525,379 active members*
2,723 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 23
  1. #1
    Registered
    Join Date
    Feb 2006
    Posts
    1770

    Learning G10: please help

    I am trying to learn the use of G10. Please confirm if my interpretation of the following codes is correct:

    G90 G10 L10 P10 R-500; (Enters -500 mm into offset number 10, as the geometry compensation value for H-code)

    G91 G10 L10 P10 R5; (Enters 5 mm incrementally into offset number 10, as the geometry compensation value for H-code, making the tool length smaller by 5 mm. So, the same tool would dig 5 mm more into the workpiece, for the same program)

    G91 G10 L11 P10 R0.5; (Enters 0.5 mm incrementally into offset number 10, as the wear compensation value for H-code. So, the wear value would increase by 0.5 mm, and hence, the same tool would dig 0.5 mm more into the workpiece, for the same program)

  2. #2
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Sinha,
    That is correct. The only thing I cannot confirm is if you have the proper “L” for the registry. I don’t have any of my data with me. Speaking of that does anyone have a master list or a spreadsheet with the “L” meaning of each registry? I always have to look it up in the book and IIRC they are not all the same per control.

    Stevo

  3. #3
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    Thanks for the reply. You are always helpful.
    As per 0i manuals,
    L2 is for work offsets,
    L20 is for additional work offsets (on milling machines only),
    L10 is for H-geometry,
    L11 is for H-wear,
    L12 is for D-geometry,
    L13 is for D-wear,
    No L is used for lathe compensation values,
    L50 is for parameter entry, and
    L3 is for tool life data entry.
    L1 can be used in place of L11.

    Other control versions may use different L values. For example, I have heard that 180i uses L52 for parameter entry.

    However, for offset and compensation data, there is not enough reason to use G10 (because one has to remember its syntax). I would prefer to use system variables. Of course, for parameter entry and tool life data entry, through a program, G10 is the only method.

  4. #4
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Your always welcom Sinha.

    Thanks for the feedback on the "L" designation.

    Stevo

  5. #5
    Registered
    Join Date
    Nov 2006
    Posts
    174
    Sinha, all your code looks good.
    Maybe not the point of your post, probably just me being picky.

    The meaning of this one
    .....
    G91 G10 L11 P10 R0.5; (Enters 0.5 mm incrementally into offset number 10, as the wear compensation value for H-code. So, the wear value would increase by 0.5 mm, and hence, the same tool would dig 0.5 mm more into the workpiece, for the same program)
    .......

    This would increase the wear comp by 0.5mm and so make your tool longer (or bigger dia if used for D value). So it would dig 0.5mm less, into the workpiece.

    e.g. need to leave more material on, then comp+
    need to take more material off, then comp-

  6. #6
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    Thanks for your comments.
    Actually, I was more interested in verifying if my interpretation was correct.
    Since, I do not have 0i M control, I can only rely on you people.

    Are other interpretations OK?
    How about this (I am repeating):

    G91 G10 L10 P10 R5; (Enters 5 mm incrementally into offset number 10, as the geometry compensation value for H-code, making the tool length smaller by 5 mm. So, the same tool would dig 5 mm more into the workpiece, for the same program)

    Wiil the tool dig more or less?

  7. #7
    Gold Member
    Join Date
    Mar 2003
    Posts
    2928
    H10 = -255.000
    G43 Z0 H10 moves tool down 255mm.

    execute G91 G10 L10 P10 R5

    H10 is now - 250.00
    G43 Z0 H10 moves tool down 250mm.

    This is assuming your control interprets R5 as 5mm, not .005mm

  8. #8
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    Thanks.
    So, in my previous post, more should be replaced by less, if we are using G43.
    Correct?

  9. #9
    Registered
    Join Date
    Aug 2009
    Posts
    677

    G10 Applications

    Hi,

    Sorry for butting in, have recently discovered G10 myself and I use it in programs to reload my previous work offsets.

    Noted that there are L-codes that relate to tool offsets - is there also a way (not necessarily G10) to load other tool information via the program, ie the tool type/tool description info, which can then be displayed in 'Current Machining'?

