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:

Rotary axis positioning & 3 axis

wing

By wing,
in Post Processor Development Forum

 Share

Recommended Posts

wing Newbie

wing

Posted
Posted

How to fix bugs in postprocessors Mpmaster & Generic not work well if you use clearance only at the start and end of operation with rotary axis control

 

G00 G17 G21 G40 G80 G90

G91 G28 Z0.
T9 M06 (4.00 CENTER DRILL)
G00 G17 G90 G54 A0. X0. Y0. S1000 M03
G43 H9 Z45.
Z41.
G94
G99 G81 Z39.5 R41. F125.
A20.
A40.
A60.
A80.
A100.
A120.
A140.
A160.
A180.
A200.
A220.
A240.
A260.
A280.
A300.
A320.
A340.
G80
G91 G28 Z0.                                               here
G00 G90 G55 A340. X0. Y0.                   here 
G43 H9 Z41.                                               here
Z45.
M05
G91 G28 Z0.
G28 Y0. A0.
G90
M30
%

 

 

Use clearance only at the start and end of operation.Z2G

Link to comment
Share on other sites
wing Newbie

wing

Posted
  • Author
Posted

This is a problem in the standard postprocessors

Try to generate  NC program of standard postprocessors:

Generic Fanuc 4X Mill

Generic Fadal Format_1 4X Mill

mpmaster - i use him

Generic Haas 4X Mill

Generic Haas_Renishaw 4X Mill

MPFAN

Don't forget to set  miscellaneous values  to default values 

Link to comment
Share on other sites
Guest

Guest

Posted
Posted

This is a problem in the standard postprocessors

Try to generate  NC program of standard postprocessors:

Generic Fanuc 4X Mill

Generic Fadal Format_1 4X Mill

mpmaster - i use him

Generic Haas 4X Mill

Generic Haas_Renishaw 4X Mill

MPFAN

Don't forget to set  miscellaneous values  to default values 

And you will see this error in the standard postprocessors !!!

 

ptlchg0$ - calls it at the end of the program

 

Doesn't matter, your reseller should be your 1st point of contact for that kind of stuff

 

Your reseller in Spain should be able to get you in the right direction

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

This is a problem in the standard postprocessors

Try to generate  NC program of standard postprocessors:

Generic Fanuc 4X Mill

Generic Fadal Format_1 4X Mill

mpmaster - i use him

Generic Haas 4X Mill

Generic Haas_Renishaw 4X Mill

MPFAN

Don't forget to set  miscellaneous values  to default values 

And you will see this error in the standard postprocessors !!!

 

ptlchg0$ - calls it at the end of the program

 

What you call an error I call a safe move. Sending the machine home between indexes is the best method for safe running of a machine. If you want different behavior then you modify the post for the behavior you want. Calling it an error is wrong plain and simple. There are switches built into the post to allow someone to decide to turn it off/on based on their need or want.

  • Like 1
Link to comment
Share on other sites
wing Newbie

wing

Posted
  • Author
Posted

What you call an error I call a safe move. Sending the machine home between indexes is the best method for safe running of a machine. If you want different behavior then you modify the post for the behavior you want. Calling it an error is wrong plain and simple. There are switches built into the post to allow someone to decide to turn it off/on based on their need or want.

 
G91 G28 Z0.                                  This home posithion             -    ret_on_indx : 1  in mpmaster  
G00 G90 G55 A340. X0. Y0.          This  G55  work offset #2     -     Crash  or not ? where machinist input G55   
G43 H9 Z41.                                   Tool lenght offset #9
You are writing the value work offset  G54 for all other G55...G59 and G54.1 P1 ........G54.1 P49  ?
 
This is a mistake of the standard postprocessors? or I not correctly create toolpath?
Link to comment
Share on other sites
Watcher Newbie

Watcher

Posted
Posted

G91 G28 Z0. This home posithion - ret_on_indx : 1 in mpmaster

G00 G90 G55 A340. X0. Y0. This G55 work offset #2 - Crash or not ? where machinist input G55

G43 H9 Z41. Tool lenght offset #9

You are writing the value work offset G54 for all other G55...G59 and G54.1 P1 ........G54.1 P49 ?

 

This is a mistake of the standard postprocessors? or I not correctly create toolpath?

You're setting it wrong. I agree with 5th axis that safe retracts in between index moves are a safe practice in post processors and that the majority of users are OK with them.

 

It seems you have a training issue, which brings another question... Are you talking to your reseller?

 

Most common thing in the world is people not well trained bashing their systems because they don't know how to properly use them or don't have much experience with certain aspects of machining.

  • Like 1
Link to comment
Share on other sites
wing Newbie

wing

Posted
  • Author
Posted

You're setting it wrong.

You can create the correct tool path and share?

 

clearance only at the start and end of operation - OFF - now

G00 G17 G21 G40 G80 G90
G91 G28 Z0.
T9 M06 (4.00 CENTER DRILL)
G00 G17 G90 G54 A0. X0. Y0. S1000 M03
G43 H9 Z45.
G94
G98 G81 Z39.5 R41. F125.
A20.
A40.
A60.
A80.
A100.
A120.
A140.
A160.
A180.
A200.
A220.
A240.
A260.
A280.
A300.
A320.
A340.
G80
M05
G91 G28 Z0.
G28 Y0. A0.
G90
M30
%

