Fanuc 11M start rejected - Page 3
Close
Login to Your Account
Page 3 of 49 FirstFirst 1234513 ... LastLast
Results 41 to 60 of 962
  1. #41
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    I think I can do that.. post the program though im not sure what it is. It is a stored program from the prior owner. I took some pictures of errors and will post soon as able. I appreciate the input and will get info soon as possible. Thank you again for all the help. Discouragement GONE!!! I owe you big time. almost 2 years working on this thing and I finally get to see it move as it should... well... almost.. but so close now.

  2. #42
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    20171013_165634.jpg20171013_165116.jpg
    What ya think?
    Let me say you guys have been great.

  3. #43
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    538

    Default

    Your Z overtravel is most likely caused by the programmed Z position and a zero length in offset 1.

    I would suggest you do not try to run programs from the previous owner unless you can read them and understand exactly what the machine is going to do.

    Before you run anything you want to set your G54 position and a tool length for tool 1.

    I would suggest you write a simple program to test the axis movements. Once you are good there, you can add tool changes, spindle commands, gear shifts, coolant, etc to test all the functions. We can help you with that if you need.

    Setup your comms and dump the programs down to to a PC, you may want to use them for references later or pull certain portions out and use them in other programs. But there is no reason to leave those old programs in the control unless you are planning to make those parts.

  4. Likes cwtoyota, Hot Headz Marine liked this post
  5. #44
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by jancollc View Post
    Your Z overtravel is most likely caused by the programmed Z position and a zero length in offset 1.

    I would suggest you do not try to run programs from the previous owner unless you can read them and understand exactly what the machine is going to do.

    Before you run anything you want to set your G54 position and a tool length for tool 1.

    I would suggest you write a simple program to test the axis movements. Once you are good there, you can add tool changes, spindle commands, gear shifts, coolant, etc to test all the functions. We can help you with that if you need.

    Setup your comms and dump the programs down to to a PC, you may want to use them for references later or pull certain portions out and use them in other programs. But there is no reason to leave those old programs in the control unless you are planning to make those parts.
    I agree, don't run unknown code, that's the fastest way to crash and destroy a machine, or potentially hurt someone.

    The Z overtravel is + direction (positive / up) so it's probably caused by a tool-offset or a work offset.
    If the machine is set up for negative values in the offset tables and there's no data in the tables, you'll get a +Z overtravel in most programs.

    Let's say the machine looks for G54 in the offset table and finds X = 0, Y = 0, Z = 0...
    When it adds that G54 data to the home position, and the program uses G90 to rapid to a positive coordinate inside the work coordinate system, that coordinate is actually going to go outside the physical envelope of the machine coordinate system.

    Tool offsets will do the same thing in Z on a vertical machine. When negative offsets are set (via parameters) the control just adds them to the work coordinate system to come up with the work coordinate system for that tool.

    By the way, keeping the old programs is a great suggestion... They may help with coding quirks of that particular machine.

  6. Likes Hot Headz Marine liked this post
  7. #45
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    Great Information..Makes since 100% to dump the programs. Good info to keep them for a reference, hadn't thought about that.
    I would absolutely appreciate the help on a new program to test the machine. I don't have an rs232 cable to plug in and am not clear on Wich one or where to purchase. Do you have a recommendation for a particular rs232 device and or PC program for a green horn?

  8. #46
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    538

    Default

    Quote Originally Posted by Hot Headz Marine View Post
    ...I don't have an rs232 cable to plug in and am not clear on Wich one or where to purchase. Do you have a recommendation for a particular rs232 device and or PC program for a green horn?
    If you are just serial to serial a null modem cable will work. You can order them from Tiger Stop, the machine end needs a 24 pin. Or you can get the pieces from Rat Shack and makeup your own cable. Search the forum for warnings about the RS232 ground wire.

    If your PC doesn't have a serial port you will need a USB to serial adapter.

