[Big Chips]

just a question to understand HOW to get this in Bobcad Haas post for V25


when i use a mastercam nc file it always shows the tools to be used in a list order on the screen at the top of the nc file...but with my Bobcad post it does not...is this something that I can change or do i need to call Bobcad to have it added and listed this way in the post?

I use this as a helpful viewing aid when i am touching off my tools...i just look a the screen and see what tool is next...but if it is a Bobcad NC file..I have to write it down on paper from the software...

[jrmach]

Is this what you would like to see?

[Big Chips]

yes! the tools list to be used in the file to cut with in the nc header when loaded in the machine


OH and another issue is...the post I used from Bobcad.com finish's the program then loads the first tool again (which I like) BUT i must press reset in order for the cycle to start again once I load in new stock....this makes the table move back to origin and well it adds alot of time

it should (like mastercam) only require me to push cycle start and then it take off again and cut the new stock. I am using the Bobcad TM post for haas tm1p should i try the OEM?


I also see a TMrev1 post file...what is the difference between them? Al?

[jrmach]

I don't know much about about those post processors,they go way over my head real quick.But I think it has something to do with the post file header.Attached is how mine reads.I use a Haas VF-2 machine.Maybe someone else can verify this.I don't want to mislead you.If you try it,make a copy of your original first.

[jrmach]

Kinda hard to see screen shot,heres post.Use at own risk.I have not used in V25 much.

[jrmach]

I just noticed you added to your post"BUT i must press reset in order for the cycle to start again once I load in new stock....this makes the table move back to origin and well it adds alot of time"I had that fixed years ago in V23.I had someone else do it.I think I need the same thing done in my new post,not sure though,I have been running V23 programs.Like I said ,not very good at post processors.I will post my V23 post for you.The answer is in there,because that one worked as you said you want.I just have not looked into it that much.Do a side by side post comparison and you can probably figure it out.

[moldmker]

....it always shows the tools to be used in a list order on the screen at the top of the nc file...but with my Bobcad post it does not...is this something that I can change or do i need to call Bobcad to have it added and listed this way in the post?....

**(see note at end) Open your post file in Notepad and add this line to line#1 and #2:
output_tool_list

...the post I used from Bobcad.com finish's the program then loads the first tool again (which I like) BUT i must press reset in order for the cycle to start again once I load in new stock....this makes the table move back to origin and well it adds alot of time....

****NOTE: Before altering a post file you should save it under a different name. Just add your initials and maybe a version number. Make all your changes to the renamed file. Be sure to point Bobcad to the new post file before posting any code.

[Big Chips]

moldmakr,

thanks will do....just one question on the last remove line thing...are you saying remove that from #1 & #2? or just #2 like the picture..???

[moldmker]

moldmakr,

thanks will do....just one question on the last remove line thing...are you saying remove that from #1 & #2? or just #2 like the picture..???

Sorry...both 1 and 2.

Actually, I think the #1 line is being "reserved for future use" as I don't think there's an instance where it's ever called.
But better to have all your duckies in a row if a Bobcad version does start to reference it.

[Big Chips]

do i just save this a .txt file back where the post are at for Bobcad? just makes sure it is named with .millpst at the end? Notepad wants to save it as a .txt file and V25 will not recognize it in the selection window


and one last thing...the current post i am using DOES Not record last cycle time how is that fixed....I like to see what how much time is left for the part to finish based on the previous part being machined...is this part of th epost or a setting that needs rest on the haas?

sorry for the question you have been a huge help..both of you...thank you both!

[moldmker]

do i just save this a .txt file back where the post are at for Bobcad? just makes sure it is named with .millpst at the end?


and one last thing...the current post i am using DOES Not record last cycle time how is that fixed....I like to see what how much time is left for the part to finish based on the previous part being machined

Yes on the .millpst save.
Here's a tip...if you right click on the post filename and select Open With...then Select Program...then Notepad and tick the Always Use This Program box...you will associate the .millpst files with Notepad, so a double click will open them and Save will update them. Very handy for never ending experimenting with post variables.