    DP

  10. #10
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    As far as I know, there is no way a message can be displayed while the machining is being done. It is, however, possible to use system variable #3006 which will halt (but not terminate) the execution and display user-specified message (up to 26 characters) on MESSAGE screen. You have to press CYCLE START again to continue further machining. Details of #3006 are given below:

    System variable #3006
    System variable #3000 generates an alarm condition and terminates the program execution, whereas variable #3006 causes temporary pause of execution which can be restarted by pressing the CYCLE START button again. In the paused state, pressing the MESSAGE key displays the user-specified message (up to 26 characters). Assigning a number to variable #3006 halts the program execution. There is no significance of this number, as message number is not displayed. So, normally, 1 is assigned. Example:
    #3006 = 1 (CHECK THE DIAMETER);
    This would temporarily stop the execution, and display “CHECK THE DIAMETER” on the message screen. If no message is typed, nothing would be displayed.

  11. #11
    Registered
    Join Date
    Aug 2009
    Posts
    677

    G10 and Tool Data

    Hi again,

    Wasn't refering to a message on screen this time.. Was hoping there was a G10 L* and R* command that could load other Tool data such as the tool's shape/orientation for use with the graphic simulation (rather than inputting it directly into tool table). Bizarre request, I know, but there it is.

    DP

  12. #12
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    The graphic feature of the control does not show tool shape. Only toolpath is drawn. Manual Guide i might be showing more realistic simulation, but I have no experience on that. I have used some third-party simulation softwares, where one has to choose the shape/orientation of the tool(s) being used in the program. It is not a part of the program. This has to be done independently, before simulation.

  13. #13
    Registered
    Join Date
    Aug 2009
    Posts
    677

    Tool Data woes

    Hi,

    Disappointed that no-one knows a way you can use G10 (programmable data input) to load extra tool data into table. I suppose the only way it could be automated is to upload complete tool data from previously saved file. Unfortunately the way I am working means that my tool table is constantly changing (see Tool Numbering thread). Hmmmm....

    DP

  14. #14
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Quote Originally Posted by christinandavid View Post
    Hi,

    Disappointed that no-one knows a way you can use G10 (programmable data input) to load extra tool data into table. I suppose the only way it could be automated is to upload complete tool data from previously saved file. Unfortunately the way I am working means that my tool table is constantly changing (see Tool Numbering thread). Hmmmm....

    DP
    I guess I am a bit confused of what exactly you want to do. Are you saying that you want to change the tool geometry, H, and D values??

    As you say your tool table is changing and if you can find a common connection to the change this could be done via macro programming.

    “See tool numbering thread”…..got a link to that thread???

    What model Fanuc are you using??

    Stevo

  15. #15
    Instead of using G10 for this data

    use the system macros (MacroB)
    Attached Thumbnails Attached Thumbnails Tool Comp Variables.JPG  
    ************************************************** *********
    *~~Darwinian Man, though well-behaved, At best is only a monkey shaved!~~*
    ************************************************** *********
    *__________If you feel inclined to pay for the support you receive__________*
    *_______Please give to charity https://www.oxfam.org.au/get-involved/_______*
    ************************************************** *********

  16. #16
    More G10 Data

    G10 L75 P1;
    N_ ; Tool management data number specification
    T_ C_ L_ I_ B_ Q_ H_ D_ S_ F_ J_ K_ ;
    P0 R_ ; Customization data 0
    P1 R_ ; Customization data 1
    P2 R_ ; Customization data 2
    P3 R_ ; Customization data 3
    P4 R_ ; Customization data 4
    N_; Tool management data number
    :
    G11;
    N_ Tool management data No. 1 to 64
    (1 to 240, 1 to 1000)
    T_ Tool type No. (T) 0 to 99,999,999
    C_ Tool life counter 0 to 99,999,999
    L_ Maximum tool life 0 to 99,999,999
    I_ Noticed life 0 to 99,999,999
    B_ Tool life state 0 to 4
    Q_ Tool information Bit format (8 bits)
    H_ Tool length compensation No. (H)
    0 to 999 (M series)
    D_ Cutter compensation No. (D)
    0 to 999 (M series)
    S_ Spindle speed (S) 0 to 99,999
    F_ Cutting feedrate (F) 0 to 99,999,999
    J_ Tool geometry compensation No. (G)
    0 to 999 (T series)
    K_ Tool geometry compensation No. (W)
    0 to 999 (T series)
    P_ Customization data No. 0 to 4 (0 to 20, 0 to 40)
    R_ Customization data value
    -99,999,999 to 99,999,999


