18i-mb parameter to restart spindle after M1 (opt stop)


Results 1 to 20 of 20

Thread: 18i-mb parameter to restart spindle after M1 (opt stop)

  1. #1
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default 18i-mb parameter to restart spindle after M1 (opt stop)

    anyone know how to set an 18i-mb to restart the spindle after stopping via opt-stop (m1)... i can't find a parameter (or mtb parameter) for it but all my other machines do it...

    thanks
    - gwarble

    Similar Threads:


  2. #2
    Member
    Join Date
    Mar 2005
    Location
    United States
    Posts
    816
    Downloads
    0
    Uploads
    0

    Default

    I've been wondering about this too.

    Greg



  3. #3
    Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1792
    Downloads
    0
    Uploads
    0

    Default

    Insert M03/M04 after M01. Even if optional stop is not being used, M03/M04 would do no harm.



  4. #4
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    this is a fine solution in some circumstances, but not always

    for programs coming from our cam system, the post can easily insert an extra M3/M4 after the M1, but besides being extra code in storage and to send via rs232 every time, its not ideal

    but more important than that, if the operator wants to add an M1 somewhere in the program to check the part/tool, there is a great possibility of error if that m3/m4 is forgot... and since all other machines in my shop will restart the spindle and coolant after an m1, i'd rather address the issue on the machine itself

    PMC keep relays that are relevant but not the solution (this is a mori seiki nh5000, msg-501 control (fanuc 18i-mb):

    K5.5: 1:M01 command does not stop the spindle/coolant
    K24.3: 1:When given an M01 command, door is unlocked

    thanks for the suggestion
    - gwarble



  5. #5
    Member
    Join Date
    Feb 2007
    Location
    USA
    Posts
    592
    Downloads
    0
    Uploads
    0

    Default

    Having a Spindle restart without an M3/M4 is a major safety violation.

    Enough that OSHA might own your company, or get your insurance canceled.

    If anyone can Insert a M01 they can also add the M03.

    Don't be stupid, if an accident happens and they find you modified the machine function its going to come out of someones pocket, and it won't be the insurance company.



  6. #6
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    well i agree, after a reset or emergency stop, but an m1 is not really the same thing... cycle start is being pressed for pete's sake (same as starting a program from the top, user doesnt have to press an extra spindle button)

    not to mention most mtb's would agree with me, as can be seen by the factory behavior of all other machine tool builder's our shop has...

    so the Mori Seiki is the one that does not restart the spindle after a cycle start after M1

    i also have:
    Fanuc (MTB and control, robodrills) 2 models 3 machines
    hardinge/bridgeport, 1 model 2 machines
    kitamura, 1 machine
    chevalier, 1 machine
    hwacheon, 1 machine
    miyano, 1 machine (lathe)

    all of these act the opposite, which is to restart the spindle after a "cycle start" is received while at an opt-stop M1 or any M0

    feedback?

    - gwarble



  7. #7
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by skullworks View Post
    If anyone can Insert a M01 they can also add the M03.
    its not about ability, its about efficiency... without sacrificing safety, ever

    what if the tool was M4/CCW and the operator didn't know the difference or check the status... there's also m5 and m19 to think about if the operator has to actaully hand code this stuff...

    or imagine you want a non-hand edited program, but has an m1 after every hole for tap chip clearing or part measuring... the door interlock takes care of all the safety concerns



  8. #8
    Member
    Join Date
    Feb 2007
    Location
    USA
    Posts
    592
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by gwarble View Post
    well i agree, after a reset or emergency stop, but an m1 is not really the same thing... cycle start is being pressed for pete's sake (same as starting a program from the top, user doesnt have to press an extra spindle button)

    - gwarble
    M1 is the same as starting from the TOP? - If that were true then yes it would be safe, except it isn't.

    The program header sets all sorts of condition variables that are often only set once. Usually a shortened sub set of these commands are used for each tool change.

    Any time an Autocycle is allowed to be interrupted a potential danger has been created. How much of a danger varies somewhat with the age of the control. A FANUC 0mB behaves differently than a FANUC 0i. After a M01 the machine will continue with the commands on the next line of code, does that line contain enough data to be a safe start point, like after one or more axis was homed.

    I believe our Mori Seiki SV50B with MSC 518 (FANUC 18) will resume after a stop if the door switch and mode switches are not disturbed. I honestly am not sure since all programs have all the needed code after any optional stop or conditional alarm stop.

    Code is cheap - fill it up. Hardware, material, tools and operators are expensive.