Re the time issue: this sounds like a controller issue....I don't recall any post commands that reference cycle time...but I'm all ears if someone else has something to add...

[BurrMan]

Yes on the .millpst save.
Here's a tip...if you right click on the post filename and select Open With...then Select Program...then Notepad and tick the Always Use This Program box...you will associate the .millpst files with Notepad, so a double click will open them and Save will update them. Very handy for never ending experimenting with post variables.

Re the time issue: this sounds like a controller issue....I don't recall any post commands that reference cycle time...but I'm all ears if someone else has something to add...

He said "the last" cycle time... Be sure the post is outputing something as end of program that tells the controller it's over correctly.

[Big Chips]

That did it...thanks for the help! Just what i wanted..

I am sure this topic will help other newbies in the future

i would think that the last cycle time is part of the post processor....??????....the machine does nto know that program is finished...seems to me...

the post i am using and just modified with the setting you showed...is below. BUT I will run this tomorrow...maybe deletion the lines you showed me will tell the machine it is done... as it stands this morning when the part is finished the machine loads T1 after the last tool specified to cut the part with and stops.....when i hit cycle start nothing happened...i had to push "reset" and then the program would go to the top and then once i pushed cycle start we were off and running AFTer the table went to origin...and the last cycle time did not read correct.


Customization file for HAAS TM - Optional Stop at Tool Change
Post variables listed in MillPostVariables.pst
****Version number MONTH DAY YEAR****
1000. Version Information = Version Month Day Year? "9.0 08 22 2008"
0. File header
default_add_spaces
"(BEGIN PREDATOR NC HEADER)"
"(MACH_FILE=HAAS - 3XVMILL.MCH)"
output_tool_list
output_stock_definition
"(END PREDATOR NC HEADER)"
" "
"%"
"O",prog_n,"(PROGRAM NUMBER)"


1. Start of file programmed zero
"(PROGRAM NAME - ",prog_name,")"
"(POST - ",machine_make,machine_model,")"
"(DATE - ",output_date,")"
"(TIME - ",output_time,")"
user_comment_1
user_comment_2
user_comment_3
user_comment_4
user_comment_5
user_comment_6
user_comment_7
user_comment_8
user_comment_9
user_comment_10
user_comment_11
user_comment_12
user_comment_13
user_comment_14
user_comment_15
" "
output_tool_list
" "
n,rapid_move,"G17",inch_mode,"G40","G49",cancel_dr ill_cycle,absolute_coord
" "
n,rapid_move,incremental_coord,"G28","Z0."

" "
"(FIRST CUT - FIRST TOOL)"
system_comment
feature_name_comment
" "
n,t,"M06"
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,,s,spindle_on
n,rapid_move,length_offset,coolant_on
output_rotary_angle

2. Start of file Standard
"(PROGRAM NAME - ",prog_name,")"
"(POST - ",machine_make,machine_model,")"
"(DATE - ",output_date,")"
"(TIME - ",output_time,")"
user_comment_1
user_comment_2
user_comment_3
user_comment_4
user_comment_5
user_comment_6
user_comment_7
user_comment_8
user_comment_9
user_comment_10
user_comment_11
user_comment_12
user_comment_13
user_comment_14
user_comment_15
" "
output_tool_list
" "
n,rapid_move,"G17",inch_mode,"G40","G49",cancel_dr ill_cycle,absolute_coord
" "
n,rapid_move,incremental_coord,"G28","Z0."

