G93 strange behavior

More
27 Mar 2023 21:47 - 27 Mar 2023 21:50 #267629 by nwallace
I have found something strange when using G93 on my CNC router that has an A axis. Below are 2 snippets of gcode that have very different behaviors:

In this snippet the last 2 lines result in what looks like rapid moves. It does not obey the feed given. My machine is not actually capable of 0.0002" movement. The smallest movement the Z can do is approximately 0.0005".

Y0. Z1.3005
G93 A178.639 F11.0982
Z1.3003 A357.443 F11.0879
Z1.3005 A360. F773.4857

This snippet behaves as expected.

Y0. Z1.3005
G93 A178.639 F11.0982
A357.443 F11.0879
A360. F773.4857

Has anyone seen this before? Have I just configured something wrong? This gcode is coming from Fusion 360. I have not figured out a way to reliably get rid of these very small Z movements in rotary tool paths. Also interested if anyone knows how to do that.
Last edit: 27 Mar 2023 21:50 by nwallace. Reason: fix formating

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

More
27 Mar 2023 22:37 #267635 by andypugh
Replied by andypugh on topic G93 strange behavior
The F11,08 line should result in a move that takes about 5 seconds. Are you saying that it is faster than that?

Possibly a bug in the blending code, it is likely to discard the .0002 move in Z, but should still spend 1/11 minutes making the move.

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

More
27 Mar 2023 23:22 #267641 by nwallace
Replied by nwallace on topic G93 strange behavior
It moves much faster than that. Pretty sure it is moving at the max speed of the A axis.

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

More
27 Mar 2023 23:34 #267643 by andypugh
Replied by andypugh on topic G93 strange behavior
Which LinuxCNC version?

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

More
27 Mar 2023 23:36 #267644 by nwallace
Replied by nwallace on topic G93 strange behavior
I am using 2.9 on debian 12

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

More
28 Mar 2023 00:08 #267648 by andypugh
Replied by andypugh on topic G93 strange behavior
I can reproduce this in a sim with 2.8.4 too.

I have raised a bug report: github.com/LinuxCNC/linuxcnc/issues/2410

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

More
28 Mar 2023 00:24 #267649 by nwallace
Replied by nwallace on topic G93 strange behavior
Thanks for looking at this! For now I think I am going to figure out some sort of script I can run on my gcode that will remove any unnecessary Z moves. I am not very experienced when it comes to scripting but I am sure I can figure it out. Something that finds the starting Z before a G93 and then removes the Z word if it is less than a set amount different. If the difference is larger, use that value as the new Z value to compare against and leave it in.

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

More
28 Mar 2023 01:05 #267655 by nwallace
Replied by nwallace on topic G93 strange behavior
I actually found a way to limit the places after the decimal for xyz in my post processor to 3 which should work for this situation. For anyone else using Fusion, the change in the post is below.

Change this:
var xyzFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true});

to this:
var xyzFormat = createFormat({decimals:(unit == MM ? 3 : 3), forceDecimal:true});

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

More
30 Mar 2023 22:25 #267943 by nwallace
Replied by nwallace on topic G93 strange behavior
After a little more investigation, I can also say that a small linear axis move of 0.001" can also cause this behavior.

This does not work:

Y0. Z1.300
G93 A178.639 F11.0982
Z1.301 A357.443 F11.0879
Z1.300 A360. F773.4857

This snippet behaves as expected.

Y0. Z1.300
G93 A178.639 F11.0982
A357.443 F11.0879
A360. F773.4857

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

More
09 May 2023 20:06 - 09 May 2023 20:07 #271062 by andypugh
Replied by andypugh on topic G93 strange behavior
I believe that this bug is now fixed.

See the bug report at github.com/LinuxCNC/linuxcnc/issues/2410 for more details.
Last edit: 09 May 2023 20:07 by andypugh.
The following user(s) said Thank You: Aciera, nwallace

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

Time to create page: 0.145 seconds
Powered by Kunena Forum