Mid program restart
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 22
  1. #1
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default Mid program restart

    Why does everything have to be so complicated Manual says When in auto mode, F1 restart, enter block number you want to start from, set axis movement (this makes no sense), then OK. The program starts running from the begining with no spindle or motion.

    Anyone have the short Mid program restart for dummies trick/tip?.

  2. #2
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4,816
    Post Thanks / Like
    Likes (Given)
    3834
    Likes (Received)
    1534

    Default

    If your trying to start at a line number just search for the line number in auto mode. It will find the line, then press cycle start.

    I usually only put a line number right before the tool change, so the TLO and work offset are called. Not sure how you would restart in the middle of a long cut.

  3. #3
    Join Date
    Sep 2012
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    84

    Default

    I would say to use "Sequence Restart" function.
    Select your line number or block number to start on, (They are NOT the same)
    Select "Restart" on the F* keys
    Type in the line number (N123) or Block number (86)
    Press "Ok"
    Then press "Sequence Restart" on the control panel.
    The Jog feed will be used to bring it to the last point, and you are set.
    Cycle start from here

    This will ensure the spindle is running, coord. is selected, anything else in the program is executed.

  4. Likes Captdave, Jorgo, pianoman8t8 liked this post
  5. #4
    Join Date
    Feb 2014
    Location
    SC, USA
    Posts
    782
    Post Thanks / Like
    Likes (Given)
    181
    Likes (Received)
    319

    Default

    I assume you are talking about your mazak captdave? I don't know how that works. On the Haas, you turn program restart on in the parameters, then simply select where in the program you want to restart. The control reads backwards (in the program) to find the correct work offset, tool number, and length offset. Not 100% how it is on finding tool as I have always done the restart with the correct tool already in the spindle.

  6. Likes Captdave liked this post
  7. #5
    Join Date
    Jan 2011
    Location
    telford, pa
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    103

    Default

    If your on an okuma listen to Mr M, with okuma you can restart ANYWHERE, canned cycles, ANYWHERE. If your on a Mazak, wrong forum, lol

  8. Likes Mr.M, Mtndew, Jashley73, pianoman8t8 liked this post
  9. #6
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    This is on a OSP 300 control.

    For example here is a hypothetical situation, say one of the many features on the part is a pocket, after the completion of the program the pocket is measured and under sized. Comp the tool and now we just want to rerun the pocket op only.

    On other controls we use this would be a simple task, pick the line number that includes the work offset prior to the tool change and the line number at the completions of the op. These are considered start and end markers and the rest of the program will be ignored till the markers are removed.

  10. #7
    Join Date
    Sep 2012
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    84

    Default

    I would position your tool so you have a "line of sight" to the pocket, do the above described method, and then just stop at the optional stop after the tool

  11. Likes Captdave, pianoman8t8 liked this post
  12. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4195
    Likes (Received)
    2754

    Default

    Quote Originally Posted by Mr.M View Post
    I would position your tool so you have a "line of sight" to the pocket, do the above described method, and then just stop at the optional stop after the tool
    This.
    Just make sure you have a clear path to the cut.. because it's going to move in ALL axis at the same time to get to its destination.

  13. #9
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,982
    Post Thanks / Like
    Likes (Given)
    6962
    Likes (Received)
    2525

    Default

    This isn't exactly a specific answer to your post, but I've started making this standard procedure on all my non-Fanuc control programs...

    O1234 (MAIN MACHINING PROGRAM)
    (SPOTS, DRILLS, TAPS HOLES, THEN MILLS POCKET)

    GOTO 10 (TOOL 1 - SPOT HOLES)
    GOTO 20 (TOOL 2 - DRILL HOLES)
    GOTO 30 (TOOL 3 - TAP HOLES)
    GOTO 40 (TOOL 4 - ROUGH-MILL POCKET)
    GOTO 45 (TOOL 4 - FINISH POCKET)

    N10(SPOT HOLES)
    Machining code goes here...
    M1

    N20(DRILL HOLES)
    Machining code goes here...
    M1

    And so on....



    On an Okuma control, you must be on the "Actual Position" or "Main Program" screen. Cursor down, and select the GOTO_ line that you want. Hold the "INTERLOCK RELEASE" button, and press CYCLE-START and you're off...

  14. Likes Captdave liked this post
  15. #10
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    So on the P300 control, from the maim program page, use number search. Type in the line number (N18540) and you can see the start marker move to that N number, with a direct path to the start point hit cycle start. Tested it with several types of cycles within a program and works perfect.

    Aren't Saturday afternoon great for this stuff, nice and quiet and no pressure to get it done now.

  16. Likes pianoman8t8 liked this post
  17. #11
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4195
    Likes (Received)
    2754

    Default

    Quote Originally Posted by Captdave View Post
    So on the P300 control, from the maim program page, use number search. Type in the line number (N18540) and you can see the start marker move to that N number, with a direct path to the start point hit cycle start. Tested it with several types of cycles within a program and works perfect.