  9. #9
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    i tend to disagree, the less code the better in most circumstances... especially when it comes to operator's proving out and prototyping parts... in a shop where rarely do parts run in a machine for more than a day or two... so a handful of parts/setups may be done in a day on each machine... the more that can be configured on each machine to make operation identical throughout the shop is proving to be more and more beneficial... standardization

    putting the safety code into macros and establishing general safe practices is the only way i can get trained but inexperienced operators to use machines safely and still be dynamic enough to and edit programs or repost as necessary from the cam system...

    on most of my fanuc controls (all prior to the 31i) there is no limitation to prevent a program from being started at any point in the program... they did finally add this warning to the 31i i've seen, which is a good error prevention measure... but otherwise transmission errors and operator errors are always a possibility... proper training and procedure definition, and simplifying code and procedures, is working for me better than anything else i've tried...

    in most cases what it boils down to in our shop is "safe" toolchange macros on all machines, which establish certain safety code necessary for each machine... followed by an m1... so the only places which programs are allowed to be started are at a tool change...

    ie (from memory):
    N3 M6 T3 (TOOL CHANGE MACRO M6 INCLUDES ALL SAFETY CODE)
    M1 (T3 - 0.500 ENDMILL)
    (MINIMUM Z=-1.0)
    M3 S12000 (SPINDLE)
    G54 Xi Yi (STARTING POSITION AT WORK OFFSET)
    G8 P1 and/or G5.1 Q1 R# (LOOKAHEAD and AI/HSM)
    G43 Zi H3 (RAPID/SAFE PLANE with TOOL OFFSET)
    /M8 (COOLANT ON)


    of course i'm always looking for improvements but its working for me now...

    again the real problem is standardization throughout the shop... so the more similarly the machines act, the better, however it is... surprises are the worst for operators...

    thanks for your feedback

    - gwarble



  10. #10
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by skullworks View Post
    M1 is the same as starting from the TOP? - If that were true then yes it would be safe, except it isn't.

    The program header sets all sorts of condition variables that are often only set once. Usually a shortened sub set of these commands are used for each tool change.
    well yes and no... its not like the TOP from the machine's perspective, but from an osha perspective it is, you have to press cycle start

    a better comparison would be to single block... unless you press reset, however the program stops certain things shouldn't be changed or codes canceled...



  11. #11
    Member
    Join Date
    Feb 2007
    Location
    USA
    Posts
    592
    Downloads
    0
    Uploads
    0

    Default

    I'd say your on the right track with the use of safe tool change macros to make the differences between machines more operator transparent.

    You can try to make things idiot proof, then someone will come along and do something even beyond what you would consider possible.



  12. #12
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    thats for sure...

    tool change macros were the key...

    the standard in our shop is the m6 t# [x0 y0] will:

    turn off coolant and AI/HSM
    reference z(1or2) (whether or not the tool is actually going to change)
    turn off tool length comp (g49)
    reference 2 x-axis on certain machines which need an x location for tool change ONLY if the tool is actually going to change (using *** when necessary)
    set absolute mode g90
    set sequence number N(tool#) for easy reference in the top right corner
    set spindle tool number to macro #148 for reference***
    unlock spindle orient if necessary

    optional x0 and y0 will optionally home those axis after homing z and turning off coolant, bringing the part to the door (ref2 g30 location) for the final toolchange of a program to toolchange to the first tool (for faster next cycle)



  13. #13
    Member
    Join Date
    Nov 2006
    Location
    USA Texas
    Posts
    418
    Downloads
    0
    Uploads
    0

    Default

    Man I sure have to say I agree with skullworks. I don't think I would allow an operator to edit a program to add an M01 if they didn't know enough about programming to know the difference between an M03 and an M04! Sure sounds like you're crippling yourself with lack of investment in your personnel training.

    As to the "less is better" in programming theory, how much is 3 characters gonna kill you? You can't just stop a program anywhere to check things out, so your operators should have been given some insight where to put the M01's and where not to...So honestly what is the major roadblock in taking them another step to understand proper coding to restart the spindle?

    I too have a couple of Robodrills, and a slew of other Fanuc controlled machines - but for consistency's sake if nothing else I include the full gamut of coding to ensure all programs read alike (so the operators can understand easily what is going on).

    I just can't for the life of me understand why it is you want to take on more risk than you already have daily in a machine shop but shortcutting...



