Ha! I was just getting ready to reply as well, but you nailed it way harder than I would have. Great reply!
1 Like
Thank so much for taking the time for this explanation, @jjneeb !!
I will go over this tomorrow when I get back into the shop and see what I can do. I’m sure you will have me straightened out with these details!
The very first toolpath I loaded into Mach4 was off by about 1 inch in X. For the life of me I couldn’t figure out why that was. I discovered there was an offset in the G54 Fixture Offset when I started Mach4. I went into the Offsets tab, highlighted the offset in G54 and entered 0.0 in the X, Y, and Z column (hitting ENTER after each reset to 0.0.) I then went back to Program Run, used the touch plate to set my X, Y, and Z zero, and the toolpath was spot on, and has been ever since. I only needed to set that offset to 0.0 that one time. It’s worked flawlessly ever since. I don’t know if that is/was the problem in this case, but that’s what I experienced.
1 Like
You may also find this helpful.
1 Like
I looked at my G54 offsets and found values assigned to each. I set X, Y & Z to 0.0 and it did not solve the error.
So I’ve been study this most of the day… I watched Jim’s video and adjusted my soft limits. I used the touch plate for my work piece. Still no luck.
One thing I notice is, I do not see my toolpath in Mach4. Jim shared his in his response above, but I see nothing when I load Gcode.
I will say that I am using the Avid Spoilboard Design File and creating the post from Fusion 360. Maybe that’s the issue… IDK.
Possibly I need different spoilboard flattening file?
G54 offset is where the touch plate script, or manually pressing the “Zero X/Y/Z” buttons on the Mach4 interface, store the values*. The distance is measured ‘from Home’ - or physical zero for each axis - established each time you home the machine.
Maybe share your gcode file for us to load and review?
*You can also setup and use other offsets (G55, G56, etc). G54 is simply the default work coordinate datum and is standard to use as your ‘live’ one. It’s common to use the others for static locations and more advanced techniques, too!
Just wanted to add another thing for those looking to decipher what appears to be a complicated message at first glance.
The message will state the axis and either softmin (minimum) or softmax (maximum).
X softmin is too far left
X max is too far right
Y min is too far to the front of the machine
Y max is too far to the back of the machine
Z min is too low
Z max is too high
So if it says ‘X-axis over softmax’ you know to look for a feature beyond the right edge of your machining boundary.
1 Like
This is my G Code.
I appreciate everyone’s input and help. Spent the entire day out here and have gotten nowhere. I’m sure it’s me…
(1001)
(T2 D=2. CR=0. - ZMIN=-0.01 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF)
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING)
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID)
(MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)
G28 G91 Z0.
G90
(FACE1)
S5000 M3
G54
M8
G0 X-1.3 Y95.0984
G43 Z0.4 H2
G1 Z0.2 F39.4
Z0.19 F13.1
G18 G2 X-1.1 Z-0.01 I0.2 K0. F39.4
G1 X0.
X48.
G17 G2 Y93.2158 I0. J-0.9413
G1 X0.
G3 Y91.3332 I0. J-0.9413
G1 X48.
G2 Y89.4506 I0. J-0.9413
G1 X0.
G3 Y87.5681 I0. J-0.9413
G1 X48.
G2 Y85.6855 I0. J-0.9413
G1 X0.
G3 Y83.8029 I0. J-0.9413
G1 X48.
G2 Y81.9203 I0. J-0.9413
G1 X0.
G3 Y80.0377 I0. J-0.9413
G1 X48.
G2 Y78.1551 I0. J-0.9413
G1 X0.
G3 Y76.2725 I0. J-0.9413
G1 X48.
G2 Y74.3899 I0. J-0.9413
G1 X0.
G3 Y72.5074 I0. J-0.9413
G1 X48.
G2 Y70.6248 I0. J-0.9413
G1 X0.
G3 Y68.7422 I0. J-0.9413
G1 X48.
G2 Y66.8596 I0. J-0.9413
G1 X0.
G3 Y64.977 I0. J-0.9413
G1 X48.
G2 Y63.0944 I0. J-0.9413
G1 X0.
G3 Y61.2118 I0. J-0.9413
G1 X48.
