lathe turning post processor

[Anonymous]

M using fanuc turning post processor

i enabled optional stop still m not getting m01 command in output.
Also i need to add m05 and m09 at the end of every operation.
m using the exact post processor from hsm library.

[boopathi.sivakumar · Accepted solution]

@Anonymous 

optional stop will be only enabled if we you any tool change.

if you want to force the spindle stop, optional stop and start call for each toolpath then you might need to modify the post processor 

go and find for this line

 var insertToolCall = forceToolAndRetract || isFirstSection() || 

 change it to like this

var insertToolCall = forceToolAndRetract || isFirstSection() || true ||

And find for this line and add the line mentioned

  if (insertToolCall || newSpindle || newWorkOffset) {
    // retract to safe plane
    if (!isFirstSection() && insertToolCall) {
      onCommand(COMMAND_STOP_SPINDLE);  // <<<<<<< Add this line
      onCommand(COMMAND_COOLANT_OFF);
    }

Save and test the post carefully

[Anonymous]

Hey boopathi thankyou for your valuable time
it worked but m still having some issues with the output

m still getting g97 before spindle stop i dont want that anywhere in my program and m01 should be before g28

and why am i getting g28 u0 only why not w0

N10 G98 G18

N11 G21

N12 G50 S800

N13 G28 U0.

(FACE1)

N14 T0101

N15 M8

N16 G99

N17 G97 S466 M4

N18 G0 X80. Z5.

N19 G50 S800

N20 G96 S117 M4

N21 G0 Z0.

N22 X60.

N23 G1 X50. F0.15

N24 X-1.6

N25 G0 X80.

N26 Z5.

N27 G97 S466 M4

N28 M5

N29 M9

N30 G28 U0.

(PROFILE ROUGHING1)

N31 M1

N32 T0101

N33 M8

N34 G99

N35 G97 S532 M4

N36 G0 X70. Z5.

N37 G50 S800

i am trying to make my program exactly look like the old post processor output which was from other software
this is an example for that:-
G21
G28 U0. W0.
N1 T0101 (DDJNL 2525M11 R0.4)
G50 S800
G96 S180 M04
(PLAIN FACE)
G0 Z3.
X65. M08
X66.
G72 W0.5 R0.5
G72 P1 Q4 U10. W0. F0.15
N1 G0 Z0.
N2 G01 X64. Z0.
N3 X16.
N4 Z2.
G0
X65.
M09
M05
M01
G28 U0. W0.
N2 T0202 (DDJNL 2525M15 R0.8)
G50 S800
G96 S180 M04
(CONTOUR TURN)
G0 Z4.
X65. M08
X66.
G71 U1.5 R0.5
G71 P5 Q28 U1. W0.1 F0.15
N5 G00 X23.
N6 G01 X23. Z2.
N7 Z0.
N8 X44.5
N9 X45.5 Z-0.5
N10 Z-3.
N11 X54.
N12 X55. Z-3.5
N13 Z-6.
N14 X59.
N15 X60. Z-6.5
N16 Z-11.5
N17 Z-22.5
N18 Z-26.5
N19 Z-36.5
N20 Z-40.5
N21 Z-50.5
N22 Z-54.5
N23 Z-64.5
N24 Z-68.799
N25 Z-80.
N26 Z-92.3
N27 X64.
N28 X66. Z-92.3
G0
X65.
M09
M05
M01
G28 U0. W0.

[boopathi.sivakumar · Accepted solution]

to avoid output the spindle speed

you can block these codes in the section end as mentioned

function onSectionEnd() {

  // cancel SFM mode to preserve spindle speed
  // if (tool.getSpindleMode() == SPINDLE_CONSTANT_SURFACE_SPEED) {
  //   startSpindle(false, true, getFramePosition(currentSection.getFinalPosition()));
  // }

Calling G97 for the first move while using Constant surface speed is intentional

carefully test the post and let me know the feedback

[Anonymous]

thankyou it worked
the last two issue m facing is:-

1. m only getting g28 u0 and not g28 u0 w0 after any operation except the last one
2. m not getting m05 at the end after m09 after last operation
3. %
   O1001
   N10 G21
   N11 G50 S800
   N12 G28 U0.
   
   
   (FACE1)
   N13 T0101
   N14 M8
   N15 G99
   N16 G97 S466 M4
   N17 G0 X80. Z0.
   N18 G96 S117 M4
   N19 G0 X60.
   N20 G1 X50. F0.15
   N21 X-1.6
   N22 G0 X80.
   N23 M5
   N24 M9
   N25 G28 U0.
   
