job stops after G96 D3500 S200 M3 without a comment

More
19 Aug 2023 15:45 #278474 by geostein8888
hello,
i have a self build lathe, where i want to start finally turning things. My first job was made with Fusion 360. When i start the job after referencing the maschine, it always stops after line N21 without any comment on screen or in the log.
My Spindle ist not set up in the ini file, while i want to make some dry runs before using it.

the gcod is:
does somebody has a idea what i'm doing wrong? (inifile follows after the gcode)
%
(CHESS_)
N10 G7
N11 G90 G18
N12 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.)
N13 G53 G0 X0.
N14 G53 G0 Z0.

(PROFIL-SCHRUPPEN1)
N15 T2 M6
N17 G90 G95 G18
N18 G54
N19 G97 S1592 M3
N20 G0 X40. Z7.
N21 G96 D3500 S200 M3
N22 G1 Z1.5 F0.5
N23 X18.
N24 Z-36.438
N25 G3 X20. Z-39.924 I-7.679 K-4.089
N26 G1 X22. Z-38.924
N27 Z1.5
N28 X16.
N29 Z-31.546
N30 G3 X16.853 Z-35.507 I-2.017 K-2.221
N31 X18. Z-36.438 I-7.105 K-5.02
N32 G1 X20. Z-35.438
N33 Z1.5
N34 X14.042
N35 Z-7.079
N36 X15.051 Z-8.466
N37 Z-13.522
N38 Z-13.524
N39 G3 X14.042 Z-15.354 I-3.799 K0.063
N40 G1 Z-30.952
N41 G3 X16. Z-31.546 I-1.038 K-2.815
N42 G1 X18. Z-30.546
N43 Z1.5
N44 X12.042
N45 Z-5.317
N46 G2 X12.861 Z-5.457 I1.723 K4.373
N47 G1 X14.042 Z-7.079
N48 X16.042 Z-6.079
N49 Z1.5
N50 X10.042
N51 Z-4.775
N52 G2 X12.042 Z-5.317 I2.723 K3.831
N53 G1 X14.042 Z-4.317
N54 Z1.5
N55 X8.042
N56 Z-3.813
N57 G2 X10.042 Z-4.775 I3.723 K2.868
N58 G1 X12.042 Z-3.775
N59 Z1.5
N60 X6.042
N61 Z0.1
N62 X6.324
N63 G2 X8.042 Z-3.813 I4.582 K-1.045
N64 G1 X10.042 Z-2.813
N65 Z1.5
N66 X4.042
N67 Z0.1
N68 X6.042
N69 X8.042 Z1.1
N70 Z1.5
N71 X2.042
N72 Z0.1
N73 X4.042
N74 X6.042 Z1.1
N75 Z1.5
N76 X0.821
N77 Z0.1
N78 X2.042
N79 X4.042 Z1.1
N80 Z1.5
N81 X-0.4
N82 Z0.1
N83 X0.821
N84 X2.821 Z1.1
N85 X16.051
N86 Z-15.354
N87 X15.042
N88 X14.042
N89 G3 X12.338 Z-16.372 I-3.295 K1.893
N90 G1 X12.042 Z-16.496
N91 Z-30.767
N92 G3 X14.042 Z-30.952 I-0.038 K-3.
N93 G1 X16.042 Z-29.952
N94 Z-16.496
N95 X13.042
N96 X12.042
N97 X10.042 Z-17.335
N98 Z-27.959
N99 X12.036 Z-28.955
N100 Z-30.767
N101 X12.042
N102 X14.042 Z-29.767
N103 Z-17.335
N104 X11.042
N105 X10.042
N106 X8.917 Z-17.807
N107 Z-27.396
N108 X10.042 Z-27.959
N109 X12.042 Z-26.959
N110 Z-17.807
N111 X9.917
N112 X8.917
N113 X7.793 Z-18.278
N114 Z-26.834
N115 X8.917 Z-27.396
N116 X10.917 Z-26.396
N117 X21.042
N118 Z-41.131
N119 X21.
N120 X20.
N121 G3 X18.447 Z-44.166 I-8.679 K0.603
N122 G1 Z-47.739
N123 X20. Z-49.872
N124 X22. Z-48.872
N125 Z-44.166
N126 X19.447
N127 X18.447
N128 G3 X16.852 Z-45.548 I-7.903 K3.639
N129 G1 X18.447 Z-47.739
N130 X20.447 Z-46.739
N131 X40.
N132 Z7.
N133 G97 S1592 M3

N134 M5
N135 G53 G0 X0.
N136 G53 G0 Z0.
N137 M30
%

Ini file
# Generated by stepconf 1.1 at Fri Aug 18 12:47:38 2023
# Änderungen an dieser Datei werden beim nächsten
# overwritten when you run stepconf again

