[stevespo]

Claude, you can use the 2nd option to create one tab on each line, but it's really intended to creating multiple tabs, one at every interval.

If you really just want a single tab per line, then disable the 2nd option, and enable the first option and that will ensure you get one tab per line that falls within the parameters.

For the kinds of things I am doing (fairly small) I find that one tab per line is plenty. I included the second option for those cases when I have long parts and want more than one tab per long line.

A possible third option might be to say "for lines longer than N units, place X tabs on each line" (evenly spaced). That might be useful in some circumstances, although option 2 probably will work just fine.

With a part like this one, I would still use double sided tape to hold the piece down and then the tabs will help prevent twisting.

It would be great to put a tab or two on the curved profile, but I have not found a way to make it work. I've written the algorithm, but don't have enough data available.

Steve

[Claude Boudreau]

Claude, you can use the 2nd option to create one tab on each line, but it's really intended to creating multiple tabs, one at every interval.

If you really just want a single tab per line, then disable the 2nd option, and enable the first option and that will ensure you get one tab per line that falls within the parameters.

For the kinds of things I am doing (fairly small) I find that one tab per line is plenty. I included the second option for those cases when I have long parts and want more than one tab per long line.

A possible third option might be to say "for lines longer than N units, place X tabs on each line" (evenly spaced). That might be useful in some circumstances, although option 2 probably will work just fine.

With a part like this one, I would still use double sided tape to hold the piece down and then the tabs will help prevent twisting.

It would be great to put a tab or two on the curved profile, but I have not found a way to make it work. I've written the algorithm, but don't have enough data available.

Steve

Hi Steve ,
Could you design it so that, on the final pass, the contour would be cut ,twice the length of your tool diameter per example, at certain places, making the tabs. (creating a void in the contour)
That way the tabs would not have to follow the curved contour... tabs would just be created by breaking up the contour.
Someone could use the points on entity to indicate the position, and the witdth of the tabs. Tabs thickness could be left as the thickness of the last cut for simplicity.

Hoping this will give you ideas,
Claude

[stevespo]

Claude, that's an interesting idea, but the post API just doesn't provide any mechanism for doing that. The program does not deal with line segments and points, but rather the actual G00/G01 movements. The G02/G03 movements are lacking information that I need to make the break and restart at a given offset. I wish it was possible, but at this point - it is not.

Steve

[Claude Boudreau]

Claude, that's an interesting idea, but the post API just doesn't provide any mechanism for doing that. The program does not deal with line segments and points, but rather the actual G00/G01 movements. The G02/G03 movements are lacking information that I need to make the break and restart at a given offset. I wish it was possible, but at this point - it is not.

Steve

If one was to create on the cad side a separate broke up contour (with cut and paste) of a diffferent color could this new contour be use on the final pass?

[MikeTheG]

They just released the update to the nesting for v23 which now has tabbing in it. If you already own the V23 nesting just download the 1812 update and it will be in there.

[Claude Boudreau]

They just released the update to the nesting for v23 which now has tabbing in it. If you already own the V23 nesting just download the 1812 update and it will be in there.

For those of us who cant or wont pay, Id wish this would have evolve some more.

[crossedout]

Stevespo,
I know this is an old thread, but what you've come up with is exactly what I need. However I can't get it to work. I've tried adapting your post to my customized HAAS post and all I can get is the "downward ZFeed: Contour Final Pass" comment. I've got the adv posting dialog and all, but can't get the output tabs


I tried your sample file with your sample file with your post. Again, I get the adv posting dialog and have the settings the same as your attached thumbnails, but still only get the doward zfeed comment.

Have you made any advancements on this. or any ideas what I'm doing wrong.

I would really appreciate your help.

[stevespo]

I'll try and help work through it, but I haven't thought about this in a long time!

The downward Zfeed comment indicates that the post processor has found the final Z pass and will be trying to add tabs.
The fact that there are no tabs is confusing, especially for my simple test case.

There are some debugging statements that might be helpful. Look for:

2010.
'
' Trap the XY Feed moves (G01)

and then scroll down to find:

' MILL_OutputText("(*** Line Feed XY Move ***)")

The single quote indicates a line that is commented out. Remove only the single quote and then scroll down further. You will see several blocks of text with:

	If 0 Then
		MILL_OutputText("(*** length: "&MILL_MakeRealString(length)&")")
                and so on...
	End If

Change the "If 0 Then" to "If 1 Then" and those debugging statements will now show up as comments in the generated output.
If you capture the output (gcode) and post it here, I'll take a look.

Steve

[crossedout]

attached is a screengrab of what I've got.
I have tried with the first and second G01 options both checked and individually checked.
[ATTACH=CONFIG]242030[/ATTACH

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3AXVMILL.MCH)
(MTOOL T1 S1 D.125 H2. DIAM_OFFSET 1 = .0625)
(SBOX X-1. Y-1. Z-1. L1. W1. H0.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - SIMPLE-TAB-TEST.NC)
(POST -  MACH 3 ROUTER)
(DATE - THU. 07/10/2014)
(TIME - 09:35AM)

N01 G20 G40 G49 G64 G80 G90 G91.1

(JOB 1  PROFILE)
(FEATURE PROFILE)

