Working on getting my machine set up and running and seem to be running into a problem in the beginning of every job. I’m using JS CNC with fusion 360 and the open builds grbl post processor. I have a 1000x1000 v-slot type machine with an xpro v5 and a huanyang spindle. I have my hope set 2.5mm off each home switch and set my work zero on the front, top, left corner of my workpiece which is pretty standard. The problem is evey time I run a job it will start up fine but then raise up in Z until hitting the limit switch, alarm, and stop. I’ve been able to mess with some of the initial lines in the code to get it to run after a lot of trial and error (G53 z-10) I think is what finally got it to work. But I want to understand exactly why this is happening and what I should be doing differently. Gcode and sample nc file here, also some screenshots I get when posting and settings from the post. ALARM:1 (Hard limit) [MSG:Reset to continue] client> ok Grbl 1.3a ['$' for help] [MSG:Check limits] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok ALARM:1 (Hard limit) [MSG:Reset to continue] client> ok Grbl 1.3a ['$' for help] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok feeder> G0 X0 Y0 Z0 ok feeder> G91 feeder> G0 Z-5 feeder> G90 ok ok ok feeder> G10 L20 P1 X0 Y0 Z0 ok ALARM:1 (Hard limit) [MSG:Reset to continue] client> ok Grbl 1.3a ['$' for help] [MSG:Check limits] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok feeder> G91 ok feeder> G0 Z-5 feeder> G90 ok ok Guru Meditation Error: Core 1 panic'ed (Coprocessor exception) Core 1 register dump: PC : 0x400df3c9 PS : 0x00060431 A0 : 0x800defcb A1 : 0x3ffbe800 A2 : 0x3ffd8530 A3 : 0x00000001 A4 : 0x000000ff A5 : 0x00000000 A6 : 0x00000001 A7 : 0x3ffc7194 A8 : 0x00000001 A9 : 0x3ffbe8c0 A10 : 0x000000ff A11 : 0x00000000 A12 : 0x3ffd8b7c A13 : 0x00000000 A14 : 0x00000000 A15 : 0x00000000 SAR : 0x0000000b EXCCAUSE: 0x00000004 EXCVADDR: 0x00000000 LBEG : 0x4000c349 LEND : 0x4000c36b LCOUNT : 0x00000000 Core 1 was running in ISR context: EPC1 : 0x400df3c9 EPC2 : 0x00000000 EPC3 : 0x00000000 EPC4 : 0x4008866c Backtrace: 0x400df3c9:0x3ffbe800 0x400defc8:0x3ffbe8f0 0x400d54fc:0x3ffbe920 0x40081f7b:0x3ffbe940 0x40082405:0x3ffbe960 0x40085e35:0x3ffbe980 0x4000bfed:0x3ffd41e0 0x40091479:0x3ffd41f0 0x4008fcf1:0x3ffd4210 0x40189346:0x3ffd4250 0x4017737c:0x3ffd4270 0x400ef7ae:0x3ffd42a0 0x400f842e:0x3ffd42e0 0x400eb2d8:0x3ffd4300 0x400eafa0:0x3ffd4320 0x400daafc:0x3ffd4340 0x4009030d:0x3ffd4360 Rebooting... ets Jun 8 2016 00:22:57 rst:0xc (SW_CPU_RESET),boot:0x17 (SPI_FAST_FLASH_BOOT) configsip: 0, SPIWP:0xee clk_drv:0x00,q_drv:0x00,d_drv:0x00,cs0_drv:0x00,hd_drv:0x00,wp_drv:0x00 modeIO, clock div:1 load:0x3fff0018,len:4 load:0x3fff001c,len:1216 ho 0 tail 12 room 4 load:0x40078000,len:9720 ho 0 tail 12 room 4 load:0x40080400,len:6352 entry 0x400806b8 [MSG:Grbl_ESP32 Ver 1.3a Date 20201212] [MSG:Compiled with ESP32 SDK:v3.2.3-14-gd3e562907] [MSG:Using machine:CNC_xPRO_V5_XYYZ_RS485_NC] [MSG:Axis count 3] [MSG:RMT Steps] Guru Meditation Error: Core 1 panic'ed (LoadProhibited). Exception was unhandled. Core 1 register dump: PC : 0x400d5a4c PS : 0x00060031 