10LIONS

how do I remove A axis G28 from each toolpath

Recommended Posts

G0G55G90X-1.0591Y-2.5204A45.S4800M3
G43H1Z7.4462M8
G98G81Z1.2R1.5462F20.
X-8.5394
X-16.0197
X-23.5
X-30.9803
X-38.4606
X-45.9409
G80
M9
M5
G64
G0G28G91Z0.
G0G28X0.Y0.
G0G28A0. ****************I need to get rid of this line, except for the close of the prgm.

Hello, i'm trying to add the A fourth axis rotation to a generic Mazak 3 axis post which is 4 axis capable, I've succeeded accept  I don't

want the A to return home every tool change, only at the end of a program do I want the A axis to go home, i'm a newbie

so if you have an answer please explain it like your teaching a beginner, thanks for your help.

Share this post


Link to post
Share on other sites
1 hour ago, 10LIONS said:

Hello, i'm trying to add the A fourth axis rotation to a generic Mazak 3 axis post which is 4 axis capable

Which "base post" is it?

 

         

 

 

Share this post


Link to post
Share on other sites

[POST_VERSION] #DO NOT MOVE OR ALTER THIS LINE# V23.00 P0 E1 W23.00 T1592475229 M23.00 I0 O0
# Post Name           : MPMAZAKM
# Product             : MILL
# Machine Name        : GENERIC MAZAK
# Control Name        : GENERIC (M32/M-Plus/Fusion)
# Description         : GENERIC MAZAK EIA MILL POST
# 4-axis/Axis subs.   : YES
# 5-axis              : NO
# Subprograms         : YES
# Executable          : MP 9.13
#
# WARNING: THIS POST IS GENERIC AND IS INTENDED FOR MODIFICATION TO
# THE MACHINE TOOL REQUIREMENTS AND PERSONAL PREFERENCE.

 

i'm afraid this is all I can think of to give you, 

Share this post


Link to post
Share on other sites

(2.5 MM CARBIDE DRILL 4MM SHANK TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .098425)
T1T2M6
G0G55G90X-1.0591Y-2.5204A45.S4800M3
G43H1Z7.4462M8
G98G81Z1.2R1.5462F20.
G80
M9
M5
G64
G0G28G91Z0.
G0G28A0. ***********************This is the code that needs to be removed
M01
N2
G0G40G80G90G94G98
G0G28G91Z0.
(M3 X .05 TAP TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .118)
T2T1M6
G0G55G90X-1.0591Y-2.5204A45.S1000M3
G43H2Z6.M8
G98G84Z1.1R1.5462F.0198
G80
M9
M5
G64
G0G28G91Z0.
G0G28X0.Y0.
G0G28A0. ***********************obviously this one kept   ( this is a better example than my first, thanks)
M30

 

Share this post


Link to post
Share on other sites
1 hour ago, 10LIONS said:

i'm afraid this is all I can think of to give you, 

Looks like Mpmaster, to confirm this look at the Revision Log just below the Header above. If it has IHS and dates it is an IN House Solutions Mpmaster post, or at least started that way.

The post blocks which control the output you are interested in are pretract which outputs the code at tool change events, pretract0 which outputs at null tool change events (operation change but tool is the same) and peof which outputs at end of file.

The line you are looking for should look something like this:

       

      pbld, n$, *sg28, protretinc, e$

This is the output line for G28 A0 and it looks like some one has added in a reiterated forced G0, there are several ways of doing this.

Comment out this line in pretract and pretract0. To do this use # at the beginning of the line.

  • Thanks 1

Share this post


Link to post
Share on other sites
5 hours ago, 10LIONS said:

i'm afraid this is all I can think of to give you, 

So it is actually a CNC generic post, I am not as familiar but should be OK.

if rot_on_x, pbld, n$, *sgcode, *sg28, protretinc, e$      *****************( not sure how to arrange this line, if at all)

#if rot_on_x, pbld, n$, *sgcode, *sg28, protretinc, e$      *****************( not sure how to arrange this line, if at all)

Add the # at the front of the line in pretract and pretract0, this will prevent the G0 G29 A0 line from being output at toolchange.

Try reposting after the edit and see where you are.

In mpmaster there is a similar line  in peof which should output the line at the end of the program, if not you might have to insert it.

One step at a time will prevent back tracking.

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

  • 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