N02 T1
N03 S10000 M03
N04 G00 G90 X-1.0625 Y.75
N05 Z.6
N06 G01 Z.25 F60.
N07 Y-.75 F120.
N08 G17 G03 X-.75 Y-1.0625 I.3125 J0.
N09 G01 X.75
N10 G03 X1.0625 Y-.75 I0. J.3125
N11 G01 Y.75
N12 G03 X.75 Y1.0625 I-.3125 J0.
N13 G01 X-.75
N14 G03 X-1.0625 Y.75 I0. J-.3125
N15 G00 Z.6
N16 Z.35
(*** Downward ZFeed: Contour Final Pass ***)
N17 G01 Z0. F60.
N18 Y-.75 F120.
N19 G03 X-.75 Y-1.0625 I.3125 J0.
N20 G01 X.75
N21 G03 X1.0625 Y-.75 I0. J.3125
N22 G01 Y.75
N23 G03 X.75 Y1.0625 I-.3125 J0.
N24 G01 X-.75
N25 G03 X-1.0625 Y.75 I0. J-.3125
N26 G00 Z.6
N27 M05
N28 M02

(END OF PROGRAM)

N29 M30
%

[stevespo]

I know you've tried both options, but for the simple part, I think you want the first "Enable G01 tabs" option selected.
The item is ~2" square with radiused corners and 1.5" G01 straight line moves. That should generate tabs for the criteria below.

  Enable G01 tabs, For Moves > 1.0 and For Moves < 2.0

If you haven't enabled the debugging (the Mill_OutputText comment lines), please do that and regenerate the gcode.
If you're still not seeing any debugging statements, then perhaps the other routines are not being called at all.

FWIW, the BobCAD VB interface is horrible and the way it's tied together is very clumsy.

program_block_8 will call the routine defined by 2008
program_block_9 will call the routine defined by 2009
and so on.

You definitely have the program_block_9/2009 configured properly but double check the other ones as well.
Look for these types of lines in your mill post and make sure that the instructions for program_block_XX are all intact.

I have 8 total in my post, but the last 3 are for the arc fix, which you might not be using.
The critical ones are program_block_8, 9, 10, 11. Block 20 is for debugging as well.

40. Start of 2axis contour.
   program_block_8
  
50. Line first rapid move Z.
   rigid_tapping_end
   program_block_11
   n,rapid_move,zr

51. Line feed move Z.
   program_block_9
   n,feed_move,z_f,feed_rate
  
53. Line feed move XY.
   program_block_10
  
71. End of 2axis cutting.
   program_block_20
  
64. Arc move XY.
   program_block_7

65. Arc move YZ.
   program_block_7

66. Arc move XZ.
   program_block_7

[crossedout]

Thank you for all of your help, even after all this time. This ability would make a big difference in what I do.

Yes, it looks like i missed some of the blocked lines. This should help.

Yes, I tried both ways, but figured I'd post the setting to match what I saw posted in another photo earlier in the thread.

I thought my post processor was complex, but i know nothing compared to you.

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3AXVMILL.MCH)
(MTOOL T1 S1 D.125 H2. DIAM_OFFSET 1 = .0625)
(SBOX X-1. Y-1. Z-1. L1. W1. H0.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - SIMPLE-TAB-TEST.NC)
(POST -  MACH 3 ROUTER)
(DATE - FRI. 07/11/2014)
(TIME - 07:39AM)

N01 G20 G40 G49 G64 G80 G90 G91.1

(JOB 1  PROFILE)
(FEATURE PROFILE)

N02 T1
N03 S10000 M03
N04 G00 G90 X-1.0625 Y.75
N05 Z.6
(********************************)
(*** Start of 2 axis contour)
(*** PassName: )
(*** SequenceNumber: 6.)
(*** OperationType: 13.)
(*** NumberOfFeatures#: 1.)
(*** FeatureNumber: 1.)
(*** FeatuerType: 20.)
(*** NumberOfContours: 1.)
(*** CurrentContourNumber: 1.)
(*** NumberOfContourEntities: 21.)
(*** CurrentContourEntityNumber: 1.)
(*** NumberOfIntMemoryLoc: 100)
(*** NumberOfDoubleMemoryLoc: 100)
(*** NumberOfStringMemoryLoc: 100)
(********************************)
N06 G01 Z.25 F60.
N07 Y-.75 F120.
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N08 G17 G03 X-.75 Y-1.0625 I.3125 J0.
N09 G01 X.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N10 G03 X1.0625 Y-.75 I0. J.3125
N11 G01 Y.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N12 G03 X.75 Y1.0625 I-.3125 J0.
N13 G01 X-.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N14 G03 X-1.0625 Y.75 I0. J-.3125
(*** 2011 ***)
(*** ZFeed: .25)
(*** PreviousZFeed: .25)
(*** ZRapid: .6)
N15 G00 Z.6
(*** 2011 ***)
(*** ZFeed: .25)
(*** PreviousZFeed: .6)
(*** ZRapid: .35)
N16 Z.35
(*** Downward ZFeed: Contour Final Pass ***)
N17 G01 Z0. F60.
N18 Y-.75 F120.
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N19 G03 X-.75 Y-1.0625 I.3125 J0.
N20 G01 X.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N21 G03 X1.0625 Y-.75 I0. J.3125
N22 G01 Y.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N23 G03 X.75 Y1.0625 I-.3125 J0.
N24 G01 X-.75
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N25 G03 X-1.0625 Y.75 I0. J-.3125
(*** 2011 ***)
(*** ZFeed: 0.)
(*** PreviousZFeed: 0.)
(*** ZRapid: .6)
N26 G00 Z.6
(********************************)
(DEBUG: End of 2 axis cutting)
(********************************)
N27 M05
N28 M02

(END OF PROGRAM)

N29 M30
%

[stevespo]

I can see the extra debugging information, but not the information I'd expect to see if tabbing was happening.
This is the critical section. The program knows that it's the final contour pass, so that is great.
It also knows when the contour ends - but it's not intercepting the straight line G01 movements to insert the tabs.

