Locate re-start point in program when stopped mid-cycle.
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED KINGDOM
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Question Locate re-start point in program when stopped mid-cycle.

    Hi all - I'm completely new to using CNC hence the newbie question.

    If using a CNC machine (Heidenhain) how would someone locate the correct re-start point in the G-code program when the machine is stopped mid-cycle?

    Thank you.

  2. #2
    Join Date
    Feb 2006
    Location
    so cal, usa
    Posts
    569
    Post Thanks / Like
    Likes (Given)
    197
    Likes (Received)
    135

    Default

    not familiar with your controls at all, but generally, you need to go back to the tool call and run from there.

  3. Likes Robert2018 liked this post
  4. #3
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    20

    Default

    I am not familiar with your control either. We run sequence numbers only at tool changes on Fanuc. So If I need to do this deep in a program I will tag the line I want to jump to with say N100 for example. Start at the desired tool. Single block the machine through the tool length callout G43 or whatever your machine uses. When at the clearance plane type N100 cursor down. Control jumps to the N100 line. Continue on.

  5. Likes Robert2018 liked this post
  6. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    3170
    Likes (Received)
    696

    Default

    Not Heidenhain either but interested in what 'They" do... And how one generally goes about getting answers to such queries ?



    Just for propaganda purposes as right now I think "They" HAAS pretty much have a "Tip of the day" for pretty much everything.

  7. Likes Robert2018 liked this post
  8. #5
    Join Date
    May 2007
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    2,599
    Post Thanks / Like
    Likes (Given)
    3051
    Likes (Received)
    479

    Default

    Yep Haas is very proactive and tries hard. It is good for anyone running a Haas.

  9. #6
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,291
    Post Thanks / Like
    Likes (Given)
    1157
    Likes (Received)
    2338

    Default

    OP is it a conversational program or G-Code?

  10. #7
    Join Date
    Nov 2018
    Country
    UNITED KINGDOM
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default

    Thanks for the replies.

    Quote Originally Posted by litlerob1 View Post
    OP is it a conversational program or G-Code?
    It's G-Code.

  11. #8
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,291
    Post Thanks / Like
    Likes (Given)
    1157
    Likes (Received)
    2338

    Default

    Gotta love just guessing. Have you tried Cursor-ing down to a Toolchange (usually a line with a N value-followed by G99-followed by T1) and pressing Cycle Start?

    Have you tried anything?

    R

  12. Likes Robert2018 liked this post
  13. #9
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    88
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    34

    Default

    Few different ways you can do it.

    The Heidenhain control I'm familiar with is the TNC530, others may be different.

    If you pause a program mid-cycle and just need to check out the workpiece or inspect the tool, hit feed-hold and then press the "manual traverse" softkey and move the spindle away from the work using the handwheel. You can then use the "restore position" softkey when you're done to move the spindle back into position. It will reverse the exact movements you used to retract the spindle, and you can continue running the program from here.

    If you have cancelled the program, I usually start a few lines up from the last tool call. A few lines up, because I have some variables that get set just before the tool call to work with the laser tool measuring/breakage detection system that will throw an error if they aren't set correctly. If you don't use this, you can start directly at the tool call.

    To do this, I use the "GOTO" button (between the directional arrows on the control) and just enter the line number I would like to start from. Cycle start and go.

    If you don't know what line number you want to start from, an easy trick is to go to the program editor on the control, and cursor down to the first tool call. Hit the left or right directional arrows, and the block with the tool call will become highlighted. If you now cursor down with the block highlighted, it will scroll directly to the next tool call and you can easily scroll through all the tool calls in the program this way.

    Now if you are re-starting a program this way, it is very important that you have the correct preset/datum/work offset active. For obvious reasons.

    I like to cycle-start from the top of the program, and then cancel out after the datum setting line before the first tool call. Then you can GOTO whatever line you need to restart from.

    You can also activate the correct offset from the datum/preset tables but I like using the program for this situation because you know for sure it will match the program you're running.

    Hope this helps

  14. Likes Robert2018 liked this post
  15. #10
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    88
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    34

    Default

    Quote Originally Posted by cameraman View Post
    Not Heidenhain either but interested in what 'They" do... And how one generally goes about getting answers to such queries ?

    Here you go: Home: Documentation - HEIDENHAIN

    Manuals are also loaded on the control, although they are kind of a pain to navigate through.

    When I get stuck, I usually just pop off an email or call to our applications guy.

