How to use G50 on Fanuc 6T - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 28 of 28
  1. #21
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1416

    Default

    Quote Originally Posted by TeachMePlease View Post
    Bill, this is common practice in Swiss machining. At least where I am. Never done it anywhere else, so I guess I can't say for sure that it's common, but I've seen it done/done it on 2 brands of machines with 3 different types of control (Siemens, Fanuc, Mitsubishi).

    Say T2 is a face/turn tool, and it establishes Z0 on the part... The centerline of the live tool is .3937" from the Z0 position/guide bushing. When you call T14 (live tool), you G50 W-.3937", and then write code as normal, rather than having to add that .3937" to all your Z coordinates. When finished, you obviously G50 W.3937" to cancel.
    Hello Teach,
    That I'm familiar with. G50 used with an Incremental address actually Shifts the Work Coordinate System and not actually sets a New Work Coordinate System. This is demonstrated by your example of using the inverse (W.3937) to cancel the W-.3937. If a Work Coordinate System is set using G50 X_ _ Z_ _, this base Coordinate System can be shifted by an Incremental amount specified by using G50 U_ _ Z_ _ and canceled by specifying the inverse of the U and W values previously specified.

    Its the same principle with a Machining Centre where the Work Coordinate System can be made to shift by an Incremental amount by specifying G92 X_ _ Y_ _ in G91 Mode. In an earlier Post stating the use of G50 with U and W seemed to state that this actually set the Coordinate System and that's what I couldn't understand. I don't believe its Possible to actually set the Coordinate System with an Incremental Value, unless a Coordinate System is initially set.

    Regards,

    Bill

  2. #22
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1416

    Default

    Quote Originally Posted by NAST555 View Post
    So Teach... for arguments sake if you could not use an offset page/wear to add on to geometry you could use this if your tool was out a bit? So instead of moving it within your program you would either add/subtract the U or W when you G50 it and just go for it?

    Reason I am asking is if you had a turret set up with all your tools and their X and Z values known, moved a boring bar in (like I mentioned above) , you could go G50 T100 and then G50 T101 -W50.0
    Hello NAST555,
    That's absolutely correct and is similar to how I've used it in early days. However, you must remember to cancel the Shift by specifying the inverse of the value originally specified before calling another tool if the Shift was only to adjust a particular tool.

    Regards,

    Bill

  3. #23
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,587
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    658

    Default

    Quote Originally Posted by angelw View Post
    Hello NAST555,
    That's absolutely correct and is similar to how I've used it in early days. However, you must remember to cancel the Shift by specifying the inverse of the value originally specified before calling another tool if the Shift was only to adjust a particular tool.

    Regards,

    Bill
    So by calling it for that specific tool it would add it to the rest of the tools because I have shifted it from where G50 was? So I have actually moved the G50 position and not only the "offset" for that tool.

    So to do it correctly I would need to cancel it in the end like Teach and yourself said at the end of that tool. So it would be G50 X200.0 Z200.0 T100 and then G50 W50.0 and the slides would move that extra 50 mm that I had shifted it when I called the tool.

    Crap, seems like a lot to get my head around. Why the hell did you guys make it so tough for us? Did you not realise that us spoilt young machinists might be running a machine the same age as themselves "ONE DAY"

  4. #24
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1416

    Default

    Quote Originally Posted by NAST555 View Post
    So by calling it for that specific tool it would add it to the rest of the tools because I have shifted it from where G50 was? So I have actually moved the G50 position and not only the "offset" for that tool.

    So to do it correctly I would need to cancel it in the end like Teach and yourself said at the end of that tool. So it would be G50 X200.0 Z200.0 T100 and then G50 W50.0 and the slides would move that extra 50 mm that I had shifted it when I called the tool.

    Crap, seems like a lot to get my head around. Why the hell did you guys make it so tough for us? Did you not realise that us spoilt young machinists might be running a machine the same age as themselves "ONE DAY"
    Hello NAST555,
    As long as the Axes Slides are at the correct position when the New G50 X_ _ Z_ _ is specified, then the New Coordinate System will be created. G50 in Incremental Mode is more often used when the position of the various tools are specified + or - of a set, base Coordinate System. In this System, the Incremental G50 Shift must be cancelled by specifying the Inverse, before executing an Incremental G50 Shift of another tool. Failure to do this will result in the Incremental Shift of the subsequent tool being added to the existing Shift.

    Regards,

    Bill

  5. #25
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    806
    Post Thanks / Like
    Likes (Given)
    471
    Likes (Received)
    314

    Default

    Quote Originally Posted by NAST555 View Post

    I know that I am probably overthinking it and have been ":spoilt" but the last 6T I ran was years ago and the G50 "toolchange" was set at a certain safe position and my offset screen had the actual geometry of my tools from what I can remember.