(*** Downward ZFeed: Contour Final Pass ***)
N17 G01 Z0. F60.
N18 Y-.75 F120.
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N19 G03 X-.75 Y-1.0625 I.3125 J0.
N20 G01 X.75  ( <== this line should be intercepted )
(DEBUG: units=0)
(DEBUG: radius=.3125, degrees=5156.6203, radians=90.)
(DEBUG: arcLength=28.125, minLength=.0025)
N21 G03 X1.0625 Y-.75 I0. J.3125
N22 G01 Y.75  ( <== this line too )

Can you double check your post and make sure that the program_block_10 and program section 2010 are configured?
It could be something else, but without this line feed XY movement, we definitely can't insert the tabs.

53. Line feed move XY.
   program_block_10

If you don't mind uploading it, I'd be happy to take a look at your full post processor and maybe I'll spot something.

Steve

[crossedout]

If I didn't say it clearly in the last post, you're great. Thank you very much.

It looks like things were right.

Thanks again.

Customization file for MACH 3 Mill - No Automatic Tool Changer - Router
Post variables listed in MillPostVariables.pst
****Version number MONTH DAY YEAR****
1000. Version Information = Version Month Day Year? "9.1 09 29 2009"
0. File header
   default_add_spaces
   "(BEGIN PREDATOR NC HEADER)"
   "(MACH_FILE=3AXVMILL.MCH)"
   output_tool_list
   "(SBOX","X",stock_min_x,"Y",stock_min_y,"Z",stock_min_z,"L",stock_max_x,"W",stock_max_y,"H",stock_max_z,")"        
   "(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
   "  "
   n,inch_mode,"G40","G49","G64",cancel_drill_cycle,absolute_coord,"G91.1"
   "  "
   system_comment
   feature_name_comment
   "  "
   n_forced,t
   n,s,spindle_on
   n,rapid_move,absolute_coord,force_x,xr,force_y,yr,rotary_xyr_angle,
   n,rapid_move,length_offset
   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
   "  "
   n,inch_mode,"G40","G49","G64",cancel_drill_cycle,absolute_coord,"G91.1"
   "  "
   system_comment
   feature_name_comment
   "  "
   n_forced,t
   n,s,spindle_on
   n,rapid_move,absolute_coord,force_x,xr,force_y,yr,rotary_xyr_angle,
   n,rapid_move,length_offset
   output_rotary_angle
  
3. Tool change
   n,spindle_off
   n,optional_stop
   "  "
   system_comment
   feature_name_comment
   "  "
   n_forced,t
   n,s,spindle_on
   n,rapid_move,absolute_coord,force_x,xr,force_y,yr,rotary_xyr_angle,
   n,rapid_move,length_offset
   output_rotary_angle
  
4. Null tool change
   "  "
   system_comment
   feature_name_comment
   "  "
   n,s
   n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angle,
   "  "
   output_rotary_angle
  
5. End of file for non-zero tool
   n,spindle_off
   n,end_of_file

  
6. 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)"

  
11. Cancel cutter compensation
   "G40"

  
12. Cutter compensation left
   "G41",d_offset

  
13. Cutter compensation right
   "G42",d_offset

  
14. Tool length compensation
   force_z,zr

  
20. Spindle speed low range
  
21. Spindle speed high range
  
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.
   program_block_8
  
50. Line first rapid move Z.
   rigid_tapping_end
   program_block_11
   n,rapid_move,zr

51. Line feed move Z.
   program_block_9
   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.
   program_block_10

  
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.
   n,g_arc_move,x_f,y_f,arc_center,feed_rate

  
71. End of 2axis cutting.
   program_block_20
  
73. High speed peck drill canned cycle.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,reference_plane,peck_drill_increment,canned_feed_rate

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

  
76. Fine boring canned cycle.
   rigid_tapping_start
   n,g_canned_cycFle,g98_g99,x_f,y_f,drill_depth,reference_plane,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,reference_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,reference_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,reference_plane,peck_drill_increment,canned_feed_rate

  
84. Tapping canned cycle.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,x_f,y_f,drill_depth,reference_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,reference_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,reference_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,reference_plane,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,reference_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,reference_plane,dwell,canned_feed_rate

  
90. Canned cycle drill point format WITH SUBPROGRAMS.
   n,x_f,y_f

  
91. Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
92. Canned cycle drill point format for standard drill canned cycle with dwell NO SUBPROGRAMS.
   n,x_f,y_f

  
93. Canned cycle drill point format for peck drill canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
94. Canned cycle drill point format for tapping canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
95. Canned cycle drill point format for boring cycle #1 canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
96. Canned cycle drill point format for boring cycle #2 canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
97. Canned cycle drill point format for back boring cycle canned cycle NO SUBPROGRAMS.
   n,x_f,y_f

