Is there an easier way to change GRBL settings? For example I carve out my project with the CNC and have $30 at 24000, now I want to Laser part of the project with another design but I need to manually go in a change $30 to 255 for the Laser. Then change it back to 24000 for the Spindle to cut the project out. I guess Im just looking for a short cut to change this setting if there is even an option to do that.
Or even better - just configure your laser CAM workflow to output 0-24000 as well (instead of 0-255) Then the Grbl Settings stays consistent and both CAM workflow outputs the right values If its Lightburn its called "S-Value Max", in the Device Settings - change that to 24000 _______________________________________________ If you are using OpenBuilds CAM its in the Settings tab > Settings button window
Thanks for the reply Peter. I guess i should have clarified that Im using the Vectric Laser Module with Aspire. Don't get me wrong I LOVE Lightburn and I use it all the time on my CO2 machine, but Lightburn will not help me in this situation on the CNC machine because of the job alignment. Unless you have a trick for that too????? For my workflow Im using the OpenBuilds Control and importing the gcode. Im not using the Openbuilds CAM software you are referring to but I know what it is. If I leave $30 at 24000 the Laser will output but it will not burn.
FYI the next main commit of grblHAL will allow binding of two spindles to the PWM output, each with its own settings (except PWM frequency). Switching between them can be done with an M-command or via tool number depending on how it is configured. If final testing goes well I expect this to become available mid december.
This is the Post im using, coupld you please tell me where to insert the Output 0-24000? +================================================ + + Grbl - Vectric machine output configuration file + +================================================ + + History + + Who When What + ======== ========== =========================== + EdwardP 11/02/2015 Written from Grbl_mm.pp but + set G20 + EdwardP 11/02/2015 Commented out arcs as these + slow GRBL performance appear + interpolated anyway. + EdwardP 18/06/2015 Explicitly set absolute mode (G90) + Mark 24/11/2015 Updated for interim 0.9 spec. + Renaming to be machine specific. + Removing M30 from Footer. + Edward 21/05/2020 Consolidated all changes from mm + Edward 02/06/2020 Consolidated all changes from mm + GrzegorzK 13/07/2020 Added X Y missing from the plunge record. + Jay 7/16/2020 Removed Z moves in this version V4 +================================================ POST_NAME = "J Tech Grbl Laser (inch) (*.gcode)" FILE_EXTENSION = "gcode" UNITS = "INCHES" DIRECT_OUTPUT = "VTransfer" LASER_SUPPORT = "YES" +------------------------------------------------ + Line terminating characters +------------------------------------------------ LINE_ENDING = "[13][10]" +------------------------------------------------ + Block numbering +------------------------------------------------ LINE_NUMBER_START = 0 LINE_NUMBER_INCREMENT = 10 LINE_NUMBER_MAXIMUM = 999999 +================================================ + + Formatting for variables + +================================================ VAR LINE_NUMBER = [N|A|N|1.0] VAR POWER = [P|C|S|1.0|10.0] VAR SPINDLE_SPEED = [S|A|S|1.0] VAR FEED_RATE = [F|C|F|1.1] VAR X_POSITION = [X|C|X|1.4] VAR Y_POSITION = [Y|C|Y|1.4] VAR Z_POSITION = [Z|C|Z|1.4] VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.4] VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.4] VAR X_HOME_POSITION = [XH|A|X|1.4] VAR Y_HOME_POSITION = [YH|A|Y|1.4] VAR Z_HOME_POSITION = [ZH|A|Z|1.4] +================================================ + + Block definitions for toolpath output + +================================================ +--------------------------------------------------- + Commands output at the start of the file +--------------------------------------------------- begin HEADER "T1" "G17" "G20" "G90" +"G0[ZH]" "G0[XH][YH]" +--------------------------------------------------- + Command output after the header to switch spindle on +--------------------------------------------------- begin SPINDLE_ON "M3" +--------------------------------------------------- + Commands output for rapid moves +--------------------------------------------------- begin RAPID_MOVE "G0[X][Y]" +--------------------------------------------------- + Commands output for the plunge move +--------------------------------------------------- begin PLUNGE_MOVE "G1[X][Y][F]" +--------------------------------------------------- + Commands output for the first feed rate move +--------------------------------------------------- begin FIRST_FEED_MOVE "G1[X][Y][P][F]" +--------------------------------------------------- + Commands output for feed rate moves +--------------------------------------------------- begin FEED_MOVE "G1[X][Y][P]" +--------------------------------------------------- + Commands output for the first clockwise arc move +--------------------------------------------------- begin FIRST_CW_ARC_MOVE "G2[X][Y][J][F][P]" +--------------------------------------------------- + Commands output for clockwise arc move +--------------------------------------------------- begin CW_ARC_MOVE "G2[X][Y][J]" +--------------------------------------------------- + Commands output for the first counterclockwise arc move +--------------------------------------------------- begin FIRST_CCW_ARC_MOVE "G3[X][Y][J][F][P]" +--------------------------------------------------- + Commands output for counterclockwise arc move +--------------------------------------------------- begin CCW_ARC_MOVE "G3[X][Y][J]" +--------------------------------------------------- + Commands output when the jet is turned on +--------------------------------------------------- begin JET_TOOL_ON "M4[P]" +--------------------------------------------------- + Commands output when the jet is turned off +--------------------------------------------------- begin JET_TOOL_OFF "M5" +--------------------------------------------------- + Commands output when the jet power is changed +--------------------------------------------------- begin JET_TOOL_POWER +"[P]" +--------------------------------------------------- + Commands output at the end of the file +--------------------------------------------------- begin FOOTER "M5" +"G0[ZH]" "G0[XH][YH]" "M2"
That last 10.0 is a multiplier - the default (0-100%) x10.0 which then gives you S0-S1000 So to get 24k you can try 100% x 240 = S24000 Explained in the POWER VARIABLE section of the docs Adapting a post-processor for Lasers
As an aside, not tested myself, but theoretically should work: You can also try to add the $32=1 into the HEADER of your Laser post, and $32=0 into your Spindle POST so you have that added for you as well. Should force the Laser Mode on/off for you and no need to remember to change that either
Someday when you want to play with this bit, do ping in with more info Trick should be a) use same origin - for example front left corner - for all CAM workflows (so you only need to zero XY once) and b) use macros to change between the offsets for center of laser and center of spindle - so they line up correctly. I like using separate coordinate systems for the two jobs.