A0 : 0x800820e3 A1 : 0x3ffbe930 A2 : 0x00000000 A3 : 0x00000000 A4 : 0x3ffc5c30 A5 : 0x00000000 A6 : 0x00000000 A7 : 0x00000003 A8 : 0x3ffd6dd8 A9 : 0x0000000c A10 : 0x00000000 A11 : 0x3ffd6dd8 A12 : 0x80093262 A13 : 0x3ffd3020 A14 : 0x00000001 A15 : 0x3ffd6dd8 SAR : 0x00000000 EXCCAUSE: 0x0000001c EXCVADDR: 0x00000000 LBEG : 0x400014fd LEND : 0x4000150d LCOUNT : 0xfffffffb Core 1 was running in ISR context: EPC1 : 0x400d5a4c EPC2 : 0x00000000 EPC3 : 0x00000000 EPC4 : 0x4008866c Backtrace: 0x400d5a4c:0x3ffbe930 0x400820e0:0x3ffbe950 0x40085e35:0x3ffbe980 0x4000bfed:0x3ffd3090 0x40091479:0x3ffd30a0 0x400ffd4a:0x3ffd30c0 0x4018e97a:0x3ffd3100 0x40082045:0x3ffd3130 0x400dec7f:0x3ffd3170 0x400d465e:0x3ffd3190 0x400d2d6f:0x3ffd31b0 0x400fb9ef:0x3ffd31d0 0x4009030d:0x3ffd31f0 Rebooting... ets Jun 8 2016 00:22:57 rst:0xc (SW_CPU_RESET),boot:0x17 (SPI_FAST_FLASH_BOOT) configsip: 0, SPIWP:0xee clk_drv:0x00,q_drv:0x00,d_drv:0x00,cs0_drv:0x00,hd_drv:0x00,wp_drv:0x00 modeIO, clock div:1 load:0x3fff0018,len:4 load:0x3fff001c,len:1216 ho 0 tail 12 room 4 load:0x40078000,len:9720 ho 0 tail 12 room 4 load:0x40080400,len:6352 entry 0x400806b8 [MSG:Grbl_ESP32 Ver 1.3a Date 20201212] [MSG:Compiled with ESP32 SDK:v3.2.3-14-gd3e562907] [MSG:Using machine:CNC_xPRO_V5_XYYZ_RS485_NC] [MSG:Axis count 3] [MSG:RMT Steps] [MSG:Init Motors] [MSG:TMCStepper Library Ver. 0x000701] [MSG:X Axis Trinamic TMC5160 Step:GPIO(12) Dir:GPIO(14) CS:GPIO(17) Disable:None Index:1 R:0.050 Limits(-790.000,0.000)] [MSG:X Axis Trinamic driver test passed] [MSG:Y Axis Trinamic TMC5160 Step:GPIO(27) Dir:GPIO(26) CS:GPIO(17) Disable:None Index:2 R:0.050 Limits(-740.000,0.000)] [MSG:Y Axis Trinamic driver test passed] [MSG:Y2 Axis Trinamic TMC5160 Step:GPIO(33) Dir:GPIO(32) CS:GPIO(17) Disable:None Index:3 R:0.050 Limits(-740.000,0.000)] [MSG:Y2 Axis Trinamic driver test passed] [MSG:Z Axis Trinamic TMC5160 Step:GPIO(15) Dir:GPIO(2) CS:GPIO(17) Disable:None Index:4 R:0.050 Limits(-73.000,0.000)] [MSG:Z Axis Trinamic driver test passed] [MSG:Initializing RS485 VFD spindle] [MSG:Undefined VFD_RS485_RTS_PIN] [MSG:VFD RS485 Tx:GPIO(4) Rx:GPIO(25) RTS:GPIO(0)] [MSG:Local access point CNC_xPRO_V5 started, 192.168.0.1] [MSG:Captive Portal Started] [MSG:HTTP Started] [MSG:TELNET Started 23] [MSG:Flood coolant on pin GPIO(21)] [MSG:Mist coolant on pin GPIO(21)] [MSG:X Axis limit switch on pin GPIO(35)] [MSG:Y Axis limit switch on pin GPIO(34)] [MSG:Z Axis limit switch on pin GPIO(39)] [MSGrobe on pin GPIO(22)] Grbl 1.3a ['$' for help] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok feeder> G91 feeder> G0 Z-5 feeder> G90 ok ok ok feeder> G91 ok feeder> G0 Z-5 feeder> G90 ok ok feeder> G10 L20 P1 X0 Y0 Z0 ok ALARM:1 (Hard limit) [MSG:Reset to continue] client> ok Grbl 1.3a ['$' for help] [MSG:Check limits] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok ALARM:1 (Hard limit) [MSG:Reset to continue] client> $X client> ok Grbl 1.3a ['$' for help] [MSG:'$H'|'$X' to unlock] client> $X [MSG:Caution: Unlocked] ok feeder> G91 feeder> G0 Z-5 feeder> G90 ok ok ok feeder> G0 X0 Y0 Z0 ok [MSG:Spindle RS485 Unresponsive 8] client> ! feeder> M5 client> ok Grbl 