  
98. Canned cycle drill point format for boring cycle #1 canned cycle with dwell NO SUBPROGRAMS.
   n,x_f,y_f

  
99. Canned cycle drill point format for boring cycle #2 canned cycle with dwell NO SUBPROGRAMS.
   n,x_f,y_f

  
100. Absolute coordinate output.
   absolute_coord

  
101. Incremental coordinate output.
   incremental_coord

  
110. Tool list format.
   "(MTOOL","T",list_tool_number,"S1","D",tool_diameter,"H",tool_length,"DIAM_OFFSET ",list_tool_number,"= ",tool_radius,")"

  
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

  
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 G and M codes? 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? 100

  
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? n

  
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? 24000

  
430. Maximum spindle speed? 24000

  
431. Spindle speed for high rangle? 24000

  
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? n

  
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

  
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"

  
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?				"MACH 3"

  
647. Machine model?				"ROUTER"

  
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"

  
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? "G87"

  
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? "G59 P1"

  
907. Work shift #8? "G59 P2"

  
908. Work shift #9? "G59 P3"

  
909. Work shift #10? "G59 P4"

  
910. Work shift #11? "G59 P5"

  
911. Work shift #12? "G59 P6"

  
912. Work shift #13? "G59 P7"

  
913. Work shift #14? "G59 P8"

  
914. Work shift #15? "G59 P9"

  
915. Work shift #16? "G59 P10"

  
916. Work shift #17? "G59 P11"

  
917. Work shift #18? "G59 P12"

  
918. Work shift #19? "G59 P13"

  
919. Work shift #20? "G59 P14"

  
920. Work shift #21? "G59 P15"

  
921. Work shift #22? "G59 P16"

  
922. Work shift #23? "G59 P17"

  
923. Work shift #24? "G59 P18"

  
924. Work shift #25? "G59 P19"

  
925. Work shift #26? "G59 P20"

  
926. Work shift #27? "G59 P21"

  
927. Work shift #28? "G59 P22"

  
928. Work shift #29? "G59 P23"

  
929. Work shift #30? "G59 P24"

  
930. Work shift #31? "G59 P25"

  
931. Work shift #32? "G59 P26"

  
932. Work shift #33? "G59 P27"

  
933. Work shift #34? "G59 P28"

  
934. Work shift #35? "G59 P29"

  
935. Work shift #36? "G59 P30"

  
936. Work shift #37? "G59 P31"

  
937. Work shift #38? "G59 P32"

  
938. Work shift #39? "G59 P33"

  
939. Work shift #40? "G59 P34"

  
940. Work shift #41? "G59 P35"

  
941. Work shift #42? "G59 P36"

  
942. Work shift #43? "G59 P37"

  
943. Work shift #44? "G59 P38"

  
944. Work shift #45? "G59 P39"

  
945. Work shift #46? "G59 P40"

  
946. Work shift #47? "G59 P41"

  
947. Work shift #48? "G59 P42"

  
948. Work shift #49? "G59 P43"

  
949. Work shift #50? "G59 P44"

  
950. Work shift #51? "G59 P45"

  
951. Work shift #52? "G59 P46"

  
952. Work shift #53? "G59 P47"

  
953. Work shift #54? "G59 P48"

  
954. Work shift #54? "G59 P49"

  
955. Work shift #55? "G59 P50"

  
956. Work shift #56? "G59 P51"

  
957. Work shift #57? "G59 P52"

  
958. Work shift #58? "G59 P53"

  
959. Work shift #59? "G59 P54"

  
960. Work shift #60? "G59 P55"

  
961. Work shift #61? "G59 P56"

  
962. Work shift #62? "G59 P57"

  
963. Work shift #63? "G59 P58"

  
964. Work shift #64? "G59 P59"

  
965. Work shift #65? "G59 P60"

  
966. Work shift #66? "G59 P61"

  
967. Work shift #67? "G59 P62"

  
968. Work shift #68? "G59 P63"

  
969. Work shift #69? "G59 P64"

  
970. Work shift #70? "G59 P65"

  
971. Work shift #71? "G59 P66"

  
972. Work shift #72? "G59 P67"

  
973. Work shift #73? "G59 P68"

  
974. Work shift #74? "G59 P69"

  
975. Work shift #75? "G59 P71"

  
976. Work shift #76? "G59 P72"

  
977. Work shift #77? "G59 P73"

  
978. Work shift #78? "G59 P74"

  
979. Work shift #79? "G59 P75"

  
980. Work shift #80? "G59 P76"

  
981. Work shift #81? "G59 P77"

  
982. Work shift #82? "G59 P78"

  
983. Work shift #83? "G59 P79"

  
984. Work shift #84? "G59 P80"

  
985. Work shift #85? "G59 P81"

  
986. Work shift #86? "G59 P82"

  
987. Work shift #87? "G59 P83"

  
988. Work shift #88? "G59 P84"

  
989. Work shift #89? "G59 P85"

  
990. Work shift #90? "G59 P86"

  
991. Work shift #91? "G59 P87"

  
992. Work shift #92? "G59 P88"

  
993. Work shift #93? "G59 P89"

  
994. Work shift #94? "G59 P90"

  
995. Work shift #95? "G59 P91"

  
996. Work shift #96? "G59 P92"

  
997. Work shift #97? "G59 P93"

  
998. Work shift #98? "G59 P94"

  
999. Work shift #99? "G59 P95"

  



