Y home when tool change.

[B Whale]

How to modify my Mpmaster.pst to output G28 Y0. when every time tool change? it only output G28 Y0. when M30.

[Mgrenier]

Whale,

 

Open your post and go to the pretract post block and ad a line taht looks like this:

 

pbld, n," ", "G28", "X0.", "Y0.", protretinc, e

 

That line was in my original mpmaster post but I had to cancel it so I am not sure of the posted result. You might want to make a backup copy of your original post before editing your post.

 

Hope that helps,

[Rob Peirolo CNC Software]

B Whale,

It's in the postblock "pretract"

add the line-

 

pbld, n, "G28", "Y0", protretinc, e

 

If the post you have incorporates rotary, this line goes just before it sends the rotary home.

[Rob Peirolo CNC Software]

Sorry Marting, I have slow fingers today.

[B Whale]

ok ! it output when tool change, but there are 2 of G28 Y0. when M30!

 

 

G00 G17 G21 G40 G80 G90

T3 M06

G00 G90 G54 X-6. Y6. S6000 M03

G43 H3 Z10. M07

G98 G81 Z-.5 R1. F1200.

G80 M09

M05

G91 G28 Z0.

G28 Y0.

M01

 

 

T4 M06

G00 G90 G54 X-6. Y6. S15000 M03

G43 H4 Z10. M07

G98 G83 Z-6.5 R1. Q1. F1000.

G80 M09

M05

G91 G28 Z0.

G28 Y0.

G28 X0. Y0.

G90

M30

%

[Rob Peirolo CNC Software]

B Whale,

I kind of thought this was coming.

Look for a postblock called "peof" and see if the G28 line is being output there. If you see a G28 in that postblock, just put a number sign in front of the whole line to "comment it out" so to speak, and mastercam will ignore that line

[B Whale]

Thanks rob p,

doing that it only G28 Y0. wnen M30. without X0.!

[Rob Peirolo CNC Software]

B Whale,

In your post, anything that is in quotation marks is called a literal string and will be output exactly as in the quotes. If you want the X0. to be output, then I believe your line should read

pbld, n, "G28", "X0.", "Y0.",e

As lone as the information in that particular line is exactly the same every time (no variable information) you can use literal strings.