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:

MasterCam Transform Toolpath


PcRobotic
 Share

Recommended Posts

Hello everyone,
   I've been chasing my tail when using TRANSFORM TOOLPATH,  TRANSLATE.

 

I have 2 separate parts and want to pickup G54 and G55 for my own locations.  However, somehow I got the G-CODES lumps 2 parts into 1 work offset.  Would you guys please help me out and tell me what i've done wrong?  

 

ps: I am using the DEFAULT post to show the issue.

 

Thank you.

 

 

========================== g-codes ================

%
O4631(A046-300011-REV00- OP1)
(DATE=DD-MM-YY - 28-04-22 TIME=HH:MM - 06:48)
(MCAM FILE - \\10.1.2.112\DEPT_SHARE\MANUFACTURING\PROGRAMS\OKUMA M560V CAM\A046-300011-REV00\SOURCE\A046-300011-REV00.MCAM)
(NC FILE - C:\USERS\SLUONG\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\A046-300011-REV00- OP1.NC)
(MATERIAL - STEEL - 304 STAINLESS)
( T22 | 1/2 BULL EM | H22 | XY STOCK TO LEAVE - 0. | Z STOCK TO LEAVE - .005 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
/ N120 G91 G28 Z0.
( LEFT - SEMIFINISH TOP SURFACE )
N150 T22 M6
N160 G0 G90 G54 X-1.5075 Y.3749 A0. S3500 M3   ===========> FIRST PART HERE AS G54
N170 G43 H22 Z1.
N180 Z.125
N190 G1 Z.02 F10.
N200 X1.2575
N210 Y.125
N220 X-1.2575
N230 Y-.125
N240 X1.2575
N250 Y-.3749
N260 X-1.5075
N270 G0 Z1.
( LEFT - SEMIFINISH TOP SURFACE )    ==================> second part here
N280 X2.5775 Y.3749       ==================> second part here
N280 G0 G90 G55 X-1.5075 Y.3749 A0. S3500 M3 ==================> G55 SHOULD APPEAR (I TYPED THIS BY HAND AND WANT IT TO SHOW LIKE THIS.)
N290 Z.125
N300 G1 Z.02 F10.
N310 X5.3425
N320 Y.125
N330 X2.8275
N340 Y-.125
N350 X5.3425
N360 Y-.3749
N370 X2.5775
N380 G0 Z1.
N390 M5
N400 G91 G28 Z0.
N410 G28 X0. Y0. A0.
N420 M30
%
Link to comment
Share on other sites
13 minutes ago, crazy^millman said:

Sorry going to need a sample file to help.

I am only allowed 2.65KB to upload the file.  May I have your email?

 

Mine is [email protected]

42 minutes ago, AHarrison1 said:

Did you create a new WCS for the 2nd part / position and then assign a work offset to that WCS?

This can be done in the Planes manager or under planes tab in toolpath parameters

 

Hello,
   That's what exactly what I've done manually.  I want to ultralize the TRANSFORM TOOLPATH.


Thanks,
   S.Luong

 

 

 

 

Link to comment
Share on other sites
15 minutes ago, #Rekd™ said:

On the Types and Method page of the Translate operation "Work offset numbering" - Assign New and make the settings.

This file was spitting out G55 instead of maintaining G54 so I had to set it to "Assign New" and set it to 0.

 

Translate.png

 

 

Hello,
   This is what I have done.  The only I have is TRANSLATE not ROTATE.

 

 

 

 

=========== gcode=========

%
O4631(A046-300011-REV00- OP1)
(DATE=DD-MM-YY - 28-04-22 TIME=HH:MM - 07:51)
(MCAM FILE - \\10.1.2.112\DEPT_SHARE\MANUFACTURING\PROGRAMS\OKUMA M560V CAM\A046-300011-REV00\SOURCE\A046-300011-REV00.MCAM)
(NC FILE - C:\USERS\SLUONG\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\A046-300011-REV00- OP1.NC)
(MATERIAL - STEEL - 304 STAINLESS)
( T21 | 1/2 SPOTTER | H21 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
/ N120 G91 G28 Z0.
/ N130 G28 X0. Y0.
/ N140 G92 X0. Y0. Z0.
( SPOT 1X .550 THRU HOLE )
N150 T21 M6
N160 G0 G90 X-.2953 Y0. A0. S1500 M3
N170 G43 H21 Z1.
N180 G98 G81 Z-.005 R.125 F1.5
N190 G80
( SPOT 1X .550 THRU HOLE )
======================================> missing G55 and XY locations here...
N200 G98 G81 Z-.005 R.125 F1.5
N210 G80
N220 M5
N230 G91 G28 Z0.
N240 G28 X0. Y0. A0.
N250 M30
%

 

 

 

 

