Hi!
I’m having an issue with my OMNIO CNC where when I hit cycle start it lowers the bit into the metal and drags it across before turning the bit on, even when it is supposed to just be drilling holes.
I’ve been generating GCode in Fusion 360 with the Mach3 post process and tried to solve this issue by lifting the bit up after zeroing and pressing cycle start, however, it did not work.
1 Like
I’m guessing you are using Mach3 to control it. Something I do on our CNC it start the spindle before hitting cycle start just as a precaution to make sure it is up to speed. Are you able to share your G-Code?
2 Likes
one thing that can happen on cnc machines with no glass scales for axis position is they will “lose” their axis position. Even if your work coordinates are set properly, the machine coordinates can behave weirdly. A lot of machines will command a tool change where it puts the spindle in tool change position, probably the top of Z axis for a router. Once the tool change has happened the machine will command work coordinates, so if your machine coordinates are in the wrong spot you will crash before the program switches to work coordinates. A good practice is to ensure machine coodinates are properly set before running the machine. Some machines do this on every start up. Mach 3 has a button “ref all home” try using this or any other machine axis reset procedure you have, then make sure your work coordinates are set properly and see if this solves your issue.
Also could have a problem with your tool length offset. some video or photos of the controller, offsets, and code would be helpful
Ok, I’ll try this
I can’t access our shop right now due to us having a snow day but I’ll send videos ASAP
Hi!
Sorry for taking so long to reply I was waiting for today so I could get the gcode off a computer in our shop, but we have a snow day today so I’ll get it to you ASAP. I’ll try running spindle at start but I don’t want to drill a line across a part that just needs holes. I am using Mach 3.
Actually I got someone to get it again, here’s the GCODE
Thank you for your time!
(3 HOLE STRAIGHT GUSSET BORE)
(MACHINE)
( VENDOR AUTODESK)
( MODEL GENERIC 3-AXIS)
( DESCRIPTION THIS MACHINE HAS XYZ AXIS ON THE HEAD)
(T2 D=3.175 CR=0. - ZMIN=-4.175 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90
(BORE1)
T2 M6
S18000 M3
G17 G90 G94
G54
M8
G0 X13.58 Y-12.7
G43 Z23. H2
G0 Z2.
G1 Z0. F360.
G3 X11.82 Z-0.086 I-0.88 J0.
X13.58 Z-0.172 I0.88 J0.
X11.82 Z-0.258 I-0.88 J0.
X13.58 Z-0.345 I0.88 J0.
X11.82 Z-0.431 I-0.88 J0.
X13.58 Z-0.517 I0.88 J0.
X11.82 Z-0.603 I-0.88 J0.
X13.58 Z-0.689 I0.88 J0.
X11.82 Z-0.775 I-0.88 J0.
X13.58 Z-0.862 I0.88 J0.
X11.82 Z-0.948 I-0.88 J0.
X13.58 Z-1.034 I0.88 J0.
X11.82 Z-1.12 I-0.88 J0.
X13.58 Z-1.206 I0.88 J0.
X11.82 Z-1.292 I-0.88 J0.
X13.58 Z-1.379 I0.88 J0.
X11.82 Z-1.465 I-0.88 J0.
X13.58 Z-1.551 I0.88 J0.
X11.82 Z-1.637 I-0.88 J0.
X13.58 Z-1.723 I0.88 J0.
X11.82 Z-1.809 I-0.88 J0.
X13.58 Z-1.896 I0.88 J0.
X11.82 Z-1.982 I-0.88 J0.
X13.58 Z-2.068 I0.88 J0.
X11.82 Z-2.154 I-0.88 J0.
X13.58 Z-2.24 I0.88 J0.
X11.82 Z-2.326 I-0.88 J0.
X13.58 Z-2.413 I0.88 J0.
X11.82 Z-2.499 I-0.88 J0.
X13.58 Z-2.585 I0.88 J0.
X11.82 Z-2.671 I-0.88 J0.
X13.58 Z-2.757 I0.88 J0.
X11.82 Z-2.843 I-0.88 J0.
X13.58 Z-2.93 I0.88 J0.
X11.82 Z-3.016 I-0.88 J0.
X13.58 Z-3.102 I0.88 J0.
X11.82 Z-3.188 I-0.88 J0.
X13.58 Z-3.274 I0.88 J0.
X11.82 Z-3.36 I-0.88 J0.
X13.58 Z-3.447 I0.88 J0.
X11.82 Z-3.533 I-0.88 J0.
X13.58 Z-3.619 I0.88 J0.
X11.82 Z-3.705 I-0.88 J0.
X13.58 Z-3.791 I0.88 J0.
