Jump to Line Causes X Soft Limit Error

[fablab]

I was running the following G-Code and I needed to jump to line 73, doing so would cause an X soft limit error.

Can anyone tell me why the Masso would do that?

Masso G3 running 4.01

Thanks!

N0010 (Filename: X-MemberFlange.tap)
N0020 (Post processor: MASSO Plasma (with THC)andScriber.scpost)
N0030 (Date: 3/13/2021)
N0040 G20 (Units: Inches)
N0050 F1
N0060 G53 G90 G40
N0070 M666 (---THC Off---)
N0080 (Part: X-MemberFlange)
N0090 (Operation: Outside Offset, 0, T30: 50 amp 3/16 steel-TESTED)
N0100 (50 Amp)
N0110 (THC Memory Slot 4)
N0120 (1.1 MM Tip)
N0130 G00 X2.4620 Y0.9675
N0140 (---Take Z reference---)
N0150 G38.2 Z -200 F19.685
N0160 G92 Z0.0
N0170 G00 Z0.0700
N0180 G92 Z0.0
N0190 G00 Z0.1400
N0200 M03 (---Torch On---)
N0210 (---Go to cutting height---)
N0220 Z0.0800
N0230 G01 F100.0
N0240 G03 X2.6280 Y0.9345 I0.0995 J0.0665 F22.0
N0250 I-0.1280 J0.1280 F25.2857
N0260 M05 (---Torch Off---)
N0270 G00 Z0.5000
N0280 X0.7800 Y1.1005
N0290 (---Take Z reference---)
N0300 G38.2 Z -200 F19.685
N0310 G92 Z0.0
N0320 G00 Z0.0700
N0330 G92 Z0.0
N0340 G00 Z0.1400
N0350 M03 (---Torch On---)
N0360 (---Go to cutting height---)
N0370 Z0.0800
N0380 G01 F100.0
N0390 G03 X0.7470 Y0.9345 I0.0665 J-0.0995 F22.0
N0400 I0.1280 J0.1280 F25.2857
N0410 M05 (---Torch Off---)
N0420 G00 Z0.5000
N0430 X0.9130 Y3.4700
N0440 (---Take Z reference---)
N0450 G38.2 Z -200 F19.685
N0460 G92 Z0.0
N0470 G00 Z0.0700
N0480 G92 Z0.0
N0490 G00 Z0.1400
N0500 M03 (---Torch On---)
N0510 (---Go to cutting height---)
N0520 Z0.0800
N0530 G01 F100.0
N0540 G03 X0.7470 Y3.5030 I-0.0995 J-0.0665 F22.0
N0550 I0.1280 J-0.1280 F25.2857
N0560 M05 (---Torch Off---)
N0570 G00 Z0.5000
N0580 X2.5950 Y3.3370
N0590 (---Take Z reference---)
N0600 G38.2 Z -200 F19.685
N0610 G92 Z0.0
N0620 G00 Z0.0700
N0630 G92 Z0.0
N0640 G00 Z0.1400
N0650 M03 (---Torch On---)
N0660 (---Go to cutting height---)
N0670 Z0.0800
N0680 G01 F100.0
N0690 G03 X2.6280 Y3.5030 I-0.0665 J0.0995 F22.0
N0700 I-0.1280 J-0.1280 F25.2857
N0710 M05 (---Torch Off---)
N0720 G00 Z0.5000
N0730 X5.4072 Y4.3697
N0740 (---Take Z reference---)
N0750 G38.2 Z -200 F19.685
N0760 G92 Z0.0
N0770 G00 Z0.0700
N0780 G92 Z0.0
N0790 G00 Z0.1400
N0800 M03 (---Torch On---)
N0810 (---Go to cutting height---)
N0820 Z0.0800
N0830 G01 F100.0
N0840 G03 X5.2875 Y4.2500 I0.0000 J-0.1197 F22.0
N0850 M667 F6 (---THC On---)
N0860 G01 Y0.3750 F55.0
N0870 G02 X4.8750 Y-0.0375 I-0.4125 J0.0000
N0880 G01 X0.3750
N0890 G02 X-0.0375 Y0.3750 I0.0000 J0.4125
N0900 G01 Y4.2500
N0910 M666 (---THC Off---)
N0920 G02 X0.0000 Y4.2875 I0.0375 J0.0000 F22.0
N0930 M667 F6 (---THC On---)
N0940 G01 X5.2500 F55.0
N0950 M05 (---Torch Off---)
N0960 M666 (---THC Off---)
N0970 G00 Z0.5000
N0980 X0.0000 Y0.0000
N0990 M05 G30 M30 (---End of program---)

