mill program

[guydrisc]

i downloaded mpmaster.. it looks like a generic post and i have to go in and edit it.. the only problem is that i have no clue on how to edit a post processor program.. hahaha.. is there a website or anything that can teach me or lead me in the right direction?

[Goldorak]

you need this generic post: MPMASTER_OKUMA, ask your reseller


here an simple exemple of a clean G-code written by hand that work well

$T.MIN%
G15H1
/T1M6
S5000M3
G56G00X1Y1Z3H1M8
G81Z-.05R.1F2
X-1
Y-1
X1
G80G00Z15M9
X-15Y15
M2
%

it's about the cleanest you can get to simply drill 4 holes

[guydrisc]

Originally Posted by Goldorak you need this generic post: MPMASTER_OKUMA, ask your reseller here an simple exemple of a clean G-code written by hand that work well $T.MIN% G15H1 /T1M6 S5000M3 G56G00X1Y1Z3H1M8 G81Z-.05R.1F2 X-1 Y-1 X1 G80G00Z15M9 X-15Y15 M2 % it's about the cleanest you can get to simply drill 4 holes

is this a program that works on an OSP? it looks like a regular fanuc post.

[broby]

When it comes to simple "plain" programming... there is very little difference in the G-Code cycles used on the OSP controllers and the Fanuc controllers.
That is why you see a lot of comments regarding modifying the default fanuc post to suit an Okuma machine.

[guydrisc]

wat would be some of the differences be in a complex program?

[broby]

When referring to "Simple" programming, I am meaning plain ol XYZ moves, drilling, tapping canned cycles and the like.
Complex programming is referring to the use of system variables, macro calls, sub programming etc...
i.e. Fanuc subprograms are called using M98 Oxxxx (or something like that!) and the subroutines end with M99 to force a return to the calling program, where Okuma uses "CALL Oxxxx" to call a subprogram and RTS at the end to return to the calling program.
Fanuc use a lot of #100 type of variable names, where Okuma has user definable names like FEED=100 or ZPOS=23.22 etc... Okuma uses Common Variables on a Lathe such as V1..V32, on a mill they are VC1..VC(xx max defined by machine).
There are many similarities between the programming methods, you just have to be able to figure out what variables the programmer is using and how they are being used.
Mind you a good programmer will document there code for ease of reading anyway... don't you?!?
I hate coming across the really old programs that have no information as to where program zero is located, what tools are required etc... a lot of the time I just start over as it takes less time to reprogram than to work out the old crap.

Hope that helps a little.
Brian.

[Goldorak]

Originally Posted by guydrisc wat would be some of the differences be in a complex program?

the biggest difference between OSP and Fanuc is the OSP DON'T need home position, simply turn the power on and hit cycle start button

to get a Fanuc G-code to work on an OSP, you only got to change a few codes

be aware, on OSP the G56 is to call the tool length offset "H**"

the reference point is called by the G15H** in fanuc this will be G55 G56 G57...



i know that okuma's book are not really easy to read, they are very basic.

[guydrisc]

ya reading the okuma books dont really help much... theya re kinda broad and dont get to the point it seems like

[Algirdas]

Okuma manuals are intended to be read by educated CNC technicians. Programming in standard GM codes a.k.a. "NC" code is widely known. The same standard is for plasma cutters, for lasers, for CNC welding machnines, even for knitting and sewing machines.
If You want just start from beginning You have options:
1. use some CAM software to create a part programs
2. use sample to modify it. Carcase - start, end, tool change - is constant.
You will find brief explanation of all G,M codes listed on Okuma programming manuals.

[broby]

Originally Posted by Goldorak the biggest difference between OSP and Fanuc is the OSP DON'T need home position, simply turn the power on and hit cycle start button to get a Fanuc G-code to work on an OSP, you only got to change a few codes be aware, on OSP the G56 is to call the tool length offset "H**" the reference point is called by the G15H** in fanuc this will be G55 G56 G57... i know that okuma's book are not really easy to read, they are very basic.

The statement about HOW the machine is Homed, is not relevant to Programming but is good to know anyway.

It is VERY IMPORTANT that you understand the difference in the way Fanuc and Okuma call up tool length offsets and the way they call up Co-ordinate systems. Get it wrong and you may crash (if you are not paying attention that is ) either that or a lot of alarms.

Last statement is quite true for a lot of manuals on the market, not just Okuma manuals.

Could be why forums such as these are available... keep asking and I am sure we will keep answering.
Cheers
Brian.