Fanuc 0T Tool Setting and Work Shift Help
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Jul 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    54
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    12

    Default Fanuc 0T Tool Setting and Work Shift Help

    I'm not super savvy with lathes so forgive me if I'm overlooking something obvious.
    New machine to me, Murata/Warner Swasey WSC6 with Fanuc 0T (not sure which version) and all jaws and parts are programmed offline in CAM.

    This machine uses work shift and does not have work offsets like on other lathes I have run. Since I have to pick one zero point and stick with it I would like to use the face of the chuck. This seems easiest to me for quick changeover of parts. For example if I put in a set of 1.5" thick pie jaws that need to be faced I could just add 1.5" to the work shift, or better yet use the face of the chuck as my zero point in CAM with my jaws modeled 1.5" thick. Is that how the work shift function is meant to be used?

    When I go to set my first OD tool T0101 I jog in Z up to the chuck and back it off while I roll a 1/2" dowel pin around until it slips through. This should put my tool at Z0.5". On the control in the offset/geometry page I enter M, Z, 0.5, input and get T0101 Z =-0.5". This seems like it could be right so far, though I kind of expected some arbitrary number, but again not sure how the work shift function might change things.
    I repeat this for a boring bar that is a very different length and end up with T0202 Z =-0.5". This does not seem right any more, as this part that is about 1" longer should show up as 1" different length in the offset/geometry page.

    It took me going down a YouTube rabbit hole to figure out that pressing M before the axis meant measure, so it is highly likely that I am missing some other step, but its also likely I'm going about this process completely wrong.
    Any advice on this would be much appreciated, this machine has been sitting idle while I manage other projects but I finally have enough work that it seems worth figuring it out.

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,137
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1756

    Default

    What you're describing are two different exercises. One is setting the Work Coordinate System and the other, the geometry setting of the cutting tools in the Z axis.

    When setting the Tool Geometry Offsets, its creating a relative difference between the length of the cutting tools, therefore, when setting the Z Tool Geometry Offsets, there is no requirement to specify a Z coordinate. Accordingly, what is used as the reference in Z is irrelevant, provided that the same reference is used. Some, for example, use a magnetic, dial indicator tool setting device that is applied to the face of the chuck, with all tools being touched off on this tool setter. In the X axis, the reference is the centre line (X0.0) of the machine and of course, this never changes (unless the machine is crashed).

    Is your control a circa 1990 FS0T, or a much later OT control? Perhaps posting a picture will help the Forum members give accurate advice.

    Its when setting the Z Workshift Offset that a Z Coordinate may have to be specified, but the process differs from setting Tool Geometry Offsets, in that the Workshift Page has to be brought to the foreground.

    Using the face of the chuck, or a dead stop in the chuck, as the Workpiece Z datum may make setting the Z Coordinate System easier (it may be the same for every job you do), but it has its own set of dangers. When using the end of the Workpiece closest to the chuck as the Z datum (Z Zero), all Z coordinates in the part program will be plus values (except where a drilling, or boring operation may pass beyond the Z Zero).

    With a Fanuc Control, coordinates must include a period, or include all trailing Zeros in a value that is an integer. For example, a control set to use a Metric units and where the least programmable increment is 0.001mm, a programmed value such as Z50 (no period included), the control will decode that as Z0.050. The Fanuc control can be set via parameter to read a coordinate where the period has been omitted as an integer, Fanuc refer to this as Pocket Calculator Mode, but the default is for the period to be included. In the default system, the above example of Z50 to be specified without a period would require the coordinate to be specified as Z50000.

    So now to cut to the chase and explain why using the end of the workpiece closest to the chuck can be risky with a control that requires the period to be included in the coordinate.

    Lest say that the length of the Workpiece from Z Zero (close to the chuck) is 100.mm. In this case, the initial approach to the Workpiece in the Z axis may be G00 X_ _ Z110., which would result is a standoff of 10.0mm in Z. If, during an edit of the program, or for whatever reason, the period was omitted and therefore the coordinate in the program appeared as Z110, the control will decode that coordinate as Z0.110. The coordinate Z0.110 is 0.110mm from the end of the Workpiece closest to the chuck and a certain, major crash if not noticed before execution.

    With the same 100.mm long part, where the Z Zero of the Workpiece is closest to the tail-stock, the same 10mm standoff for the initial approach is achieved with the following command block:

    X_ _ Z10.