X11.82 Z-3.877 I-0.88 J0.
X13.58 Z-3.964 I0.88 J0.
X11.82 Z-4.05 I-0.88 J0.
X13.58 Z-4.136 I0.88 J0.
X12.828 Y-11.829 Z-4.175 I-0.88 J0.
X12.572 Y-13.571 I-0.128 J-0.871
X12.828 Y-11.829 I0.128 J0.871
G0 Z8.
X13.58 Y-38.1
Z2.
G1 Z0. F360.
G3 X11.82 Z-0.086 I-0.88 J0.
X13.58 Z-0.172 I0.88 J0.
X11.82 Z-0.258 I-0.88 J0.
X13.58 Z-0.345 I0.88 J0.
X11.82 Z-0.431 I-0.88 J0.
X13.58 Z-0.517 I0.88 J0.
X11.82 Z-0.603 I-0.88 J0.
X13.58 Z-0.689 I0.88 J0.
X11.82 Z-0.775 I-0.88 J0.
X13.58 Z-0.862 I0.88 J0.
X11.82 Z-0.948 I-0.88 J0.
X13.58 Z-1.034 I0.88 J0.
X11.82 Z-1.12 I-0.88 J0.
X13.58 Z-1.206 I0.88 J0.
X11.82 Z-1.292 I-0.88 J0.
X13.58 Z-1.379 I0.88 J0.
X11.82 Z-1.465 I-0.88 J0.
X13.58 Z-1.551 I0.88 J0.
X11.82 Z-1.637 I-0.88 J0.
X13.58 Z-1.723 I0.88 J0.
X11.82 Z-1.809 I-0.88 J0.
X13.58 Z-1.896 I0.88 J0.
X11.82 Z-1.982 I-0.88 J0.
X13.58 Z-2.068 I0.88 J0.
X11.82 Z-2.154 I-0.88 J0.
X13.58 Z-2.24 I0.88 J0.
X11.82 Z-2.326 I-0.88 J0.
X13.58 Z-2.413 I0.88 J0.
X11.82 Z-2.499 I-0.88 J0.
X13.58 Z-2.585 I0.88 J0.
X11.82 Z-2.671 I-0.88 J0.
X13.58 Z-2.757 I0.88 J0.
X11.82 Z-2.843 I-0.88 J0.
X13.58 Z-2.93 I0.88 J0.
X11.82 Z-3.016 I-0.88 J0.
X13.58 Z-3.102 I0.88 J0.
X11.82 Z-3.188 I-0.88 J0.
X13.58 Z-3.274 I0.88 J0.
X11.82 Z-3.36 I-0.88 J0.
X13.58 Z-3.447 I0.88 J0.
X11.82 Z-3.533 I-0.88 J0.
X13.58 Z-3.619 I0.88 J0.
X11.82 Z-3.705 I-0.88 J0.
X13.58 Z-3.791 I0.88 J0.
X11.82 Z-3.877 I-0.88 J0.
X13.58 Z-3.964 I0.88 J0.
X11.82 Z-4.05 I-0.88 J0.
X13.58 Z-4.136 I0.88 J0.
X12.828 Y-37.229 Z-4.175 I-0.88 J0.
X12.572 Y-38.971 I-0.128 J-0.871
X12.828 Y-37.229 I0.128 J0.871
G0 Z8.
X13.58 Y-63.5
Z2.
G1 Z0. F360.
G3 X11.82 Z-0.086 I-0.88 J0.
X13.58 Z-0.172 I0.88 J0.
X11.82 Z-0.258 I-0.88 J0.
X13.58 Z-0.345 I0.88 J0.
X11.82 Z-0.431 I-0.88 J0.
X13.58 Z-0.517 I0.88 J0.
X11.82 Z-0.603 I-0.88 J0.
X13.58 Z-0.689 I0.88 J0.
X11.82 Z-0.775 I-0.88 J0.
X13.58 Z-0.862 I0.88 J0.
X11.82 Z-0.948 I-0.88 J0.
X13.58 Z-1.034 I0.88 J0.
X11.82 Z-1.12 I-0.88 J0.
X13.58 Z-1.206 I0.88 J0.
X11.82 Z-1.292 I-0.88 J0.
X13.58 Z-1.379 I0.88 J0.
X11.82 Z-1.465 I-0.88 J0.
X13.58 Z-1.551 I0.88 J0.
X11.82 Z-1.637 I-0.88 J0.
X13.58 Z-1.723 I0.88 J0.
X11.82 Z-1.809 I-0.88 J0.
X13.58 Z-1.896 I0.88 J0.
X11.82 Z-1.982 I-0.88 J0.
X13.58 Z-2.068 I0.88 J0.