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_rate


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


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


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_angle,drill_depth,reference_plane,peck_drill_increment,canned_feed_rate
 

171. Left handed tapping canned cycle.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_angle,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_angle,drill_depth,reference_plane,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_angle,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_angle,drill_depth,reference_plane,dwell,canned_feed_rate


176. Peck drill canned cycle.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_angle,drill_depth,reference_plane,peck_drill_increment,canned_feed_rate


177. Tapping canned cycle.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_angle,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_angle,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_angle,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_angle,drill_depth,reference_plane,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_angle,drill_depth,reference_plane,dwell,canned_feed_rate


182. Boring cycle #2 canned cycle with dwell.
   rigid_tapping_start
   n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_angle,drill_depth,reference_plane,dwell,canned_feed_rate

 
183. Canned cycle drill point format for standard drill canned cycle NO SUBPROGRAMS.
273. Output programmable rotary axis codes? y

690. Prefix for X Rotation Move? "A" 

64. Arc move XY.
   program_block_7

65. Arc move YZ.
   program_block_7

66. Arc move XZ.
   program_block_7
   
640. Prefix for arc Z center? "K"
691. Prefix for XY Machining Plane? "G17"
692. Prefix for XZ Machining Plane? "G18"
693. Prefix for YZ Machining Plane? "G19"

2007.
'**********************************************************************
'  Min Arc Length Check 2009/10/20 by Steve Spodaryk
'
'  Based on: Max Arc Check 2009/09/15 by Chris R. (Bird)
'
'  Purpose: Any VERY small arc segments will be converted to a
'  straight line movement (G01) to avoid problematic "crop circles".
'
'  Experience seems to indicate that arcs smaller than .001" are a
'  potential problem for many controllers, and are interpreted as full
'  circles.
'
'  - Choose the min size by modifying the arcMinLength below.
'  - Set inchUnits = 0, if you are using MM for your CAD/CAM units
'
'  For installation instructions and more history about this problem:
'
'  http://www.cnczone.com/forums/bobcad...p-circles.html
'  Installation and scripts in posts 44, 51, 56, etc
'
'***********************************************************************

dim PI
dim arcMinLength
dim arcRadius
dim arcAngleDegrees
dim arcPlane
dim arcLength
dim inchUnits

' These variables should be included in each code section
TAB_ENABLED = 0
SMALL_TAB_ENABLED = 1
LARGE_TAB_ENABLED = 2
FINAL_DOC = 0
TAB_HEIGHT = 1
GREATER_THAN = 2
LESS_THAN = 3
MIN_UNIT = 4
UNIT_INTERVAL = 5
MEMORY_LOC_CONTOUR = 100
START_OF_CONTOUR = 1.0
NO_CONTOUR = 0.0
PI = 3.141592653589793

arcRadius = MILL_GetArcRadius()
arcPlane = MILL_GetArcMachiningPlane()

' if this is METRIC, units are based on MM
inchUnits = 1						' set to 1, for inches
if inchUnits = 0 Then 				' MILL_GetUnits() does not work as expected
	' this conversion should not be necessary, but is currently required
	arcAngleRadians = MILL_GetArcAngleDegrees() / 25.4
	arcMinLength = 0.0635			' units in MM
Else
	arcAngleRadians = MILL_GetArcAngleDegrees()
	arcMinLength = 0.0025			' units in inches
End If

' calculate degrees and overall arc length
arcAngleDegrees = arcAngleRadians * 180.0 / PI
arcLength = (arcAngleDegrees/360.0)*(2.0*PI*arcRadius)

If 1 Then
	MILL_OutputText("(DEBUG: units="&MILL_GetUnits()&")")
	MILL_OutputText("(DEBUG: radius="&MILL_MakeRealString(arcRadius)&", degrees="&MILL_MakeRealString(arcAngleDegrees)&", radians="&MILL_MakeRealString(arcAngleRadians)&")")
	MILL_OutputText("(DEBUG: arcLength="&MILL_MakeRealString(arcLength)&", minLength="&MILL_MakeRealString(arcMinLength)&")")
End If

'check the length of the arc, calculated as a fraction of circumference
If arcLength < arcMinLength Then

	'Make it a straight line vector
	MILL_OutputText("(*** Arc too small ["&MILL_MakeRealString(arcLength)&"], use G01 instead ***)")
	MILL_ProcessPostLine("n,feed_move,x_f,y_f,z_f,feed_rate") 

ElseIf arcPlane = 0 Then 'XY Plane Output

	' This was some experimental code to create tabs on arcs
	' Instead, just process the post and continue

	MILL_ProcessPostLine("n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate")

ElseIf arcPlane = 1 Then 'YZ Plane Output

	MILL_ProcessPostLine("n,g_arc_plane,g_arc_move,y_f,z_f,arc_center,feed_rate")

ElseIf arcPlane = 2 Then 'XZ Plane Output

	MILL_ProcessPostLine("n,g_arc_plane,g_arc_move,x_f,z_f,arc_center,feed_rate")
	
End If

2008. 
'
' Start of 2 axis contour
' Output some values for debugging
'
If 1 Then
	MILL_OutputText("(********************************)")
	MILL_OutputText("(*** Start of 2 axis contour)")