    The data transfer program will depend on your PC operating system. There are a bunch of them out there for free download. Use the forum search for suggestions from other members, I use old software that you couldn't get today even if you wanted to.

    In the meantime, you can type in a short test program at the control. But first you have to set your zeros. I assume you know how to home out and origin all axis. Do you know how to set your work coordinate and tool offsets? If not, PM me and I will walk you through it.

    Also, do you have the Fanuc books that came with your machine? You need the programming and parameters manuals for an 11M. If you don't have them, you should get them.

    So...Starting with a homed out machine, all axis origined. Jog the table in X and Y to the middle of the travels. Set G54 X and Y to this location. Leave G54 Z at zero.

    Set Tool 1 height offset to -5.0". Leave the spindle empty, and set your rapid override switch to 25%.

    Go to the program page, In edit mode, type in O1234 <eob> <insert>. This should create an empty program O1234. Note the first letter is the letter "O", not a zero.

    Put the cursor on the ; after O1234. Everything you type in will be added after the cursor, and ach line needs the ; (eob) symbol at the end.

    Simple program to see if the machine moves around okay:

    O1234;
    N1 G90 G17 G40 G49 G80;
    T1 M06;
    S400 M3;
    G0 G54 X0 Y0;
    G43 H1 Z1.0;
    G01 Z0 F20.0;
    Y2.0;
    G03 X0 J-2.0;
    G01 Y-2.0;
    G02 X0 J2.0;
    G01 Y0;
    G0 Z1.0;
    M05;
    M19;
    G91 G28 Z0;
    G28 Y0;
    T2 M06;
    T1M06;
    M30;

    It's been a lot of years since I ran an 11M, so bear with me if I missed something, and don't be afraid to hit the big red button if something looks amiss.

    The program should turn on the spindle, rapid to G54 zero location, rapid to Z 1.0, feed to Z0, feed to Y2.0, feed CCW full circle 4" dia., feed to Y-2.0, feed CW full circle 4" dia., feed to Y0, rapid to Z1.0, turn off spindle, orient spindle, rapid Z axis to tool change position, rapid table all the way to the Y limit, execute tool change to tool 2, execute tool change to tool 1, return to start of the program.

  9. Likes cwtoyota, Hot Headz Marine liked this post
  10. #47
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by jancollc View Post
    If you are just serial to serial a null modem cable will work. You can order them from Tiger Stop, the machine end needs a 24 pin. Or you can get the pieces from Rat Shack and makeup your own cable. Search the forum for warnings about the RS232 ground wire.

    If your PC doesn't have a serial port you will need a USB to serial adapter.

    The data transfer program will depend on your PC operating system. There are a bunch of them out there for free download. Use the forum search for suggestions from other members, I use old software that you couldn't get today even if you wanted to.

    In the meantime, you can type in a short test program at the control. But first you have to set your zeros. I assume you know how to home out and origin all axis. Do you know how to set your work coordinate and tool offsets? If not, PM me and I will walk you through it.

    Also, do you have the Fanuc books that came with your machine? You need the programming and parameters manuals for an 11M. If you don't have them, you should get them.

    So...Starting with a homed out machine, all axis origined. Jog the table in X and Y to the middle of the travels. Set G54 X and Y to this location. Leave G54 Z at zero.

    Set Tool 1 height offset to -5.0". Leave the spindle empty, and set your rapid override switch to 25%.

    Go to the program page, In edit mode, type in O1234 <eob> <insert>. This should create an empty program O1234. Note the first letter is the letter "O", not a zero.

    Put the cursor on the ; after O1234. Everything you type in will be added after the cursor, and ach line needs the ; (eob) symbol at the end.

