Hi everyone i think im a real noob because i have the exact same issue everytime i start a job the z go to top and hit the limit switch and alarm and i really dont know what is the issue its on a 1000 x 1000 queen ant pro v2 witn blackbox X32 and openbuild control
Hi everyone i know ima real noob but never have this issue with previous cnc and gcode file everytime i start a new job , the z axis go up and hit the limit switch and gave me an alarm, i read a post here but no real answer (in fact no answer i can understand) to my issue here what i do create my toolp[ath in Fusion 360 postprocess with openbuild postprocessor in openbuild control: home my cnc (queenant pro v2 1000 x 1000 with Blackbox X32) set my 0,0,0 (lower left and top of stock for Z) start my job and z axis go up and hit limit switch and alarm i really dont know what to do to fix this here my Gcode if can help (Made in : Autodesk CAM Post Processor) (G-Code optimized for Grbl 1.1 / BlackBox controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.32) (Units = mm) (Drawing name : waste board metric v1) (Program Name : 1 - recess waste board for queen ant) (1 Operation (1 : recess for tnuts) ( Tool 1: Flat End Mill 1 Flutes, Diam = 6.35mm, Len = 25.40mm) ( Spindle : RPM = 12000) ( Machining time : 13 min 23 sec) G90 G94 G17 G21 (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.) (Operation 1 of 1 : recess for tnuts) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 G0 X679.003 Y24.365 S12000 M3 G4 P1.8 G0 X679.003 Y24.365 Z15 F1505 G1 Z-0.3 Z-1.665 ....... G0 Z15 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 M5 G0 X-10 Y-10 M30 please help i really dont know where to search
Are you homing your machine? G53 co-ordinates will only work reliably if you establish a home position (the back, right, up corner has to be set to zero) as G53 uses that as a reference point. Try setting the start/end Z position to -10, 5 mm might still be triggering the switch. Alex.
my home is a z top, y back and X right i always home my machine before anything ihave limit switch on all axis, (3 switch) ( then move to my stock left bottom coer for X and Y and top of stock for Z then set 0 for all then start the job and z go up and hit the limit switch what happen if i remove G53 G0 Z-10 form Gcode and simply move manually the z axist before start the job? i know its not the solution but im really lost and its same with -10, -5 -30 -40 all have same result, o know its something really stupid i did because previous job made for previous controller (shapeoko) or wizard surfacing work great thats why i think removing this G53 line will work
This is a lot more informative than your other post. If you remove the G53 G0 Z move Z axis will not move at the start of the job. Your error though says that you have a soft limits error, so its not the G53 move causing the problem. It's more likely the G0 line with the Z15 move in it - have you got 15 mm above the surface of the workpiece for that move? If not you need to look at your heights settings in Fusion cam setup. Alex.
the G0 Z15 is at end of the job , i simply dont put the whole Gcode becase to big for nothing everything happen at beginning of the job, press start job then z go high and stop with alarm
ok if i use another post processor everything work like carbide 3d post processor, everything seem to work flawlessly and i just change the postprocessor, nothing else i know its something i don't understand somewhere, i really want to know and use the right post here my Grbl setting $0=10.0 ; Step pulse time, microseconds $1=255 ; Step idle delay, milliseconds $2=0 ; Step pulse invert, mask $3=2 ; Step direction invert, mask $4=0 ; Invert step enable pin, boolean $5=7 ; 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=0 ; Hard limits enable, boolean $22=1 ; Homing cycle enable, boolean (Grbl) / mask (GrblHAL) $23=0 ; Homing direction invert, mask $24=100.0 ; Homing locate feed rate, mm/min $25=3000.0 ; Homing search seek rate, mm/min $26=250 ; Homing switch debounce delay, milliseconds $27=2.500 ; Homing switch pull-off distance, millimeters $28=0.100 ; G73 retract distance, in mm $29=5.0 ; Step pulse delay (ms) $30=24000.000 ; Maximum spindle speed, RPM $31=0.000 ; 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=1 ; Wifi Mode $74= ; Wifi network SSID $75= ; Wifi network PSK $100=160.000 ; X-axis steps per millimeter $101=160.000 ; Y-axis steps per millimeter $102=320.000 ; Z-axis steps per millimeter $110=3000.000 ; X-axis maximum rate, mm/min $111=3000.000 ; Y-axis maximum rate, mm/min $112=1500.000 ; Z-axis maximum rate, mm/min $120=250.000 ; X-axis acceleration, mm/sec^2 $121=250.000 ; Y-axis acceleration, mm/sec^2 $122=250.000 ; Z-axis acceleration, mm/sec^2 $130=720.000 ; X-axis maximum travel, millimeters $131=720.000 ; Y-axis maximum travel, millimeters $132=90.000 ; Z-axis maximum travel, millimeters $300=Grbl ; Hostname $302=192.168.5.1 ; IP Address $303=192.168.5.1 ; Gateway $304=255.255.255.0 ; Netmask $305=23 ; Telnet Port $306=80 ; HTTP Port $307=81 ; Websocket Port $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=30 ; 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
Hi I am going to add comments to the gcode below to explain what it is doing (Made in : Autodesk CAM Post Processor) (G-Code optimized for Grbl 1.1 / BlackBox controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.32) (Units = mm) (Drawing name : waste board metric v1) (Program Name : 1 - recess waste board for queen ant) (1 Operation (1 : recess for tnuts) ( Tool 1: Flat End Mill 1 Flutes, Diam = 6.35mm, Len = 25.40mm) ( Spindle : RPM = 12000) ( Machining time : 13 min 23 sec) G90 G94 G17 ; set the modes we want, absolute movement, XY plane for arcs G21 ; all numbers in millimeters G54 ; select the G54 workspace (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 ; move Z up to 10mm below the home position (the -10mm can be set in the post options) G0 X679.003 Y24.365 ; rapid move to the cut start position S12000 M3 ; start the spindle at 12000rpm G4 P1.8 ; delay to allow spindle to speed up G0 X679.003 Y24.365 Z15 F1505 ; move Z to 15mm above the workpiece zero G1 Z-0.3 ; move at cut feedrate to -0.3mm below the workpiece zero Z-1.665 ; move at cut feedrate to -1.665mm below the workpiece zero ....... G0 Z15 ; move to 15mm above workpiece zero (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 ; move Z to 10mm below home M5 ; turn spindle off G0 X-10 Y-10 ; go to 10mm lft and 10mm below the workpiece X0 Y0 M30 ; end of program The boldface ones are of particular interest. my question is: how much space is there between the top of the work and Z home? if that is less than 15mm then you need to adjust your heights in Fusion360 to allow for both the retract AND not hitting the switch. Here is how Z-limits on job start, post problem?
I was referring to the line at the beginning of your g-code immediately after the G4 line. See @David the swarfer's explanation above. Alex.
ohh ok thanks for your help, really appreciate i have more than 15mm, maybe 80 if not more, if you look at my alarm screenshot , the Z is 68mm over the Z 0 and this because i set the 0 in air over the stock i dont think its the issue, i tried with 10 and 5mm total (in fusion) and same issue
1) Home the machine 2) hover the mouse over each of the DROs and note down the Mpos values shown (note just after homing. Don't change anything else. No jogging, nothing) 3) post these. Want to make sure your Home is correct (all negative space, Z should be 0-homingpulloff= - 10 for example)
Now execute G53 G0 Z-10 and your Z should move down from -2.5 to -10 (7.5mm of downward movement). Confirm by observation and rechecking MPos afterwards. Take the gcode line by line... Serial console tab has a textbox where you can send single commands. If it does, the G53 is working as it should. If it doesn't, feedback shown position data again, and description or video of what it does
Ps. Hitting the switch, and the Soft Limits error are contradictory (read error in screenshot). It would error for Hard Limit if switch was hit... Soft Limits arent beginner friendly turn it off... But the rest we trust your observation that it did hit the switch... Contradictary error message in hand, do you stand by it, or could it have missed the switch and instead just had the soft limit alarm all along?
i think you found the issue i will disable the soft limit for sure but why i think you and Alex Chamber are right i Alex told me about Z travels, i simply change max Z travel from 90 to 130 and work like charm now maybe related to this soft limit? why i was thinking it was limit switch (proximity switch, not mechanical) its because the light on it light up anyway seem to work flawlessly now Thanks to both of you for your help
Yes Max Travel is used for the Soft Limits calc. In Z thats a moving target (endmill lengths differ) so not really useful, might as well as it to 200mm (or Disable soft limits)