[EMC]
MACHINE = lathe_ohne
DEBUG = 0
VERSION = 1.1

[DISPLAY]
DISPLAY = axis
EDITOR = gedit
POSITION_OFFSET = RELATIVE
POSITION_FEEDBACK = ACTUAL
ARCDIVISION = 64
GRIDS = 10mm 20mm 50mm 100mm 1in 2in 5in 10in
MAX_FEED_OVERRIDE = 1.2
MIN_SPINDLE_OVERRIDE = 0.5
MAX_SPINDLE_OVERRIDE = 1.2
DEFAULT_LINEAR_VELOCITY = 5.00
MIN_LINEAR_VELOCITY = 0
MAX_LINEAR_VELOCITY = 50.00
INTRO_GRAPHIC = linuxcnc.gif
INTRO_TIME = 5
PROGRAM_PREFIX = /home/georg/linuxcnc/nc_files
INCREMENTS = 5mm 1mm .5mm .1mm .05mm .01mm .005mm
PYVCP = custompanel.xml
LATHE = 1

[KINS]
JOINTS = 2
KINEMATICS = trivkins coordinates=XZ

[FILTER]
PROGRAM_EXTENSION = .png,.gif,.jpg Greyscale Depth Image
PROGRAM_EXTENSION = .py Python Script
PROGRAM_EXTENSION = .nc,.tap G-Code File
png = image-to-gcode
gif = image-to-gcode
jpg = image-to-gcode
py = python

[TASK]
TASK = milltask
CYCLE_TIME = 0.010

[RS274NGC]
PARAMETER_FILE = linuxcnc.var

[EMCMOT]
EMCMOT = motmod
COMM_TIMEOUT = 1.0
BASE_PERIOD = 100000
SERVO_PERIOD = 1000000

[HAL]
HALUI = halui
HALFILE = lathe_ohne.hal
HALFILE = custom.hal
POSTGUI_HALFILE = postgui_call_list.hal

[HALUI]
# HalUI-MDI-Befehle hier einfügen (max. 64)

[TRAJ]
COORDINATES =  X Z
LINEAR_UNITS = mm
ANGULAR_UNITS = degree
DEFAULT_LINEAR_VELOCITY = 5.00
MAX_LINEAR_VELOCITY = 50.00

[EMCIO]
EMCIO = io
CYCLE_TIME = 0.100
TOOL_TABLE = tool.tbl

[AXIS_X]
MAX_VELOCITY = 30.0
MAX_ACCELERATION = 900.0
MIN_LIMIT = -0.001
MAX_LIMIT = 200.0

[JOINT_0]
TYPE = LINEAR
HOME = 0.0
MIN_LIMIT = -0.001
MAX_LIMIT = 200.0
MAX_VELOCITY = 30.0
MAX_ACCELERATION = 900.0
STEPGEN_MAXACCEL = 1125.0
SCALE = 160.0
FERROR = 1
MIN_FERROR = .25
HOME_OFFSET = 150.000000
HOME_SEARCH_VEL = 10.000000
HOME_LATCH_VEL = 3.125000
HOME_SEQUENCE = 1

[AXIS_Z]
MAX_VELOCITY = 50.0
MAX_ACCELERATION = 1000.0
MIN_LIMIT = -200.0
MAX_LIMIT = 400.0

[JOINT_1]
TYPE = LINEAR
HOME = 0.0
MIN_LIMIT = -200.0
MAX_LIMIT = 400.0
MAX_VELOCITY = 50.0
MAX_ACCELERATION = 1000.0
STEPGEN_MAXACCEL = 1250.0
SCALE = 160.0
FERROR = 1
MIN_FERROR = .25
HOME_OFFSET = 0.000000
HOME_SEARCH_VEL = 15.000000
HOME_LATCH_VEL = 3.125000
HOME_SEQUENCE = 2

hal file:
# Generated by stepconf 1.1 at Fri Aug 18 12:47:38 2023
# Änderungen an dieser Datei werden beim nächsten
# overwritten when you run stepconf again
loadrt [KINS]KINEMATICS
loadrt [EMCMOT]EMCMOT base_period_nsec=[EMCMOT]BASE_PERIOD servo_period_nsec=[EMCMOT]SERVO_PERIOD num_joints=[KINS]JOINTS
loadrt hal_parport cfg="0 out"
setp parport.0.reset-time 5000
loadrt stepgen step_type=0,0

addf parport.0.read base-thread
addf stepgen.make-pulses base-thread
addf parport.0.write base-thread
addf parport.0.reset base-thread

addf stepgen.capture-position servo-thread
addf motion-command-handler servo-thread
addf motion-controller servo-thread
addf stepgen.update-freq servo-thread
net spindle-cmd-rpm     <= spindle.0.speed-out
net spindle-cmd-rpm-abs <= spindle.0.speed-out-abs
net spindle-cmd-rps     <= spindle.0.speed-out-rps
net spindle-cmd-rps-abs <= spindle.0.speed-out-rps-abs
net spindle-at-speed    => spindle.0.at-speed

setp parport.0.pin-02-out-invert 1
net xenable         => parport.0.pin-02-out
net xdir            => parport.0.pin-04-out
setp parport.0.pin-05-out-invert 1
net xstep           => parport.0.pin-05-out
setp parport.0.pin-05-out-reset 1
net zdir            => parport.0.pin-08-out
setp parport.0.pin-09-out-invert 1
net zstep           => parport.0.pin-09-out
setp parport.0.pin-09-out-reset 1
net all-limit       <= parport.0.pin-10-in-not
net home-z          <= parport.0.pin-11-in
net home-x          <= parport.0.pin-12-in