When I said I tested it what I meant was I tested the laser and it worked perfectly. I have the laser connected to the PWM output and the VFD to the 0-10v output but something isnt right. The spindle worked properly before I had the laser plugged in the PWM. When I ran a job on the CNC yesterday the spindle powered up to 24K when it should have been at 18K. I used the correct post processor for the CNC and I disabled $32. I think Im missing something.
Double check the S-values in your GCODE - did it send S18000 or S24000 Double check that you did calibrate the 0-10v: docs:blackbox-x32:connect-vfd [OpenBuilds Documentation] Double check your Grbl Settings
The G-Code is (VECTRIC POST REVISION) (56212E927830674764AC4F06308F889F) T1 G17 G20 G90 G0Z0.8000 G0X0.0000Y0.0000 S18000M3 The only thing changed on the GRBL is the $32 to disable I calibrated the 0-10v to exactly 10volts
Well Peter that did not work either.. Im using the Openbuilds Post now and changed the $30 to 22000 and its not scaling down. Ive changes the post as well and made the S Value 18000 and the VFD still runs at 24000. The voltage at the 0-10 is less than 5 volts. I can manually change the tool output on the control software. When i first started up this X32 and ran the spindle I got 10 volts now Im only getting less than 5 volts. I started a job making a cribbage board and while it was peck drilling the pin holes I noticed that the holes were not round but oval. So i checked the Axis steps and Im dead on with all 3 Axis. I then ran a test. It was a 2x2 inch square and Im measuring 1.98 in the X and 1.99 in the Y. All that might be the tool im using so I'll run that again with another tool. I didnt have these issues with the X-Ctontroller but I also didnt have the Laser functionality with it either.
Post a Grbl Settings backup for review Calibration just corrects for manufacturing tolerances, it needs a solid mechanical setup underneath. Oval cuts are often mechanical (slipping shaft couplers on leadscrew machines or loose pulley or damaged belt on belt driven machines)
I think I was getting some backlash on the X. Here is my GRBL settings: $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=7 ; Invert limit pins, boolean/mask $6=1 ; Invert probe pin, boolean $7=0 ; Disable spindle with 0 speed, boolean $8=0 ; Ganged axes direction invert as bitfield $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=0 ; 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=500.0 ; Homing search seek rate, mm/min $26=250 ; Homing switch debounce delay, milliseconds $27=5.000 ; Homing switch pull-off distance, millimeters $28=0.100 ; G73 retract distance, in mm $29=0.0 ; Step pulse delay (ms) $30=18000.000 ; Maximum spindle speed, RPM $31=0.000 ; Minimum spindle speed, RPM $32=0 ; Laser-mode enable, boolean $33=400.0 ; 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=198.129 ; X-axis steps per millimeter $101=198.129 ; Y-axis steps per millimeter $102=200.101 ; Z-axis steps per millimeter $110=2500.000 ; X-axis maximum rate, mm/min $111=2500.000 ; Y-axis maximum rate, mm/min $112=1000.000 ; 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=787.000 ; X-axis maximum travel, millimeters $131=965.000 ; Y-axis maximum travel, millimeters $132=153.000 ; 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=100.0 ; Tool Change Probe Pull Off rate $370=0 ; Invert I/O Port Inputs (mask) $384=0 ; Disable G92 Persistence $I=custom
Mainly I'm saying avoid changing settings off guesswork without researching them. That one pops out as obviously changed from default. What else you changed, you'd know better. I am not in the office to lookup the default for you, but its not 400. I think its 5000 so try that. Especially comments like that sits in contrast to messed with settings, the implication being that somehow its an X32 problem (; Lets work the problem, without that sort of thing please
Apologies, I didn't mean to imply there's something wrong with the X32 I know I have some kind of setting wrong. I have another small CNC with the exact same spindle and the X32 and it works flawlessly and those are the settings I used. So I changed the $33 to 5000 and ran a test file. The spindle ramps up to 24000 when I have it set for 18000 at $30 and the g-code is M3S18000.
Disconnect spindle. Measure voltage output from Blackbox . Use CONTROL's tool menu. At 10% should be +-1v. At 20% +-2v etc up to 10v at 100% See if it does, if not, still Grbl Settings If the output is fine but the VFD acts funny, then its something in the VFD parameters
I reset the VFD and changed my GRBL settings to where they aught to be and Im all set now. It runs within parameters Thanks for your help and patience Peter. Much appreciated
