case, believe it's something in the way F360 constructs the compound moves of a tool path with a continuously varying radius combined with a smooth ramp-down. The two ways I've worked around it are:

1. Turn off Allow Helical Moves in the F360 post processor options
2. Turn of Lead In and Lead Out in the CAM>Operation>Linking options.

If you're not using F360, I'm not sure if this helps. I know this isn't the ideal solution to the problem, but it can get you back to work. I haven't broken any tools with this approach...yet. I have been distracted by other priorities, so I haven't had time to dig into a more appropriate fix. It could be a bug, but I don't know enough to make that claim.

Please Log in or Create an account to join the conversation.

More
12 Apr 2018 18:17 #108893 by aosowski
Replied by aosowski on topic Radius to end of arc error
Hi Dan! I am not using Fusion for this project, but I will keep that in mind for future projects. I am currently using vectric aspire. I have been able to get two lines further by changing G90 to G90.1 at the beginning of the file, but am still getting the error.

Please Log in or Create an account to join the conversation.

More
12 Apr 2018 22:05 #108911 by tommylight
That happens when you try to run a arc that is a segment of a radius, or if you have tool compensation and the selected tool is thicker than the smallest radius in the gcode.

Please Log in or Create an account to join the conversation.

More
13 Apr 2018 03:11 #108925 by aosowski
Replied by aosowski on topic Radius to end of arc error
An update: I ended up editing the post processor file in aspire. I changed the arc parameters from I J to R. This seemed to fix the issue.

Please Log in or Create an account to join the conversation.

More
13 Apr 2018 22:20 #108975 by tommylight
Nice.

Please Log in or Create an account to join the conversation.

More
19 Apr 2018 23:56 #109319 by erikg
Replied by erikg on topic Radius to end of arc error
Check this page out if you're having a problem with this - you're in the wrong arc distance mode:

linuxcnc.org/docs/html/gcode/g-code.html#gcode:g90.1-g91.1

Please Log in or Create an account to join the conversation.

More
25 Apr 2018 17:56 #109602 by trober14
Replied by trober14 on topic Radius to end of arc error
I'm having a similar issue. The funny thing is, the problem has been cropping up more and more often. Things I've tried:
-Remove helix moves from program. This helped on a couple programs I ran but not all.
-Increase accuracy in CAM software. Turned a 1 minute path generation into 1 hour, still no luck.
-Remove lead in/lead out moves. The error was cropping up on this type of move, when removed, the error showed up on the arc directly after the lead in.
-I've already checked the code and it was running G91.1 already.

Any other ideas? Attached is the g-code. Fails at line 18.
Attachments:

Please Log in or Create an account to join the conversation.

More
25 Apr 2018 19:38 #109610 by aosowski
Replied by aosowski on topic Radius to end of arc error
@trober14 - Are you using fusion 360?

If so, when you are selecting the post processor, select linuxcnc, then go down and select properties. Under properties there is an option called "radius arcs". Try enabling that and see if it works.

Please Log in or Create an account to join the conversation.

More
26 Apr 2018 17:26 #109674 by trober14
Replied by trober14 on topic Radius to end of arc error
SOLVED! Someone on a reddit forum recommended looking at the linux side of things since the code looked fine. I noticed in the error window, the arc start did not correspond to what the code was saying should be the start. Next I realized there was a tool table file that was installed with funky offsets that corresponded to the radius error. Deleted the offsets and all is happy. Seems odd that the offset only affected one side of the arc? Shouldnt the entire arc have shifted in the x or y direction by the value of the offset?
The following user(s) said Thank You: paulsao

Please Log in or Create an account to join the conversation.

Time to create page: 0.216 seconds
Powered by Kunena Forum