556,751 active members*
6 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 31
  1. #1
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Tool zero macro

    I have acquired a tool setter and the most aggravating thing about it is that I have to set tool zero length each time the machine is powered up. It winds up being quicker to measure the tool with the height gage and enter it manually........


    I am thinking a Macro or keystroke that calls tool 0 and the X, Y and Z coordinates to put it in position with a keystroke or two?? Linux is definitely not my strong suit, and maybe someone has already done this??

    any insight on this would be much appreciated,

    thanks
    mike sr

  2. #2

    Join Date
    Mar 2020
    Posts
    211

    Re: Tool zero macro

    It does seem like a g37.2 or something would be a nice feature to add to do this on machine power up. If it could be that simple, I'd just add it to the end of my regular warmup cycle. Though with the bt30 spindle, the lack of spindle positioning would be a problem as that only gets enabled when you have an ATC.

  3. #3
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    I have a 10 year old 1100 s3 without the tool changer, when I power down the computer and restart it I need to reset tool zero. Once the machine is referenced, a Macro/keystroke to set the XY coordinates would work I am thinking?? I have the toolsetter mounted on a pedestal with a magnet in the base so I can remove it easily when not in use, maybe I will get used to this over time who knows. It just seems like it should be bit more automated than it is.........
    mike sr

  4. #4
    Registered
    Join Date
    Jun 2005
    Posts
    631

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    I have acquired a tool setter and the most aggravating thing about it is that I have to set tool zero length each time the machine is powered up. It winds up being quicker to measure the tool with the height gage and enter it manually..........
    Kinda confused here. Are you setting a length for tool number zero? How do you setup tool offsets in general?

  5. #5
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    Quote Originally Posted by shred View Post
    Kinda confused here. Are you setting a length for tool number zero? How do you setup tool offsets in general?
    What I want to do is reference the spindle nose without the hassle of positioning it by eye.
    At my age confusion, loosing train of thought is kind of normal for me Ha!

    I wrote a small code that positions the Z X Y which is basically what I wanted
    G54 G0 Z5
    X12 Y2
    this puts the spindle over the tool setter in the correct position for my machine to reference the spindle nose position.
    It would be nice if there was a way to select the spindle ref button in the code as well, but the aggravating part was the positioning of the spindle so that its the same each time its referenced.
    mike sr

  6. #6
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    I tried out the code and it didnt work out, I changed it to
    g55 g0 z-5
    x18.25 y-4.125

    this seems to work OK.
    the Axes are all z0x0y0 after referencing, then the above code works at least for now.
    I have lots to learn about hand coding!
    mike sr

  7. #7
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    I have always set tool heights with a digital height gage and entered them manually.

    This tool setter is new to me and I dont have a handle on it yet.
    I am setting the tool 0 - spindle nose touch off in the ETS setup column.
    then setting the tools by entering the tool number and press set "tool height" in the offsets page and it does it automatically.

    my hangup is setting the spindle position so that its in the same position each time. I may be just over thinking it though.

    thanks all for your efforts guys!
    mike sr

  8. #8
    Registered
    Join Date
    Nov 2007
    Posts
    2146

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    I have always set tool heights with a digital height gage and entered them manually.

    This tool setter is new to me and I dont have a handle on it yet.
    I am setting the tool 0 - spindle nose touch off in the ETS setup column.
    then setting the tools by entering the tool number and press set "tool height" in the offsets page and it does it automatically.

    my hangup is setting the spindle position so that its in the same position each time. I may be just over thinking it though.

    thanks all for your efforts guys!
    I think you need to download the most recent version of path pilot manual and look at ets setup section
    I would also guess you might need to be on the most recent version of PP install for manual to fully apply

    That said my router uses a electronic tool setter. The PP control has an ets setup tab-page and there is a button to go to the ets location. There is also a button you press to set the ets location.
    Then in router programs it calls for a tool and goes over to the ets location and waits for tool change and to set tool height.
    Codes g37 and g37.1 control the ets automatically these codes were added to PP ver 2.4.0

    anyway here is a
    copy clip from manual to set position

    Set the G37 Position
    1. Remove the collet nut and the tool from the spindle.
    2. From the PathPilot interface, in the Tool DRO field, type
    0. Then select the Enter key.
    3. Jog the spindle until it's over the ETS, and center the
    spindle over its contact pad.
    4. Jog the Z-axis up (+Z) until it's at a safe clearance height
    for your longest tool.
    NOTICE! If the Z-axis is set below the highest
    position, there's a risk of tool collision.
    5. From the PathPilot interface, on the ETS Setup tab, find
    the ETS G37 Position Setup group, and select Set G37
    ETS Position.
    Figure 7-46: Set G37 ETS Position on the Probe tab.
    The G37 position is now set.
    6. Verify that the X, Y, and Z ETS position displayed in their
    DRO fields are accurate.