G2 Y59.3292 I0. J-0.9413
G1 X0.
G3 Y57.4466 I0. J-0.9413
G1 X48.
G2 Y55.5641 I0. J-0.9413
G1 X0.
G3 Y53.6815 I0. J-0.9413
G1 X48.
G2 Y51.7989 I0. J-0.9413
G1 X0.
G3 Y49.9163 I0. J-0.9413
G1 X48.
G2 Y48.0337 I0. J-0.9413
G1 X0.
G3 Y46.1511 I0. J-0.9413
G1 X48.
G2 Y44.2685 I0. J-0.9413
G1 X0.
G3 Y42.3859 I0. J-0.9413
G1 X48.
G2 Y40.5034 I0. J-0.9413
G1 X0.
G3 Y38.6208 I0. J-0.9413
G1 X48.
G2 Y36.7382 I0. J-0.9413
G1 X0.
G3 Y34.8556 I0. J-0.9413
G1 X48.
G2 Y32.973 I0. J-0.9413
G1 X0.
G3 Y31.0904 I0. J-0.9413
G1 X48.
G2 Y29.2078 I0. J-0.9413
G1 X0.
G3 Y27.3252 I0. J-0.9413
G1 X48.
G2 Y25.4426 I0. J-0.9413
G1 X0.
G3 Y23.5601 I0. J-0.9413
G1 X48.
G2 Y21.6775 I0. J-0.9413
G1 X0.
G3 Y19.7949 I0. J-0.9413
G1 X48.
G2 Y17.9123 I0. J-0.9413
G1 X0.
G3 Y16.0297 I0. J-0.9413
G1 X48.
G2 Y14.1471 I0. J-0.9413
G1 X0.
G3 Y12.2645 I0. J-0.9413
G1 X48.
G2 Y10.3819 I0. J-0.9413
G1 X0.
G3 Y8.4994 I0. J-0.9413
G1 X48.
G2 Y6.6168 I0. J-0.9413
G1 X0.
G3 Y4.7342 I0. J-0.9413
G1 X48.
G2 Y2.8516 I0. J-0.9413
G1 X0.
G3 Y0.969 I0. J-0.9413
G1 X48.
G18 G2 X48.2 Z0.19 I0. K0.2
G1 Z0.4
G17
M9
M5
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30
Thanks David.
Are you ready for the DUMBEST question of the day? Here goes…
If X Softmin = too far left, what is the fix?
One or both of these are catching you. If you’re trying to cut a spoilboard, and that spoilboard covers your entire machine, and your X-zero is at the very left of your machine, it cannot possibly drive to X-1.3 (1.3 inches left of your machine’s physical limitation).
1 Like
Maybe you need to zoom out some, do you at lease see the yellow dashed line all the way around? that is the envelope of your machine’s cutting range. Zoom out with the mouse wheel, maybe your toolpath is just off screen.
However, David is right, you’re trying to a long way negative for a spoilboard. I would assume that the corner of your spoil board is very close to machine 0, 0.
I don’t know if you’ve already done this, but I always suggest people clamp down a couple pieces of scrap mdf or something in the interior of the machine and cut a few basic squares or circles first just to get the hang of it, see what the toolpaths look like on Mach4, etc., and then go for the spoilboard fine tuning. Here you can switch back and forth between machine and work coordinates and get a good feel for what they mean and how they relate to each other as well as you use your touchplate in a couple of locations.
1 Like
Looks to me like it’s going to do a lead-in. Maybe just disabling the lead-in feature in Fusion will reduce the attempts to travel off the table.
Thanks guys! I will look into this tomorrow morning and start by setting the X to 0.0.
I didn’t write this G Code. This came from the Avid site. PRO CNC and Standard CNC Machines - CNC Spoilboard.
Great conversation with insights I haven’t thought about being a new CNC user. I’ve seen this warning as well and didn’t understand what it was telling me. I have a lot to learn and short on patients. Can anyone recommend a good source to learn to understand gcode? In
When I have seen this , it is because when designing in vectric software or fusion360, I have told the CNC to move to a location beyond the soft limits of the machine . ie, start cutting a piece that measures 20 inches wide placed 10 inches from the far x edge of the CNC work area. Mach4 will recognize it can’t go there.