    Aren't Saturday afternoon great for this stuff, nice and quiet and no pressure to get it done now.
    Yep, that's for Number Search... you can also do a Restart anywhere in the program.. just hit Restart and then Sequence Restart..... use the Dry Run feedrate to let ALL axis' move to the position and then hit Cycle Start.

  18. Likes Captdave liked this post
  19. #12
    Join Date
    Sep 2012
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    84

    Default

    Quote Originally Posted by Mtndew View Post
    Yep, that's for Number Search... you can also do a Restart anywhere in the program.. just hit Restart and then Sequence Restart..... use the Dry Run feedrate to let ALL axis' move to the position and then hit Cycle Start.
    Yes, CaptDave, that will not activate any modes before that line in the program. I use it sometimes but prefer actually using the "Restart" F key and the "Sequence Restart" on the control panel. Much safer that way. Glad you are making progress!

  20. Likes Captdave liked this post
  21. #13
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Quote Originally Posted by Mr.M View Post
    Yes, CaptDave, that will not activate any modes before that line in the program. I use it sometimes but prefer actually using the "Restart" F key and the "Sequence Restart" on the control panel. Much safer that way. Glad you are making progress!
    When testing I started the program at the tool change line to pick up the offsets and M codes.

    IIRC correctly, the restart key had you search for a block number as opposed to a line number or am I missing something. The way my CAM is setup it only outputs line numbers only.

  22. #14
    Join Date
    Sep 2012
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    84

    Default

    Block Number OR Line Number. The block number is displayed in the upper RH corner of the "Program" display IIRC. I generally just use line numbers to start on though

  23. #15
    Join Date
    Feb 2014
    Location
    SC, USA
    Posts
    782
    Post Thanks / Like
    Likes (Given)
    181
    Likes (Received)
    319

    Default

    Wow that all sounds like a royal pain in the ass! I guess if you are familiar with the control (I have never used one) maybe it is easier to do than it sounds? I like the Haas way, turn the parameter on, rerun wherever you like. BUT, that has some drawbacks too, forget to turn it off and your programs slow way down as it is looking for the "correct" offsets and such, even if it is at the beginning of the tool with everything called up.
    Question, can you page thru the program to a certain tool and just start at the toolchange line? The Haas, and I think most Fanuc do this with no parameter change or special sequence. I was referring to in the middle of a tool cutting you have to turn this feature on. If you want to start at a toolchange line you just page down to it and hit cycle start.

  24. #16
    Join Date
    Sep 2012
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    84

    Default

    You can do both methods and it needs no parameter change. Just hold down "Interlock Release" and hit the green button

  25. #17
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4195
    Likes (Received)
    2754

    Default

    Quote Originally Posted by 6061Mike View Post
    BUT, that has some drawbacks too
    Yeah, it's a Haas.

    It's really not a pain in the ass. It's accomplished in seconds. Restart... N300.... enter....cycle start.

  26. Likes pianoman8t8 liked this post
  27. #18
    Join Date
    Jan 2011
    Location
    telford, pa
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    103

    Default

    Like he said, not a pain in the ass at all, it actually relieves alot of worry knowing the machine will take care of all the worry, as long as you maintain that "line of sight". Ive bounced back and forth from fanuc, siemens, and osp for years and ive always been on the fence, but im finally convinced osp is the best(for me) it feels like the control works for me, the others make me feel like i work for them. Plus tons of memory and easy editing. I cant believe how many fanucs dont have "ex-edit", how is that not a basic function? Mid auto manual and sequence restart are the best functions ive ever seen on a control. I like the others dont get me wrong, but i prefer osp.

  28. Likes Mtndew, Mr.M liked this post
  29. #19
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4195
    Likes (Received)
    2754

    Default

    Quote Originally Posted by james siffel View Post
    Mid auto manual and sequence restart are the best functions ive ever seen on a control.
    I've been saying this since we got our first Okuma back in 1994! Mid auto manual is awesome.

  30. Likes Mr.M liked this post
  31. #20
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4195
    Likes (Received)
    2754

    Default

    I'm not sure if this was mentioned yet but if you restart at a line number BE WARNED that the line number is observed by the control in 2 different ways....
    Say you have a long program, N100 Facemill, N200 Pocket, N300 Drill etc... If you start the program from the beginning, by the time you get to N300 you may be on line 475 (just a number for example purposes). BUT.. if you Number search from N300 you will be starting at line 1.

    This can benefit you or hurt you if you're not careful.
    If you have a super long program, you can Number Search to N300 so it's faster AND THEN restart at a line number so you don't have to wait for the control to read from the very beginning of the program. But if you do it this way, your line number starts at 1 from N300.

    Hopefully you can follow my gibberish explanation.

  32. Likes pianoman8t8 liked this post

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
  •