Dear reader, I'm having trouble starting a job. After homing and pressing start job I get error 9 Alarm 2. See attached screenshot. I have great issues detecting the problem here. The jobs has no odd parameters exceeding the travel limits. It also occurs when loading older, previously succesfully run jobs. Soft limits are ON. I've checked GRBL and the $130/131/132 maximum travel settings are good. v1.0.376, grblHAL 1.1f Status: ready, connected, idle Any thoughts or suggestions? Many thanks!
Home, then Set Zero, then start the job. Skipping SetZero means work coordinates are not set. The moves are in work coordinates, and work coordinates must fall withing machine coordinates. Have a read: Frequently Asked Questions
Hi Peter, Forgot to mention but I did. Homing, position spindle for job, set zero , run job —> error 9 thanks for your swift reply!
Then might indeed be something in the job (provide for review along with a Grbl Settings backup for review)
Hi Peter, I'm not sure it's the job. It is occurring with multiple jobs. I've attached the job! Thank you for your help. Below the grbl: $0=10.0 ; Step pulse time, microseconds $1=255 ; Step idle delay, milliseconds $2=0 ; Step pulse invert, mask $3=7 ; Step direction invert, mask $4=0 ; Invert step enable pin, boolean $5=0 ; Invert limit pins, boolean/mask $6=1 ; Invert probe pin, boolean $8=0 ; Ganged axes direction invert as bitfield $9=1 ; PWM Spindle as bitfield where setting bit 0 enables the rest $10=511 ; Status report options, mask $11=0.010 ; Junction deviation, millimeters $12=0.002 ; Arc tolerance, millimeters $13=0 ; Report in inches, boolean $14=0 ; Limit pins invert, mask $15=0 ; Coolant pins invert, mask $16=0 ; Spindle pins invert, mask $17=0 ; Control pins pullup disable, mask $18=0 ; Limit pins pullup disable, mask $19=0 ; Probe pin pullup disable, boolean $20=1 ; Soft limits enable, boolean $21=1 ; Hard limits enable, boolean $22=1 ; Homing cycle enable, boolean (Grbl) / mask (GrblHAL) $23=3 ; Homing direction invert, mask $24=100.0 ; Homing locate feed rate, mm/min $25=1000.0 ; Homing search seek rate, mm/min $26=250 ; Homing switch debounce delay, milliseconds $27=1.000 ; Homing switch pull-off distance, millimeters $28=0.100 ; G73 retract distance, in mm $29=5.0 ; Step pulse delay (ms) $30=25000.000 ; Maximum spindle speed, RPM $31=3500.000 ; Minimum spindle speed, RPM $32=0 ; Laser-mode enable, boolean $33=5000.0 ; Spindle PWM frequency $34=0.0 ; Spindle off Value $35=0.0 ; Spindle min value $36=100.0 ; Spindle max value $37=0 ; Stepper deenergize mask $39=1 ; Enable printable realtime command characters, boolean $40=0 ; Apply soft limits for jog commands, boolean $43=1 ; Homing passes $44=4 ; Homing cycle 1 $45=3 ; Homing cycle 2 $46=0 ; Homing cycle 3 $62=0 ; Sleep Enable $63=2 ; Feed Hold Actions $64=0 ; Force Init Alarm $65=0 ; Require homing sequence to be executed at startup $70=7 ; Network Services $73=0 ; Wifi Mode $74=WONDERBYWOOD.com ; Wifi network SSID $75=Heineken12345 ; Wifi network PSK $100=199.100 ; X-axis steps per millimeter $101=199.100 ; Y-axis steps per millimeter $102=199.100 ; Z-axis steps per millimeter $110=2500.000 ; X-axis maximum rate, mm/min $111=2500.000 ; Y-axis maximum rate, mm/min $112=2500.000 ; Z-axis maximum rate, mm/min $120=150.000 ; X-axis acceleration, mm/sec^2 $121=150.000 ; Y-axis acceleration, mm/sec^2 $122=150.000 ; Z-axis acceleration, mm/sec^2 $130=1250.000 ; X-axis maximum travel, millimeters $131=1250.000 ; Y-axis maximum travel, millimeters $132=100.000 ; Z-axis maximum travel, millimeters $300=Grbl ; unknown $302=192.168.5.1 ; unknown $303=192.168.5.1 ; unknown $304=255.255.255.0 ; unknown $305=23 ; unknown $306=80 ; unknown $307=81 ; unknown $341=0 ; Tool Change Mode $342=30.0 ; Tool Change probing distance $343=25.0 ; Tool Change Locate Feed rate $344=200.0 ; Tool Change Search Seek rate $345=200.0 ; Tool Change Probe Pull Off rate $346=1 ; Restore position after M6 as boolean $370=0 ; Invert I/O Port Inputs (mask) $384=0 ; Disable G92 Persistence $396=800 ; WebUI timeout in minutes $397=0 ; WebUI auto report interval in milliseconds $398=35 ; Planner buffer blocks $481=0 ; Autoreport interval in ms $I=custom
OK last question, if you jog over to where you zero, click SetZero, hover mouse over the DROs to show the Machine Coordinates, what are the machine coordinates at Work Zero for X, Y and Z?
I notice your g-code file extension is *.tap and there are some codes missing from the header of the g-code file that I would expect from a grbl compatible post processor. What post processor are you using? Can I suggest you use this one? docs:software:vectric [OpenBuilds Documentation] Alex.
Hi Alex, Thanks I was not aware. I will update the post processors. You think that might be the cause?
Right, so Keep in mind (or if not read yet, please do Frequently Asked Questions ) that the entire machine lies in negative quadrant space. Axes Max = 0 in machine coordinates. Z is at machine coordinates of -18mm Meaning, it can move a max of 18mm before it would go outside the negative envelope in Z (i.e violate the Soft Limit) Yet, your GCODE: Tries to do a Z20.320mm lift - and correctly 20mm is more than the 18mm available, so the Soft Limit is absolutely correct Try lowering your clearances in Vectric, doesn't need to go that high. Your entire job, including clearance moves has to fit in the machine envelope. (Soft limits hard to understand sometimes, because it works in machine coordinates, might want to disable it and if you are really worried, fit the Min/Max endstops as shown in BlackBox Docs > Xtensions Limits section)
And yes, please use the correct Post Processors (not related to soft limits issue, but still good practice) docs:software:cam [OpenBuilds Documentation]
yes, your code contains a line T1M6 which is a tool change instruction that GRBL does not understand. The correct postprocessor will not include codes that GRBL does not understand.
@Peter Van Der Walt @Alex Chambers @David the swarfer Many thanks for the help! We changed the post processor (never knew that existed)! And Peter, your advice on the Z coordinates was the solution! should I calbrate the cnc to get coordinates closer to 0? thanks!
Coordinates are not calibration affected. Real world distances are. Calibration sets the difference between theoretical distance in steps per mm to actual - last 1% taking manufacturing tolerances into account basically
