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:

How to set G55 as default ?


megaman
 Share

Recommended Posts

I have been programming for a number of years but only getting into it full time in the last year. I recently programmed a part and missed the offset default of G54 in my program,  and it made it to the floor and crashed!  on the machine I programmed it uses G54 as a home to store the center of rotation for the trunnion  "A" and "c"  .

The only time we  should see G54 on the machine is when we use dynamic offsets 

image.png.a4549b32041a9227cb350702a7e46bf0.png

 When looking at a lot of code I missed that it was supposed to be G55 without any dynamic offset since this  was when I didn't  need any tilt or rotation . 

G55 is my  WCS. having this as a default would have saved me.

g55.jpg.16537bcef7471905580aedbe92b86123.jpg

 

Thanks for any feedback or constructive  criticism  in advance!!

Link to comment
Share on other sites
50 minutes ago, megaman said:

I have been programming for a number of years but only getting into it full time in the last year. I recently programmed a part and missed the offset default of G54 in my program,  and it made it to the floor and crashed!  on the machine I programmed it uses G54 as a home to store the center of rotation for the trunnion  "A" and "c"  .

The only time we  should see G54 on the machine is when we use dynamic offsets 

image.png.a4549b32041a9227cb350702a7e46bf0.png

 When looking at a lot of code I missed that it was supposed to be G55 without any dynamic offset since this  was when I didn't  need any tilt or rotation . 

G55 is my  WCS. having this as a default would have saved me.

g55.jpg.16537bcef7471905580aedbe92b86123.jpg

 

Thanks for any feedback or constructive  criticism  in advance!!

There are two ways to control this.

The first would be to go into your Planes Manager in Mastercam, and force all of the planes that you are using (WCS, T/C Planes), to use the same "manual" Work Offset Number. In this case, a setting of "1" is what you want, to force G55 for all Ops.

The other option will depend on what Post Processor you are using. There is an option in the MPMaster Posts called "Lock on 1st Work Offset", which reads the 1st Work Offset number, from the first Toolpath Operation, and then forces all Work Offset outputs to match that "initial number".

 

 

Link to comment
Share on other sites

You can Call your datums on your control.  You can call any loaded program for any datum.  In this case the loaded program is the same for the first three  datum then calls a different program for the last three datums.  So simple to scroll down on the control and enter four numbers after the M98P....all you need is the M99 on the last line of your posted program instead of the M30.

O1(PROGRAM CALL);
(6 datums 54,55,56,57,58,59);
G0G91G28Z0;
G28X0Y0;
G0G90G54M105;  example G0G90G54.1M105: on most fanuc controls highlight the item to ALTER type the ALTER information press ALTER
G05P0;
M98P1111;
M01;
M5;
G90;
G0G91G28Z0;
G28X0Y0;
G0G90G55M105;
G05P0;
M98P1111;
M01;
M5;
G90;
G0G91G28Z0;
G28X0Y0;
G0G90G56M105;
G05P0;
M98P1111;
M01;
G90;
G0G91G28Z0;
G28X0Y0;
G0G90G57M105;
G05P0;
M98P2222;
M01;
M5;
G90;
G0G91G28Z0;
G28X0Y0;
G0G90G58M105;
G05P0;
M98P2222;
M01;
M5;
G90;
G0G91G28Z0;
G28X0Y0;
G0G90G59M105;
G05P0;
M98P2222;
M01;
M5;
G05P0;
G0G91G28Z0.0M115;
G28X0.0Y0.0;
T14M6;
G0X2.5Y-2.5Z-2.5;
M84;
G49;
G90;
M30;

 


O1111 
(added three contour paths)
N1G20
N2G00G17G40G80G94G90
N3T14M06(0.249 FLAT ENDMILL)
N4G00G17G90X-1.2001Y.2786S20000M03
N5G43H14Z.25
N6M83
N7G94
N8G05P10000

...

N2348Z.25
N2349G05P0
N2350M05
N2351G91G00G28Z0.
N2352G28X0.Y0.
N2353M84
N2354G49
N2355G90
N2356M99

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...