Curving between corners
28 Sep 2018 07:13 #118091
by justinj
Curving between corners was created by justinj
I'm having an issue where corners are being rounded when there is no compensation or curves set in the GCode file, in fact the file specifically contains a G40 and G49 at the beginning to cancel any compensatory moves.
I've used the same GCode files before on my old install so I'm assuming it's either a wrongly configured setting or something new in LinuxCNC since my old install (2.6.4). This is the first time I've used these files since my upgrade (I changed my controller to a GeckoDrive from a cheap Chinese one at the same time as upgrading) and the only thing that I think is different is the max speed and velocity (The only one had to be quite low to avoid skipping steps).
I did notice the same issue occurring on vertical moves in other files where it would start lifting just before it got to the end but I had assumed that was to do with the higher speeds it was running at which is evidently not the case now I have encountered this file.
I've used the same GCode files before on my old install so I'm assuming it's either a wrongly configured setting or something new in LinuxCNC since my old install (2.6.4). This is the first time I've used these files since my upgrade (I changed my controller to a GeckoDrive from a cheap Chinese one at the same time as upgrading) and the only thing that I think is different is the max speed and velocity (The only one had to be quite low to avoid skipping steps).
I did notice the same issue occurring on vertical moves in other files where it would start lifting just before it got to the end but I had assumed that was to do with the higher speeds it was running at which is evidently not the case now I have encountered this file.
(Generated with: DXF2GCODE, Version: PyQt4 Beta, Date: $Date: Tue Jun 9 17:40:00 2015 +0200 $)
(Created from file: /home/cnc/Documents/CAD Drawings/Letters/N.dxf)
(Time: Sun Aug 27 21:02:48 2017)
G21 (Units in millimeters) G90 (Absolute programming) G64 (Default cutting) G17 (XY plane) G40 (Cancel radius comp.) G49 (Cancel length comp.)
G0 Z 15.000
(*** LAYER: Letters ***)
T906 M6
S14000
(* SHAPE Nr: 0 *)
G0 X 42.286 Y 19.286
M3 M8
G0 Z 3.000
F100
G1 Z -1.200
F1200
G1 X 42.286 Y 65.689
G1 X 63.714 Y 19.311
G1 X 63.714 Y 65.714
F100
G1 Z -2.400
F1200
G1 X 63.714 Y 19.311
G1 X 42.286 Y 65.689
G1 X 42.286 Y 19.286
F100
G1 Z 3.000
G0 Z 15.000
M9 M5
G0 X 0.000 Y 0.000
M2 (Program end)
Please Log in or Create an account to join the conversation.
28 Sep 2018 12:29 #118106
by andypugh
Replied by andypugh on topic Curving between corners
This sounds like it is due to the new trajectory planner. If your machine has relatively low acceleration and high speed then the changes will become more obvious.
linuxcnc.org/docs/2.7/html/user/user-con...#_trajectory_control
Should explain the changes you can make. You can have the old behaviour back, or configure somewhere in between to get some of the speed improvement that the new TP provides.
linuxcnc.org/docs/2.7/html/user/user-con...#_trajectory_control
Should explain the changes you can make. You can have the old behaviour back, or configure somewhere in between to get some of the speed improvement that the new TP provides.
The following user(s) said Thank You: justinj
Please Log in or Create an account to join the conversation.
28 Sep 2018 13:21 #118110
by justinj
Replied by justinj on topic Curving between corners
Ahh that's definitely what's going on. I turned up the feed speed on the file and it cut the corner off even more. My max speed is 4x what it used to be now I don't get skipped steps but I had to keep the accel down to avoid wobble in the gantry in hard stops/starts. I didn't realise it had any effect on paths so I was happy with the accel that I had left it at until now...
I think I might set it back to the old method as I'd rather expected results over slightly faster cuts.
Thanks for the help, I didn't even realise it was a thing!
I think I might set it back to the old method as I'd rather expected results over slightly faster cuts.
Thanks for the help, I didn't even realise it was a thing!
Please Log in or Create an account to join the conversation.
28 Sep 2018 13:35 #118111
by justinj
Replied by justinj on topic Curving between corners
How do I disable that so it instead follows the path exactly?
I've tried setting ARC_BLEND_ENABLE = 0 and COORDINATES = {blank} in the INI file under [TRAJ] but it is still doing some kind of trajectory plan.
I've tried setting ARC_BLEND_ENABLE = 0 and COORDINATES = {blank} in the INI file under [TRAJ] but it is still doing some kind of trajectory plan.
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Away
- Platinum Member
-
Less
More
- Posts: 4981
- Thank you received: 1378
28 Sep 2018 14:08 #118114
by Todd Zuercher
Replied by Todd Zuercher on topic Curving between corners
The best solution is to set G64 P0.001 (or what ever P tolerance is appropriate for your machine and application) in the preamble of each g-code file. Or you can set the machine to G61 (exact path) mode, but then the machine will halt a every corner in the g-code.
The default G64/G61 setting in Linuxcnc is G64 with no P tolerance, which equals constant velocity (or as near as possible) with maximum blending.
This has always been the case, but with the new trajectory planner, higher feed rates are possible with some g-code due to the farther read ahead (more than 1 line) when planning accelerations. The result is greater corner rounding than with the old system when no blending tolerance is specified.
The default G64/G61 setting in Linuxcnc is G64 with no P tolerance, which equals constant velocity (or as near as possible) with maximum blending.
This has always been the case, but with the new trajectory planner, higher feed rates are possible with some g-code due to the farther read ahead (more than 1 line) when planning accelerations. The result is greater corner rounding than with the old system when no blending tolerance is specified.
The following user(s) said Thank You: justinj
Please Log in or Create an account to join the conversation.
28 Sep 2018 14:31 #118118
by justinj
Replied by justinj on topic Curving between corners
Thanks for clarifying that. I think it's a combination effect of both the new planner and the higher speeds I am now running at that caused it to be so off. Those files all specified G64 with no tolerance specified hence the significant deviation. I guess that's something I'm going to have to be mindful about in the future and revisiting the machine's acceleration settings is going to be worthwhile too.
Please Log in or Create an account to join the conversation.
Time to create page: 0.087 seconds