Instant fail: Error X Axis commanded over softmin?

Hello! I’m not a total noob, but I’m new Mach4 for sure.

Just got my new PRO4896 up and running. I ran the Vectric squaring and tramming file and the machine is dead on square. Pretty sweet. Coming from an X-Carve…this machine is quite the improvement and I’m super excited to party.

I have a 36"x 36" sheet of 3/4" MDF secured to the machine as a temporary wasteboard and I drew up a simple program to drill some 1/4" holes for some alignment dowel pins. My material setup in Vectric looks good. I homed the machine and then used the touch plate to set my material X,Y,Z…However, when I run the G-Code it fails on line 23 with “Error X Axis commanded over Soft Min”

Is it actually failing on line 24 and Mach just shows the last line ran? I’m guessing it’s failing on line 24. Either way…I have no idea why it’s failing with that error.

23 X0.0000Y0.0000F150.0
24 G00X2.0000Y12.0000Z0.2000

I looked and I don’t have a “Soft Min” set for X which further confuses me. I’d get this error if I DID have a soft minimum set.

( WasteBoardHoles )
( File created: Sunday November 06 2022 - 03:52 PM)
( for Avid CNC Machines, post processor v3.0 )
( Material Size: X= 36.000, Y= 36.000, Z= 0.750)
( Z Origin for Material = Material Surface)
( XY Origin for Material = Bottom Left Corner)
( Min Program Extents: X= 0.000, Y= 0.000, Z= -0.750)
( Max Program Extents: X= 36.000, Y= 36.000, Z= 0.000)
( Home Position: X =X0.0000 Y =Y0.0000 Z =Z0.8000)
( Safe Z = Z0.2000)
()
(Toolpaths used in this file:)
(Drill 1)
(Tools used in this file: )
(1 = End Mill {1/4"} - Up-Cut: Plywood\Softwood\MDF)
G00 G94 G20 G17 G90 G40 G49 G80
G91.1
T1M6
M07
G00 G43Z0.8000H1
S17000M03
(Toolpath: Drill 1 Tool: End Mill {1/4"} - Up-Cut: Plywood\Softwood\MDF)
X0.0000Y0.0000F150.0
G00X2.0000Y12.0000Z0.2000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00Y6.0000
G1Z-0.1250F30.0
G00Z0.0000

When you say you don’t have a soft min set for X, where are you looking?
The table is in the Mach4 control setup and should look something like this (except your Y will be more like 97).

Yep. That is where I was looking. This is what mine looks like.

1 Like

Mach4 has a look-ahead feature of something like 20 lines of code by default. I’m guessing you have a high X movement commanded on or around line 44.

Ah! Excellent insight! I will look closer at that. Thank you!

Hmmmmm I still don’t see anything weird or out of bounds…

( WasteBoardHoles )
( File created: Sunday November 06 2022 - 03:52 PM)
( for Avid CNC Machines, post processor v3.0 )
( Material Size: X= 36.000, Y= 36.000, Z= 0.750)
( Z Origin for Material = Material Surface)
( XY Origin for Material = Bottom Left Corner)
( Min Program Extents: X= 0.000, Y= 0.000, Z= -0.750)
( Max Program Extents: X= 36.000, Y= 36.000, Z= 0.000)
( Home Position: X =X0.0000 Y =Y0.0000 Z =Z0.8000)
( Safe Z = Z0.2000)
()
(Toolpaths used in this file:)
(Drill 1)
(Tools used in this file: )
(1 = End Mill {1/4"} - Up-Cut: Plywood\Softwood\MDF)
G00 G94 G20 G17 G90 G40 G49 G80
G91.1
T1M6
M07
G00 G43Z0.8000H1
S17000M03
(Toolpath: Drill 1 Tool: End Mill {1/4"} - Up-Cut: Plywood\Softwood\MDF)
X0.0000Y0.0000F150.0
G00X2.0000Y12.0000Z0.2000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00Y6.0000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00Y4.0000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00X4.0000Y2.0000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00X6.0000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00X12.0000
G1Z-0.1250F30.0
G00Z0.0000
G1Z-0.2500F30.0
G00Z0.2000
G00Z0.8000
G00X0.0000Y0.0000
M05
M09
M30
%

Just curious, when you get the error, can you toggle back to machine coordinates and see where the x-axis is showing? It may have something to do with your machine home position. Let us know what you see.

Good idea. I will try that tonight and report back.

Ok, that looks right. You do have a soft min for X, it is 0, in machine coordinates. So you would be looking for a location in Gcode where it is commanded past 0. It could be 20 or more lines ahead due to the lookahead buffer. It will be in work coordinates in the Gcode though, so you have to convert.

Ahhh interesting. That makes sense. Hopefully we are onto something here.

1 Like

I read ‘over’ and jumped to thinking in ‘maximum’ but you clearly stated ‘Soft Min’ that’s my bad!

Ok here we go…I tried again just a few minutes ago. Same error…

I hommed the machine like normal and then I used the touch plate to set my work coordinates.

Work Coordinates:

Machine Coordinates:

Looking through the GCode I can’t see anything below the “0” soft limit? Wouldn’t that be a negative number in the code if it was?

There isn’t anything funkey from what I can tell…but I also just popped out of a fried rice carb coma…I’m totally stumped.

maybe check your x home sensor and block,make sure its tight,
the x home sensor and the x softmin are related

Ya, it should tecnically be negative in both work and machine coordinates. However, the difference between your X machine and work coordinates is only about 15 thousandths, and you do have it going to X=0 in the Gcode, so it is getting very close.

What happens if you set your work X and Y zero just a quarter inch in from the machine X and Y zero, does the toolpath run ok then? You can just set Z0 an inch or two high so it doesn’t cut anything).

1 Like

Man, that worked…and at first it made ZERO sense why…I couldn’t understand how I could get a negative number, but now I see that what I’m looking at for the WC includes the touch plate offset…SOOOO the actual 0,0 location it’s calculating is LESS than the MC 0,0 resulting in the negative number. The math wasn’t adding up for me, but I wasn’t considering the offset…Sheesh.

Most people have their working area X and Y zero a bit inward of the Machine X and Y zero, but I suspect if you run the work right at the edge all the time you’ll probably have this problem sometimes.

I usually have my stops set more in the middle so I have room for clamps and junk around what I’m working on, and I only get close to the soft limit boundaries when I’m working on something really big.

Yep, exactly. At first I was a bit worried, but now that I understand this situation, it shouldn’t be a problem moving forward. I was zeroing on the spoil board to peck some holes it for work alignment. Either way I lost less than 0.25" so I’m golden.

Thank you all for your help. Normally I don’t really care for public forums, but so far this one is shaping up to be different. Really excited about the community we are building here.

This one is good, and the Facebook AVID group is very good as well. I’ve learned a lot there as well.