I have upgraded the following since I last ran a job. I installed the replacement Shapeoko Controller I have have in the drawer for a bit (over a year). I loaded GRBL 1.1 onto the new board and moved to UGS Platform. All of these changes are in preparation for the Shapeoko Touch Probe when they are back on the shelf. I use Fusion 360 for my CAD/CAM.
My Problem. . .
I can navigate around with UGS Platform and everything seems to work fine. However, when I go to run a simple little test job composed of 2 small circles cut into a piece of wood I encounter problems. When I start the job, the Z axis goes straight up until it trips the limit switch and halts the execution of the program. It has erred out with a couple different messages, but the result was the same, it stopped after hitting the limit switch.
I also tried to run the job with Carbide Motion v4 with the little two circle job I created (*.nc). It did the same thing except it moved to the x or y axis limit switch during the start-up sequence at the beginning of the job and stopped the job right at the beginning.
I also tried a couple of small jobs I had from before on my original installation (where I used the original controller board, GRBL .08? and and a pre Platform version of UGS along with Fusion 360). Same issue. As soon as you click “go”, it moves up the Z axis until it trips the limit switch.
The unit goes through the homing cycle perfectly.
Any thoughts that might help me get by this?
Thanks in advance for any guidance.
I also have a second error “M1 T6” which is in the .nc code file for a tool change (which is not applicable here)? Says it doesn’t support that command and if I bracket it out, it gets past that error and heads to the Z-axis limit switch error.
I could maybe see that if I didn’t get the same issue with files that worked perfectly before I made the upgrades. I also only raised the Z a half inch or so above the 0,0,0 datum point, so if it went in the wrong direction, it should only have been for that half inch and not the two inches up to the limit switch.
It is like it wants to execute a homing cycle before it starts the job file, but when it gets to the limit switch, unlike in a homing procedure where the limit switches only indicate the end of the line and then allows for the home locating, here it ignores that and just does a limit switch type stop.
To establish Z0, I do the homing cycle, then jog the bit to the point on the material that I want to use as my X0,Y0,Z0, then set zero. If I jog the bit away and then hit the return to zero, it moves directly to the spot I had set a Z0,Y0,Z0.
Again, I ran an old *.nc file that I have cut a number of times before I did the upgrade to the new board, GRBL 1.1 and UGS Platform. I also get similar problem when I try to cut the *.nc file from Carbide Motion 4, except that it limits out on the X or Y limit switches (can’t be sure which one as it is to the back right corner when it hits either or both switches and dies.
I was actually doing the little file with 2 circles to see if I needed to calibrate the mm/step parameters, just never got to that point. It shouldn’t be the big problem as as best I can figure, it should be either 20 or 40 for the Carbide3D controler in any event. As well, I jog around in increments that seem to match what the software thinks the distance is when I measure a larger jog step.
It is like it is trying to do a homing cycle before it starts to cut the job, but instead of the homing cycle using the limit switches as a guide as to where the physical limits are, it treats the limits switches in that physical sense where it shut things off.
When I wiped the EEPROM with the Upgrade file from Carbide3D, I did go and reset a couple parameters to enable the limit switches and homing. I also changed the table dimensions back to the ~ 450 for X and Y.
The G28 is generated by the Post Process in Fusion 360. Tomorrow I will run the file with the 3 lines with G28, which are
at the top of the code:
G28 G91 Z0
at the bottom of the code area:
G28 G91 Z0
G28 X0 Y0
The G28 code was in the files I used to run on the old Skapeoko controller and GRBL .08 and the old UGS processor. Any idea why it would be a problem with GRBL 1.1 and UGS Platform 4 as well as Carbide_Motion_4?
G28 G91 Z0 - will move the Z axis to its G28 location. When you cleared your EEPROM, your G28 position reset to 0,0,0. That means that your G28 location is 0mm from your machine zero which is your limit switches.
I’d recommend disabling the G28 feature in your post processor from Fusion.
As a question, how would I restore my Z28 offsets and what would they be?
I think i know a little less than I need to be dangerous.
---------Update----------
Yes, when I strip out the line with the Z28 I can run the job from UGS Platform. It would be nice to be able to get back to those original offsets though, so I don’t have to go and strip the Z28 lines out of every file.
G28 is a location. If you jog to your location you want to be G28, send G28.1, and that location will be your new G28. I use mine as a tool change location.
That is it!!! Worked perfectly. I relocated the G28 - XYZ position to one I like, then sent a G28.1 command to the controller. Ran a job successfully. Shut it off a and ran a job a few more times. Works perfectly!!!
My guess is that as people start to move to GRBL 1.1 there may well be some sharing my day of frustration out of the gate.
As a totally somewhat unrelated thing…I’ve attached the whole collection of posts for fusion360 I’ve accumulated. In it is a “mikep dewalt” post I use all the time. I didn’t write it. It’s been working really well for me. Among other things, it will inject the right speed dial settings into a comment in the top of the file if you set RPM up in the CAM. It doesn’t do any of the G28 business. (if you clear the property for “isdewalt” it returns the settings for makita) . Helixes work.
Example header:
%
(Made in : Autodesk CAM Post Processor)
(G Code optimized for Carbide3D SO 3 DEWALT611 with GRBL V0.9j controller)
(Program Name : 1001)
(Program Comments : 1 8 4edge 2up)
(5 Operations
(1 : Face1)
( Work Coordinate System : G53)
( Tool : Flat End Mill 2 Flutes, Diam = 3.175mm, Len = 12.7mm)
( Spindle : RPM = 5000, set router dial to 1)
( Machining time : 1 min 37 sec)
(2 : Features)
( Work Coordinate System : G53)
( Tool : Flat End Mill 2 Flutes, Diam = 3.175mm, Len = 12.7mm)
( Spindle : RPM = 10000, set router dial to 1)
( Machining time : 4 min 27 sec)
(3 : 2D Pocket1)
( Work Coordinate System : G53)
( Tool : Flat End Mill 2 Flutes, Diam = 3.175mm, Len = 12.7mm)
( Spindle : RPM = 5000, set router dial to 1)
( Machining time : 2 min 16 sec)
(4 : 2D Features Final)
( Work Coordinate System : G53)
( Tool : Flat End Mill 2 Flutes, Diam = 3.175mm, Len = 12.7mm)
( Spindle : RPM = 5000, set router dial to 1)
( Machining time : 53 sec)
(5 : 2D Outside)
( Work Coordinate System : G53)
( Tool : Flat End Mill 2 Flutes, Diam = 3.175mm, Len = 12.7mm)
( Spindle : RPM = 5000, set router dial to 1)
( Machining time : 2 min 24 sec)
