[PhoenixMetal]

I'll just post this here to document a simple post modification that I worked up to make a working post for my Kitamura Mycenter 1 vertical machining center with Yasnac i80M controls...

Mastercam's "Generic Fanuc 3X Mill.PST" was almost perfect to run the machine. However with the generic post, my machine wouldn't do a tool change. I don't remember if it just sat there and did nothing, or if it had an alarm. Anyhow, the Kitamura requires that the Z axis is at home (zero) prior to a tool change. I'm guessing that some other machines automatically zero the z axis whenever a tool change is called.

So, a simple modification is needed to the generic post to make it work for the Kitamura / Yasnac. The post needs to tell the Z axis to go to zero prior to each tool change.

Here's how to do it:
Make a copy of the Generic Fanuc 3X Mill.PST and rename it for your machine. The file is located in [installation directory]\mill\posts.

Scroll down to the label "# Start of File and Toolchange Setup"

After the block that says:
if mi1$ <= one, #Work coordinate system
[
absinc$ = one
pfbld, n$, sgabsinc, *sg28ref, "Z0.", e$
pfbld, n$, *sg28ref, "X0.", "Y0.", e$
pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
absinc$ = sav_absinc
]

Add a new line that says:
n$, *sg28ref, "Z0.", e$ #Added by [insert your name here] to make toolchange work on Kitamura.

You should also add some comments to the header of the file describing the changes that you made. You can put comments anywhere - just start them with a '#'.

Thank god for those late nights learning programming as a computer science major back in college. I think I would have been totally lost otherwise, as the Mastercam post processor system is pretty complex.

Hope this helps and good luck!

[bearracecars]

Phoenixmetal

I was wondering is the post processor going to be the same as far as the i80m or is it going to machine specific with the i80m? Reason i am asking is because i just got a shizuoka mill that has the i80m controller on it. so until i can afford it, (mastercam) a friend of mine is going to do the cam for me. I talked to mastercam and they said "we'll do the post but run it tell us what doesn't work and what does then rewrite it and do it again. I'm trying not to impose on my friend that much. Being that he is extremely busy and he is doing this as a favor.


thanks
bear

[PhoenixMetal]

I'm guessing that the change I needed to make was specific to my particular combination of machine+control.

It is very possible that the Generic Fanuc 3X Mill.PST file will work fine for your machine. Unfortunately, I don't think there is any way to know for sure until you try it out and see if it works or not.

But in any case, so long as Mastercam (the company) will do the post modifications as needed, trying and testing through multiple iterations doesn't mean that you are necessarily imposing on your friend. Your friend only needs to do the Mastercam work once, and swapping out post processor files to regenerate the G-code is only a few mouseclicks each time.