    G10L30;Tool data entry mode setting
    N_P_R_;Tool data entry

    G11;Tool data entry mode cancel

    N_ : Tool data No. or multiple tool data No. +200
    P01 : Tool No. or multi-tool No. setting
    P02 : Turret position or angle for indexing turret of multiple tool setting
    P03 : X-axis tool offset setting
    P04 : Y-axis tool offset setting
    P05 : Tool change No. setting
    P06 : Punch count setting
    P07 : Tool life setting
    P08 : Tool figure setting for graphic operation
    P09 : X dimension of a tool setting for graphic operation
    P10 : Y dimension of a tool setting for graphic operation
    P11 : Tool angle setting for graphic operation
    R_ : Tool data setting value
    ************************************************** *********
    *~~Darwinian Man, though well-behaved, At best is only a monkey shaved!~~*
    ************************************************** *********
    *__________If you feel inclined to pay for the support you receive__________*
    *_______Please give to charity https://www.oxfam.org.au/get-involved/_______*
    ************************************************** *********

  17. #17
    Registered
    Join Date
    Aug 2009
    Posts
    677

    G10 Again

    Hi,

    Thanks to sinha nsit for starting this thread.

    Thanks to Mystic Monkey for pointing me in the right direction.

    To clarify: - I am running Fanuc 31i on a horizontal machining centre.
    Tool Table has two tabs/pages. First page is your H & D offsets and Wear offsets - these can be altered with G10 L10-L13 etc. have got this working (along with L20 to alter my G54.1 Work offsets). No Probs.

    2nd tab of tool table is for 'Tool Data' which comprises: -

    'Set' in which you input 1-4 (tool orientation for simulation purposes).

    Next bit is 'Form' or type/shape of tool you are using. You can overwrite the standard description with your own string (8 characters max). As well as more realistic simulation this info pops up on screen while running program.

    Finally depending on 'Form' another box will pop up for tool angle/diameter.

    Inputting all this manually is a pain, and as the position of my tools will vary on each run I can't simply save the complete tool table data to a file.

    I want to be able to use G10 to reset the entire table to its initial blank state and then load this information back in (through my program) to the tools currently in use. As well as giving me realistic simulation and on-screen info I believe it would be a nice way to 'highlight' the tools currently in use when scrolling through the table.

    Manual does not appear to describe G10 in much depth (have found more info through this site). I don't want to start poking around with it having no idea what I might be altering.

    Mystic Monkey suggests L75 and L30 for tool data yet I am still a bit dubious as the descriptions do not tally with what I am looking at (L30 descriptions look likely but seem to relate to Turning - ie 'T' series, not 'M'? Please correct me if I am wrong).

    Thanks for all the help - if anyone has more info relating to my particular control it would be greatly appreciated.

    Happy Holidays!

    DP

  18. #18
    Gold Member
    Join Date
    Mar 2003
    Posts
    2928
    Christian,

    Unless I'm way off base, you must be using Manual Guide-i. You should be able to input and output Tool Data to the memory card.

    In EDIT mode, display the tool data screen.
    Insert a memory card in the slot.
    Using the < or > soft keys, until you see soft keys for OUTPUT and INPUT
    Press OUTPUT. You should see a window titled "OUTPUT TOOL DATA TO MEMORY CARD"
    Enter an 8 digit filename with a .dat extension.
    Press OUTPUT.

    I believe when you INPUT tool data, it clears out the existing tool data.

  19. #19
    Registered
    Join Date
    Aug 2009
    Posts
    677

    Tool Data

    Hi, thanks for response,

    As previously stated, the way I am working means that my tool numbers will alter every time I set up a particular operation. The reason I need to explore the G10 possibilities is because I can then substitute the Tool Number (P) with a variable. I may have overcomplicated the issue...

    DP

  20. #20
    Gold Member
    Join Date
    Mar 2003
    Posts
    2928
    No, you didn't overcomplicate the issue, I just couldn't find a way (after searching the PDF manuals) to load the tool data with G10. You CAN, however, load the tool data for each setup from the memory card.

    You may also be able to do it at the start of a program with the embedded macros, i.e. G1932 D1.0 H2.0 defines a 2" long 1" diameter end mill.

Page 1 of 2 12

Similar Threads

  1. Learning about CAM
    By blackout1985 in forum Uncategorised CAM Discussion
    Replies: 0
    Last Post: 07-19-2013, 07:47 PM
  2. Learning CNC
    By clayman in forum General MetalWork Discussion
    Replies: 8
    Last Post: 02-23-2012, 09:21 PM
  3. Replies: 5
    Last Post: 12-12-2011, 04:59 PM
  4. Learning!
    By CNCadmin in forum EnRoute
    Replies: 7
    Last Post: 11-09-2011, 12:54 AM
  5. Learning...Need help with PSU
    By h3ndrix in forum General CNC Machine Related Electronics
    Replies: 0
    Last Post: 02-24-2007, 11:38 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •