Haas Safe Tool Change Posistion with Parameter 210 & 266
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    Join Date
    Dec 2011
    Location
    Whitehall, MI
    Posts
    565
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    139

    Default Haas Safe Tool Change Posistion with Parameter 210 & 266

    I just found out how to get the Haas mills to go to a set posistion whenver M06 or ATC FWD/ ATC REV Button is pushed, using Paramter 210 and Paramter 266 for X axis. But if the Z axis is down by the part, and you do a tool change all three axis move to the tool change posistion at the same time. Does anyone know how to have the Z axis come up first?

    (The program itself is set for safe tool change posistion, but sometimes the operator will want to look at a tool and not think about what's going to happen and whack the part or fixture. I also always make it so they just have to go to MDI and push start and it moves to the safe posistion, but......)

  2. #2
    Join Date
    Jan 2009
    Location
    CA, USA
    Posts
    835
    Post Thanks / Like
    Likes (Given)
    148
    Likes (Received)
    201

    Default

    Quote Originally Posted by brian.pallas View Post
    But if the Z axis is down by the part, and you do a tool change all three axis move to the tool change posistion at the same time. Does anyone know how to have the Z axis come up first?
    What year machine? This has never been the case on any Haas I've ever been on...in fact, it is pretty bad practice IMO to move all three on a tool change. (as is the reason for your post...). Every Haas I've ever been on only moves Z to the tool change position.




    Quote Originally Posted by brian.pallas View Post
    I also always make it so they just have to go to MDI and push start and it moves to the safe posistion, but......)
    So, IOW, MDI, which is easily altered, is engrained in their fingers as a quick safe move? This could go bad quick.

  3. #3
    Join Date
    Dec 2011
    Location
    Whitehall, MI
    Posts
    565
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    139

    Default

    If you use parameter 210 and type in an X number and then go to paramter 266 and set "Zero Axis TC" to 1, the machine will move to that spot you defined whenever any toolchange is commanded, even using an ATC FWD or REV button.

    Except that if the Z isn't home it will move Z to home while it's moving to the safe X posistion, with pushing the ATC FWD button.

    The question I have is does anyone know a way in this setup to have the Z come up first?

    I'm just looking to prevent a crash as much as possible.

  4. #4
    Join Date
    Jan 2011
    Location
    South Florida
    Posts
    624
    Post Thanks / Like
    Likes (Given)
    64
    Likes (Received)
    118

    Default

    Why are you adding an X move to the tool change?????

  5. #5
    Join Date
    Jan 2009
    Location
    CA, USA
    Posts
    835
    Post Thanks / Like
    Likes (Given)
    148
    Likes (Received)
    201

    Default

    Quote Originally Posted by machineit2 View Post
    Why are you adding an X move to the tool change?????
    Only reason would be some crazy high setup on the table that needs to be avoided.

  6. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,725
    Post Thanks / Like
    Likes (Given)
    311
    Likes (Received)
    1822

    Default

    Quote Originally Posted by tc1999 View Post
    Only reason would be some crazy high setup on the table that needs to be avoided.

    Nah, that would still be a problem!
    Think about it. If the toolchange must be done at a very specific X and Y position for the Z to clear, then you would have the same problem getting to that X and Y position WHILE the head is at Z0.

    And yes, having a standard MiniMill I do need to be aware of what's where on the table, so often times I need to make sure it moves appropriately, and by that I need to know where I am at and how to get to the safe
    spot.

    OTOH, Brian only mentioned an X move before the toolchange, not Y. This doesn't make much sense other than perhaps the case where the rotary axis is mounted on the left ( I have it that way on the VF4 with the 6" rotary )
    In that case you may not want to have your umbrella swinging with long tools just anywhere, or your sidemount to whack right above. A single X move is sufficient, but then the question is why can't one make sure the tool is above the part
    before initiating a FWD/RV change?

    To the OP, sorry, I can't answer that. I also can't answer why most mills do not have an incremental axis command such as on the lathes. ( U, W, V etc. )

  7. #7
    Join Date
    Jan 2011
    Location
    South Florida
    Posts
    624
    Post Thanks / Like
    Likes (Given)
    64
    Likes (Received)
    118

    Default

    Quote Originally Posted by tc1999 View Post
    Only reason would be some crazy high setup on the table that needs to be avoided.
    True, but that would be different for each set-up.

    I run shafts in my mill that require me to run with Z in a positive position of sometimes 3+ inches and I program my clearance moves into the program itself. But, I would never leave it in the control for all programs. That just makes little sense to me.

    Mike

  8. #8
    Join Date
    Jan 2009
    Location
    CA, USA
    Posts
    835
    Post Thanks / Like
    Likes (Given)
    148
    Likes (Received)
    201

    Default

    Quote Originally Posted by SeymourDumore View Post
    Nah, that would still be a problem!
    Think about it. If the toolchange must be done at a very specific X and Y position for the Z to clear, then you would have the same problem getting to that X and Y position WHILE the head is at Z0.
    I have thought about it and have actually needed to do it...

    -Current tool goes to a Z-clearance move (which may be above the tool change position),
    -then move table, change tools to a long tool,
    -then you call a G43 after the tool change with a positive Z move (obviously)so that new tool clears before moving table.

    I've done it a bunch in the past...also, not sure in this scenario, but what about a SMTC? You may be OK at Z0 on every tool but what happens when the arm drops 4"



    Quote Originally Posted by machineit2 View Post
    True, but that would be different for each set-up.

    I run shafts in my mill that require me to run with Z in a positive position of sometimes 3+ inches and I program my clearance moves into the program itself. But, I would never leave it in the control for all programs. That just makes little sense to me.

    Mike

    I couldn't agree more which is why I said what I said. (some crazy high setup...i.e: not normal...)

  9. #9
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,725
    Post Thanks / Like
    Likes (Given)
    311
    Likes (Received)
    1822

    Default

    TC

    That's the point!
    If your setup is high, you need to do this:

    Quote Originally Posted by tc1999 View Post
    I have thought about it and have actually needed to do it...

    -Current tool goes to a Z-clearance move (which may be above the tool change position),
    -then move table, change tools to a long tool,
    -then you call a G43 after the tool change with a positive Z move (obviously)so that new tool clears before moving table.
    To be specific,, your clearance is above the toolchange Z!

    But Brian wants this:

    Except that if the Z isn't home it will move Z to home while it's moving to the safe X posistion, with pushing the ATC FWD button.

    The question I have is does anyone know a way in this setup to have the Z come up first?
    He only wants to move to Z-home, which will still interfere with the toolchange.

  10. #10
    Join Date
    Jan 2009
    Location
    CA, USA
    Posts
    835
    Post Thanks / Like
    Likes (Given)
    148
    Likes (Received)
    201

    Default

    LOL ...So really, he just needs to move Z to home before the machine moves out of the way?...

    I guess the answer is there is no way to do it in regards to how he is trying...? I have never put a X or Y more in the parameters for tool changes.

    Even if I had to do 1 program a month this way I would just do it manually I think. Since you manually have to change the parameters back and forth, I think I would just as soon make the program have the safe moves with the way the machine normally changes tools...

  11. #11
    Join Date
    Jan 2009
    Location
    CA, USA
    Posts
    835
    Post Thanks / Like
    Likes (Given)
    148
    Likes (Received)
    201

    Default

    Just thought of this also as an option...how about a post modification so you do a "G28 G91Z0" move before the tool change then when the M6 is called it will go to your X and Y position while Z is already home...?

  12. Likes RoboMiller liked this post
  13. #12
    Join Date
    Dec 2012
    Location
    Northeast USA
    Posts
    336
    Post Thanks / Like
    Likes (Given)
    299
    Likes (Received)
    76

    Default

    Quote Originally Posted by tc1999 View Post
    Just thought of this also as an option...how about a post modification so you do a "G28 G91Z0" move before the tool change then when the M6 is called it will go to your X and Y position while Z is already home...?
    i guess u could command z positive then have an m6 to get that extra clearance. but i have not done this

  14. #13
    Join Date
    Jul 2015
    Country
    CROATIA
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default

    hey guys, tomorrow I'm mounting 5 axis trunion to vf2 and I'll need a crash course how not to crash on tc.

    I know when the haas tec was here that he tried doing it through raw data (debug mode) and enter encoder value to it but it didnt work so he just said that i should use the safe loc in postproc.

    Thats not a solution for me, I need a way to do this every time the ATC forward or rev is pressed or m06 activated:
    1) Z goes to home position for TC
    2) X and Y go to my safe TC location (defined in parameters?)
    3) trunion goes to home (0 degree) in A and B axis (stupid how haas calls B axis what is really a C axis)
    4) tool change occurs

    in that order.

  15. #14
    Join Date
    Mar 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    633
    Post Thanks / Like
    Likes (Given)
    240
    Likes (Received)
    245

    Default

    How to Command a Safe Tool Change Position to Avoid Fixtures and Rotaries – Haas Tip of the Day - YouTube . Not shure if it works with the atc fwd /rev but you should not be in a habit of hitting that with tall fixxures etc on the table.

  16. Likes mkd liked this post
  17. #15
    Join Date
    Feb 2006
    Location
    greensboro, nc
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Exclamation Safe tool change position

    Quote Originally Posted by MK Proto View Post
    How to Command a Safe Tool Change Position to Avoid Fixtures and Rotaries – Haas Tip of the Day - YouTube . Not shure if it works with the atc fwd /rev but you should not be in a habit of hitting that with tall fixxures etc on the table.
    Mark's tip of the day refrenced above is perfect for your problem.
    i aliases the M6 code. very good and thorough explination.