	MILL_OutputText("(*** PassName: "&MILL_GetPassName()&")")
	MILL_OutputText("(*** SequenceNumber: "&MILL_MakeRealString(MILL_GetSequenceNumber())&")")
	MILL_OutputText("(*** OperationType: "&MILL_MakeRealString(MILL_GetOperationType())&")")

	MILL_OutputText("(*** NumberOfFeatures#: "&MILL_MakeRealString(MILL_GetNumberOfFeatures())&")")
	MILL_OutputText("(*** FeatureNumber: "&MILL_MakeRealString(MILL_GetCurrentFeatureNumber())&")")
	MILL_OutputText("(*** FeatuerType: "&MILL_MakeRealString(MILL_GetFeatureType())&")")

	MILL_OutputText("(*** NumberOfContours: "&MILL_MakeRealString(MILL_GetNumberOfContours())&")")
	MILL_OutputText("(*** CurrentContourNumber: "&MILL_MakeRealString(MILL_GetCurrentContourNumber())&")")
	MILL_OutputText("(*** NumberOfContourEntities: "&MILL_MakeRealString(MILL_GetNumberOfContourEntities())&")")
	MILL_OutputText("(*** CurrentContourEntityNumber: "&MILL_MakeRealString(MILL_GetCurrentContourEntityNumber())&")")

	MILL_OutputText("(*** NumberOfIntMemoryLoc: "&MILL_GetNumberOfIntMemoryLoc&")")
	MILL_OutputText("(*** NumberOfDoubleMemoryLoc: "&MILL_GetNumberOfDoubleMemoryLoc&")")
	MILL_OutputText("(*** NumberOfStringMemoryLoc: "&MILL_GetNumberOfStringMemoryLoc&")")
	MILL_OutputText("(********************************)")
End If


2009.
'
' Line feed move Z
'    n,feed_move,z_f,feed_rate
'

' This is called when a Z movement is performed.  If tabs are enabled, and the current Z level
' is equal to the final DOC, then it's time to add tabs.  We'll set 
' MEMORY_LOC_CONTOUR = START_OF_CONTOUR, and the XY movement routine will handle the tabs.
'

' These variables should be included in each code section
TAB_ENABLED = 0
SMALL_TAB_ENABLED = 1
LARGE_TAB_ENABLED = 2
FINAL_DOC = 0
TAB_HEIGHT = 1
GREATER_THAN = 2
LESS_THAN = 3
MIN_UNIT = 4
UNIT_INTERVAL = 5
MEMORY_LOC_CONTOUR = 100
START_OF_CONTOUR = 1.0
NO_CONTOUR = 0.0
PI = 3.141592653589793

MILL_SetDoubleMemoryLoc MEMORY_LOC_CONTOUR, NO_CONTOUR

If MILL_GetUserCheckBoxVariable(TAB_ENABLED) And _
	(MILL_GetUserCheckBoxVariable(SMALL_TAB_ENABLED) Or _
	MILL_GetUserCheckBoxVariable(LARGE_TAB_ENABLED)) Then

	If MILL_GetZFeed() < MILL_GetPreviousZFeed() Then
		' downward movement
		If MILL_GetZFeed() = MILL_GetUserEditRealVariable(FINAL_DOC) Then
			' final DOC
			MILL_OutputText("(*** Downward ZFeed: Contour Final Pass ***)")
			MILL_SetDoubleMemoryLoc MEMORY_LOC_CONTOUR, START_OF_CONTOUR
		End If
	ElseIf MILL_GetZFeed() > MILL_GetPreviousZFeed() Then
		MILL_OutputText("(^^^ Upward Z Feed ^^^)")
	Else
		MILL_OutputText("(--- No Z Change ---)")
	End If

End If

2010.
'
 Trap the XY Feed moves (G01)
'
' If we have the start of a contour, then this is the first linear move
' Find the breakpoints, and create a small tab at each point
'
' One limitation is that this only looks to create a tab on the final pass.
' If you are doing many small downward Z movements, we're not enforcing a tab
' until the final pass.  This could be corrected, but isn't necessary for my use.
'

' These variables should be included in each code section
TAB_ENABLED = 0
SMALL_TAB_ENABLED = 1
LARGE_TAB_ENABLED = 2
FINAL_DOC = 0
TAB_HEIGHT = 1
GREATER_THAN = 2
LESS_THAN = 3
MIN_UNIT = 4
UNIT_INTERVAL = 5
MEMORY_LOC_CONTOUR = 100
START_OF_CONTOUR = 1.0
NO_CONTOUR = 0.0
PI = 3.141592653589793

 MILL_OutputText("(*** Line Feed XY Move ***)")
If MILL_GetDoubleMemoryLoc(MEMORY_LOC_CONTOUR) = START_OF_CONTOUR And _
	(MILL_GetUserCheckBoxVariable(LARGE_TAB_ENABLED) Or _
	MILL_GetUserCheckBoxVariable(SMALL_TAB_ENABLED)) Then

	prevX = MILL_GetPreviousXFeed()
	prevY = MILL_GetPreviousYFeed()
	currX = MILL_GetXFeed()
	currY = MILL_GetYFeed()
	