" "
"(FIRST CUT - FIRST TOOL)"
system_comment
feature_name_comment
" "
n,t,"M06"
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,,s,spindle_on
n,rapid_move,length_offset,coolant_on
output_rotary_angle

3. Tool change
n,coolant_off
n,spindle_off
n,rapid_move,incremental_coord,"G28","Z0."
n,optional_stop
" "
"(NEXT CUT - NEXT TOOL)"
system_comment
feature_name_comment
" "
n,t,"M06"
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,,s,spindle_on
n,rapid_move,length_offset,coolant_on
output_rotary_angle

4. Null tool change
" "
"(NEXT CUT - SAME TOOL)"
system_comment
feature_name_comment
" "
n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angl e,,s
output_rotary_angle

5. End of file for non-zero tool
n,coolant_off
n,spindle_off
n,rapid_move,incremental_coord,"G28","Z0."
n,rapid_move,incremental_coord,"G28","Y0."
n,first_tool_with_prefix,"M06"
n,end_of_file
" "
"(END OF FILE)"


6. Optional Stop
optional_stop


7. Sub program call
n,sub_call,sub_num,"(SUBPROGRAM CALL)"


8. Sub definition
" "
sub_num_with_prefix,sub_comment


9. Sub program return
rigid_tapping_end
n,sub_return,"(SUBPROGRAM RETURN)"

10.Rotary axis index string
n,"A",rotary_angle

11. Cancel cutter compensation
"G40"


12. Cutter compensation left
"G41",d_offset


13. Cutter compensation right
"G42",d_offset


14. Tool length compensation
" G43",h,force_z,zr


20. Spindle speed low range
"M41","(LOW RANGE SPINDLE)"


21. Spindle speed high range
"M42","(HIGH RANGE SPINDLE)"


22. Rigid tapping start.


23. Rigid tapping end.
n,cancel_drill_cycle


24. File trailer.
"(END OF PROGRAM)"
" "
n,"M30"
"%"


25. Format for offset when using offset registers.


26. Set debug.
debug_off


27. First Rapid Move.
n,rapid_move,zr


28. Rapid Move.
n,rapid_move,zr


40. Start of 2axis contour.


50. Line first rapid move Z.
rigid_tapping_end
n,rapid_move,zr


51. Line feed move Z.
n,feed_move,z_f,feed_rate


52. Line rapid move XY.
n,rapid_move,xr,yr,rotary_xyr_angle,


53. Line feed move XY.
n,feed_move,x_f,y_f,feed_rate


54. Line rapid move XYZ.
n,rapid_move,xr,yr,zr


55. Line feed move XYZ.
n,feed_move,x_f,y_f,z_f,feed_rate


56. Line feed move XY on Leadin.
n,cc,feed_move,x_f,y_f,feed_rate


57. Line feed move XY on Leadout.
n,cc,feed_move,x_f,y_f,feed_rate


64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,fe ed_rate

65. Arc move YZ.
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,fe ed_rate

66. Arc move XZ.
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,fe ed_rate


71. End of 2axis cutting.


73. High speed peck drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,peck_drill_increment,dwell,canned_feed_ rate


74. Left handed tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,canned_feed_rate


76. Fine boring canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,peck_drill_increment,dwell,canned_feed_ rate


80. Drill canned cycle cancel.


81. Standard drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,canned_feed_rate


82. Standard drill canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,dwell,canned_feed_rate


83. Peck drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,peck_drill_increment,dwell,canned_feed_ rate


84. Tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,canned_feed_rate


85. Boring cycle #1 canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,canned_feed_rate


86. Boring cycle #2 canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,canned_feed_rate


87. Back boring cycle canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,peck_drill_increment,dwell,canned_feed_ rate


88. Boring cycle #1 canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,dwell,canned_feed_rate


89. Boring cycle #2 canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,refer ence_plane,dwell,canned_feed_rate


90. Canned cycle drill point format WITH SUBPROGRAMS.
n,x_f,y_f, zr_no_output
91. Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
92. Canned cycle drill point format for standard drill canned cycle with dwell NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
93. Canned cycle drill point format for peck drill canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
94. Canned cycle drill point format for tapping canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
95. Canned cycle drill point format for boring cycle #1 canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
96. Canned cycle drill point format for boring cycle #2 canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
97. Canned cycle drill point format for back boring cycle canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
98. Canned cycle drill point format for boring cycle #1 canned cycle with dwell NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
99. Canned cycle drill point format for boring cycle #2 canned cycle with dwell NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output
100. Absolute coordinate output.
absolute_coord