  16. #11
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    20

    Default

    Quote Originally Posted by litlerob1 View Post
    Gotta love just guessing. Have you tried Cursor-ing down to a Toolchange (usually a line with a N value-followed by G99-followed by T1) and pressing Cycle Start?

    Have you tried anything?

    R
    What do you mean just guessing?

  17. #12
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,291
    Post Thanks / Like
    Likes (Given)
    1157
    Likes (Received)
    2338

    Default

    Quote Originally Posted by VTM View Post
    What do you mean just guessing?
    I mean that WE are just guessing. WE have no information on which Heidenhain control it is, which method of programming it is, what year make and model, and more importantly what the OP has tried thus far. WE are guessing.

  18. Likes cameraman liked this post
  19. #13
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    3170
    Likes (Received)
    696

    Default

    Quote Originally Posted by litlerob1 View Post
    I mean that WE are just guessing. WE have no information on which Heidenhain control it is, which method of programming it is, what year make and model, and more importantly what the OP has tried thus far. WE are guessing.

    Also reason for stopping mid cycle and number of axes of machine + machine layout. (might be handy too).

    Some machines may also execute a couple of moves/ rotations for safe tool retraction... So question is how best to pick up thread from what is essentially a "State" machine ? [I don't have answers for that (very machine dependent).].

    __________________________________________________ __________________________________________________ ______________________

    As an aside might be easier (task) on newer MAZAK controls (like Smooth X) as you have 3D graphics of exact tool paths (as they relate to part geometry too), so you can select tool path in 3d graphically and pull up corresponding lines of G-code / part of the program you are in.

    Thinking long programs + complex curves (mold work or sim 5 axis ).

  20. #14
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,291
    Post Thanks / Like
    Likes (Given)
    1157
    Likes (Received)
    2338

    Default

    Quote Originally Posted by cameraman View Post
    As an aside might be easier (task) on newer MAZAK controls (like Smooth X) as you have 3D graphics of exact tool paths (as they relate to part geometry too), so you can select tool path in 3d graphically and pull up corresponding lines of G-code / part of the program you are in.

    Thinking long programs + complex curves (mold work or sim 5 axis ).
    I just read this Article (disrupting the OP's topic sorry). AFAIS the tech assosiated with that is exclusive to the Quick EIA option, which is not the same as just a regular G-Code program. It's generated the same as Mazatrol programs, just outputs editable G-Code. I could be wrong. BUT begs the question; will the Smooth X be able to run a full simulation of any G-Code program or only the ones generated by the control using Quick EIA? (sounds a little like VQC from Haas)

    https://www.google.com/url?sa=t&rct=...SVuZILsc3N6RFx

    FWIW everything in that Article that they are bragging about, has been standard on OSP controls since the 5000 Including View Surf.

    R

  21. Likes cameraman liked this post
  22. #15
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,022
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2600

    Default

    depends on machine AND program
    .
    1) horizontal mill table rotation not always restated at tool change. could be 5 tool changes back. had cnc i checked grid shift at B0 and restarted program which at tool change did NOT call a B180 so big mill hit back end of part.
    .
    2) work offset like G55 if not default like G54. many cnc parameters setup if reset pressed G54 is active. obviously if G55 not restated could be using wrong work offset
    .
    3) tool comp like length and dia. usually restated at tool change but depending on how program written watch movement causing tool to crash. initial Z should clear part but not always in some positions. depends on program
    .
    4) active plane like G17, G18, G19..... default like G17 when you need different one could mess up tool comp
    .
    5) G98 G99 and drill cycles whether drill go to R or back to initial Z often matters. same as G81 being canceled by reset to G80
    .
    6) turn spindle on..... added M0 between tapped holes it taps 2nd hole without spindle turning. obviously didnt work that well
    .
    7) coolant on.... again program might not restate although usually does if tool changed cause obviously coolant off during tool change
    .
    8) really some cnc on reset press really changes many things like work offset, turn tool comp off, turn drill cycle off, go to G17 plane, etc... also feed is it inch per minute or inch per rev..... that definitely matters depending how program written
    .
    really got to understand what reset press does. clearing #100 to #199 if macro used can matter too. badly written program trying to control spindle rpm and if math is bad, rpm could go to max and be more than cutter or tool holder or chuck can take
    .
    same as some cnc if tool change given and tool already in spindle it is ok and other cnc will error or alarm. so restarting just before tool change some machines ok with that others are not (got to mdi and put tool back in tool magazine) . obviously if wrong tool in spindle that will be a problem.
    .
    restarts can be very different depends on cnc and how program written


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
  •