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:

G13 AND G12 TO REPLACE LONG GCODES OF CIRCLE MILL FUNCTION?


Recommended Posts

Hi everyone,

We just bought an old FANUC control CNC MILL of which has G13 AND G12. One of the problem is it has limited of memory, we have to make quite lots of holes and is there away we can shorten the GCODEs in the CIRCLE MILL to G13 or G12?

 

This would be nice if we can do that so it can fit into any equipment because nearly ALL of the FANUC can run G13 and G12 to make perfect holes.

 

 

 

Thank you for helping.

Link to comment
Share on other sites

I know this doesn't answer your question, but if you're limited on space, you can use macros. We use a bunch of different macro for things like that and I use MasterCams custom drilling cycles to programs.

 

For example this line " G65 P9996 Z-1.0 R.1 D.75 T.375 Q.05 F20. " would helical bore a hole. The arguements tell the macro, depth, tool diameter, feed, rapid plane, etc.

 

And here is the macro in the machine.

 

O9996( G65 P9996 Z R D T Q F S-W/OPT. )
( Z = #26-FINAL Z DEPTH )
( R = #18-RAPID PLANE )
( D = #7-FINISH DIAMETER OF HOLE )
( Q = #17-Z DEPTH PER DIAMETER )
( T = #20-TOOL DIAMETER )
( F = #9-FEEDRATE )
( S = #19-SPRING PASSES )
( W = #23-FEEDRATE OVERRIDE 0=OFF/1=ON )
IF[[#20*#7*#9*#17]EQ0]GOTO990
#104=#[13000+#4107]
#100=#5003
#101=#5001
#102=[[#7-#20]/2]-#104( CALC. SWING )
#103=#26+[#17*2]
#149=#19
#119=#9
IF[[#23*1]EQ0]GOTO20
#135=[#102*2]*3.14
#136=[[#102*2]+#20]*3.14
#137=#135/#136
#119=#9*#137
N20
G0G90Z#18
G91
G1G41X#102F#119
IF[#26GT#18]GOTO30
WHILE[#5003GT#103]DO1
G3I-#102Z-#17
END1
GOTO40
N30
#103=#26-[#17*2]
WHILE[#5003LT#103]DO1
G3I-#102Z#17
END1
N40
G90
G03I-#102Z#26
I-#102
F[#119/2]
WHILE[[#149*1]GT0]DO1
G03I-#102
#149=#149-1.
END1
G01G40X#101F#9
G00Z#100
GOTO999
N990#3000=150(DATA LACKING)
N999M99

Link to comment
Share on other sites

Using G12/G13 is very similar to inputting info for a macro, you just define the parameters of the cut

 

Consider using a customer drill cycle to achieve this

 

There is a TON of info on this forum about custom drill cycles ifyou use the search, I seem to remember some years back someone else wanting add this as well

 

Just remember, all you're going to be providing is the info for the cycle, Mastercam will not show you that path as a backplot or verify

Link to comment
Share on other sites
  • 2 weeks later...
  • 2 weeks later...

Is it really so big problem to answer to this question in more detail?

 

No, but not so simple.

BUT I see a way to solve it. For example if you program a Circle Mill OP in MCAM, you can post it as G65 Pxxxx instead of G2/G3.

So yes, it can be solved by posting out a macro call (or G12/G13 on HAAS). I made some similar in the past and some macros combined into NC code by post, so it's possible for sure.

BUT this takes time and... ;)

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...