101. Incremental coordinate output.
incremental_coord


108. Rectangular stock format.
"(SBOX","X",stock_min_x,"Y",stock_min_y,"Z",stock_ min_z,"L",stock_length,"W",stock_width, "H",stock_height,")"

109. Rotary stock format.
"(SCYL",rotation_axis,"X0","Y0","Z0",rotary_stock_ diameter,rotary_stock_length,")"

110. Tool list format.
"(MTOOL","T",list_tool_number,mtool_type,"D",tool_ diameter,mtool_corner_rad,mtool_angle,"H",tool_len gth,")"


113. Canned cycle drill point format for high speed peck drill canned cycle NO SUBPROGRAMS.
n,x_f,y_f


114. Canned cycle drill point format for left handed tapping canned cycle NO SUBPROGRAMS.
n,x_f,y_f

116. Canned cycle drill point format for fine boring canned cycle NO SUBPROGRAMS.
n,x_f,y_f, zr_no_output


152. Line rapid move XY.
n,rapid_move,xr,rotary_xyr_angle,


153. Line feed move XY.
n,feed_move,rotary_xy_f,rotary_xyr_angle,feed_rate


154. Line rapid move XYZ.
n,rapid_move,xr,rotary_xyr_angle,zr


155. Line feed move XYZ.
n,feed_move,rotary_xy_f,rotary_xy_angle,z_f,feed_r ate


156. Line feed move XY on Leadin.
n,cc,feed_move,rotary_xy_f,rotary_xy_angle,feed_ra te


157. Line feed move XY on Leadout.
n,cc,feed_move,rotary_xy_f,rotary_xy_angle,feed_ra te


164. Arc move.
n,g_arc_move,rotary_xy_angle,arc_center,feed_rate


170. High speed peck drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,peck_drill_incremen t,dwell,canned_feed_rate


171. Left handed tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,canned_feed_rate


172. Fine boring canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,peck_drill_incremen t,dwell,canned_feed_rate


173. Drill canned cycle cancel.


174. Standard drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,canned_feed_rate


175. Standard drill canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,dwell,canned_feed_r ate


176. Peck drill canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,peck_drill_incremen t,dwell,canned_feed_rate


177. Tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,canned_feed_rate


178. Boring cycle #1 canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,canned_feed_rate


179. Boring cycle #2 canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,canned_feed_rate


180. Back boring cycle canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,peck_drill_incremen t,dwell,canned_feed_rate


181. Boring cycle #1 canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,dwell,canned_feed_r ate


182. Boring cycle #2 canned cycle with dwell.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,dwell,canned_feed_r ate


183. Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS.
n,rotary_xy_f,rotary_xy_angle