	'slope = (currY - prevY) / (currX - prevX)
	'yIntercept = currY - (slope * currX)
	
	finalDOC = MILL_GetUserEditRealVariable(FINAL_DOC)
	tabHeight = finalDOC + MILL_GetUserEditRealVariable(TAB_HEIGHT)
	toolDiameter = MILL_GetToolDiameter()
	length = Sqr(Abs(currX - prevX)^2 + Abs(currY - prevY)^2)
	
	makeTabs = 0
	minLength = MILL_GetUserEditRealVariable(GREATER_THAN)
	maxLength = MILL_GetUserEditRealVariable(LESS_THAN)
	If MILL_GetUserCheckBoxVariable(SMALL_TAB_ENABLED) And _
		(length >= minLength And length <= maxLength) Then
		makeTabs = 1
		interval = length / 2
	ElseIf MILL_GetUserCheckBoxVariable(LARGE_TAB_ENABLED) Then
		minLength = MILL_GetUserEditRealVariable(MIN_UNIT)
		interval = MILL_GetUserEditRealVariable(UNIT_INTERVAL)
		If interval = 0.0 Then
			interval = length
		End If
		If length >= minLength Then
			makeTabs = 1		
		End If
	End If
	
	If 1 Then
		MILL_OutputText("(*** length: "&MILL_MakeRealString(length)&")")
		MILL_OutputText("(*** minLength: "&MILL_MakeRealString(minLength)&")")
		MILL_OutputText("(*** makeTabs: "&MILL_MakeRealString(makeTabs)&")")
		MILL_OutputText("(*** slope: "&MILL_MakeRealString(slope)&")")
		MILL_OutputText("(*** yIntercept: "&MILL_MakeRealString(yIntercept)&")")
	End If
	
	If makeTabs And length > (toolDiameter * 2) Then
	
		' Find angle of line relative to orgin (currX, currY) in degrees 0-360
		' We perform these tests to avoid divide by 0 errors when performing the trig functions
		If currX = prevX Then
			If currY > prevY Then 
				angle = 90.0
			Else 
				angle = 270.0
			End If
		ElseIf currY = prevY Then
			If currX > prevX Then 
				angle = 0.0
			Else 
				angle = 180.0
			End If
		Else
			' find the actual angle (relative to x orgin) based on quadrant.			
			If currX > prevX And currY > prevY Then
				angle = Atn((currY-prevY)/(currX-prevX))*180/PI
			ElseIf currX < prevX And currY > prevY Then
				angle = 90.0 + Atn((prevX-currX)/(currY-prevY))*180/PI
			ElseIf currX < prevX And currY < prevY Then
				angle = 180.0 + Atn((prevY-currY)/(prevX-currX))*180/PI
			Else
				angle = 270.0 + Atn((currX-prevX)/(prevY-currY))*180/PI
			End If
		End If
		
		numSegments = CInt(length / interval)
		If numSegments < 2 Then
			numSegments = 2
		End If
		
		cosA = Cos(angle*PI/180)	' small optimization
		sinA = Sin(angle*PI/180)
		
		If 1 Then
			MILL_OutputText("(*** angle: "&MILL_MakeRealString(angle)&")")
			MILL_OutputText("(*** Cos: "&MILL_MakeRealString(cosA)&")")
			MILL_OutputText("(*** Sin: "&MILL_MakeRealString(sinA)&")")
			MILL_OutputText("(*** segments: "&MILL_MakeRealString(numSegments)&")")
		End If
		
		For I = 1 To numSegments-1
		
			r = (length/numSegments*I)	' another small optimization
		
			' Output the intermediate moves to create the tab
			MILL_OutputText("(*** Start Tab ***)")
			MILL_SetXFeed(prevX + (r-toolDiameter) * cosA)
			MILL_SetYFeed(prevY + (r-toolDiameter) * sinA)
			MILL_ProcessPostLine("n,feed_move,x_f,y_f,z_f,feed_rate") 

			MILL_SetZFeed(tabHeight)
			MILL_ProcessPostLine("n,feed_move,z_f,feed_rate") 

			MILL_SetXFeed(prevX + (r+toolDiameter) * cosA)
			MILL_SetYFeed(prevY + (r+toolDiameter) * sinA)
			MILL_ProcessPostLine("n,feed_move,x_f,y_f,z_f,feed_rate") 

			MILL_SetZFeed(finalDOC)
			MILL_ProcessPostLine("n,feed_move,z_f,feed_rate") 

			MILL_OutputText("(*** End Tab ***)")
			
		Next

		MILL_SetXFeed(currX)
		MILL_SetYFeed(currY)

	End If

End If

MILL_ProcessPostLine("n,feed_move,x_f,y_f,feed_rate")

2011.
'
' Z Rapid move
'
' A rapid Z movement signifys the end of tabbing for this particular profile
'

' These variables should be included in each code section
TAB_ENABLED = 0
SMALL_TAB_ENABLED = 1
LARGE_TAB_ENABLED = 2
FINAL_DOC = 0
TAB_HEIGHT = 1
GREATER_THAN = 2
LESS_THAN = 3
MIN_UNIT = 4
UNIT_INTERVAL = 5
MEMORY_LOC_CONTOUR = 100
START_OF_CONTOUR = 1.0
NO_CONTOUR = 0.0
PI = 3.141592653589793