    Edit
    I also copied a clip of code for a tool change using an e.t.s.

    N10 G90 G64 G50 G54 G80 G17 G40 G49
    N20 G20 (Inch)


    (Roughing waterline surface)
    N30 G30
    N40 G37.1
    N50 T4 M6
    N60 G37
    N70 G43 H4
    (Fly Cutter)
    N80 S11000 M3
    N90 G0 G94 X-2.2494 Y-3.0146
    .
    .
    .
    .

  9. #9
    Registered
    Join Date
    Jun 2005
    Posts
    631

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    What I want to do is reference the spindle nose without the hassle of positioning it by eye.
    At my age confusion, loosing train of thought is kind of normal for me Ha!

    I wrote a small code that positions the Z X Y which is basically what I wanted
    G54 G0 Z5
    X12 Y2
    this puts the spindle over the tool setter in the correct position for my machine to reference the spindle nose position.
    It would be nice if there was a way to select the spindle ref button in the code as well, but the aggravating part was the positioning of the spindle so that its the same each time its referenced.
    That makes more sense. Does your work setup require re-zeroing off the spindle every time? When I was doing something similar, if all my tools needed had lengths already set, I'd ref the machine, load up the first tool in the program (or a Haimer once I got one of those), drive it over to the workpiece and zero work coordinates there and run, but I was programming parts off the stock and had a lot of pre-set tools.

    edit: the G37 stuff above looks cool too. I'll have to check it out.

  10. #10
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    Does your work setup require re-zeroing off the spindle every time?
    I usually re probe for each program change then may run several parts off that program, I do not rezero for each individual part.
    I also have most of my tools preset for the ones that I use most often.

    Most of my parts are proven programs (unless they want changes) then thats a bear that they dont understand!

    This tool setter is new and I will figure it out but its going to take some time.......

    mike sr

  11. #11
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    I now have it set up for G59 (an unused one) this works as long as I reference the machine and set G59 all axes to 0. then run the small program to position the spindle to the tool setter.
    edit: I did add a g54 at the end of the program to put it back to g54 as I forget to do that..
    I am using 2.8.3 PathPilot. mill Is an 1100 s3.

    I will check out the router version for the spindle locate function. Thanks MD
    mike sr

  12. #12
    Registered
    Join Date
    Jun 2005
    Posts
    631

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post

    I usually re probe for each program change then may run several parts off that program, I do not rezero for each individual part.
    I also have most of my tools preset for the ones that I use most often.

    This tool setter is new and I will figure it out but its going to take some time.......
    Yeah, it changes things quite a bit, but they are very useful. I had to redo how I did tool lengths when I went to a BT30 machine and that took a while to set in.

    If your tools are already set you should just be able to probe and go and skip zeroing the toolsetter.

  13. #13
    Registered
    Join Date
    Nov 2007
    Posts
    2146

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    I

    I will check out the router version for the spindle locate function. Thanks MD
    The router is the only machine I have that uses a e.t.s. so I used it as an example.
    If you look in manuals this was all added to path pilot for use with the mills.
    I would guess it is very useful for mx mills with bt taper tool holders and tool changers. Offline tool height setting would be less then desirable.
    Anyway I dont see a reason to use a g offset to find your tool setter location. It is built into the PP software to use the g37 location.
    Hope this helps!

  14. #14
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    I understand the g37 location, what I am trying to achieve is to get the spindle position the same reference position each time for the spindle height from the nose for tool zero the height can vary somewhat if the spindle isnt in the exact location as it was previously used.
    This needs to be done each time the power is cycled, so the height will vary slightly depending on the exact position of the spindle to the tool setter as that little plate isnt perfectly flat.I am probably splitting hairs who knows?? That little program positions the spindle to the toolsetter the same each time for me as my toolsetter is always in the same position on the table.

