1. Configuring LinuxCNC
  3. Basic Configuration
  5. G0 XY move fail

G0 XY move fail

More
07 Sep 2015 03:48 #62173 by looping
G0 XY move fail was created by looping
Hello
I currently setting up my CNC powered by a Gecko G540 and V2.6.9. So far, first tests were perfect : everything in stepconf testing axis is OK
The default linuxCNC GCode program executed nicely :)

But with the attached program, the line 49 doesn't product the correct move : the Y move that should be 50mm, but only a small Y move occurs.10mm at most.
I have the same failure each time I run the program, on the same line

I tried to
1) to change the line
from: X61.1344 Y83.995
to: G1 X61.1344 Y83.995
=> the program run to the end with no other malfunction

2) to change the XY move into a X move, then an Y move: I change the line 49
from: X61.1344 Y83.995
to: X61.1344
Y83.995
=> the program run to the end with no other malfunction

3) Reduce the max_acceleration down to 60mm/s2 with no success.

4) I changed the origin but the same failure still occurs always on line 49

Is it possible that someone try my program on his hardware, I let me know ?

regards
Attachments:

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

More
07 Sep 2015 05:54 #62174 by PCW
Replied by PCW on topic G0 XY move fail
Is the DRO readout correct after the X/Y move?
( that is, is this a hardware issue or a interpreter/trajectory planner issue )

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

More
07 Sep 2015 12:33 #62181 by Rick G
Replied by Rick G on topic G0 XY move fail
Have you tried changing

O1 (LG_PCB)
(COMPENSATION-WEAR)
(REV-0.70)
(AUG-22-2015-11:01:41AM)

G90 
G17 
G54 
M06 T1 ()
(interrupteur)
S1000

To
O1 (LG_PCB)
(COMPENSATION-WEAR)
(REV-0.70)
(AUG-22-2015-11:01:41AM)

G40 ( turn cutter compensation off.) 

G90 
G17 
G54 
M06 T1 ()
(interrupteur)
S1000

It appears that the line you refer to is the first X move in the positive direction.

Rick G

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

More
07 Sep 2015 13:28 #62182 by looping
Replied by looping on topic G0 XY move fail
Thanks for you help

@PCW
After line 49, the readout shows values Y => 83.995
The the next and last G0 command on XY (line 82) is execute correctly.

@Rick G
I'll try the G40.
But if it was about compensation, it should also happen after the program modification n°2 when I change to :
...
G00 Z25.
X61.1344
Y83.995
Z2.
...
But like this, it's ok :S

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

More
07 Sep 2015 15:25 #62185 by ArcEye
Replied by ArcEye on topic G0 XY move fail
I assume this is what your plot should look like?





I removed the % top and bottom, changed the header so that G40 was applied before the tool change and G43 applied where it should be, immediately after
the M6T? (not after a linear move that will go to the wrong place) and it seems to run as intended.
G90 
G17 
G54 
G40

M06 T1
G43

S1000 
M03 
G00 X120.1703 Y36.7129 

Z25. 
Z2. 
G01 G40 Z-0.5 F100. 
G02 X120.1703 Y36.7129 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X120.1703 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X120.1703 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X120.1703 Y36.7129 I-4.8 J0. F200. 
G00 Z25. 
X88.0584 
Z2. 
G01 Z-0.5 F100. 
G02 X88.0584 Y36.7129 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X88.0584 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X88.0584 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X88.0584 Y36.7129 I-4.8 J0. F200. 
G00 Z25. 
X49.9203 
Z2. 
G01 Z-0.5 F100. 
G02 X49.9203 Y36.7129 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X49.9203 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X49.9203 Y36.7129 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X49.9203 Y36.7129 I-4.8 J0. F200. 
G00 Z25. 
X61.1344 Y83.995 
Z2. 
G01 Z-0.5 F100. 
G02 X61.1344 Y83.995 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X61.1344 Y83.995 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X61.1344 Y83.995 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X61.1344 Y83.995 I-4.8 J0. F200. 
G00 Z25. 
X86.6995 
Z2. 
G01 Z-0.5 F100. 
G02 X86.6995 Y83.995 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X86.6995 Y83.995 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X86.6995 Y83.995 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X86.6995 Y83.995 I-4.8 J0. F200. 
G00 Z25. 
X111.909 
Z2. 
G01 Z-0.5 F100. 
G02 X111.909 Y83.995 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X111.909 Y83.995 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X111.909 Y83.995 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X111.909 Y83.995 I-4.8 J0. F200. 
G00 Z25. 
X180.5271 Y143.4564 
Z2. 
G01 Z-0.5 F100. 
G02 X180.5271 Y143.4564 I-4.8 J0. F200. 
G01 Z-1. F100. 
G02 X180.5271 Y143.4564 I-4.8 J0. F200. 
G01 Z-1.5 F100. 
G02 X180.5271 Y143.4564 I-4.8 J0. F200. 
G01 Z-1.9 F100. 
G02 X180.5271 Y143.4564 I-4.8 J0. F200. 
G00 Z25. 
M2

regards
Attachments:

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

More
07 Sep 2015 19:24 #62195 by looping
Replied by looping on topic G0 XY move fail
Thanks ArcEye
Yes this is exactly my plot.
I didn't dig into tool compensation yet :blush:
I don't event know the content of my tool.tbl

I 'll try your code soon and learn tool compensation .
I'll keep you posted
Regards

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

More
08 Sep 2015 16:47 #62235 by looping
Replied by looping on topic G0 XY move fail
Hello
I could only do a few test la night:
1) With ArcEye's modifications, I still have the same wrong move.
2) I removed lines tools related (M06, M40 and M43) and the move is performed correctly
So it seems to be linked with compensation.

I'm using a 3mm endmill

Here's my current tool.tbl
T1 P1 D0.125000 Z+0.511000 ;1/8 end mill
T2 P2 D0.062500 Z+0.100000 ;1/16 end mill
T3 P3 D0.201000 Z+1.273000 ;#7 tap drill
T99999 P99999 Z+0.100000 ;big tool number

I guess it should be :
T1 P1 D3.000000 Z+0.000000 ; 3mm end mill
I'll make this update and retry tonight ArcEye's modifications

Regards

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

More
09 Sep 2015 13:16 - 10 Sep 2015 21:38 #62303 by looping
Replied by looping on topic G0 XY move fail
Hello

I updated tool.tbl with
T1 P1 D3.000000 Z+0.000000 ; 3mm end mill

and now everything works fine, even the initial GCode post at the beginning of the thread.
Thanks a lot for your help

Regards
Last edit: 10 Sep 2015 21:38 by looping.

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

  1. Configuring LinuxCNC
  3. Basic Configuration
  5. G0 XY move fail
Time to create page: 0.092 seconds
Powered by Kunena Forum