how to add sequential block numbers before each operation

[Zoffen]

hello all,

 

i'm trying to get my post to add a sequential block number before each operation.

i.e. post a N1 before operation 1, a N2 before operation 2, etc.

is there anyway i can do this?

 

I am using a modified mpmaster post.

 

thanks a bunch!

[Zoffen]

lol,

 

looked through some posts here and figured it out so far.

 

if this is op 1 my post will now post: N 1

 

i want it to post N1

 

how do i make it not put in a space?

 

thanks!

[Zoffen]

nevermind, figured it out.

 

for anyone interested in how i did it:

 

sav_spc = spaces$

spaces$ = 0

pbld, "N",sOpSeqNo, e$

!op_id$

spaces$ = sav_spc

 

really beat my head against a wall for a while until i figured out the spaces$ variable controlled the spaces between stuff. DUH. My brain is fried.

[BernieT]

Good job !!

 

[TK-32™]

i have a bad habit that I can't shake off from my programming by hand days.

I got used to to having N100 for #1 op, N200 for #2 etc, I'm gonna try this tomorrow.

[Zoffen]

oh and i followed alot of stuff from the post trick thread that has recently been up.

 

http://www.emastercam.com/board/index.php?showtopic=59543

 

and also does anyone know where i could get some documentation on what the variables are called so i can access stuff from mastercam?

[Mr. Wizzard]

This was posted in another thread a few days ago. It's the most complete post editing documentation I have seen yet. Should give you everything you need.

Good luck.

 

 

ftp://ftp.mastercam.com/From%20Mastercam/rbb/MP_documentation.pdf

[BrianP.]

I have my post so that it only puts out N# at each tool with an M01 and the N# matches the tool number. Makes it real easy to get to certain tools when jumping around. Just type N# cursor down and there I am.

[ThRaSH]

This was posted in another thread a few days ago. It's the most complete post editing documentation I have seen yet. Should give you everything you need.

Good luck.

 

 

ftp://ftp.mastercam.com/From%20Mastercam/rbb/MP_documentation.pdf

 

The link no longer works? Does anyone have a download link for this?

[Mr. Wizzard]

The NCI & parameter reference and post debugger guide are on the mastercam site under support > downloads. I'm having trouble locating the complete MP Documentation file. It would be nice if it was placed on the top of the forum or with the MPMaster post download part. It is the most essential tool for editing and understanding posts, yet it seems as if it's always been hard to locate the info......

[Paul Decelles]

Contact your dealer, the download has been placed on our extranet (where it belongs). They can grab you a copy from there.

[Mic6]

I have my post so that it only puts out N# at each tool with an M01 and the N# matches the tool number. Makes it real easy to get to certain tools when jumping around. Just type N# cursor down and there I am.

 

+1, plus a saftey line, so no matter where my tool is, I can hit N3 (down arrow), cycle start and the tool will retract, move to position and start tool 3.

[Colin Gilchrist]

As a Tip for future reference: you can use the 'no_spc$' between output parameters to remove the space character. It is a little easier than saving the current value of 'spaces$', assigning 'spaces$' a value of zero, then reassigning the previous value after you have output your code.

 

Your modified line would look like this:

 

pbld, n$, no_spc$, sOpSeqNo, e$

[Zoffen]

As a Tip for future reference: you can use the 'no_spc$' between output parameters to remove the space character. It is a little easier than saving the current value of 'spaces$', assigning 'spaces$' a value of zero, then reassigning the previous value after you have output your code.

 

Your modified line would look like this:

 

pbld, n$, no_spc$, sOpSeqNo, e$

 

YES!

 

thats what i was looking for. i love learning things back assward!

 

thanks!

[Newbeeee™]

Go Colin go! Only been there a month and now you're flying

 

We have our post modded (thanks Phill @ 4D in the UK) so it outputs sequentially

N0101 (T1, 1st time called)

N0102 (T1, 2nd time called)

N1001 (T10, 1st time called) etc

 

Obviously we can only go to 99 tools with 99 calls, but heh!

It makes searching and starting mid program (or 1st thing in the morning after switching off overnight) a whole lot easier.

[BrianP.]

+1, plus a saftey line, so no matter where my tool is, I can hit N3 (down arrow), cycle start and the tool will retract, move to position and start tool 3.

 

Mic6 what type of safety line? If I stop in the middle of a program I immediately dial up and off the part so I have never had the need for one. I have had this discussion at my new place with one of the guys. At The start of all of their programs they have the lines:

G0G28G91Z0

G0G28G91Y0

G52X0Y0Z0

 

In my opinion wasted moves especially on a large machine with more than 30 inches of travel in both Z and Y. He stated that if he stops in a part he wants his first line to retract Z. I stated under no circumstance would I ever hit the cycle start button with a tool inside a part after stopping. Also this safety line is only at the start of the program so starting down at tool 3 or something it would be useless.