setp stepgen.0.position-scale [JOINT_0]SCALE
setp stepgen.0.steplen 1
setp stepgen.0.stepspace 0
setp stepgen.0.dirhold 35000
setp stepgen.0.dirsetup 35000
setp stepgen.0.maxaccel [JOINT_0]STEPGEN_MAXACCEL
net xpos-cmd joint.0.motor-pos-cmd => stepgen.0.position-cmd
net xpos-fb stepgen.0.position-fb => joint.0.motor-pos-fb
net xstep <= stepgen.0.step
net xdir <= stepgen.0.dir
net xenable joint.0.amp-enable-out => stepgen.0.enable
net home-x => joint.0.home-sw-in
net all-limit => joint.0.neg-lim-sw-in
net all-limit => joint.0.pos-lim-sw-in

setp stepgen.1.position-scale [JOINT_1]SCALE
setp stepgen.1.steplen 1
setp stepgen.1.stepspace 0
setp stepgen.1.dirhold 35000
setp stepgen.1.dirsetup 35000
setp stepgen.1.maxaccel [JOINT_1]STEPGEN_MAXACCEL
net zpos-cmd joint.1.motor-pos-cmd => stepgen.1.position-cmd
net zpos-fb stepgen.1.position-fb => joint.1.motor-pos-fb
net zstep <= stepgen.1.step
net zdir <= stepgen.1.dir
net zenable joint.1.amp-enable-out => stepgen.1.enable
net home-z => joint.1.home-sw-in
net all-limit => joint.1.neg-lim-sw-in
net all-limit => joint.1.pos-lim-sw-in

net estop-out <= iocontrol.0.user-enable-out
net estop-out => iocontrol.0.emc-enable-in

loadusr -W hal_manualtoolchange
net tool-change iocontrol.0.tool-change => hal_manualtoolchange.change
net tool-changed iocontrol.0.tool-changed <= hal_manualtoolchange.changed
net tool-number iocontrol.0.tool-prep-number => hal_manualtoolchange.number
net tool-prepare-loopback iocontrol.0.tool-prepare => iocontrol.0.tool-prepared

net spindle-at-speed => spindle.0.at-speed
sets spindle-at-speed true

thanks for all help
Georg

Please Log in or Create an account to join the conversation.

More
19 Aug 2023 16:59 #278477 by cmorley
G96 uses spindle RPM feedback to calculate the surface speed.
It's surely waiting for the feedback.
Try switching to G97 as a test

Please Log in or Create an account to join the conversation.

More
20 Aug 2023 05:23 #278521 by geostein8888
i cant switch this to g97, i get directly an error while loading the nc file. When i take the complete line N21 out, i have still the same result, the program stops at N22

Please Log in or Create an account to join the conversation.

More
20 Aug 2023 06:13 #278522 by Aciera

cant switch this to g97, i get directly an error while loading the nc file

What does the error message say?

Note that you can't use G95 without spindle feedback (eg encoder) so maybe try to change g95 to g94

Please Log in or Create an account to join the conversation.

More
20 Aug 2023 07:04 #278526 by cmorley
with HALmeter check if spindle.0.at-speed is true

I see you have the line
net spindle-at-speed => spindle.0.at-speed
twice - I wonder if a silent error is making it miss the last line that sets the signal true.

But yes g95 is not going to work properly without the spindle feedback for sure!

Please Log in or Create an account to join the conversation.

More
20 Aug 2023 15:49 #278552 by PCW
Actually I would say its all working as expected, since the RPM is 0, the feed rate is 0...

Please Log in or Create an account to join the conversation.

More
20 Aug 2023 16:40 #278555 by smc.collins
it's waiting for the spindle at speed command and yes, without encoder feedback, it will absolutely sit at feed of zero.

Please Log in or Create an account to join the conversation.

More
21 Aug 2023 07:57 #278591 by rodw

it's waiting for the spindle at speed command and yes, without encoder feedback, it will absolutely sit at feed of zero.

If you want it to move, use a time delay component fed from spindle.0.on for spindle.0.at-speed

Please Log in or Create an account to join the conversation.

More
21 Aug 2023 08:18 #278594 by geostein8888
Hello,
with all your help i got it to work.
i changed some parameters on the beginning and now the job runs through
(PROFIL-SCHRUPPEN1)
N15 T2 M6
N17 G90 G94 G18
N18 G54
N19 G97 S1500 M3
N20 G0 X40. Z7.
N21 G96 D1500 S200 M3
N22 G1 Z1.5 F50

now i have to find out the correct values for 
MAX_VELOCITY = 30.0
MAX_ACCELERATION = 900.0

while it looks like the values i have here are way to hight - the z axis driver is going offline  during the job and the axis are turnig very slow but on away that it looks that its needing a lot of power to do so

my steppers are at 200 wit 4 microsteps, Nema 23, the longer ones

Georg

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.121 seconds
Powered by Kunena Forum