X11.82 Z-2.154 I-0.88 J0.
X13.58 Z-2.24 I0.88 J0.
X11.82 Z-2.326 I-0.88 J0.
X13.58 Z-2.413 I0.88 J0.
X11.82 Z-2.499 I-0.88 J0.
X13.58 Z-2.585 I0.88 J0.
X11.82 Z-2.671 I-0.88 J0.
X13.58 Z-2.757 I0.88 J0.
X11.82 Z-2.843 I-0.88 J0.
X13.58 Z-2.93 I0.88 J0.
X11.82 Z-3.016 I-0.88 J0.
X13.58 Z-3.102 I0.88 J0.
X11.82 Z-3.188 I-0.88 J0.
X13.58 Z-3.274 I0.88 J0.
X11.82 Z-3.36 I-0.88 J0.
X13.58 Z-3.447 I0.88 J0.
X11.82 Z-3.533 I-0.88 J0.
X13.58 Z-3.619 I0.88 J0.
X11.82 Z-3.705 I-0.88 J0.
X13.58 Z-3.791 I0.88 J0.
X11.82 Z-3.877 I-0.88 J0.
X13.58 Z-3.964 I0.88 J0.
X11.82 Z-4.05 I-0.88 J0.
X13.58 Z-4.136 I0.88 J0.
X12.828 Y-62.629 Z-4.175 I-0.88 J0.
X12.572 Y-64.371 I-0.128 J-0.871
X12.828 Y-62.629 I0.128 J0.871
G0 Z23.
M9
M5
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30
our procedure for starting the cnc is
- zero it xyz
- bring it up ~4 inches
- start it, if it goes straight down, stop it. it should go up for a second, stop, spin up, then go down
have you been able to get the bit to start spinning at all?
2 Likes
Yeah I’m just lazy and do this as well so there’s plenty of space between the start position and Z height. Raise it up before cycle start. Crude but it works.
So if its not turning the spindle on it is not getting to the m3 command. So the issue is in the few lines before that. g28 sends the machine to your home position (machine home not work coordinates) so I really think your machine zero isnt right.
As others have said you are sending the head to machine 0 (G28) It goes
G28 G91 Z0.
The problem is machine 0 and the over-travel limit switch is in basically the same place so it trips the limit switch often. I used to edit the G-code. But now in the fusion post processor I change the “safe retract” option to “clearance height” which eliminates it trying to go to machine zero. I always manually position the router safe place before starting the program.
1 Like
when we make our gcode we get rid of g28 so it doesnt re home itself
1 Like
The bit turns on eventually, just after dragging everywhere. I can’t test anything because it’s dumping snow in my area, but I’ll try this. I’m thinking that its the machine home issue, I didn’t really know what ref all home did so I was just zeroing the part and then running it. I’m guessing I bumped the button at some point in a bad spot. I think changing to clearance height will fix the issue.
Thanks for all the help, we don’t have anyone on our team or mentors who know how to use a CNC machine so its just been struggle 
1 Like
Why? and fyi g28 doesn’t set the home, it sends the machine to the set home position (just so we are speaking the same language)
I don’t use Mach 3, I have a Laguna, but I did have to modify the Post Processor to prevent it from going to z0 at the start of the program
I can find what I did if that’s useful
Your startup code looks almost identical to what we get when we use Fusion. G28 G91 Z0. returns the Z axis (and it should only move the Z axis) to its reference position which is the position where it hits the limit switch. If you don’t reference the machine first, it goes to where it thinks this position is.
I may be missing something, but I don’t see any other code that would move the spindle in the X and Y positions before it is turned on. When we run code on our machine it goes to the Z reference and turns on the spindle.
We always reference the OMIO when we turn it on because we don’t trust the last state of the machine. It could have been improperly shut down or somebody could have turned the knobs on the steppers.
Almost.
G28 sends the router to machine home. Z is the first axis to move. That is your problem.
G91 set incremental move Z0 doesn’t move in incremental mode.
No I respectfully disagree, when you only specify one axis it only moves that axis. Our machine does not go back to the X and Y axis references. Also: G28 G-Code - the go home command for Gcode
G28 G91 X0 Y0 Z0;
Just stating G28; with no axis or axis set to zero as the above line would return all axis to the home position in a linear rapid move.the G28 zero return g-code can be used to return one axis or multiple. The block G28 G91 Z0.0; would return the Z-axis to its reference position while G28 G91 X0.0 Y0.0 Z0.0; would return the 3 Axis X, Y and Z.
The mach3 post processor is known to have random bug issues, I recommend using this one, which shouldn’t do random things during the start/end of ops.
1 Like
Maybe so. I will play with it when I get some time.