Hello, Under my basic assumption that my spindle does what it is told to do from gcode, and that the post processor files are machine specific I am asking my question here… I am using a new VFD water cooled spindle which has to spin up therefore needing a dwell command. I have inserted the dwell right after the M3 command but my spindle in pausing prior to spinning up. It is also spinning down during rapid moves and back up before plunge. Obviously this is all dangerous as it will damage my work and bits as the bit is reaching down before the spindle is at full speed. im using the OB mm Post processor Any ideas?
I'll assume you are referring to some Vectric flavor since you mentioned OB mm. If that's the case, you'll want to edit the processor here Change G4 Px to how long you want in seconds.
If the spindle is slowing down during a job we need to see your g-code to get an idea of what's happening. Upload a file here. Alex.
Yes the issue is based upon increasing G4. It simply pauses then spin up rather than starts spinning then pausing. g code is being posted in the below message.
Here is the PP g code… POST_NAME = "OpenBuilds GRBL (mm) (*.GCODE)" FILE_EXTENSION = "GCODE" UNITS = "MM" DIRECT_OUTPUT = "VTransfer" LASER_SUPPORT = "YES" MIN_ARC_RADIUS = 1 +------------------------------------------------ + 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|1.3] VAR Y_POSITION = [Y|C|Y|1.3] VAR Z_POSITION = [Z|C|Z|1.3] VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.3] VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.3] VAR X_HOME_POSITION = [XH|A|X|1.3] VAR Y_HOME_POSITION = [YH|A|Y|1.3] VAR Z_HOME_POSITION = [ZH|A|Z|1.3] +================================================ + + Block definitions for toolpath output + +================================================ +--------------------------------------------------- + Commands output at the start of the file +--------------------------------------------------- begin HEADER "T1" "G17" "G21" "G90" "G0[ZH]" "G0[XH][YH]" +--------------------------------------------------- + Command output after the header to switch spindle on +--------------------------------------------------- begin SPINDLE_ON "M3" "G4 P1.5" +--------------------------------------------------- + Commands output for rapid moves +--------------------------------------------------- begin RAPID_MOVE "G0[X][Y][Z]" +--------------------------------------------------- + Commands output for the plunge move +--------------------------------------------------- begin PLUNGE_MOVE "G1[X][Y][Z][F]" +--------------------------------------------------- + Commands output for the first feed rate move +--------------------------------------------------- begin FIRST_FEED_MOVE "G1[X][Y][Z][P][F]" +--------------------------------------------------- + Commands output for feed rate moves +--------------------------------------------------- begin FEED_MOVE "G1[X][Y][Z][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]" "G4 P5" +--------------------------------------------------- + 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"
I did change to 5. But when I run the session my head moves up and pauses for the duration but the spindle does not spin up. It still only starts spinning up after the dwell period despite the M3 being before the G4.
In the pp you posted it says 1.5. The stock PP has 1.8. So just want to confirm that you changed it to P5 and not P1.5. Can you also confirm that your M3 command has a S value with it?
That’s probable just me playing around with it, but it was at 5 and not 1.5. I even had it at 20 just to see the change. Regarding the M3, it is my assumption that the parameters after M3 in the PP master will be populated with the value fed to it from Vectric tool setup.
Spindle speed is a variable that the post processor will assign to the S command after the M3. If there is no "S" the post processor can't assign a value to it. Alex.
Yep. But since you didnt post your gcode, we can only assume that its correct. Just trying to rule out obvious issues.
Sorry, I thought that you meant the PP Code, here is the Gcode for one of the runs... T1 G17 G21 G90 G0Z20.320 G0X0.000Y0.000 M3S12000 G04P5 G0X0.000Y191.675Z5.080 G1Z0.000F2032.0 G1X-5.464Y191.597Z-3.000 G1X-10.923Y191.364Z-6.000 G1X-5.464Y191.597Z-9.000 G1X0.000Y191.675Z-12.000 G3X-191.675Y0.000I0.000J-191.675F2540.0 G3X0.000Y-191.675I191.675J0.000 G3X191.675Y0.000I0.000J191.675 G3X0.000Y191.675I-191.675J0.000 G1X0.000Y196.755 G3X-196.755Y0.000I0.000J-196.755 G3X0.000Y-196.755I196.755J0.000 G3X196.755Y0.000I0.000J196.755 G3X0.000Y196.755I-196.755J0.000 G0Z5.080 G0X0.000Y202.245 G1Z0.000F2032.0 G1X5.461Y202.171Z-3.000 G1X10.917Y201.950Z-6.000 G1X5.461Y202.171Z-9.000 G1X0.000Y202.245Z-12.000 G2X202.245Y0.000I0.000J-202.245F2540.0 G2X0.000Y-202.245I-202.245J0.000 G2X-202.245Y0.000I0.000J202.245 G2X0.000Y202.245I202.245J0.000 G1X0.000Y207.325 G2X207.325Y0.000I0.000J-207.325 G2X0.000Y-207.325I-207.325J0.000 G2X-207.325Y0.000I0.000J207.325 G2X0.000Y207.325I207.325J0.000 G0Z5.080 G0X0.000Y191.675 G1Z-12.000F2032.0 G1X-5.464Y191.597Z-15.000 G1X-10.923Y191.364Z-18.000 G1X-5.464Y191.597Z-21.000 G1X0.000Y191.675Z-24.000 G3X-191.675Y0.000I0.000J-191.675F2540.0 G3X0.000Y-191.675I191.675J0.000 G3X191.675Y0.000I0.000J191.675 G3X0.000Y191.675I-191.675J0.000 G1X0.000Y196.755 G3X-196.755Y0.000I0.000J-196.755 G3X0.000Y-196.755I196.755J0.000 G3X196.755Y0.000I0.000J196.755 G3X0.000Y196.755I-196.755J0.000 G0Z5.080 G0X0.000Y202.245 G1Z-12.000F2032.0 G1X5.461Y202.171Z-15.000 G1X10.917Y201.950Z-18.000 G1X5.461Y202.171Z-21.000 G1X0.000Y202.245Z-24.000 G2X202.245Y0.000I0.000J-202.245F2540.0 G2X0.000Y-202.245I-202.245J0.000 G2X-202.245Y0.000I0.000J202.245 G2X0.000Y202.245I202.245J0.000 G1X0.000Y207.325 G2X207.325Y0.000I0.000J-207.325 G2X0.000Y-207.325I-207.325J0.000 G2X-207.325Y0.000I0.000J207.325 G2X0.000Y207.325I207.325J0.000 G0Z5.080 M5 G0Z20.320 G0X0.000Y0.000 M2
Problem solved. It was that $32 was set to 1 enabling Laser which explains why the spindle was also stopping when doing a fast Z travel. Thanks for the input.
turn off laser mode! set laser mode to disabled click the save button at top left (it will change color when soemthing needs to be saved reset the BB if prompted
Thank you for the info. I had already done that and it solved the problem. I did it from the OB c controls app rather than from G-code prompt. See above.
