Old Dynapath, Old version of Mastercam Tool # format

[znegative]

Hi All.

New to Mastercam.

Have an older version...X8 mill level 1.

Have an old Dynapath control.

have been playing with the .pst file to get it the way I want.

Here is my issue:

I need to have my code for tools to be posted in this format: T0101.

T of course is for tool, the first two digits are the tool number and the last two digits are the length offset. (diameter offset is handled with D)

Can't figure out how to get the .pst file to do this...

So...I tried just changing the tool number when doing tool paths...but...it drops the leading 0. making 0101 into 101. Not what I want.

Anybody have any idea how to fix this?

 

[crazy^millman]

Will need to do a little bit of work for something of this nature for a mill post. I would look at a lathe post and use it to reverse engineer what you need.

[Colin Gilchrist]

You need to add a Format Statement, that formats 4, forced, integer digits.

 

fs 30 4 0l

 

Then edit the Format Assignment line for the Tool Number:

 

Fmt "T" 30 t$

 

Finally, just prior to output, form the Tool Number + Offset number.

 

t$ = (t$ * 100) + tloffno$

 

 

And, just for fun, add some error checking:

 

If t$ > 99 | tloffno$ > 99, result = mprint ("Tool or offset greater then 99 detected!")