    Any help is much appreciated.
    I had quite a few older machines with 6T controls. The G50 command for setting tool offsets is "ok" but I very much prefer Mike Lynch's version, where the measured inputs are placed into the Tool registry and the whole G50 line is omitted.

    So, if using G50 like the bad old days, you would call up the Tool = T01000, then instate the G50 from the home position - G50 Xxxxx Zxxxx; then instate tool offset, T0101, then cut. When through, you would have to cancel, with T0100. Then index, T0200, and repeat.

    One little type and whoops!

    What I learned was to take the values that would have been in the G50 line and put them in the X and Z offset registers. Now, all you do is call up T0101, and it's there. Simply cancel with T0100, then T0202, and off you go. Most later controls cancel the active offset when another is called, but many 6's do not - hence the cancellation.

  6. #26
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,587
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    658

    Default

    Ok, so thanks to all of you.

    I have finally settled in here and see how they work their system. It does not matter which tool you set off with... you move it away that certain safety amount off the part and then origin it... then home the machine and start the program with the W-difference between the two. Then touch off all tools from that distance and see the difference between them. So your new G50 when you retract a tool is the difference between your touch off tool and the tool that is currently in the turret. So the position that you always return to according to the machine co-ordinates is the same no matter which offset is active. That way you can see if you are off with a tool, when you G50 retract and it does not match up wit the machine position from home to your first "workshift" then you know that something is wrong.

    In X just take a cut, measure, then go into machine lock and move the measured distance in X. Then zero X and home it. That would be your G50 X value for that tool.

    And the way that they do it is return to a position at the top of the program without having to home every time. So the top of the program tells it to go G28 U0.0 W0.0 and then to G00 U-50.0 W-500.0 (theoretically where the first tool is 150.0 mm away in Z and the X is just off it's home) but at the bottom of the program it does not tell it to go back to the start, it tells it to go to just after that block so that the machine does not have to home before every cycle, just starts from where it is.

    So if the operator moves the Axis at all they have to do is "reset" "program" and it does the whole homing again and starts from the correct G50 position.

  7. #27
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1416

    Default

    Quote Originally Posted by NAST555 View Post
    Ok, so thanks to all of you.

    I have finally settled in here and see how they work their system. It does not matter which tool you set off with... you move it away that certain safety amount off the part and then origin it... then home the machine and start the program with the W-difference between the two. Then touch off all tools from that distance and see the difference between them. So your new G50 when you retract a tool is the difference between your touch off tool and the tool that is currently in the turret. So the position that you always return to according to the machine co-ordinates is the same no matter which offset is active. That way you can see if you are off with a tool, when you G50 retract and it does not match up wit the machine position from home to your first "workshift" then you know that something is wrong.

    In X just take a cut, measure, then go into machine lock and move the measured distance in X. Then zero X and home it. That would be your G50 X value for that tool.

    And the way that they do it is return to a position at the top of the program without having to home every time. So the top of the program tells it to go G28 U0.0 W0.0 and then to G00 U-50.0 W-500.0 (theoretically where the first tool is 150.0 mm away in Z and the X is just off it's home) but at the bottom of the program it does not tell it to go back to the start, it tells it to go to just after that block so that the machine does not have to home before every cycle, just starts from where it is.

    So if the operator moves the Axis at all they have to do is "reset" "program" and it does the whole homing again and starts from the correct G50 position.

    Hello NAST555,
    Effectively, its the method I described in my Post#10, except that the Reference Return and Incremental Shift at the start of the program are able to be Block Skipped so that that move is not performed every cycle of the machine.

    Quote Originally Posted by angelw
    Rather than have the machine perform a Reference Return and then an Incremental Shift each new cycle of the machine, its also quite common to have the program arranged as follows:

    /G28 U0.0 W0.0
    /G00 U-100.0 W-500.0
    G00 T0100
    G50 X300.0 Z100.0
    G50 S3000
    G96 S200 M03
    G00 X50.0 Z10.0 T0101 M08
    --------------
    --------------
    --------------
    G00 X300.0 Z100.0 T0100 M09
    M01
    It does matter "which tool you set off with". It should be the tool protruding the most forward from the face of the Tool Turret. Set this tool at a safe distance and all other tools will clear by a greater margin.

    Regards,

    Bill

  8. Likes NAST555 liked this post
  9. #28
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,587
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    658

    Default

    Yup,
    Exactly Bill. I just needed to see it and work with it a bit to wrap my head around it. They use a M99 P3 at the end of every program so it cycles back to just after the home part of the program.
    So it looks something like this

    G28 U0.0
    G28 W0.0
    G00 U-50.0 W-500.0
    N3
    bla bla bla
    M99 P3

    So if the operator moves the position of the turret at all he starts from the top of the program, or else if just runs as normal without homing before every cycle.


Tags for this Thread

Bookmarks

Posting Permissions

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