Sharp 90* turn in gcode becomes a large sweeping turn

More
09 Mar 2020 20:57 #159598 by lumberjack_jeff

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

More
09 Mar 2020 21:10 #159602 by PCW
can you post your gcode or a portion of it that exhibits this issue?

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

More
09 Mar 2020 22:23 #159608 by lumberjack_jeff
Apologies for the fairly large file, I'm not at my controller computer, so I can't tell you exactly which lines the problem occurs on.
The toolpath is in three passes, and as the photo of the result shows, pass #1 does not superimpose pass #2 or #3.
Attachments:

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

More
10 Mar 2020 02:24 #159621 by lumberjack_jeff
I changed the max acceleration value to 17. Re-ran the file (no load). The track shown in the preview window conformed to the path plotted (i.e performed as expected)
It would be nice to know if that was the problem, or if it's still lurking.

I have also been getting frequent random shutdowns ("estop reset" is the status) with no error messages. I had written it off as a loose connection... Could it be related?

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

More
10 Mar 2020 03:16 - 10 Mar 2020 03:23 #159623 by PCW
I cannot duplicate this with either 2.7.15 or 2.9

LinuxCNC 2.7:

LinuxCNC 2.9:


both with accel of 12 ips/s

Not sure about the estop issue, that sounds like hardware to me,
I would put a debounce in this connection

net estop-ext <= parport.0.pin-10-in
Attachments:
Last edit: 10 Mar 2020 03:23 by PCW.
The following user(s) said Thank You: lumberjack_jeff

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

More
10 Mar 2020 05:07 #159635 by BobsGotCnc
My ini file settings. I will be re-doing this shortly as I move to new DM542T drivers. The settings below were from the previous owner.

Y
MAX_VELOCITY = 3
MAX_ACCELERATION = 4.0
STEPGEN_MAXVEL = 7.21
STEPGEN_MAXACCEL = 5.00


Z
MAX_VELOCITY = 1.0
MAX_ACCELERATION = 5.0
STEPGEN_MAXVEL = 1.25
STEPGEN_MAXACCEL = 6.25


X
MAX_VELOCITY = 2.5
MAX_ACCELERATION = 10.0
STEPGEN_MAXVEL = 2.92
STEPGEN_MAXACCEL = 12.50

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

More
10 Mar 2020 13:08 - 10 Mar 2020 13:09 #159649 by PCW
Unless you are using G64 Pxxx, rounded corners are _expected_ so its not likely your INI
settings are involved (other that the fact that you have very low acceleration settings so you
will get very large radius blends with plain G64). Did you try G64 P0.0005 as cmorely suggested?
Last edit: 10 Mar 2020 13:09 by PCW.
The following user(s) said Thank You: BobsGotCnc

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

More
10 Mar 2020 20:52 #159699 by lumberjack_jeff
Thank you for the troubleshooting help.

Can you please advise me about debouncing pin 10?

I think I need to replace this wscnc.hal code
...
net estop-ext       <= parport.0.pin-10-in
...
#limits debounce to stop false triggers
loadrt debounce cfg=2 #change  to the number you want
setp debounce.0.delay 100 #this sets the delay 100 iterations of the base thread
addf debounce.0 base-thread
net deb-probe-in debounce.0.0.in <= parport.0.pin-12-in-not
net probe-in debounce.0.0.out
with
...
loadrt debounce cfg=2 #I think I only need two
setp debounce.0.delay 100 
setp debounce.1.delay 100 
addf debounce.0 base-thread
addf debounce.1 base-thread
net deb-probe-in debounce.0.0.in <= parport.0.pin-12-in-not
net deb-estop-ext debounce.1.0.in       <= parport.0.pin-10-in
net probe-in debounce.0.0.out
net estop-ext debounce.1.0.out

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

More
11 Mar 2020 01:05 #159729 by BobsGotCnc
G64 P0.0005 resolved the sweeping 90* turn.

So I am still a CNC newb. When I am in the CAM phase, how would I detect such an issue in the future as to reduce the likelihood that I destroy valuable material when running the gcode? At this point in my learning (about 4 months in), I feel like every other new design I take to the CNC destroys a piece of material. Each time I learn something new, but it is getting a bit discouraging that it feel rare to generate gcode, execute it, and have the piece I designed. Maybe this is part of the hobby cnc router process?

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

More
11 Mar 2020 02:22 #159738 by PCW
Probably best way is to have your CAM program insert a gcode preamble that includes
important modal gcodes like G64 Pxxx.

Also with new code and expensive material, take time to study the preview,
or run it in simulation to see if its doing what you expect or perhaps
do an run on scrap material
The following user(s) said Thank You: BobsGotCnc

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

Time to create page: 0.242 seconds
Powered by Kunena Forum