1.3a ['$' for help] [MSG:Spindle RS485 Unresponsive 8] > $$ $0=4 (Step pulse time, microseconds) $1=255 (Step idle delay, milliseconds) $2=0 (Step pulse invert, mask) $3=2 (Step direction invert, mask) $4=1 (Invert step enable pin, boolean) $5=0 (Invert limit pins, boolean) $6=1 (Invert probe pin, boolean) $10=1 (Status report options, mask) $11=0.010 (Junction deviation, millimeters) $12=0.002 (Arc tolerance, millimeters) $13=0 (Report in inches, boolean) $20=0 (Soft limits enable, boolean) $21=1 (Hard limits enable, boolean) $22=1 (Homing cycle enable, boolean) $23=0 (Homing direction invert, mask) $24=200.000 (Homing locate feed rate, mm/min) $25=2000.000 (Homing search seek rate, mm/min) $26=250.000 (Homing switch debounce delay, milliseconds) $27=2.500 (Homing switch pull-off distance, millimeters) $30=12000.000 (Maximum spindle speed, RPM) $31=8000.000 (Minimum spindle speed, RPM) $32=0 (Laser-mode enable, boolean) $N1= $N0= $100=400.000 (X-axis travel resolution, step/mm) $101=400.000 (Y-axis travel resolution, step/mm) $102=400.000 (Z-axis travel resolution, step/mm) $103=200.000 $104=100.000 $105=100.000 $110=3000.000 (X-axis maximum rate, mm/min) $111=3000.000 (Y-axis maximum rate, mm/min) $112=3000.000 (Z-axis maximum rate, mm/min) $113=1000.000 $114=1000.000 $115=1000.000 $120=300.000 (X-axis acceleration, mm/sec^2) $121=300.000 (Y-axis acceleration, mm/sec^2) $122=300.000 (Z-axis acceleration, mm/sec^2) $123=200.000 $124=200.000 $125=200.000 $130=790.000 (X-axis maximum travel, millimeters) $131=740.000 (Y-axis maximum travel, millimeters) $132=73.000 (Z-axis maximum travel, millimeters) $133=300.000 $134=300.000 $135=300.000
G53 Z-10 is a clearance move. It will move to 10mm below your z limit switch. Then move to the first position. By the looks of the log it doesnt look like you are re-homing your machine after the reset. If you've correctly homed your machine, then set your work zeros, it should work. The message you're getting from Fusion is just a warning that you havent selected a WCS in your setup so its going to default to G54. If you want to avoid that message in the future, go into any setup, set WCS to 1, right click and select save as default. Then any new setup will automatically be set to 1 which is G54.
The post processor options allow you to set the Z clearance, which it will then use for the G53 safety move. If you are getting a G53 G0 Z0 move (will always alarm) then it means YOU changed the default value, so you should know where to change it back (-: The G53 safety moves rely on proper homing to function correctly. Please read this Home, Fusion360 and G53 Z moves (there has to be a clearance value because GRBL, the software in the controller, requires it. Moving to the axis 0 will always trigger the limit switch and cause an alarm).
maybe I have my order of operations wrong, I powerful the machine, send it home, load my gcode, set my work offsets to 0,0,0 at the front left too point of my stock then run it. should I home it again in there somewhere? Alternatively, if I set WCS To 1 how would it behave differently? david just seeing your reply and reading on it now.