    If the period were to be omitted in the above example, the control would decode Z10 as Z0.010. In this case, if the tool was not clear of the Workpiece in X, then the tool would finish very close to the end of the Workpiece without hitting (if the part had already been faced to finished length), or hitting by only the finish allowance in Z. In the scenario where the tool hit by the finishing allowance, the insert will probably be damaged and perhaps the tool holder, or at worst the Workpiece may be dislodged, but the result wont be the catastrophic crash from the tool trying to get to Z0.110 at the chuck end of the Workpiece.

    Regards,

    Bill

  3. Likes yardbird liked this post
  4. #3
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,383
    Post Thanks / Like
    Likes (Given)
    360
    Likes (Received)
    855

    Default

    Sounds like my control. You have two considerations: G50 and TXXXX.

    The best way I've found is to set your G50 when your cutoff is at Z0 X0. Then set all your other tool offsets from there. That way you home the machine and call a G50 X___ Z____ that sets your work zero at the cutoff tool zero and all your other tools get set off this.

    The thing is you need something to reference the center of that chuck, and using your cutoff tool seems to be a great way to do it.

    So, cancel all tool offsets and home the machine.

    Move your cutoff tool to where you want X0 Z0 to be for that tool.

    These machine coordinates will be your G50 line in all your programs (mine shows machine in metric always, no way to change it that I can find, so I have to convert to inch to put it into a program).

    Your cutoff tool will have no geometry offsets.

    Now you write a program that just calls that G50 line and you can touch off your other tools. Mine is just:

    O0001;
    G50 X_____ Z_____;
    M30;

    Run the program and touch off your other tools in X and Z, entering the coordinates in their geometry offsets. Mine does not have an Input C. or Measure function so I have to hand enter them.

    If you need to double check just MDI the tool offset and check your position before moving to the next tool.

    I then have a G28 U0 W0 line followed by a G27 position check, followed by the G50 line in the startup code of all my programs. THis homes the machine, check to make sure it is homed, and then sets the machine work offset.

    Hope this helps.

    EDIT: Spelling

  5. Likes LostFab liked this post
  6. #4
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,931
    Post Thanks / Like

    Default

    Excellent explanation of how and why tool setting and work shift setting works, Bill.

    Lostfab:

    In your description of the procedure you use I see two things that don't seem right to me.

    1, You are setting your tool with offset applied i.e. T0101. I have always used T0100. Your machine may have tool parameters set differently than mine.

    2. I don't see the OFSET MESUR button in your sequence. Should be: M -> Z___ -> OFSET MESUR -> INPUT This is the sequence I use in tool setting and work shift setting.

    Once the Z is established for tool 1, I use whatever location tool 1 is in Z as the keyed in Z value for work shift.

    Pages from my manual for 0TC:

    tool-setting-1.jpg tool-setting-2.jpg work-shift.jpg

  7. Likes LostFab liked this post
  8. #5
    Join Date
    Jul 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    54
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    12

    Default

    I should have included the year, I believe it is 1988.

    I understand that the work offset and tool offsets are different. I don't understand how a work shift is different than a work offset. It seems like a work shift means there is only one work offset. If I only have one I want to use the chuck face because everything will be programmed relative to that in CAM. If I swap between collets, pie jaws, etc..., I already have them modeled relative to the chuck face.
    In my head that process means I should never have to change the work shift or tool offsets regardless of what parts and work holding I am running, set it once and then leave it forever...
    Like how I set up on a mill but without the convenience of multiple work offsets for vise stations, tools are set to the table once and a vise as the work offset, G54 Z isn't necessarily zero but it never needs to be changed.

    I do not have an offset measure button. In a YouTube video I watched someone pressed the M key on the control, followed by the axis, the value (either 0 for Z, or part dia for X) and input.

    I'm wondering what the sequence is to set my tool lengths. I don't want to manually enter the value from the position page into the offset page. That seems like a recipe for disaster, as Bill mentioned adding or missing a 0 or . could cause a crash.

    pxl_20210531_163959838.jpg

    Right now when I press "M, Z, 0, INPUT" it just changes Z to 0, rather than the tool length. If I try that for two tools that are 3" different length I would expect that value to be 3" different, but they are both 0.

  9. #6
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,931
    Post Thanks / Like

    Default

    Post picture of your complete control panel.



    Not the best picture in the world. OFSET MESUR button is (was) white button, top row, far right of lower keypad.
    9517_marathon-sl320-b-2.jpg

  10. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,137
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1756

    Default

    Quote Originally Posted by LostFab View Post
    I should have included the year, I believe it is 1988.

