Block Numbers at Tool Changes Only?

[tsewyek]

Hi All,

 

How difficult would it be in my post, to add block numbers at the tool changes only? I am attempting this with a modified Mazak Post, programming for an old H500 Horizontal Mazak.

Thanks in advance to all that reply and have a great weekend!

[cg777]

not difficult at all,

 

but i'll leave this to someone whoes been playing

with there post recently.

 

i'm just getting back on mc, it's been a little wile. i'm sure you will have your answer shortly.

[Allan Brown]

Turn omitseq to yes at the top of your post.

 

Find your tool call line

 

e.g.

change this:

n, *t, "M6", e

 

to this:

*n, *t, "M6", e

 

add a * before the n.

Starting number and increment are set by the Mastercam parameters, but can be override with n, seqno, and seqinc variables depending and where you place them.

[Guest CNC Apps Guy 1]

... and if you really want to get trick, you can make your line numbers match your Tool Number by putting "n=t" the line before your toolchange and off the left margin.

[tsewyek]

Thanks Again, You Guys Are the Greatest!

[Reece L Gibson]

Be careful when you do James trick on a Lathe post using Canned Cycles. P and Q may not match in the G71 command. Other wise it is a slick trick.

[Guest CNC Apps Guy 1]

quote:

---

Be careful when you do James trick on a Lathe post using Canned Cycles. P and Q may not match in the G71 command. Other wise it is a slick trick.

---

+100

 

I should have said, "Don't do this with Lathe".