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
Re: YASNAC MX-3 post modification for tool changer
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
Anyway, give this one a try first
Re: YASNAC MX-3 post modification for tool changer
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
Last edited by L98FIERO; 01-20-2019 at 12:11 AM.
Reason: add video link
Re: YASNAC MX-3 post modification for tool changer
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
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
Last edited by The Engine Guy; 01-20-2019 at 03:11 PM.
Re: YASNAC MX-3 post modification for tool changer
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.
Re: YASNAC MX-3 post modification for tool changer
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