  18. #16
    Join Date
    Mar 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    633
    Post Thanks / Like
    Likes (Given)
    240
    Likes (Received)
    245

    Default

    I just watched the whole video. he tells you how to lock the operator panel so that you cant use the atc fwd/rev.

  19. #17
    Join Date
    Sep 2009
    Location
    PA
    Posts
    1,464
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    407

    Default

    Quote Originally Posted by bill mccandless View Post
    Mark's tip of the day refrenced above is perfect for your problem.
    i aliases the M6 code. very good and thorough explination.

    did you have to turn off H/T code agreement?

    I have tried to implement the code in the video and have run into the H/T code don't match error. I have called the HFO, asked on the video and IG but have yet to get a response. I like having the H/T code agreement check and would rather not turn it off if possible.

    This is on a 2011 VF3.

    M6 alias for safe tool change

  20. #18
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,426
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1618

    Default

    Quote Originally Posted by allenp View Post
    hey guys, tomorrow I'm mounting 5 axis trunion to vf2 and I'll need a crash course how not to crash on tc.

    I know when the haas tec was here that he tried doing it through raw data (debug mode) and enter encoder value to it but it didnt work so he just said that i should use the safe loc in postproc.

    Thats not a solution for me, I need a way to do this every time the ATC forward or rev is pressed or m06 activated:
    1) Z goes to home position for TC
    2) X and Y go to my safe TC location (defined in parameters?)
    3) trunion goes to home (0 degree) in A and B axis (stupid how haas calls B axis what is really a C axis)
    4) tool change occurs

    in that order.
    Ya, well on the UMC it is B and C axis! Although the button on machine says A/C then has a little B in yellow, like they are too lazy to make a new button labeled correctly??

  21. #19
    Join Date
    Jun 2014
    Location
    Canada,Ontario,Barrie
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I wasn't happy with the Haas parameter trick myself (VF3 Y/T). It would move to a safe tool position but it would move axes simultaneously with the Z axis. It's too bad because this trick would work with the ATC FWD/REV buttons too. Maybe there is a solution out there but even a Haas rep wasn't sure how to get around it. I ended up aliasing M6 .
    Pro - You can move any axis however you want to. Z axis moves up first.
    Con - Doesnt work with ATC FWD rev buttons.

    How to set it up;
    1) Press settings button, turn off parameter 7
    2) While in setting turn off parameter 23
    3) Press param/dgnos button, set value parameter 81 to 6.
    4) Load M6 alias program below into memory. NOTE - If you have any programs named specifically O9000 you will have to rename your alias program to another 9000 program number and put the 6 value in the corresponding parameter (81=O9000).

    % O09000 (TOOL CHANGE)
    G103 P1
    IF [ #3026 EQ #4120 ] GOTO1
    G00 G91 G28 Z0
    G00 G90 G53 X-40. Y-26.
    G103 P0
    M16
    M99
    N1
    G103 P0
    M99
    %

    Additional Notes

    Edit the G53 X,Y value to whatever you want you spindle to go during a tool change. I would recommend putting parameter lock back on setting 7 & 23 once you are finished. You will need to load a non O9000 program to do this.

    Hope this helps 😄

  22. #20
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    695
    Post Thanks / Like
    Likes (Given)
    103
    Likes (Received)
    361

    Default

    Quote Originally Posted by roundybitland View Post
    I wasn't happy with the Haas parameter trick myself (VF3 Y/T). It would move to a safe tool position but it would move axes simultaneously with the Z axis. It's too bad because this trick would work with the ATC FWD/REV buttons too. Maybe there is a solution out there but even a Haas rep wasn't sure how to get around it. I ended up aliasing M6 .
    Pro - You can move any axis however you want to. Z axis moves up first.
    Con - Doesnt work with ATC FWD rev buttons.

    How to set it up;
    1) Press settings button, turn off parameter 7
    2) While in setting turn off parameter 23
    3) Press param/dgnos button, set value parameter 81 to 6.
    4) Load M6 alias program below into memory. NOTE - If you have any programs named specifically O9000 you will have to rename your alias program to another 9000 program number and put the 6 value in the corresponding parameter (81=O9000).

    % O09000 (TOOL CHANGE)
    G103 P1
    IF [ #3026 EQ #4120 ] GOTO1
    G00 G91 G28 Z0
    G00 G90 G53 X-40. Y-26.
    G103 P0
    M16
    M99
    N1
    G103 P0
    M99
    %

    Additional Notes

    Edit the G53 X,Y value to whatever you want you spindle to go during a tool change. I would recommend putting parameter lock back on setting 7 & 23 once you are finished. You will need to load a non O9000 program to do this.

    Hope this helps 😄
    Setting 6 will disable atc fwd/rev buttons.

    YouTube


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
  •