YASNAC MX-3 post modification for tool changer

I just got a 1989 Matsuura MC-510V with a YASNAC MX-3 control and need some advice on how to modify a post so it does tool changes as shown in the Operators Manual. I started with a FANUC 16M post which looks pretty close but I need the tool changes done differently, here is the sample from the manual

G17 G20 G40 G49 G80 G90
T1 M6(TOOL 1)
G0 G54 X2. Y2. T2 S100 M3 ............ (CALLS NEXT TOOL IN CAROUSEL)
...........
.............
G0 M9
G28 G91 Z0 M29 ......................... (M29 orients the carousel tool pocket for faster tool changes)
M6(TOOL 2)
G0 G54 X2. Y2. T0 S100 M3 ........ (CALLS TOOL 0, EMPTY SPINDLE)
............
............
G0 M9
G28 G91 Z0 M29
M6................................................ .. (takes tool out of spindle)
G28 G91 X0 Y0
M30

Optionally I'd like to put the first tool in the spindle to prevent the spindle taper being contaminated when fixtures are cleaned.

Anyone have a suggestion on how to do this or a post I can lift some code from?

I have modified a Fanuc 0M post as I don`t have a Fanuc 16M one but it should give you some G code that will be near what you want.

I have only done the first and last requests as I`m not just sure what is needed for the tool change, does the machine have to have a seperate command to clear the spindle before it can put the next tool in the spindle? Just asking as most machines will automatically clear the spindle when it gets an T* M06 command, let me know how near/far the attached Post is for your needs.
If you particularly want it done on a Fanuc 16M Post then Zip yours up and attach it to your reply and I will have a go with that for you :D
Anyway, give this one a try first :D :D

Regards
Rob

Thanks for posting that Rob, but what I'm trying to do is have the program call up the next tool right after the current tool change. It's a random select changer so the idea is to have the carousel move to the location of the next tool while the current one is running, the M29 at the end of the current tool orients the tool pocket vertically so that when the M6 is called the tool change is just a matter of the double arm simultaneously removing the tool from the spindle and the carousel pocket, rotating 180° and putting the respective tools in their locations.
Actually, my old(er) machine was an Om-c but with no tool changer so I already have that one, it just doesn't do tool changes and realistically, I haven't seen much difference between the OM-C and the 16M anyway. That might come back to bite me but I haven't seen an issue yet.
This isn't my machine but it's the same kind https://www.youtube.com/watch?v=60DosWs8kqw

OK, so it is a straight forward swing arm side carousel changer, have a look at this code for a simple 2D pocket + a drilled hole and let us know if it is now nearer what you want :D

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=YASNAC MC510 - 3XVMILL.MCH)
(MTOOL T1 S1 D10. H105. A0. C0. DIAM_OFFSET 1 = 5.)
(MTOOL T2 S1 D8. H100. A0. C0. DIAM_OFFSET 2 = 4.)
(MTOOL T3 S4 D4. H57.15 A118. C0. DIAM_OFFSET 3 = 2.)
(SBOX X-25.4 Y-25.4 Z-25.4 L50.8 W50.8 H25.4)
(END PREDATOR NC HEADER) Header can be easily removed if not required

%
O1234
(PROGRAM NUMBER)

(FIRST MACHINE SETUP - Machine Setup - 1)

(PROGRAM NAME - POCKET TEST_YASNAC-MOD.NC)
(POST - FANUC 0M MODIFIED FOR YASNAC MX-3)
(DATE - SUN. 01/20/2019)
(TIME - 10:58AM)

N10 G17 G20 G40 G49 G80 G90

N20 G00 G91 G28 Z0.
N30 G91 G28 X0. Y0.

(Machine Setup - 1 Pocket)
(SIMPLE POCKET+DRILL HOLE)