200. Is X modal? y
201. Is Y modal? y
202. Is Z modal? y
203. Are the g codes modal? y
204. Are the g codes (G02 and G03) modal in arc milling? y
205. Are the xy (or yz or xz) coordinates modal in arc milling? n
206. Are work coordiantes modal ? n
207. Output sequence numbers in subprograms ? y
208. Output sequence numbers? y
209. Number of places for sequence numbers? 2
210. Delete the decimal point? n
211. Delete leading zeros? y
212. Delete trailing zeros? y
213. English or Metric format (E/M)? E
214. Places before decimal point for reals (X, Y, Z)? 1
215. Number of places for Tool Numbers? 1
216. Places after decimal for feedrate ? 4
217. Scale factor for feedrate ? 1
219. Add spaces to the program? y
221. Break arcs into quadrants? n
222. Arc center a=absolute, b=incremental, d=unsigned inc., e=radius? b
223. Break arcs into two pieces if greater than 180 degrees? n
227. Output G40 after, rather than with, the last linear or arc move? y
230. Use Standard drilling canned cycle? y
231. Use peck drill canned cycle? y
232. Use High speed peck drill canned cycle? y
233. Use tapping canned cycle? y
234. Use boring cycle #1 canned cycle? y
235. Use boring cycle #2 canned cycle? y
236. Use back boring cycle canned cycle? y
237. Use left hand tap cycle canned cycle? y
238. Use fine boring cycle canned cycle? y
240. Amount to add to t to obtain t1? 0
241. Amount to add to t to obtain t2? 0
242. Value of t1 at t = 0? 0
243. Value of t2 at t = 0? 0
258. Maximum number of work offsets? 26
262. Add sign to all coordinate values? n
267. Amount to add to tool # for tool register value? 0
272. Rigid tapping? y
273. Output programmable rotary axis codes? y

313. Z clearance for auto Z programming for XY move? 0.20000
314. Z clearance for auto Z programming for cutting? 0.00000
315. Minimum part heigth? 0.00000

414. Number of decimal places for metric numbers ? 3
415. Number of decimal places for english numbers? 4
425. Number of decimal for angles? 3
426. Number of leading decimal places for angles? 2
427. Tapping feed rate (1=ipm 2=ipr)? 2
428. Feed rates other than tapping (1=ipm 2=ipr)? 1
429. Maximum spindle speed for tapping? 10000
430. Maximum spindle speed? 10000
431. Spindle speed for high rangle? 10000
432. Add amount for tool number in tool list? 0
433. Maximum sequence number allowed (used when #534 is y)? 9999

511. Use incremental coordinates? n
512. Use block delete for stop codes (M00)? n
513. Output F feedrate values? n
515. Output G99 instead of G98 in drilling? y
516. Output G98/G99 in drilling? y
518. Output M00 codes? n
526. Start renumbering from start number for subprograms? n
527. Create subdirectory for nc file? n
531. Replace spaces in comment with commas ? n
533. Output suprograms at the beginning of the program? n
534. Re-Start sequence numbering once max sequence number is reached? n
535. Are Feed Rates modal? y
536. Force all codes to upper case ? y

540. Check each output line with scripting? n

605. Spindle speed prefix? "S"
606. Feedrate prefix? "F"
607. Dwell prefix? "P"

610. Miscellaneous end of file string? ""
613. Pattern contour subprogram start code? ""
614. Inch mode machining? "G20"
615. Metric mode machining? "G21"