 

clearance only at the start and end of operation - ON - now

G00 G17 G21 G40 G80 G90
G91 G28 Z0.
T9 M06 (4.00 CENTER DRILL)
G00 G17 G90 G54 A0. X0. Y0. S1000 M03
G43 H9 Z45.
Z41.
G94
G99 G81 Z39.5 R41. F125.
A20.
A40.
A60.
A80.
A100.
A120.
A140.
A160.
A180.
A200.
A220.
A240.
A260.
A280.
A300.
A320.
A340.
G80
G91 G28 Z0. ?
G00 G90 G55 A340. X0. Y0. ?
G43 H9 Z41. ?
Z45.
M05
G91 G28 Z0.
G28 Y0. A0.
G90
M30
%

 

IF clearance only at the start and end of operation - ON - it should look like this 

G00 G17 G21 G40 G80 G90
G91 G28 Z0.
T9 M06 (4.00 CENTER DRILL)
G00 G17 G90 G54 A0. X0. Y0. S1000 M03
G43 H9 Z45.
Z41.
G94
G99 G81 Z39.5 R41. F125.
A20.
A40.
A60.
A80.
A100.
A120.
A140.
A160.
A180.
A200.
A220.
A240.
A260.
A280.
A300.
A320.
A340.
G80
Z45.
M05
G91 G28 Z0.
G28 Y0. A0.
G90
M30
%
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

 

G91 G28 Z0.                               This home posithion             -    ret_on_indx : 1  in mpmaster  
G00 G90 G55 A340. X0. Y0.          This  G55  work offset #2     -     Crash  or not ? where machinist input G55   
G43 H9 Z41.                               Tool lenght offset #9
You are writing the value work offset  G54 for all other G55...G59 and G54.1 P1 ........G54.1 P49  ?
 
This is a mistake of the standard postprocessors? or I not correctly create toolpath?
 

 

 

When you don't set the workoffset in the operation and use the auto increment function of the CAM program then yes I would expect to get those results. When you set the workoffset in the operation the correct way then you get the correct output. Go into the operation and set the workoffset to the 0 to get the G54 output and repost your code and you will see the results come out as expected.

 

Your program with a workoffset set correctly.

%
O0000(O1111)
(DATE=DD-MM-YY - 10-10-16 TIME=HH:MM - 12:04)
(MCX FILE - C:\USERS\RON\APPDATA\LOCAL\TEMP\WZDA9A\USE CLEARANCE ONLY AT THE START AND END OF OPERATION.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\MILL\NC\O1111.NC)
(MATERIAL - ALUMINUM MM - 2024)
( T9 | 4.00 CENTER DRILL | H9 )
N100 G21
N102 G0 G17 G40 G49 G80 G90
N104 T9 M6
N106 G0 G90 G54 X0. Y0. A0. S1000 M3
N108 G43 H9 Z45.
N110 Z41.
N112 G99 G81 Z39.5 R41. F125.
N114 A20.
N116 A40.
N118 A60.
N120 A80.
N122 A100.
N124 A120.
N126 A140.
N128 A160.
N130 A180.
N132 A200.
N134 A220.
N136 A240.
N138 A260.
N140 A280.
N142 A300.
N144 A320.
N146 A340.
N148 G80
N150 G55 X0. Y0. Z41. A340.
N152 Z45.
N154 M5
N156 G91 G28 Z0.
N158 G28 X0. Y0. A0.
N160 M30
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Your 2nd Operation with a workoffset. Anything else that is an error from the software?

%
O0000(O1112)
(DATE=DD-MM-YY - 10-10-16 TIME=HH:MM - 12:06)
(MCX FILE - C:\USERS\RON\APPDATA\LOCAL\TEMP\WZDA9A\USE CLEARANCE ONLY AT THE START AND END OF OPERATION.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\MILL\NC\O1112.NC)
(MATERIAL - ALUMINUM MM - 2024)
( T9 | 4.00 CENTER DRILL | H9 )
N100 G21
N102 G0 G17 G40 G49 G80 G90
N104 T9 M6
N106 G0 G90 G54 X0. Y0. A0. S1000 M3
N108 G43 H9 Z45.
N110 Z41.
N112 G99 G81 Z39.5 R41. F125.
N114 A20.
N116 A40.
N118 A60.
N120 A80.
N122 A100.
N124 A120.
N126 A140.
N128 A160.
N130 A180.
N132 A200.
N134 A220.
N136 A240.
N138 A260.
N140 A280.
N142 A300.
N144 A320.
N146 A340.
N148 G80
N150 Z45.
N152 M5
N154 G91 G28 Z0.
N156 G28 X0. Y0. A0.
N158 M30
Link to comment
Share on other sites
wing Newbie

wing

Posted
  • Author
Posted

Or they are using a Cracked version of the software, and come here trying to get help...

 

From the first reports I realized that the need to immediately write a reseller  :clap:

Why did not close this thread  "Post Processor Development Forum" ?

Why not just say it's a mistake toolpath or it is a mistake postprocessor?

I’m sorry!

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

From the first reports I realized that the need to immediately write a reseller  :clap:

Why did not close this thread  "Post Processor Development Forum" ?

Why not just say it's a mistake toolpath or it is a mistake postprocessor?

 

One minute phone call to your Reseller and you wouldn't have even needed to post a question.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Why was it necessary to develop this discussion, if you can respond immediately. Thank you! :unworthy:

 

Your tone controlled the discussion. You came in ripping apart something without providing good information. Many people want to rip things apart and you are number 2476 to come in and do that. Imagine how tired we are of seeing it over and over and over again for more than a decade for some of us.

 

Once you provided a better idea what you are having an issue with your got a better answer.

Link to comment
Share on other sites
Watcher Newbie

Watcher

Posted
Posted

Why was it necessary to develop this discussion, if you can respond immediately. Thank you! :unworthy:

 

Don´t be so sure next time you come around... Consider yourself a lucky guy for what you got here with minimal input from your end and without any evidence you´re a legit user...

 

Just saying...

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...