[closed] FreeCAD path, strange movement in Z axis
03 Apr 2021 15:27 #204630
by andypugh
Right, this sounds like hardware / config.
It seem that the Z axis might be stalling. Try reducing the MAXACCEL value for Z. Initially by a lot, ie divide by 10. Just to see if that makes a difference.
Replied by andypugh on topic FreeCAD path, strange movement in Z axis
If you look at the DRO in the video you can see that right after the first G1 command the DRO goes to -0.1 But the spindle itself didn't move at all in the Z direction, it is physicaly still at 5 (in this case, I changed the gcode file a little).
Right, this sounds like hardware / config.
It seem that the Z axis might be stalling. Try reducing the MAXACCEL value for Z. Initially by a lot, ie divide by 10. Just to see if that makes a difference.
Please Log in or Create an account to join the conversation.
03 Apr 2021 17:07 #204642
by ikkuh
These are the values now. Not sure how low acceleration should go
Full .ini file at: git.cnckloon.nl/CNCZone/mesa_2019/raw/br...wZaxis/mesa_2019.ini
Replied by ikkuh on topic FreeCAD path, strange movement in Z axis
Right, this sounds like hardware / config.
It seem that the Z axis might be stalling. Try reducing the MAXACCEL value for Z. Initially by a lot, ie divide by 10. Just to see if that makes a difference.
These are the values now. Not sure how low acceleration should go
[AXIS_Z]
MIN_LIMIT = -200
#0
MAX_LIMIT = 0.01
#541
MAX_VELOCITY = 15
MAX_ACCELERATION = 20
[JOINT_3]
MIN_LIMIT = -200
#0
MAX_LIMIT = 0.01
#541
HOME = 0
#POSITIE NA HOMING
HOME_OFFSET = 0
HOME_SEARCH_VEL = -17
HOME_LATCH_VEL = 2.5
HOME_SEQUENCE = 1
HOME_USE_INDEX = false
HOME_IGNORE_LIMITS = false
MAX_VELOCITY = 18
MAX_ACCELERATION = 25
TYPE = LINEAR
SCALE = -400
STEPGEN_MAX_VEL = 18.0
STEPGEN_MAX_ACC = 28.0
#FERROR = 0.0051
MIN_FERROR = 0.0025
DIRSETUP = 100000
DIRHOLD = 100000
STEPLEN = 22000
STEPSPACE = 22000
DEADBAND = 0
P = 1000
I = 0
D = 0
FF0 = 0
FF1 = 1
FF2 = 0.00013
BIAS = 0
MAX_OUTPUT = 0
MAX_ERROR = 0.0127Full .ini file at: git.cnckloon.nl/CNCZone/mesa_2019/raw/br...wZaxis/mesa_2019.ini
Please Log in or Create an account to join the conversation.
03 Apr 2021 19:36 #204653
by andypugh
Replied by andypugh on topic FreeCAD path, strange movement in Z axis
It's odd that your limits are different for joint and axis, if this is a cartesian machine. But it isn't likely to be the problem.
Your acceleration is already rather low. Acceleration of 10/s * velocity is more common.
So, try reducing the max velocity instead.
Also, listen very carefully. Can you hear the Z axis stall?
Can you definitely jog down to -0.1?
Your acceleration is already rather low. Acceleration of 10/s * velocity is more common.
So, try reducing the max velocity instead.
Also, listen very carefully. Can you hear the Z axis stall?
Can you definitely jog down to -0.1?
Please Log in or Create an account to join the conversation.
04 Apr 2021 13:33 - 04 Apr 2021 13:44 #204763
by ikkuh
Replied by ikkuh on topic FreeCAD path, strange movement in Z axis
It was the G43 command.
Somehow there is something wrong there. Maybe it is one of the gmoccapy settings.
Thanks for all your help, it was quitte an experience.
forum.linuxcnc.org/41-guis/29398-semi-ma...es-in-gmoccapy#60521
Somehow there is something wrong there. Maybe it is one of the gmoccapy settings.
Thanks for all your help, it was quitte an experience.
forum.linuxcnc.org/41-guis/29398-semi-ma...es-in-gmoccapy#60521
wiki.linuxcnc.org/cgi-bin/wiki.pl?GmoccapyPlease note, that gmoccapy takes care of its own to update the offsets,
sending an G43 after any tool change, but not in auto mode!
Attachments:
Last edit: 04 Apr 2021 13:44 by ikkuh.
Please Log in or Create an account to join the conversation.
04 Apr 2021 13:42 #204764
by andypugh
Replied by andypugh on topic FreeCAD path, strange movement in Z axis
That doesn't make sense.
If you have a G43 between the two Z moves, and the tool length in the table is exactly the right value, then you might see no Z movement.
But if there is a G43 and _then_ two Z moves, the Z should move.