620. Absolute coordinates? "G90"
621. Incremental coordinates? "G91"
622. Coordinate zero set? "G92"
625. End of file? "M02"
626. Stop? "M00"
627. Optional Stop? "M01"
628. Subprogram call? "M98"
629. Subprogram return? "M99"
630. Comment Start? "("
631. Comment End? ")"
639. Cancel wire offset? "G40"
640. Prefix for arc Z center? "K"
641. Prefix for radius values? "R"
642. Prefix for arc X center? "I"
643. Prefix for arc Y center? "J"
645. Subprogram prefix? "O"
646. Machine maker? "HAAS"
647. Machine model? "TM"
648. Part Height prefix? "None"
649. Reference Plane prefix? "R"
650. Wire comp left? "G41"
651. Wire comp right? "G42"
656. Block delete? "/"
658. Subprogram call subnumber prefix? "P"
659. Add these characters to the end of each line? ""
670. Spindle forward string? "M03"
671. Spindle reverse string? "M04"
672. Spindle off string? "M05"
673. Coolant on string? "M08"
674. Coolant off String? "M09"
675. First peck prefix? "I"
676. Peck drill prefix? "Q"
677. Drill depth prefix? "Z"
678. Cutter offset prefix? "D"
679. Cancel drilling canned cycle? "G80"
680. GCode for Rapid Move? "G00"
681. GCode for Feed Move? "G01"
682. GCode for Arc CW? "G02"
683. GCode for Arc CCW? "G03"
684. Prefix for X Move? "X"
685. Prefix for Y Move? "Y"
686. Prefix for Z Move? "Z"
687. Prefix for drill canned cycle feed rate? "F"
688. Prefix for tool length offset? "H"
689. Prefix for initial plane? "I"
690. Prefix for X Rotation Move? "A"
691. Prefix for XY Machining Plane? "G17"
692. Prefix for XZ Machining Plane? "G18"
693. Prefix for YZ Machining Plane? "G19"
694. Prefix for Y Rotation Move? "B"
695. Prefix for tapping feed rate (variable tapping_feedrate)? "FF"
696. Prefix for tapping spindle speed (variable tapping_spindle_speed)? "SS"
697. Prefix for threads per inch (variable threads_per_inch)? "?"
698. Prefix for thread lead (variable thread_lead)? "?"
699. Prefix for Tool Angle (variable mtool_angle)? "A"
700. Prefix for Tool CornerRadius (variable mtool_corner_rad)? "C"
701. Prefix for Tool Type (variable mtool_type)? "S"
702. Prefix for rotation axis (variable rotation_axis)? "S"
703. Prefix for rotary stock diameter (variable rotary_stock_diameter)? "D"
704. Prefix for rotary stock length (variable rotary_stock_length)? "L"
705. Prefix for Z Feed Rate? "F"
706. Coolant Mist code? "M07"
707. Coolant Air code? "M07"
708. Coolant Oil code? "M07"

800. Standard drilling cycle no dwell #1? "G81"
801. Peck drill cycle no dwell #2? "G83"
802. High speed peck drill cycle no dwell #3? "G73"
803. Tapping cycle no dwell #4? "G84"
804. Boring cycle #1 no dwell #5? "G85"
805. Boring cycle #2 no dwell #6? "G86"
806. Back boring cycle no dwell #7? "G87"
807. Left hand tapping cycle no dwell #8? "G74"
808. Fine boring cycle no dwell #9? "G76"
809. Hole making cycle no dwell #10?""
810. Hole making cycle no dwell #11?""
811. Hole making cycle no dwell #12?""
820. Standard drilling cycle with dwell #1? "G82"
821. Peck drill cycle with dwell #2? "G83"
822. High speed peck drill cycle with dwell #3? "G73"
823. Tapping cycle with dwell #4? "G84"
824. Boring cycle #1 with dwell #5? "G88"
825. Boring cycle #2 with dwell #6? "G89"
826. Back boring cycle with dwell #7? "G77"
827. Left hand tapping cycle with dwell #8? "G74"
828. Fine boring cycle with dwell #9? "G76"
829. Hole making cycle with dwell #10?""
830. Hole making cycle with dwell #11?""
831. Hole making cycle with dwell #12?""