If 1 Then
	MILL_OutputText("(*** 2011 ***)")
	MILL_OutputText("(*** ZFeed: "&MILL_MakeRealString(MILL_GetZFeed())&")")
	MILL_OutputText("(*** PreviousZFeed: "&MILL_MakeRealString(MILL_GetPreviousZFeed())&")")
	MILL_OutputText("(*** ZRapid: "&MILL_MakeRealString(MILL_GetZRapid())&")")
End If

If MILL_GetZFeed() = MILL_GetPreviousZFeed() Then
	MILL_SetDoubleMemoryLoc MEMORY_LOC_CONTOUR, NO_CONTOUR
End If

2012.
'
'
'
MILL_OutputText("(*** Lead In XY Move ***)")

2013.
'
'
'
MILL_OutputText("(*** Lead Out XY Move ***)")

2020.
'
' End of 2 axis cutting
'
If 1 Then
	MILL_OutputText("(********************************)")
	MILL_OutputText("(DEBUG: End of 2 axis cutting)")
	MILL_OutputText("(********************************)")
End If

[stevespo]

It looks to me like you've done everything correctly! The one thing that jumps out is that your post has this section that might be used for XY moves.
With Mach, it uses the 53 section, but I'm wondering if your Haas is using the 153 section? Do you have a 4th axis or a rotary table? Perhaps this is the problem.

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

Try changing the 153 block to include the call to the program_block_10 (2010)
The G01 parameters might not be compatible, but it should tell us if this is the culprit.

153. Line feed move XY.
   program_block_10

If you get an error above, then just try this one instead. It will insert some debugging which is enough to help.

153. Line feed move XY.
   program_block_20

[crossedout]

I'll try this as soon as I can.

With the post processor that I just posted, it was your mach post. I can't get it working. I haven't even tried mine again.
So, I'm using your sample part and your post and can't seem to get it working on my system.

Thank you again. I'll reply as soon as I can.

[crossedout]

I tried both ways and got the same results (the post code that I posted earlier).

Like I said, though, this is using the files from your download. I haven't even gotten into the complication of getting mine to work. I can't think of anything special with my install of bobcad that would make things different.

Again, your help is very appreciated. If this can work, it will probably be exactly what I need. I cut alot of round objects, but it is only the parts with straight sides that I need to tab. So, that part is great.

Thanks again.
Brad

[crossedout]

If it is helpful, I'll post a shot of how simple our parts normally are.

We cut simple 2(.5) D parts out of .434 plates with a single roughing pass with a 3/8 end mill. That pass leaves a .030 web at the bottom. Then a 5/16 finisher comes thru and cuts that out. All of this is done on a magnetic table.

What I'm hoping you can help me accomplish is to be able to add tabs to this simple part. One tab on each flat end of part. This would allow us to eliminate this finish pass while still adding material that keeps the part from moving on the table.

In the image, you'll see a little bit of who I've set up the post processor to run duplicates of the same part.

I do hope you can help. Thank you very much for your help. I know we're all busy, so thank you for taking the time to help me get this working. (Or if you've got other ideas, thank you)

Attachment 242596

[jrmach]

"We cut simple 2(.5) D parts out of .434 plates with a single roughing pass with a 3/8 end mill. That pass leaves a .030 web at the bottom. Then a 5/16 finisher comes thru and cuts that out. All of this is done on a magnetic table. "



Man,you are putting a lot of time and effort in this.Do you have a ton of different parts ? If so,get the nesting.Otherwise,or even if you have lot's of different parts,,3D engrave is just soo easy to incorporate here.It will also give you complete control of the tool path.
If drawing simple 3D wireframe is something you would like help with,just ask.

[crossedout]

Man,you are putting a lot of time and effort in this.Do you have a ton of different parts ? If so,get the nesting.Otherwise,or even if you have lot's of different parts,,3D engrave is just soo easy to incorporate here.It will also give you complete control of the tool path.
If drawing simple 3D wireframe is something you would like help with,just ask.

Thank you for your input. Really, yes, we do a ton of these kind of parts (all different sizes and features). I have been trying out bobnest, but can't get a good trial of it. There are a number of reasons why I'm not using it and hesitant on using it:
1) We use V25 and are happy with it. To try the nesting I can only get a trial of V26 and I'd have to install it on a different computer (can't run it on the same v25 computer per technical support)
2) I can nest plates much more efficiently than bobnest - but I would like the speed of Bobnest, if it were more efficient.
3) About half of our parts have multiple features (chamfers, notches, bevels with a ball nose) and bobnest on it's own won't accommodate all of these without extra programming to run in addition to bobnest (done per part on the plate).
4) I already have 75% of incoming part orders programmed individually.
etc etc.

I would love it if bobnest would be able to overcome these issues. I would buy it in a heartbeat.

I haven't tried the 3d engrave. Are you saying that if I basically draw the tool path around the profile and add in the tabs (zaxis up), that the 3d engrave will follow that. Hmmm. Interesting.

Today, I was fulling around with using multiple features at different z depths to accomplish it - and ultimately it would, but it's still more work that I think it should be.

Thanks for your input. I just might take you up on asking for more information.

[jrmach]

"I haven't tried the 3d engrave. Are you saying that if I basically draw the tool path around the profile and add in the tabs (zaxis up), that the 3d engrave will follow that. Hmmm. Interesting.

Today, I was fulling around with using multiple features at different z depths to accomplish it - and ultimately it would, but it's still more work that I think it should be.

Thanks for your input. I just might take you up on asking for more information."



Yup,that is exactly what I am saying.