    I understand that the work offset and tool offsets are different. I don't understand how a work shift is different than a work offset. It seems like a work shift means there is only one work offset. If I only have one I want to use the chuck face because everything will be programmed relative to that in CAM. If I swap between collets, pie jaws, etc..., I already have them modeled relative to the chuck face.
    In my head that process means I should never have to change the work shift or tool offsets regardless of what parts and work holding I am running, set it once and then leave it forever...
    Like how I set up on a mill but without the convenience of multiple work offsets for vise stations, tools are set to the table once and a vise as the work offset, G54 Z isn't necessarily zero but it never needs to be changed.

    I do not have an offset measure button. In a YouTube video I watched someone pressed the M key on the control, followed by the axis, the value (either 0 for Z, or part dia for X) and input.

    I'm wondering what the sequence is to set my tool lengths. I don't want to manually enter the value from the position page into the offset page. That seems like a recipe for disaster, as Bill mentioned adding or missing a 0 or . could cause a crash.

    pxl_20210531_163959838.jpg

    Right now when I press "M, Z, 0, INPUT" it just changes Z to 0, rather than the tool length. If I try that for two tools that are 3" different length I would expect that value to be 3" different, but they are both 0.
    The single Workshift and Work Offsets (as in G54 to G59) are basically the same. With a control that is equipped with the Work Offset option, you will often (typically) see the Offsets, G54 to G59, also labeled `1 to 6 respectively. There will also be another Work Offset on the same page typically labeled Ext and "0". This Work Offset is in fact G52 and values applied to that Offset affect all other offsets G54 to G59.

    Programmatically, G52 can be used to apply what Fanuc refer to as a Child Offset with in the part program. One use, for example, is if a number of parts were set on the machine table, all requiring the same machining operations. In this case, an initial Work Offset, say G54, could be used to establish the Work Coordinate System for the fixture or first component, then G52 executed with a relative coordinate to the first part Zero. To cancel and come back to the initial G54 Offset, the following command is executed:

    G52 X0.0 Y0.0

    When using G52 in the part program, the values registered in the Ext (number "0" Work Offset) are typically Zero.

    With a lathe that has just the one Worshift, it works the same as the Ext Work Offset of a control that has the G54 to G59 Offset option, only there are no other Work Offsets to which its value is applied.

    I wouldn't expect the value to be calculated by the control to be Zero, but the value calculated would be the same for whatever tool is used in the Work Offset setting process. Whatever Workshift Offset value that is set will be correct for every tool used in the program; accordingly, it would be logical for the same value to be calculated by the control irrespective of the tool used in the Workshift Setting process. The control takes into account the Tool Offset of the tool being used in the setting process. As shown in Alphonso's Post showing pictures of pages from the operator's manual, the tool and its offset are called up for use in setting the Workshift Offset.

    Regards,

    Bill

  11. #8
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,383
    Post Thanks / Like
    Likes (Given)
    360
    Likes (Received)
    855

    Default

    If he has an A or B, then I don't think it has the measure function.

    OP, you are correct that work shift is basically one work offset system. Re-read my post; you can set your G50 zero as the front of the chuck, but you need to reference it to something. WHAT is at the front of your chuck when the machine thinks it is at G50 X0Z0? That's why I like using the cutoff tool. Other than maybe a bar puller, it is most likely to be the tool that gets closest to the spindle face during operation.

    Also, you cannot have a work offset active when you measure work offsets on an 0TA. You can T0000 or I suppose you could T0100 for Tool 1, but I see no reason to ever use anything but T0000? You will have parameters that change how the control treats two digit or four digit tool offset calls.

    The only time I used work shift was when programming a very old turret punch press, that used work shifts and then relative movements to punch all the features for parts on a single large sheet. The was on a General Numeric GN-6...

    EDIT: BTW, the other reason I like my method is that it eliminates problems with the tool offset being called during work shift setting, because the tool offsets for the cutoff tool are always zero.