900. Work shift #1? "G54"
901. Work shift #2? "G55"
902. Work shift #3? "G56"
903. Work shift #4? "G57"
904. Work shift #5? "G58"
905. Work shift #6? "G59"
906. Work shift #7? "G110"
907. Work shift #8? "G111"
908. Work shift #9? "G112"
909. Work shift #10? "G113"
910. Work shift #11? "G114"
911. Work shift #12? "G115"
912. Work shift #13? "G116"
913. Work shift #14? "G117"
914. Work shift #15? "G118"
915. Work shift #16? "G119"
916. Work shift #17? "G120"
917. Work shift #18? "G121"
918. Work shift #19? "G122"
919. Work shift #20? "G123"
920. Work shift #21? "G124"
921. Work shift #22? "G125"
922. Work shift #23? "G126"
923. Work shift #24? "G127"
924. Work shift #25? "G128"
925. Work shift #26? "G129"
926. Work shift #27? ""
927. Work shift #28? ""
928. Work shift #29? ""
929. Work shift #30? ""
930. Work shift #31? ""
931. Work shift #32? ""
932. Work shift #33? ""
933. Work shift #34? ""
934. Work shift #35? ""
935. Work shift #36? ""
936. Work shift #37? ""
937. Work shift #38? ""
938. Work shift #39? ""
939. Work shift #40? ""
940. Work shift #41? ""
941. Work shift #42? ""
942. Work shift #43? ""
943. Work shift #44? ""
944. Work shift #45? ""
945. Work shift #46? ""
946. Work shift #47? ""
947. Work shift #48? ""
948. Work shift #49? ""
949. Work shift #50? ""
950. Work shift #51? ""
951. Work shift #52? ""
952. Work shift #53? ""
953. Work shift #54? ""
954. Work shift #54? ""
955. Work shift #55? ""
956. Work shift #56? ""
957. Work shift #57? ""
958. Work shift #58? ""
959. Work shift #59? ""
960. Work shift #60? ""
961. Work shift #61? ""
962. Work shift #62? ""
963. Work shift #63? ""
964. Work shift #64? ""
965. Work shift #65? ""
966. Work shift #66? ""
967. Work shift #67? ""
968. Work shift #68? ""
969. Work shift #69? ""
970. Work shift #70? ""
971. Work shift #71? ""
972. Work shift #72? ""
973. Work shift #73? ""
974. Work shift #74? ""
975. Work shift #75? ""
976. Work shift #76? ""
977. Work shift #77? ""
978. Work shift #78? ""
979. Work shift #79? ""
980. Work shift #80? ""
981. Work shift #81? ""
982. Work shift #82? ""
983. Work shift #83? ""
984. Work shift #84? ""
985. Work shift #85? ""
986. Work shift #86? ""
987. Work shift #87? ""
988. Work shift #88? ""
989. Work shift #89? ""
990. Work shift #90? ""
991. Work shift #91? ""
992. Work shift #92? ""
993. Work shift #93? ""
994. Work shift #94? ""
995. Work shift #95? ""
996. Work shift #96? ""
997. Work shift #97? ""
998. Work shift #98? ""
999. Work shift #99? ""

[moldmker]

I program for a Haas only about 4 times a year.
But the only cycle time feedback I know of is provided by the Haas controller...since it is affected by feedrate overrides set at the machine.

The fact that you have to hit reset says something in the program is hanging the controller.
A cursory glance at my modified Haas post shows this difference:

625. End of file? "M30"

Might be the issue, as I remember having to change this.
Post a complete G-code program if problems continue.

[BurrMan]

On an unrelated side note. Find these in your post:

rotary_xyr_angle

And remove the "r".

This is for V24 and 25.

[SBC Cycle]

I program for a Haas only about 4 times a year.
But the only cycle time feedback I know of is provided by the Haas controller...since it is affected by feedrate overrides set at the machine.

The fact that you have to hit reset says something in the program is hanging the controller.
A cursory glance at my modified Haas post shows this difference:

625. End of file? "M30"

Might be the issue, as I remember having to change this.
Post a complete G-code program if problems continue.

I've only had Haas machines for a little over a year so I'm no expert but yeah, if it needs a reset at the end then it must not be getting an M30. Without an M30 at the end, it doesn't "rewind" back to the beginning (I had a machine that used punch tape, it would literally rewind, lol).

The M30 also "sets" the cycle time. Without it it won't show the last part's cycle time. Without that, no countdown to the end of cycle.

[SBC Cycle]

He said "the last" cycle time... Be sure the post is outputing something as end of program that tells the controller it's over correctly.

Yes, that's it! Sorry didn't see your post here. If I stop the program before it hits the M30, the cycle time counter resets to the last part that DID record an M30. If that makes any sense at all