 

[cncnutz]

Hi Fablab

The problem with soft limits is they are transient. depending on how you setup your material for the cut you are doing you may exceed a limit today and tomorrow you move your starting point a fraction and the limit will no longer trip. As such all relevant information has to be collected at the time of the soft limit so that it can be analyzed and the cause found. The one thing I can tell you for sure is the soft limit was not on line 73 but in a line beyond that as MASSO looks many lines ahead.

When you get your soft limit jog your machine to each end of the axis that reported the soft limit alarm, (X in your case), and when you hit the soft limit at each end write down the working coordinate shown on the DRO.
Then look through the Gcode file and see if there is any Gcode than moves that axis that exceeds one of these values and if there is then that is why the soft limit is being tripped.

Alternatively to figure out why a soft limit is tripping you need to provide the following. (Gather this information before trying the the above method or positional information will be lost)

• A screen print of the F2 screen at the time of the soft limit
  
• A screen print of the F4 screen at the time of the soft limit
  
• A copy of your printable settings file
  
• A copy of the Gcode file you were cutting at the time
  

If you can provide this information then it will be possible to establish why by calculating current position and future positions.

Hope this helps
Cheers Peter

 

[fablab]

I guess just to be clear my table has almost 60" of travel in both X & Y.

In this case work X Y zero was @ machine coordinate X1.9346 Y 20.9474

As you can see from the G-Code above there are no moves that would bring me anywhere near a limit (in work or machine coordinates).

Maybe what I should add is I get similar odd behavior every time I load a file, if I load a file and don't click the rewind button at least twice the X axis will go to the extreme + direction when I do a cycle start. (My Dad has a G2 and has the same issue)



One question when "jumping to a line" does the Masso re-read the G-Code from line 1 and start at the commanded line or does it just start from the commanded line?

 

[cncnutz]

Hi Fablab

Without solid information I cannot explain why your machine behaves like this.
For example. At the end of your file you have a G30.
This might be outside the machines soft limits and so causes an alarm.

I'm probably entirely wrong but without any information I can only make wild guesses.
If you can provide settings files, Gcode files and some screen prints there is a good chance that the problem can be explained.
We first need to reproduce what you are seeing and then go from there.
Since you are dealing with a issue that seems to be repeatable it should be a lot easier to reproduce and explain.

Cheers Peter

 

[fablab]

Understood Peter,



I just reproduced the issue & uploaded the requested files.

I agree with you on the G30, I will remove it a retest..

 

[fablab]

Removed the G30, same results... No change limit error still occurs

 

[cncnutz]

Sorry I'm not seeing the files you uploaded.
You might need to zip them all up as there is a limited format that the forum will accept.
Note also the size limit of 8Mb but they shouldn't be anywhere near that size.
If you can provide both the Machine settings file and printable settings file as one is readable and the other I can load if needed.

Can you also provide a step by step process to follow to reproduce the problem.
for example.

• Start MASSO
  
• Home MASSO
  
• Load File
  
• Jump to line 73
  

X axis alarm will occur at this time

Cheers Peter

 

[fablab]

Step By Step
(1) Start Masso
(2) Home Masso
(3) Load File
(4) Jog to Start Position
(5) Zero X and Y
(6) Jump to line 73
(7) click start from line
(8) click Run
X limit error occurs

Thanks for the help!!

 

[cncnutz]

Hi Fablab

Thank you for the test files and method to reproduce.

I have now replicated and found the issue is a software bug in the jump to line routine.
When using imperial, the coordinates are converted to metric values which account for the large movements when getting into position. eg 1" becomes 25.4"
I have documented this and created a ticket for this bug to be corrected.

Cheers Peter