  12. #9
    Join Date
    Jul 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    54
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    12

    Default

    Quote Originally Posted by Rick Finsta View Post
    Also, you cannot have a work offset active when you measure work offsets on an 0TA. You can T0000 or I suppose you could T0100 for Tool 1, but I see no reason to ever use anything but T0000? You will have parameters that change how the control treats two digit or four digit tool offset calls
    That is the Fanuc control panel, the rest if it is the W&S specific control
    pxl_20210531_232548418-1-.jpg

    So to call up a tool when I want to set I should use T__00 (ex. T1=T0100, or T12=T1200)? Ang every program should call up a G50 like I use a G54 on a mill?
    I have just been using the turret fwd/rev buttons after I zero ref the axis, not actually using MDI to call a tool.
    I guess what I really want to know is do I just have to enter the position values manually? I was really hoping there was a "tool offset measure" function hidden away in some combination of keys but it sounds like that wont be the case on this control...
    Attached Thumbnails Attached Thumbnails pxl_20210531_163959838.jpg  

  13. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,137
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1756

    Default

    Quote Originally Posted by LostFab View Post
    That is the Fanuc control panel, the rest if it is the W&S specific control
    pxl_20210531_232548418-1-.jpg

    So to call up a tool when I want to set I should use T__00 (ex. T1=T0100, or T12=T1200)? Ang every program should call up a G50 like I use a G54 on a mill?
    I have just been using the turret fwd/rev buttons after I zero ref the axis, not actually using MDI to call a tool.
    I guess what I really want to know is do I just have to enter the position values manually? I was really hoping there was a "tool offset measure" function hidden away in some combination of keys but it sounds like that wont be the case on this control...
    The way in which the tool geometry and workshift is applied is up to the MTB. Accordingly, not all machines with the same model control have the same procedure.

    Do you have the operator's for the machine? I see a Set Up button on the control panel; I suspect that may have something to do with tool and workshift setting.

    Regards,

    Bill

  14. Likes LostFab liked this post
  15. #11
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,383
    Post Thanks / Like
    Likes (Given)
    360
    Likes (Received)
    855

    Default

    Quote Originally Posted by LostFab View Post
    So to call up a tool when I want to set I should use T__00 (ex. T1=T0100, or T12=T1200)? Ang every program should call up a G50 like I use a G54 on a mill?
    I have just been using the turret fwd/rev buttons after I zero ref the axis, not actually using MDI to call a tool.
    I guess what I really want to know is do I just have to enter the position values manually? I was really hoping there was a "tool offset measure" function hidden away in some combination of keys but it sounds like that wont be the case on this control...
    I just use T0000 (gang tool machine), but TXX00 should correct for a turret machine to cause it to index but not make the tool offset active.

    You can either use G50 on every program like you would G54, etc. or you can just program your individual tool offsets without ever using G50 and they will all be referenced to machine zero. I like using G50 because it allows me to glance at offset number and know if they make sense. It also allows me to change my Z offset for a certain program or in the middle of a program and all the tools move respective to that change, and respective to my cutoff tool for easy visual reference (for me).

    Lots of ways to skin this particular cat. Hopefully you figure out a way to automatically input offset numbers. On mine the instructions are very convoluted, assuming you are going to set up the table at a certain zero and program everything off that point, so they want you to write a program and execute it in single block and somehow the control will update the offsets, but it doesn't make *any* sense to me at all. So I just take a cell phone picture of the numbers and enter them on the table. I can verify they make sense with a scale or tape measure relative to my cutoff tool.

  16. Likes LostFab liked this post
  17. #12
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    3,008
    Post Thanks / Like
    Likes (Given)
    585
    Likes (Received)
    959

    Default

    LostFab- everything you are doing is ok. You are setting your geom offsets in Z @ .5 from the chuck face. When you call the tool T0101 your position display is Z.5. With your tool 1 offset active that's what you should get (with a Z workshift of zero) That's what you told the machine! All is good. Go look at the Z geom offset value- it will be a large number- the distance from your Z home position to when the tool is .5 from the chuck face. On edit- you should not have any tool offsets or work shifts active when setting geometry offsets- home the machine, jog your tools to your dowel pin, go to the geom offset page, scroll to the tool line and then "M Z # enter. NOW after your tools are set- you need to use the WORK SHIFT Z value to tell the control how far from your dowel pin to your programmed part Zero. Remember one thing- its a work SHIFT - not a work OFFSET- you are moving the part- not the tool- all it really means is its opposite of a an offset. ALWAYS have your work shift value at Zero when setting your geometry offsets. One last thing for a sanity check- ALWAYS add an extra 3" or other safe value to your workshift value to run your 1st part- then use a ruler to check your Z positions. One last comment- and just a preference of mine as I totally understand how G50 works- don't use it if you have Geometry offsets- its much easier and less prone to crashes if you go brain dead for a second. Use G50 to clamp your spindle speed only.

  18. Likes LostFab liked this post

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
  •