counter question

[Rick Henrickson 65]

I got the counter working with the N number and tool number

Start of tool 26 posts like this

N2600

I can't figure out how to get it to add the offset

like T26 offset G54

N2654

any ideas?

[Guest]

Try this

 

pbld, n$, no_spc, p_wcs, e$

[Rick Henrickson 65]

Ill give it a try

[Rick Henrickson 65]

I am not having any luck

here is the code

 

ptlchg_com #Tool change common blocks

pcom_moveb

c_mmlt$ #Multiple tool subprogram call

#ptoolcomment

n$ = t$+p_wcs #*100

#pbld, n$, no_spc, p_wcs, e$

 

I blocked the n$ first time and added your line under now I have it blocked and tried this

[Todd Tracey from Fastech]

Did you try it with the # sign removed from the line you added?

[crazy^millman]

Post lesson for you here.

 

# means do not read or use this information when posting. So you will need to add a line for what he has for move the # to included what he gave you.

 

HTH

[Guest]

I was thinking the p_wcs will probably output like such

 

N26G54

 

to drop the G

 

format a variable

wcs_no : 0

Then place this before that line

 

code:

---

wcs_no = p_wcs

pbld, n$, no_spc, wcs_no, e$

---

[Rick Henrickson 65]

thanks John I will try that

 

Crazy, I know the # doesn't read I just turned it off while Im working on it

[Rick Henrickson 65]

ok I did this

 

ptlchg_com #Tool change common blocks

pcom_moveb

c_mmlt$ #Multiple tool subprogram call

#ptoolcomment

n$ = t$*100

wcs_no:0

wcs_no = p_wcs

pbld, n$, no_spc, wcs_no, e$

 

still just get N2600

[Rick Henrickson 65]

wanted to get this back on the list

[brilu397]

What would happen if you removed the *100 from the "n$ = t$*100" line? It looks to me like the output should currently read "/ N260054".

[Rick Henrickson 65]

thats what i was hoping for then I would remove it. but it still posts n2600

[Tim Johnson]

Try;

 

wcs_no:0

wcs_no = (t$ * 100) + p_wcs

pbld, n$, no_spc$, wcs_no, e$

[Rick Henrickson 65]

man I still cant get this to work. where does the post get the Woff# from your view manager

[Tim Johnson]

Operation manager, click an operation, parameters, planes, click the work offset box, 0=G54, 1= G55, ect...

[Tim Johnson]

Sorry, p_wcs should be g_wcs

[Rick Henrickson 65]

I still cannot get this to work, anyone else doing this?

[Roger Martin from CNC Software]

# This code in the toolchange postblock ->

"==============", e$ #

"tool number = ", *t$, e$ #

"offset number = ", ~g_wcs, e$ #

n$ = (t$ * 100) + g_wcs

pbld, n$, *t$, sm06, e$

"==============", e$ #

 

 

Produces this output ->

==============

tool number = T26

offset number = G54

N2654 T26

==============

[Rick Henrickson 65]

Thank you very much for all the help