Starting mid program when running g-code, VTC200B

[naytep]

I only program g-code because I dont like all the limitations of the Fusion Mazatrol format. But it seems to limit me with the g-code also. I cannot start mid program when running in g-code format. Is there a way around this?
With my fanuc machines I merely put the curser on the line before the tool change and hit start. The control reads the offset and runs the program. Cant do with mazatrol.
In an unrelated question I have a post for my 99 VTC200B from Gibbs as well as several out of Postehaste. However all of them require some editing in order to get the mazatrol to read it. I have tried modifying a few templates but no luck yet. Does anyone have a gibbs or posthaste post that works with there vtc-200B?

[jimiscnc]

Two ways - modal and non-modal.

non-modal - select the PROGRAM MONITOR display. It looks identical to the program editor display. In auto mode, there should be restart softkeys - cursor down to where you want to restart and hit go.

Modal - In auto, on the position page, there is a restart softket to the right. It gives you a dialog window -

[1] Work No. - just hit input unless dealing with a sub
[2] Sequence No. - N word you want to point to
[3] Block No - lines from the N word you want to restart at
repeat number - how deep you are nested in a sub program - usually 0

QUIRK - will MODALLY RESTART everything fro mwher eyou dial it in, EXCEPT for SPINDLE START.

Technique - MDI mode - S2000M3 to start the spindle by program, then go to memory and do the modal restart.

practive this repeatedly - the TWO RESTARTS on a mazatrol fusion are both BEAUTIFUL! - the thing not as beautiful is the unfortunate choice of words "block" and "sequence" - which do not mean the same as what an American CNC programmer takes them to mean!

good luck

another quirk - if you moved the slides, they move from point in space to program position by manual feed rate over ride setting until its where the program wants it to be, then program FR will take over once it's read again - which is why practice is good.

GOOD LUCK!

Jim

[culminater]

from command screen right menu key eia moniter cursor dto the block i want and restart nonmodal start only from the beginning of a tool also add G90 G80 G40 G0
BEFORE TOOL CHANGE
THIS IS ON M PLUS CONTROL