Custom Macro?

[cncwhiz]

I cant seem to find the fanuc macro b forum. I think I recall that there was one here? I have a Hitachi Seiki HG400iii With a seicos controller on it. I have a macro program that I built that allows my retracts to be controlled by the system variable that stores work offsets. Mike Lynch gave me the system variable that works on a Hitachi seiki with a fanuc 15. The seicos has a fanuc system 10 running in the backround. I am calling the "#4014" system variable and it works great. The seicos controller must not be using this system variable as that it is just showing me a "67." and it is not changing. Does someone know the correct system variable or how to find it? I will drop a dime to Mike in the morning as well.

TIA

[dpuch]

http://www.cnczone.com/forums/parametric_programing/

It is a sub section of the G-code forum. A few lines down from the this one.

I do not see why you would not get the correct value from #4014 = G(54-59)
Do you have extended work offsets? Still that does not explain a 67 value.

We also have some Hitachi Seiki HG400iii's 1 with a 15 control, and 2 with the sigma 10 control. The sigma 10 is a Fanuc 16 (not 16i) with other software for the user interface and a few other things. Refer to a Fanuc 16 manual for reference information.

Variable number Function
#4001 G00, G01, G02, G03, G33 (Group 01)
#4002 G17, G18, G19 (Group 02)
#4003 G90, G91 (Group 03)
#4004 (Group 04)
#4005 G94, G95 (Group 05)
#4006 G20, G21 (Group 06)
#4007 G40, G41, G42 (Group 07)
#4008 G43, G44, G49 (Group 08)
#4009 G73, G74, G76, G80–G89 (Group 09)
#4010 G98, G99 (Group 10)
#4011 G50, G51 (Group 11)
#4012 G65, G66, G67 (Group 12)
#4013 G96,G97 (Group 13)
#4014 G54–G59 (Group 14)
#4015 G61–G64 (Group 15)
#4016 G68, G69 (Group 16)
: ::
#4022 (Group 22)
#4102 B code
#4107 D code
#4109 F code
#4111 H code
#4113 M code
#4114 Sequence number
#4115 Program number
#4119 S code
#4120 T code
#4130 P code (number of the currently selected additional workpiece coordinate system)

As I recall the 15 includes additional #4201-4320 for reading the same as above, but for the current block instead of preceding block.

Dale

[cncwhiz]

Your reply is a keeper in my inbox for sure. I just went down on the floor and built a simple program.

O1234
#105=#4001
M99

I started changing the 4001 number until I got to "#4012" and it output what I was looking for. This machine is oddball. It uses a "G841" for rigid tap an for extended work offsets it uses G540, G550 etc... Thanks for the list of system variables I will use them for sure.

[dpuch]

Well as long as you know what it is doing.
Hmm.. Well we do use the system setting Fanuc 15 compatibility mode.
See the last page of the programming book.
That accounts for some if not all of the G-code confusion I had.

[cncwhiz]

Which book is that in? I would love to re-format this control so I don't have to do extra post processor work just for this machine. The control has some pretty fancy stuff that my other controls don't have. Its almost like they tried to do what yasnac did with their controllers.

[dpuch]

The Hitachi programming manual for the sigma 10. The last page has Fanuc 15 system setting, and what it changes. I think it was something like 3409.7 <-- verify that!

I do use the same post for our 15 and 16 based Hitachi Seiki HG400iii's There probably are differences but I do not use any of those.

Bit 6 of the same one was for more of a Yasnak i80M compatibility.

[cncwhiz]

Ah yes, nothing like finding out all the countless hours of tweeking posts and making sure that you posted the correct code for this machine only to find out a parameter can un%$#* it . Its working now so if it is not broke don't fix it. I work with other programs that the developers thought too much and built a monster "pro engineer" like this control.

[sinha_nsit]

A pretty good reference material for 0i series controls:

http://www.mhprofessional.com/produc...sbn=0071713328

[fanuc-support.c]

Nice plug Sinha.

Here is my plug.

Free macro b variable tool download here.

http://www.fanuc-support.com/downloads.html

[sinha_nsit]

Originally Posted by fanuc-support.c Nice plug Sinha. Here is my plug. Free macro b variable tool download here. http://www.fanuc-support.com/downloads.html

I could not install it on my computer, though I was able to download it. I did follow the instructions, but it did not work.

Incidently, if you wish to use this book in your macro training course, send a mail to bulksales@mcgraw-hill.com, for quantity discount.