If you have a G43 between the two Z moves, and the tool length in the table is exactly the right value, then you might see no Z movement.
But if there is a G43 and _then_ two Z moves, the Z should move.
Please Log in or Create an account to join the conversation.
04 Apr 2021 13:48 - 04 Apr 2021 13:50 #204766
by ikkuh
The G43 was early on in the program, before the G1 moves.
I removed the G43 from the program and everything works as expected.
Will try to find out what is going wrong. But it does like G43 is the guilty command here. The z-axis would move in LinuxCNC's idea but it was just the offset that was stored in G43 (and that kinda works out with the numbers, G43 offset was 21.43 mm and that was about the amount of space that the bit was positioned above the spoilboard). The tool gets measured with a toolheight sensor every time I run the program and gmoccapy stores the offset in the LinuxCNC tooltable.
Replied by ikkuh on topic FreeCAD path, strange movement in Z axis
That doesn't make sense.
If you have a G43 between the two Z moves, and the tool length in the table is exactly the right value, then you might see no Z movement.
But if there is a G43 and _then_ two Z moves, the Z should move.
The G43 was early on in the program, before the G1 moves.
I removed the G43 from the program and everything works as expected.
Will try to find out what is going wrong. But it does like G43 is the guilty command here. The z-axis would move in LinuxCNC's idea but it was just the offset that was stored in G43 (and that kinda works out with the numbers, G43 offset was 21.43 mm and that was about the amount of space that the bit was positioned above the spoilboard). The tool gets measured with a toolheight sensor every time I run the program and gmoccapy stores the offset in the LinuxCNC tooltable.
Last edit: 04 Apr 2021 13:50 by ikkuh.
Please Log in or Create an account to join the conversation.
04 Apr 2021 19:38 - 04 Apr 2021 19:49 #204805
by jbraun
Replied by jbraun on topic FreeCAD path, strange movement in Z axis
Break the problem into pieces without red herrings?So running the above code stops the tool 6mm above G54 Z0 ?
But rerunning with the brackets on the 2nd last line doesn't stop the tool at -0.1mm ?
ooops meant to say without the brackets
G17 G54 G40 G49 G80 G90
G21
G54
M5
M6 T1
G43 H1
M3 S8123
G0 Z6.000
(G01 Z-0.1 F900)
M02But rerunning with the brackets on the 2nd last line doesn't stop the tool at -0.1mm ?
ooops meant to say without the brackets
Last edit: 04 Apr 2021 19:49 by jbraun.
Please Log in or Create an account to join the conversation.
04 Apr 2021 19:50 - 04 Apr 2021 19:52 #204806
by ikkuh
Exactly, that is what is happening.
=====> Z physicaly goes to 4 as it should
Z should now be physically -0.1 and under the surface of the spoilboard, but it is still physically 4 as was set by the G0 command. The DRO changed though, it displays now -0.1
As I said before, when I remove the G43 command all works as expected.
Replied by ikkuh on topic FreeCAD path, strange movement in Z axis
Break the problem into pieces without red herrings?
So running the above code stops the tool 6mm above G54 Z0 ?G17 G54 G40 G49 G80 G90 G21 G54 M5 M6 T1 G43 H1 M3 S8123 G0 Z6.000 (G01 Z-0.1 F900) M02
But rerunning with the brackets on the 2nd last line doesn't stop the tool at -0.1mm ?
Exactly, that is what is happening.
G17 G54 G40 G49 G80 G90
G21
G54
M5
M6 T1
G43 H1
M3 S8123
M7
G0 Z6.000
G0 X-0.100 Y536.751
G0 Z4.000G1 X-0.100 Y536.751 Z-0.100 F900.000 G1 X5.249 Y542.100 Z-0.100 F900.000 As I said before, when I remove the G43 command all works as expected.
Last edit: 04 Apr 2021 19:52 by ikkuh.
Please Log in or Create an account to join the conversation.
05 Apr 2021 11:49 #204882
by Aciera
Replied by Aciera on topic FreeCAD path, strange movement in Z axis
Can we see what you've got in your tooltable?
Please Log in or Create an account to join the conversation.
05 Apr 2021 12:26 - 05 Apr 2021 12:38 #204887
by ikkuh
That was after removing the *.var files and setting G54 to new corner and starting LinuixCNC. After running the first program gmoccapy added the toollength offset as seen above.
Replied by ikkuh on topic FreeCAD path, strange movement in Z axis
Can we see what you've got in your tooltable?
cat tool.tbl
T0 P0 ;
T1 P0 Z+41.690621 ;flat003That was after removing the *.var files and setting G54 to new corner and starting LinuixCNC. After running the first program gmoccapy added the toollength offset as seen above.
Last edit: 05 Apr 2021 12:38 by ikkuh.
Please Log in or Create an account to join the conversation.
Time to create page: 0.122 seconds