I’m going to read the link you sent but one thing to add is that I haven’t edited this code at all this was a direct fresh dump from fusion.
no. you do need to rehome after any errors or alarms, USB reconnect, or power cycle. It will use WCS G54 (the default) and will not warn you about it not being set. The critical thing is to set the Z home offset in Fusion360's post options to -something, where the something is enough to avoid hitting the limit switch. if 1mm is enough, then use -1, if you need more, then use that value. I am not at my Fusion computer now otherwise I would send a screenshot
to clarify the .nc file I attached is a direct dump from fusion, the stuff I pasted into my post was edited but pulled from my console after a run. So to me it sounds like my post is incorrectly adding a positive z offset value which is causing me to limit out? Or maybe there is a setting in there somewhere I’m missing.
ok, so the G53 G0 Z-10 is hitting the limit switch at the top of Z travel? lets just make sure we have the basics.... Z positive tool travel is 'away from the work' negative travel is 'toward the work' Z home is at the positive end, safely UP and away from the work thus if the top of the work is set as WCS z=0 all retract, non cutting moves will be at positive Z levels and all cutting will be at negative Z levels. This is indeed the case in your file, the first move of the facing operation is to plunge down to about -7mm. your settings indicate Code: $27=2.500 (Homing switch pull-off distance, millimeters) and you said the 2.5mm does not affect where home is, it is a pulloff distance to clear the switch. GRBL cannot handle it if an axis goes to 0 and hits a switch, that is a hard limit error. This allow one to have a switch at both ends of travel to stop the machine crashing into itself. If 2.5mm is a reliable pulloff, you can use that in the post settings so your code gets G53 G0 Z-2.5 to reliably raise Z to safe height before the first positioning move. however, there is something else set incorrectly if G53 G0 Z-10 actually hits the limit switch.
oh! you edited your post! please use the unaltered OB post and lets see what the machine does. once that is all correct you can alter the post if you need to , but NOT to fix machine setup issues, please (-:
Apologies, the .gcode file I posted I edited manually. I have not edited the post. Was still a bit foggy from waking up and I'm trying my best to keep the terminology straight. So I have used the fusion 360 grbl post as well as the OB post, both seem to result in the same z limit issue right at the beginning of the job. I have my home set properly (as far as I know) my WCS zero is somewhere near the middle of the workspace at the corner of my stock. I pulled this from the gcode I posted at the top of this thread: G90 G94 G17 G21 ... G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 Couple questions: G54 tells the machine to home? G53 G0 Z-10 tells it to go to z-10 or to raise -10mm regardless of where it is at when it starts?
Maybe I just need to figure out why the G0 is stuck in there after G53, because if I'm understanding everything right G53 Z-10 shouldn't cause any problems.
G53 (move in machine coordinates) G0 (its a rapid move) Z (in the Z axis) -10 (to -10mm below the Z axis limit switch because its in Machine coordinates, and run it at Rapids speed as its a G0 move) The post is correct - law of the masses - it works for everyone else remember The Grbl post in Fusion doesn't use G53 it uses G28 and its a lot more confusing. Use ours - it only needs you machine to be set up correctly and for you to remember to home (and not accidentally enter positive values in Start/End of Job position field - the tooltip tells you it has to be negative) - nothing else
G54 doesn't tell the machine to home - it tells grbl which (the first one) of the 6 available WORKPLACE coordinates systems you are going to use. Alex.
