post help needed

[Sandybar]

We just bought a Fadal with a fanuc control. Fadal does not like the M6 tool change after the tool number. I simply want to get a genric fanuc post and convert all the M6 to be befoire the tool number. ie. M6 T1 not T1 M6.

 

I know this sounds simple but I'm aware that it is not as simple to change my post?

 

Please don't flame me I'm not asking for a post.

 

Thanks

[Jimmy Wakeford from Barefoot CNC]

If you open the post in a text editor look for "M06" or "M6" (whichever is coming out in nc.)

 

it will be in a line like:

*t$, "M06",e$

make it:

*t,e$

[connormac]

in psof$ and ptlchg$ change

 

pbld, n$, *t$, "M6", e$

to

 

pbld, n$, "M6" ,*t$, e$

[connormac]

Dang Jimmy you beat me while I was typing

[Sandybar]

thanks

 

I will try it.

[john316]

.

 

Jimmy's answer removes the M6. connormac's answer switched the order. I think he wanted the switch not the removal.

 

.

[connormac]

Make sure to make a back-up copy of your post before you start. HTH

[Jimmy Wakeford from Barefoot CNC]

I also left out psof$ change. Connormac has better readin skills, dangit!

[Sandybar]

OK I have the M6 T1 moved around, now I need to change my safe line and add a G53 Z0. How do I go about it? Do I just force the commet by putting in G53 Z0 on both the psof$ and ptlchg$

 

 

Thanks

[Guest]

Sandybar,

 

Where do you need that addition to the start of your program only?

 

If so, go into the psof section and add

 

pbld, n$, "G53 Z0.", e$

 

PLace it where you need it to output

[Sandybar]

Thanks John, That did the trick.

 

Now one more question. How do I get a safe block on every tool change?

[chris m]

Copy the whole f-ing mess into ptlchg and you'll get it like you want

[Sandybar]

Cool! That worked. Thank you everyone for your input.