Haas "Run from here"
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    201
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default Haas "Run from here"


    Not sure if my terminology is right, but I've used this function on other controllers. Just that nothing jumps out at me on the Haas keypad for this type of command. Not sure if it even exists on my controller.

    Does anyone know if it is possible to do a "run from here" on a Haas VF non-ngc classic controller? As in scroll down to a particular section/tool change and continue where you were interrupted on a long run program. If so, how?

    Need to be able to do this after a tool change fault or broken tool replacement.

  2. #2
    Join Date
    Jun 2015
    Country
    CROATIA
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    4

    Default

    Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

    Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

    Sent from my SM-G965F using Tapatalk

  3. #3
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    201
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by Locker View Post
    Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

    Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

    Sent from my SM-G965F using Tapatalk
    Thank you. I'll check it out!

  4. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,275
    Post Thanks / Like
    Likes (Given)
    844
    Likes (Received)
    1285

    Default

    Just a caution, the machine will move to the last XYZ position before the line you choose to restart at.

  5. Likes bryan_machine, ranchak liked this post
  6. #5
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    201
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by Locker View Post
    Its setting 36 on both control versions, NGC and preNGC, its called PROGRAM RESTART.

    Turn the setting on and you are good to go, you can start from any line, you can even start with the wrong tool in the spindle, wrong wcs, it reads program from the begining to the line you choose, and it will force wcs change and tool change if needed.

    Sent from my SM-G965F using Tapatalk
    My setting #36 was turned OFF.
    Turned it on and worked just fine. Afterward, I also tried same thing with it turned off. Didn't think it would let me, but it started up. I cancelled it out quickly not certain if the machine still had the program start routines in memory.

    Wouldn't think it's a good idea, but has anyone tried continuing a program without the "Program Restart" turned on?

  7. #6
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,275
    Post Thanks / Like
    Likes (Given)
    844
    Likes (Received)
    1285

    Default

    I program with a "safety line" at the beginning of each tool. I restart at the beginning of a tool all the time without "Program Restart".

    Program Restart is mostly for restarting in the middle of a tool.

  8. Likes Tryhard liked this post
  9. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,323
    Post Thanks / Like
    Likes (Given)
    1679
    Likes (Received)
    2038

    Default

    Quote Originally Posted by Booze Daily View Post
    I program with a "safety line" at the beginning of each tool. I restart at the beginning of a tool all the time without "Program Restart".

    Program Restart is mostly for restarting in the middle of a tool.
    On Haas machines you can start (without program reset enabled) at any tool change line without issue. As booze said, it is mostly for restarting something like a long surfacing program or such...

  10. Likes Tryhard liked this post
  11. #8
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,275
    Post Thanks / Like
    Likes (Given)
    844
    Likes (Received)
    1285

    Default

    I don't know how big your programs are, but here's a little trick that may or may not be of use.

    Say you have an endmill that does lots of roughing. Hundreds of lines of code.
    Your endmill breaks somewhere in the middle of the program. Hit Feed Hold. Do not hit Reset yet.

    Setting 31 - Reset Program Pointer: Turn this OFF.

    Now hit Reset. This will not reset the cursor to the beginning of the program. The cursor will stay on the same line it was on when you hit Feed Hold.

    Now you can go into Edit, insert a line no. (N1000), change your endmill, turn on Program Restart and restart where you endmill broke (N1000) without having to cut air up to that point.

    Make sure to change all your settings back when you're done to avoid any nasty surprises.

  12. Likes Tryhard liked this post
  13. #9
    Join Date
    Feb 2004
    Location
    Staten Island NewYork USA
    Posts
    3,836
    Post Thanks / Like
    Likes (Given)
    1143
    Likes (Received)
    1880

    Default

    Program will start from where your courser is in the program with Setting 36 On or OFF.

    The difference is one Setting has the machine read through the entire program turning on or off Offsets, coolant, Speeds, feeds, puts the last Tool used, goes to the last position - then changes to the present Tool and starts from that SAFE programed position. Very good mindless Setting that avoids any complications...Only on Lengthy programs it can take awhile for machine to read through.

    The other option is turn that Setting off and hit start. It runs the line its one with the tool and offsets that were last called up at the position its in. So if machine has a drill in a hole At X0 Y0 Z-2.00 and the line your on has a GO X3.3...the machine is making a Rapid move in to X 3.3. Could be a G90 or G91, no retract before move...spindle may be on..or not.

    Great for long programs and you know Program can run from that point as all your settings are given after the Start is pressed.

    Few of my programs are long enough to outweigh the benefits of having machine run through the program.


    I had one gent turn the option off as he frequently started and stopped having to wait a couple seconds here and a couple there. He wanted to optimize the time. Unfortunately he would loose time when tooling took a short cut or coolant wasn't turned on or the P-cool didn't catch the count change. We had words and I changed back...the other issue was the other guys didn't know about the difference and just hit start. Not Good. Point is...set it up the way it works for you...but consider it something that needs to be across the board for all machines. Unless guys are assined to specific machines.

  14. Likes eaglemike, Tryhard liked this post
  15. #10
    Join Date
    Dec 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Also, there's a Haas youtube video that covers this =)

  16. Likes Tryhard 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
  •