Link to comment
Share on other sites

BbWtA45.png%
O4631(A046-300011-REV00- OP1)
(DATE=DD-MM-YY - 28-04-22 TIME=HH:MM - 11:14)
(MCAM FILE - C:\USERS\JOHNP\DESKTOP\A046-300011-REV00.MCAM)
(NC FILE - C:\USERS\JOHNP\DOCUMENTS\MY MASTERCAM 2023\MASTERCAM\MILL\NC\A046-300011-REV00- OP1.NC)
(MATERIAL - STEEL - 304 STAINLESS)
( T22 | 1/2 BULL EM | H22 | XY STOCK TO LEAVE - 0. | Z STOCK TO LEAVE - .005 )
G20
G0 G17 G40 G49 G80 G90
( VERTICAL )
( BEAM POSITION MONITORS ACCELERATOR )
( MDC )
( LEFT - SEMIFINISH TOP SURFACE )
T22 M6
G0 G90 G54 X-1.5075 Y.3749 A0. S4500 M3
G43 H22 Z1.
M8
Z.125
G1 Z.005 F50.
X1.2575
Y.125
X-1.2575
Y-.125
X1.2575
Y-.3749
X-1.5075
G0 Z1.
( VERTICAL )
( BEAM POSITION MONITORS ACCELERATOR )
( MDC )
( RIGHT - SEMIFINISH TOP SURFACE )
G55 X-1.5075 Y.3749 Z1. A0.
Z.125
G1 Z.005 F50.
X1.2575
Y.125
X-1.2575
Y-.125
X1.2575
Y-.3749
X-1.5075
G0 Z1.
M09
M5
G91 G28 Z0.
G28 X0. Y0. A0.

 

yOU HAVE YOUR MISC INT SET WRONG

 

and you're not actually using Tansform in that file

 

Link to comment
Share on other sites
On 4/28/2022 at 8:15 AM, JParis said:

BbWtA45.png%
O4631(A046-300011-REV00- OP1)
(DATE=DD-MM-YY - 28-04-22 TIME=HH:MM - 11:14)
(MCAM FILE - C:\USERS\JOHNP\DESKTOP\A046-300011-REV00.MCAM)
(NC FILE - C:\USERS\JOHNP\DOCUMENTS\MY MASTERCAM 2023\MASTERCAM\MILL\NC\A046-300011-REV00- OP1.NC)
(MATERIAL - STEEL - 304 STAINLESS)
( T22 | 1/2 BULL EM | H22 | XY STOCK TO LEAVE - 0. | Z STOCK TO LEAVE - .005 )
G20
G0 G17 G40 G49 G80 G90
( VERTICAL )
( BEAM POSITION MONITORS ACCELERATOR )
( MDC )
( LEFT - SEMIFINISH TOP SURFACE )
T22 M6
G0 G90 G54 X-1.5075 Y.3749 A0. S4500 M3
G43 H22 Z1.
M8
Z.125
G1 Z.005 F50.
X1.2575
Y.125
X-1.2575
Y-.125
X1.2575
Y-.3749
X-1.5075
G0 Z1.
( VERTICAL )
( BEAM POSITION MONITORS ACCELERATOR )
( MDC )
( RIGHT - SEMIFINISH TOP SURFACE )
G55 X-1.5075 Y.3749 Z1. A0.
Z.125
G1 Z.005 F50.
X1.2575
Y.125
X-1.2575
Y-.125
X1.2575
Y-.3749
X-1.5075
G0 Z1.
M09
M5
G91 G28 Z0.
G28 X0. Y0. A0.

 

yOU HAVE YOUR MISC INT SET WRONG

 

and you're not actually using Tansform in that file

 

Thank you it worked.  By the way, how do I use it for MP MASTER MILL POST of which I downloaded from this forum?

It worked as the DEFAULT POST from MASTERCAM.

On the other side, I would like to use the MPMASTER post of which I downloaded from this forum.  Would you point it out?  

 

 

Thanks,
    S.Luong
================ORIGINAL POST CODES==================

pwcs            #G54+ coordinate setting at toolchange
      if wcstype = two | wcstype > three,
        [
        sav_frc_wcs = force_wcs
        if sub_level$ > zero, force_wcs = zero
        if sav_mi9 = 1, workofs$ = sav_workofs
        if workofs$ < 0, workofs$ = 0
        if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,
          [
          if workofs$ < 6,
            [
            g_wcs = workofs$ + 54
            *g_wcs
            ]
          else,
            [
            if haas,
              [
              p_wcs = workofs$ - five        #G154 P1 to P99
              "G154", *p_wcs
              #g_wcs = workofs$ + 104        #G110 to G129
              #*g_wcs
              ]
            else,
              [
              p_wcs = workofs$ - five
              "G54.1", *p_wcs
              ]
            ]
          ]
        force_wcs = sav_frc_wcs
        !workofs$
        ]

 

 

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...