The Grbl Wiki is a must-read: Home · gnea/grbl Wiki Homing command is discussed here: Grbl v1.1 Commands · gnea/grbl Wiki
The posts do not have an issue, your machine, or how you are setting it up, is the issue. In Fusion you must set the origin to the top of the stock. Then on the machine you set Z=0 with the tip of the tool on the top of the stock. no. G54 to G59 are Work Coordinate Systems. this is a modal setting, like many others, once set it stays set until changed. You do really need to read all of the GRBL wiki Home · gnea/grbl Wiki and follow that link in the Gcode and read all about it, homing and coordinate systems are not something you can gloss over, you really do need to know how they work. [/quote] G53 is the Machine Coordinate System. The homing cycle sets 0,0,0 for this, and all other coordinates are relative to this. G53 is not modal, you have to use it on every line that needs it. What the line is saying is 'use Machine Coordinates and Rapid (G0) to Z-10. -10 relative to machine 0! so top of Z travel, less 10mm G0 is rapid, ie as fast as possible, NOT used for cutting G1 is 'cut at given feedrate F in a straight line' G2 and G3 are arcs, also for cutting. going back to your first post Code: feeder> G91 feeder> G0 Z-5 feeder> G90 ok ok ok feeder> G10 L20 P1 X0 Y0 Z0 ok ALARM:1 (Hard limit) That looks like a Z jog down followed by a 'setzero' followed immediately by a hard limit error, when the machine was not moving. Is that what happened? This would indicates an EMI issue. docs:blackbox:faq-emi [OpenBuilds Documentation]
I'm now sure that I am the issue, I was initially unsure whether or not the posts needed to be adjusted somehow to accommodate my machine. I now realize that is not the case. The problem is, I really think I am doing everything correctly but for some reason my gcode is always telling my machine to go up so far it hits the limits. I'm just trying to figure out what I'm doing wrong in my setup that's causing that. I am homed properly, I set my WCS properly, but i'm not confident in my gcode. Something in these lines is causing me to limit our, maybe it's the Z15? This is using WCS as the reference now i'm assuming and if my material is so thick i don't have 15mm between the top of my stock/work zero and the z-limit, I will hit a hard stop. Maybe this is a function of the heights settings in fusion? G90 G94 G17 G21 (Operation 1 of 3 : Face1) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 G0 X201.95 Y1.515 S12000 M3 G4 P1.8 G0 X201.95 Y1.515 Z15 F900 Z5 I'm confident I understand homing, but not too good at reading the code yet, apologies for any incorrect responses/assumptions I really appreciate everyone's help.
Having read through all of this and the associated links, none of them solved my issue. The issue was in the post-processor and can be found in the screenshot 1/2 down this thread… Solved: G53 Z0. when changing work offsets - Autodesk Community And I don’t want to just drop that on there. You can select G28, G53 or Clearance Height. 28 kept causing issues (and seemed to have changed to the default all on its own). 53 seemed to work once. On the next operation, it crashed Z. Then I regenerated with Clearance Height and it’s cruising along now. We’ll see if that holds through the next few ops. Mildly irritating b/c the first operation, from the day prior, ran flawlessly. Then the next operation caused me to have to chase this down. Nothing in the setup had changed. I re-homed a dozen times and telling the machine to go to WCS was right on the money. So it was a weird one.
Those options tell me you are not using the OpenBuilds postprocessor for Fusion360. Get it here docs:software:fusion360 [OpenBuilds Documentation] It always uses the machine coordinate system for Z safety moves. This relies on homing, as does G28 G53 is the machine coordinate system (MCS) G28 is an offset from the MCS - so for this to work sensibly, G53 has to be homed GRBL based controllers reset home when they are turned on, and when they get a serial connection , this means you need to rehome everytime the controller resets or the GUI disconnects and reconnects. grblHAL based controllers like the BlackBox X32 DO NOT do this reset. However, this does not mean that the home is stable through power cycles and reconnects, instead it is 'unknown'. Always rehome if in any doubt, and use that 'goto WCS' button to cross check where it thinks home is. Also, GRBL/grblHAL based controllers will trigger an alarm if they go to Z0, that will always trigger the switch. In the OB post, there is a hold off distance that defaults to -10mm, so the start and end code becomes G53 G0 Z-10 which raises the Z safely but avoids hitting the switch by 10mm (always negative, 0 is as high as Z can go). 10mm is too much for most switches, most will be missed by just 1mm, so you can set it to -1 and test and that will give you the most clearance, safely. Home, Fusion360 and G53 Z moves