  14. #14
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    i think i started some confusion...

    i by no means allow untrained operator's to edit programs in the control or cut ANY corners that would sacrifice safety in anyway, nor for higher level personnel...

    i posted wondering about the machine's ability... as i pointed out neither opinion is a regulated procedure for machines being osha safe or not on all the other machines in my shop... most modern machines i've used satisfy the safety concerns with the door interlock (opt stop even unlocks the door on most) stopping spindle and slowing feeds...

    i, myself or other fully experienced personnel, may want to use such a feature for perfectly safe and legitimate procedures... the beauty of these expensive controls we've all inve$ted lots in is the customizability and dynamic nature...

    a simple example:
    a lathe running in continuous bar feed mode
    i want to periodically check parts on the machine, with the least down time
    i can quickly walk up to the machine, and an m1 at each toolchange will leave me the shortest down time (ie if i turn off continuous i have to wait til the m30, but some earlier point in the program may be a fine time to check the part or tool via M1)

    or on a mill:
    tapping an array of 1000 holes in crappy material. for the first time so you don't know how much life to expect from the tool... so you code like:
    M29 S10
    G90 G83 blah blah X.1
    M1
    X.2
    M1
    X.3
    M1
    X.4
    etc...
    G80
    M30

    so i can walk up to the machine at any point, turn on opt-stop, and have an unlocked and ready machine whenever the tool is next clear of the part...

    also its a waste of time and adds more possibility for error when things aren't standardized and every keystroke is a possibility for a mistake... and hand coding a program from scratch for someone fully experienced is a lot faster/easier/safer when you use macros extensively and leave the possibility for error out...

    i think we all agree about safe procedures and training's importance... we wouldnt last long in this industry without it

    but using a machine set up from the factory and only copying the example program from the book and modifying to your needs, is a waste of time and money... efficiency is key



  15. #15
    Registered
    Join Date
    Jul 2010
    Location
    USA
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default

    So does anyone have an answer to the original question?

    I have one 18i machine where the spindle restarts after M1
    I have 6 other machines where the spindle restarts after M1

    And my machine that I just acquired has a 160is that doesn't restart after M1

    I would like to make an adjustment to make the 160is operate like the others.

    Last edited by dynomite; 07-28-2010 at 01:39 PM.


  16. #16
    Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1792
    Downloads
    0
    Uploads
    0

    Default

    There appears to be no parameter to control this. This is possibly decided by MTB, the way they design the ladder. Ask them. They may have an answer.



  17. #17
    Member dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2932
    Downloads
    0
    Uploads
    0

    Default

    On a Doosan DNM500, for example, keep relay #K03.4 controls this. You may have a similar keep relay on your machine.



  18. #18
    Registered
    Join Date
    Jun 2008
    Location
    United States
    Posts
    1511
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by dynomite View Post
    So does anyone have an answer to the original question?

    I have one 18i machine where the spindle restarts after M1
    I have 6 other machines where the spindle restarts after M1

    And my machine that I just acquired has a 160is that doesn't restart after M1

    I would like to make an adjustment to make the 160is operate like the others.
    Are the 2 18i machines made by the same MTB? I have never come across a parameter dealing with this. I have however had this work and not work at a 50/50 split across all of the machines I have worked on.

    My best guess is it is a MTB thing if they set it up that way or not.

    Stevo



  19. #19
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    99
    Downloads
    0
    Uploads
    0

    Default

    yup, all the info i could find would lead this to be a setting either hard-set by the MTB or controlled via pmc params/keep relays

    some of my machines of various MTBs have keep relays to control this...

    my mori seiki NH5000 with an MSG-501 control (a pc-embedded fanuc 18i) has no way to control this from what i could find, i'm planning to call them cuz sometimes keep relays are undocumented or poorly translated

    regarding DYNOMITE's post, my single machine that acts differently is that mori, which acts identical to the 160i in function... with an embedded PC... but i don't know why that would affect a feature like this

    good luck
    - gwarble

    one possible workaround i've thought to try is an M1 macro that restarts M3/M4/M5/M19 and S# after the internal M1, but i havent fully debugged the logic or tried it since the difference in operation is relatively small



  20. #20
    Member
    Join Date
    Jul 2010
    Location
    South Africa
    Posts
    118
    Downloads
    0
    Uploads
    0

    Default

    the action of M01 function and the "cycle start" there-after is 100% controlled by the MTB through the pmc program.(possible keep-relay's are pre-programmed for this selection)
    so the right way is to ask the MTB or their local service office, specially if the machine is under warranty.



Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

18i-mb parameter to restart spindle after M1 (opt stop)

18i-mb parameter to restart spindle after M1 (opt stop)