    This at least gives us something to read besides facebook!!
    mike sr

  15. #15
    Registered
    Join Date
    Dec 2008
    Posts
    740

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    I understand the g37 location, what I am trying to achieve is to get the spindle position the same reference position each time for the spindle height from the nose for tool zero the height can vary somewhat if the spindle isnt in the exact location as it was previously used.
    This needs to be done each time the power is cycled, so the height will vary slightly depending on the exact position of the spindle to the tool setter as that little plate isnt perfectly flat.I am probably splitting hairs who knows?? That little program positions the spindle to the toolsetter the same each time for me as my toolsetter is always in the same position on the table.

    This at least gives us something to read besides facebook!!
    Hi Mike. I‘ve not been here for some time. Just saw your question.
    If I understand your issue correctly I think you might be looking for G53. Use the coordinates you specified earlier and it should move to that position, irrespective of the current table position. Just make sure you have enough Z clearance!
    Step

  16. #16
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    Thank you Step, Its really good to hear from you again!
    I will check out the G53 as thats what I am looking for is a command that will give me the same position each time regardless. The little program does what I want but I have to reference the machine and set all axes to 0 to get it to work the same each time. It just seems odd to me that this isnt built into the tool setting routine.
    mike sr

  17. #17

    Join Date
    Mar 2020
    Posts
    211

    Re: Tool zero macro

    G53 is just machine coordinates without a work offset. As I was reading through this morning and saw that you were using G54 and then 59, I had the same thought. G53 will always be pure machine position, with no offset that can ever be changed by the user so it will be much more stable than any WCS, even an used one. Just take your existing program and change the G59 to G53, everything else can stay the same. Doesn't help with the automatic checking of the nose but it's something at least. Now that all this has been discussed, I think I'm going to do the same and add the move to the end of my warmup cycle so all I have to do is hit the ets ref button.

    For what it's worth, referencing my ets every power cycle typically sees the offset vary by .0001-.0008 anecdotally so it's not a lot but it's there. I've started doing the referencing on power up AND I set my tool length after every tool change and I have noticed an improvement in my parts, specifically when pocketing with a larger tool and then finishing the corners/edges with a smaller one. I used to always have a slight mismatch in the Z of the floor between the too tools but that hasn't happened since adding those two steps to my workflow. Each tool gets probed and length set as soon as it's loaded in the spindle (part of David Loomes's post processor). It adds time to the tool changes but it's been worth it for the improvement in the parts.

  18. #18
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    thank you sir, I will try that........
    I just cant see doing something by eye when the machine can do it.
    mike sr

  19. #19
    Member
    Join Date
    Jun 2014
    Posts
    1728

    Re: Tool zero macro

    g53 g0 z6
    x18.25 y2.5

    This works as long as g54 is set all axes 0 after referencing the machine, then the program works, it doesnt if a work offset is set in g54 after referencing, then the program is run again.
    This works after a machine startup reference is done and all axes set to 0, then it will work fine.
    mike sr

  20. #20
    Registered
    Join Date
    Dec 2008
    Posts
    740

    Re: Tool zero macro

    Quote Originally Posted by popspipes View Post
    g53 g0 z6
    x18.25 y2.5

    This works as long as g54 is set all axes 0 after referencing the machine, then the program works, it doesnt if a work offset is set in g54 after referencing, then the program is run again.
    This works after a machine startup reference is done and all axes set to 0, then it will work fine.
    Try
    g53 g0 z6 x18.25 y2.5
    on ONE line. G53 is non-modal so it reverts back to your G54 for the x/y move.
    I can‘t get it to NOT work!
    Step

Page 1 of 2 12

Similar Threads

  1. Replies: 0
    Last Post: 09-24-2019, 11:09 AM
  2. Need help with Macro for checking tool length before tool change
    By mioduz in forum Tormach Personal CNC Mill
    Replies: 11
    Last Post: 04-18-2014, 08:43 PM
  3. tool change and measure tool lenght, macro?
    By Charon in forum Mach Wizards, Macros, & Addons
    Replies: 3
    Last Post: 03-20-2012, 06:56 PM
  4. Tool Change Macro Help Please
    By Ecmdrw5 in forum Fanuc
    Replies: 0
    Last Post: 04-08-2011, 12:46 PM
  5. Replies: 0
    Last Post: 02-14-2010, 07:26 PM

Tags for this Thread

Posting Permissions

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