N40 T01 M06 ( 10mm 4FL End Mill Aluzip)
N50 G90 G54 X-5.29 Y-5.4875 T02 S4000 M03 ( Next tool is now being called on this line as you requested)
N60 G43 H01 Z30. M08
N70 Z5.
N80 Z2.
N90 G01 Z0. F568.96
N100 X-5.4875 Z-.0069
N110 Y-.4875 Z-.1815
N120 X-.4875 Z-.3561
N130 Y.4875 Z-.3902
N140 X2.075 Z-.4796
N150 Y-.4875 Z-.5137
N160 X-.4875 Z-.6032
N170 X2.075 Z-.6927
N180 Y.4875 Z-.7267
N190 X-.4875 Z-.8162
N200 Y-.4875 Z-.8502
N210 X-5.4875 Z-1.0248
N220 Y-5.4875 Z-1.1994
N230 X-2.5625 Z-1.3016
N240 X-5.4875 Z-1.4037
N250 Y-.4875 Z-1.5783
N260 X-.4875 Z-1.7529
N270 Y.4875 Z-1.787
N280 X2.075 Z-1.8765
N290 Y-.4875 Z-1.9105
N300 X-.4875 Z-2.
N310 X2.075 F1000.
N320 Y.4875
N330 X-.4875
N340 Y-.4875
N350 X-5.4875
N360 Y-5.4875
N370 X7.075
N380 Y5.4875
N390 X-5.4875
N400 Y-.4875
N410 X-10.4875
N420 Y-10.4875
N430 X12.075
N440 Y10.4875
N450 X-10.4875
N460 Y-.4875
N470 Y-10.4875
N480 X-15.4875
N490 Y-14.2875
N500 G17 G03 X-14.2875 Y-15.4875 I1.2 J0.
N510 G01 X15.875
N520 G03 X17.075 Y-14.2875 I0. J1.2
N530 G01 Y14.2875
N540 G03 X15.875 Y15.4875 I-1.2 J0.
N550 G01 X-14.2875
N560 G03 X-15.4875 Y14.2875 I0. J-1.2
N570 G01 Y-10.4875
N580 G00 Z5.
N590 Z30.
N600 M09
N610 M05
N620 G91 G28 Z0. M29 (End of operation Carousel call done as machine moves to Machine Z zero for tool change)
(Machine Setup - 1 Profile Finish)
(SIMPLE POCKET+DRILL HOLE)

N630 T02 M06 ( 8mm 4FL End Mill Aluzip)
N640 G90 G54 X6.758 Y14.307 T03 S4000 M03 (Tool change completed and next tool called as requested)
N650 G43 H02 Z30. M08
N660 G00 Z5.
N670 Z2.
N680 G01 Z-2. F284.48
N690 G41 D02 X4.258 Y18.638 F568.96
N700 G17 G03 X.794 Y20.638 I-3.464 J-2.
N710 G01 X-14.288
N720 G03 X-20.638 Y14.288 I0. J-6.35
N730 G01 Y-14.288
N740 G03 X-14.288 Y-20.638 I6.35 J0.
N750 G01 X15.875
N760 G03 X22.225 Y-14.288 I0. J6.35
N770 G01 Y14.288
N780 G03 X15.875 Y20.638 I-6.35 J0.
N790 G01 X.794
N800 G03 X-2.67 Y18.638 I0. J-4.
N810 G40 G01 X-5.17 Y14.307
N820 G00 Z5.
N830 Z30.
N840 M09
N850 M05
N860 G91 G28 Z0. M29 (End of operation Carousel call done as machine moves to Machine Z zero for tool change)
(Machine Setup - 1 Drill)
(STANDARD FEATURE MILL HOLE - 4.0000)

N870 T03 M06 ( 4.000 Dia.118.000 Deg. 8.202 CL)
N880 G90 G54 X-22.349 Y22.044 T01 S1891 M03 (Tool change completed and next tool called as requested)
N890 G43 H03 Z30. M08
N900 G00 Z5.
N910 G81 G98 X-22.349 Y22.044 Z-8.202 R2. F67.2762
N920 G00 Z30.
N930 M09
N940 M05
N950 G91 G28 Z0. M29 (End of operation Carousel call done as machine moves to Machine Z zero for tool change)
N960 G91 G28 X0. Y0.
N970 T01 M06 (This will do a tool change at the end of the program to put T01 back in the spindle so it is ready to run the program again)
N980 M30

(END OF PROGRAM)
%

Post attached that generated the above code.
Regards
Rob

Rob, that looks really good but, where do the 'next_tool_with_prefix' and 'first_tool_with_prefix' come from? Is it from the BcCamPostExe program that will not run on my Windows 7 computer? Also, the post you made will run with V31 but not with V30, both were used with old files that had already been run? I'd like to figure this out so I don't have to keep asking for help and maybe be able to help others instead.

All the stuff I have used comes from .PDF files that should be in your BobCAD-CAM Data folder, nothing to do with the Post .exe install program.

On my PC Win 7 Pro the path is :-

Computer> Local Disk ( C: ) > BobCAD-CAM Data > BobCAD-CAM V31 > Posts > Documentation (I used the .PDFs in the "Legacy" folder)

There you will find all the Variables, Advanced Posting, API References, Scripting References etc, etc.

I used V28 to generate the program/code as I only have the Demo of V31, I junked V29 and V30 as they were too "clunky" and "buggy", they took a long time to even load never mind compute 3D Mold toolpaths !!!

I have attached the little test program I did in V28 to prove the code out so you can see how it was setup, it should run OK in V31 for you and post out properly :D :D

Hope that`s of some help to you :D :D :D

Regards
Rob