   
   (PROFILE ROUGHING1)
   N26 M1
   N27 T0101
   N28 M8
   N29 G99
   N30 G97 S532 M4
   N31 G0 X70. Z5.
   N32 G96 S117 M4
   N33 G0 Z0.6
   N34 X51.2
   N35 G71 U1.2 R1.
   N36 G71 P37 Q45 U0.2 W0.1 F0.15
   N37 G0 X14.075
   N38 G1 Z0.
   N39 G18 G3 X21.285 Z-2.598 K-3.8
   N40 G1 X29.61 Z-15.085
   N41 G3 X30. Z-16.287 I-3.605 K-1.202
   N42 G1 Z-50.092
   N43 G2 X30.464 Z-51.076 I2.2
   N44 G1 X49.198 Z-69.809
   N45 X49.343 Z-69.963
   N46 G0 X70. Z0.6
   N47 Z5.
   
   
   N48 M9
   N49 G28 U0.
   N50 G28 W0.
   N51 M30
   %
4.  

[boopathi.sivakumar · Accepted solution]

@Anonymous 

while post processing you can set the safe retract method to Both

and to output m05 in the last section you need to find this one

onImpliedCommand(COMMAND_STOP_SPINDLE);

Change it to 

onCommand(COMMAND_STOP_SPINDLE);

 Save the post and test it carefully

[Anonymous]

that worked for me thankyou!

m facing issues from the first solution my m01 command output is on the start of next operation
m getting g99 in canned cycle i dont want that to display

also i want my coolant to turn on after g96
m really sorry for asking too many questions as m a newbie to cam

%
O1001
N10 G21
N11 G50 S800
N12 G28 U0.

(FACE1)
N13 T0101
N14 M8
N15 G99
N16 G97 S466 M4
N17 G0 X80. Z0.
N18 G96 S117 M4
N19 G0 X60.
N20 G1 X50. F0.15
N21 X-1.6
N22 G0 X80.
N23 M5
N24 M9
N25 G28 U0.

(PROFILE ROUGHING1)
N26 M1
N27 T0101
N28 M8
N29 G99
N30 G97 S532 M4
N31 G0 X70. Z5.
N32 G96 S117 M4
N33 G0 Z0.6
N34 X51.2
N35 G71 U1.2 R1.
N36 G71 P37 Q45 U0.2 W0.1 F0.15
N37 G0 X14.075
N38 G1 Z0.
N39 G18 G3 X21.285 Z-2.598 K-3.8
N40 G1 X29.61 Z-15.085
N41 G3 X30. Z-16.287 I-3.605 K-1.202
N42 G1 Z-50.092
N43 G2 X30.464 Z-51.076 I2.2
N44 G1 X49.198 Z-69.809
N45 X49.343 Z-69.963
N46 G0 X70. Z0.6
N47 Z5.
N48 M5
N49 M9
N50 G28 U0.

(PROFILE FINISHING1)
N51 M1
N52 T0101
N53 M8
N54 G99
N55 G97 S532 M4
N56 G0 X70. Z5.
N57 G96 S117 M4
N58 G0 Z1.414
N59 X19.151
N60 G1 X11.247 F0.15
N61 X14.075 Z0.
N62 G18 G3 X21.285 Z-2.598 K-3.8
N63 G1 X29.61 Z-15.085
N64 G3 X30. Z-16.287 I-3.605 K-1.202
N65 G1 Z-50.092
N66 G2 X30.464 Z-51.076 I2.2
N67 G1 X49.198 Z-69.809
N68 X52.992 Z-70.441
N69 G0 X70.
N70 Z5.

N71 M9
N72 M5
N73 G28 U0. W0.
N74 M30
%

[Anonymous]

hey i figured out few things
just the m01 output at the start of next operation is bothering
idk if that matters
thanks man

you made my life easy.

[Matt_Leon]

hello sorry for the intrusion 🙂

is it possible to update the Okuma post with the directions I wrote below?

%
(1001.MIN)
G50 S1000
G0 X800.
G0 Z150.
(FACCIA1)
.N12.T121212 (you can add * N + tool number * as an example between the dots?)
M8
-->G95 (it is not needded)
-->G97 S241 M3 M41 (it is not needded)

G0 X330. Z3.

-->G50 S1000
-->G96 S250 M3 M41 (this double block is fine but should be placed on top instead of G95-G97)

G0 Z1.7
G1 X320. F0.2
X115.6 F0.35
X119.843 Z3.821 F0.2
G0 X330.
Z0.2
G1 X320. F0.2
X115.6 F0.35
X119.843 Z2.321 F0.2
G0 X330.
Z5
-->G97 S241 M3 M41 (it is not needded/can be deleted)
.
.
*other operation*

thanks