Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

B-axis on Mazak 400y Integrex


Dixon113a
 Share

Recommended Posts

Hello, I am have a problem when I post. The code that I am get will not run in the machine this is the code

O1000 ( BEADFEEDER )

G20

( TOOL - 23 OFFSET - 23 )

( 2" FACE MILL )

G17 G53

M302

G28 Y0.

G28 U0. W0.

M200

M01

T2323.00 B40

G97 S850 M203

M250

B20.

M251

G126 X0. Y0. Z0. R0 S0.

G0 X4.8052 Y-3.6546 Z.9115

C90.

M9

the program stops at the G126 right after it locks the b-Axis with the 251. Can some one tell me what I am doing wrong thanks

Link to comment
Share on other sites

The macro for the G126 is likely giving you the problem. What is the error line at the bottom of the screen? Should either be black line or a red line. I think it should be red with some text. We have gone thru this a number of times-

 

Chime in here Harry, you helped me thru this one once before and we are still using your macro edits.

Link to comment
Share on other sites

Look in the parameters for the K constants - The numbers for the programs that are assigned to the g126 code are listed in the K values and it looks as though the machine doesn't recognize the g code as there is no entry to correspond to the macro. Send me an email directly and I will forward the information in .pdf

Link to comment
Share on other sites

On the parameters page, look for the cutting parameters for k1-96. In the column on the right hand side there are the parameters for k81-k88. This is where the g126 macro needs to be registered so that everytime you call a g126, it picks up the macro program. I suspect that the program is not registered. (This is an easy fix and I hope that this is it)

 

I have attached a file that I want you to load into the machine memory and call it

 

99999126

 

In one of the registers for k81-k88 (doesn't matter which one)

register 126 in the code column and the number column should contain 99999126

 

 

This should do the trick - by the way, you must call up the tool in a horizontal orientation - TXXXX.8 for this one to work right.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...