Sign in to follow this  
Leon82

Is it possible to get a comma to post after each block number?

Recommended Posts

Try changing your format for the N to N,

fmt  "N" 21 n$          #Sequence number

to

fmt  "N," 21 n$          #Sequence number

  • Like 2

Share this post


Link to post
Share on other sites
Just now, JParis said:

Try changing your format for the N to N,

fmt  "N" 21 n$          #Sequence number

to

fmt  "N," 21 n$          #Sequence number

Close, but not quite.

fmt  "N" 4  n$ ","

 

  • Like 3

Share this post


Link to post
Share on other sites
12 minutes ago, Zaffin said:

Close, but not quite.

fmt  "N" 4  n$ ","

 

Yup...that's what I get for working on the fly  :)

Share this post


Link to post
Share on other sites

Yes, as Zaffin pointed out, the Format Assignment function inside MP-based Posts was enhanced to allow you to output both a "Prefix String", and a "Suffix String". So you can output "string characters" before or after the numeric value being output.

I like to do this for outputting "Feed Variables". I like to output my Feeds as " F[#501] ", where the "F" value is called as a Permanent Common Variable.

Inside Mastercam, I enter "501." for the Feed, "502." for the Plunge rate, and "503." for the Retract Rate.

I have logic built into the Post to detect "Feedrates above 499", which will then "swap format assignments" on-the-fly. I also add some logic to check MR4, MR5, and MR6. I use these three MR values to pass along the actual "Feedrate value" which I want assigned to each variable.

At the start of a new Operation (Tool Change), I get something like this:

#501 = 130.
#502 = 200.
#503 = 500.

Which gives me a single place where I can change any of the Feed values (cut, plunge, or retract), and it will now read that variable value as part of the NC Code.

M01
N1(SEQUENCE #1.)
(TOOL# 5 - 0.1875 FLAT ENDMILL -  DIA. - .1875)
(MAX - Z-1.0519)
G0 G17 G40 G80
G00 G90 G53 Z0.
#501=130.
#502=200.
#503=500.
T5 M06
(FLATS)
G00 G17 G90 G54 X-2.4243 Y-1.1527 S9876 M03
G43 H5 Z2. M83
Z-.26
G01 Z-.31 F[#502]
X-2.425 Y-1.1525 Z-.3152
X-2.4269 Y-1.1519 Z-.32
X-2.4299 Y-1.1509 Z-.3241
X-2.4338 Y-1.1497 Z-.3273
X-2.4384 Y-1.1482 Z-.3293
X-2.4434 Y-1.1466 Z-.33
G02 X-2.4748 Y-1.134 Z-.3311 I.0697 J.218 F[#501]
X-2.5078 Y-1.1098 Z-.3324 I.0661 J.125
G03 X-2.537 Y-1.1108 Z-.3332 I-.0141 J-.0143
G01 X-2.5565 Y-1.1317 Z-.3333
G03 X-2.5563 Y-1.1582 I.0124 J-.0131
G01 X-2.5432 Y-1.1724
X-2.5263 Y-1.1907 Z-.3341
X-2.3937 Y-1.2583 Z-.3389
X-2.361 Y-1.2679 Z-.34

 

  • Thanks 1

Share this post


Link to post
Share on other sites

I had to delete the string n$ from the tool change line because I was getting 2 line numbers, one after the other.

Is there a different setting that outputs an N number on the tool change?

 

I have it set to output block numbers on all lines in the control def

Increment 1, start 1

 

 

 

Share this post


Link to post
Share on other sites

Hi Leon, I am not completely sure what sort of output you are looking for but if you are using an MPMASTER style post, I would point you towards tseqno in the general output settings at the top of the post.

tseqno      : 0     #Output sequence number at toolchanges when omitseq = yes
                    #0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number

  • Like 1

Share this post


Link to post
Share on other sites

Ok I'll look at it.

 

It is a generic fanuc post, it's been here for at least 10 years.

 

I only see a seq reference for knot sequence numbers CD var and it say no as I checked it to output them

Share this post


Link to post
Share on other sites

The last CNC software update to it was in 2005.

But what I am experimenting on is a manual entry test for camplete.

It uses what it calls a custom gcode label for manual entry.

 

So the format is

ME1, m00

ME2, (comment)

 

So instead of a sub program for probing or a dovetail op on the table wings it would output directly into the program via manual entry text file..

 

Camplete won't simulate it, but neither will a sub program.

 

 

 

 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us