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:

Is this toolpath moving the primary or secondary rotary axis?


Recommended Posts

I am setting up some lock code stuff in a post I have been working on for a while.... Is there a conditional statement or something that I could put in the toolchange postblock to tell me if any part of this toolpath moves the rotary (something that would pre-read the entire toolpath)? The post is Generic Fanuc 5 ax mill.

Thanks in advance...

Link to comment
Share on other sites

There is "mill5$". It is a variable that is set to "1" when doing 5 axis (or 4 axis) milling and is set to "2" for multi-axis. We check this on our post to check if we are going to do a 4 or 5 axis tool path. If so, we keep the rotaries unlocked for the whole tool path. I assume that is what you are trying to do?

Link to comment
Share on other sites

This will get me close, thanks pimp.

I set up 2 curve ops 1 locked to 4 ax and the other a full 5 ax path, both return mill5$ values of 1....

Going to try and dig up the params for "output type" 4 or 5 ax, maybe i can use that to get the last piece of the puzzle..

Link to comment
Share on other sites

Ok, I am pretty close but...

 

N100 G00 G91 G28 Z0.
N110 G0 G17 G20 G40 G49 G80 G90 G94 G98 H00
( .501 SPOT DRILL   )
( 4AX DRILL WITH 5th POSITIONING )
N120 M21 (UNLOCK C)
N130 M11 (UNLOCK 
N140 T01 M06
N150 M00
( CONFIRM T01 H01 D01 DIA = 0.5010 )
N160 G0 G17 G20 G40 G49 G80 G90 G94 G98 H00
N170 G0 G17 G90 G54 X-2.9164 Y0. C292.5 B105. S100 M3<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<need "B" to lock after this line...
N180 G43 H01 Z18.8477
N190 G81 G98 Z14.2477 R15.0977 F10.
N200 C337.5
N210 C22.5
N220 G80
N230 M5
N240 G0 G28 G91 Z0.
N250 M19
N260 M30
%

 

For the code above I needed to have the output format set to 5 ax so I can get the right B position on the G54 line...

that wont allow me to use mill5$ or parameter # 12019 (drill output format...) to access my lock codes...

 

Going to look into using s_inc in the drilling postblocks.....

Anyone else have an idea???

Link to comment
Share on other sites

The Generic Fanuc 5X Mill.pst already contains clamping logic that is enabled when the use_clamp swtich is enabled. The logic was reworked 2 years ago to better handle clamping/unclamping for drilling and 4/5-axis style output. I would recommend taking a look at a post released since then and encorporating the changes if you are currently using an older post. I'd suggest sending in examples if you have specific cases where you wish to modify the clamping behavior beyond the default output. We should be able to tailor things by using cuttype, opcode$ or tool_op$ if need be.

Link to comment
Share on other sites

From stock Generic Fanuc 5x post...

 

M11   	<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock
M79   	<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock
T1 M6
G0 G54 G90 X-1. Y2. C180. B-90. S100 M3
M10   	<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<lock
M78   	<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<lock
G43 H1 Z17.
G1 Z16. F20.3
M5
G0 G28 G91 Z0.
G28 C0. B0.	<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< go home without unlocking ??????
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
( .501 SPOT DRILL   TOOL - 1  DIA. OFF. - 1  LEN. - 1  DIA. - .501 )
( 4AX DRILL )
M11
M79
T1 M6
G0 G54 G90 X-1. Y0. C180. B-90. S1500 M3
M10
M78
G43 H1 Z19.1
G81 G98 Z14.9 R15.35 F5.
M79
C135.
M78<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<lock
M79<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock
C90.
M78<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<lock
M79<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock
C45.

 

I won't be using that..... The first path sends the rotarys home at the end without unlocking :blink:

and the 2nd with all the locks and unlocks in betweeen each drill point, not what I was expecting....

Link to comment
Share on other sites

It might but to start with something thats not right (by not right i mean not right for what i want)..... no thanks.

I have got it for the drilling...

( 4AX DRILL WITH 5 POSITIONING )
( .501 SPOT DRILL   )
M21 (UNLOCK C)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<initial unlocking
M11 (UNLOCK <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
T01 M06
M00
( CONFIRM T01 H01 D01 DIA = 0.5010 )
G0 G17 G20 G40 G49 G80 G90 G94 G98 H00
G0 G17 G90 G54 X-2.9164 Y0. C292.5 B105. S100 M3
G43 H01 Z18.8477
M10 (LOCK <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<lock both after initial move
M11 (LOCK C)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
G81 G98 Z14.2477 R15.0977 F10.
M21 (UNLOCK C)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock only the one that needs to be !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
C337.5
C22.5
G80
M5
G0 G28 G91 Z0.
M19
M00
( 5AX DRILL )
( .423 DRILL   )
M21 (UNLOCK C)
M11 (UNLOCK 
T02 M06
M00
( CONFIRM T02 H02 D02 DIA = 0.4230 )
G0 G17 G20 G40 G49 G80 G90 G94 G98 H00
G0 G17 G90 G54 X-2.9164 Y0. C292.5 B105. S1500 M3
G43 H02 Z18.8477
M10 (LOCK 
M11 (LOCK C)
G83 G98 Z14.2477 R15.0977 Q.1 F10.
M11 (UNLOCK 
M21 (UNLOCK C)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<unlock both cause they are both used
X1. Z14.5 C315. B90. R15.35
X-2.9164 Z14.2477 C337.5 B105. R15.0977
X1. Z14.5 C0. B90. R15.35
G80

 

I don't need/want them to lock in between each hole, unnecessary and a time killer.

 

still working on the 5ax contouring paths..

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...