    Simple program to see if the machine moves around okay:

    O1234;
    N1 G90 G17 G40 G49 G80;
    T1 M06;
    S400 M3;
    G0 G54 X0 Y0;
    G43 H1 Z1.0;
    G01 Z0 F20.0;
    Y2.0;
    G03 X0 J-2.0;
    G01 Y-2.0;
    G02 X0 J2.0;
    G01 Y0;
    G0 Z1.0;
    G91 G28 Z0;
    G28 Y0;
    T2 M06;
    T1M06;
    M30;

    It's been a lot of years since I ran an 11M, so bear with me if I missed something, and don't be afraid to hit the big red button if something looks amiss.

    The program should turn on the spindle, rapid to G54 zero location, rapid to Z 1.0, feed to Z0, feed to Y2.0, feed CCW full circle 4" dia., feed to Y-2.0, feed CW full circle 4" dia., feed to Y0, rapid to Z1.0, rapid Z axis to tool change position, rapid table all the way to the Y limit, execute tool change to tool 2, execute tool change to tool 1, return to start of the program.
    I run 11M every day in my shop. This program looks good/safe for the OP to run.

    On some machines (like my Kuraki) you can't put the T1 and the M06 in the same block. Those machines kick an alarm saying "Tool not set."
    I program my tool change z returns with a tool offset H0 in the same block like this: G28H0Z0T2

  11. Likes Hot Headz Marine liked this post
  12. #48
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by Hot Headz Marine View Post
    Great Information..Makes since 100% to dump the programs. Good info to keep them for a reference, hadn't thought about that.
    I would absolutely appreciate the help on a new program to test the machine. I don't have an rs232 cable to plug in and am not clear on Wich one or where to purchase. Do you have a recommendation for a particular rs232 device and or PC program for a green horn?

    Modern computers don't have RS-232 (seria1 COM) ports. I use a USB to RS232 adapter as suggested by jancollc. The one I suggest is made by IOGear and the model number is GUC-232A. It has been 100% reliable with my Fanuc control as well as other RS-232 devices. I tried a crappy (cheap) chinese USB adapter as well as a few others and had nothing but problems with them.

    CADEM has a free software called NC NetLite that makes it pretty easy to communicate to the Fanuc control.
    There are tons of other software out there, but that's a quick download that could get you started.

    There are some settings necessary on the machine (parameters) to get it talking with the PC...
    If you can't get things working, PM me and I'll send you my known good settings from my 11M control.

  13. Likes jancollc, Hot Headz Marine liked this post
  14. #49
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    538

    Default

    Quote Originally Posted by cwtoyota View Post
    I run 11M every day in my shop. This program looks good/safe for the OP to run.

    On some machines (like my Kuraki) you can't put the T1 and the M06 in the same block. Those machines kick an alarm saying "Tool not set."
    I program my tool change z returns with a tool offset H0 in the same block like this: G28H0Z0T2
    I added a spindle stop and orient.

    I remember that about Kuraki. First 11M I ran was on a KV1000. They want the tool number first because the tool changer pre-stages the next tool and remembers which pot each tool is in. I like that system, there's no waiting on the carousel.

  15. Likes cwtoyota, Hot Headz Marine liked this post
  16. #50
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    I do have the 11M manuals.
    Are you meaning Zero Return the axis when you say set G54.?
    Here's a rundown of what I do to start the machine, I turn it on I start with any axis in zero return mode and Jog it off its limits and it automatically switches directions and goes back slowly to whatever zero was set from the prior owner. I do that on all four access and the lights come on for those axis both the plus and minus lights. Then I can run something in MDI or in memory does that sound correct?

  17. #51
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    Quote Originally Posted by jancollc View Post
    If you are just serial to serial a null modem cable will work. You can order them from Tiger Stop, the machine end needs a 24 pin. Or you can get the pieces from Rat Shack and makeup your own cable. Search the forum for warnings about the RS232 ground wire.

    If your PC doesn't have a serial port you will need a USB to serial adapter.

    The data transfer program will depend on your PC operating system. There are a bunch of them out there for free download. Use the forum search for suggestions from other members, I use old software that you couldn't get today even if you wanted to.

    In the meantime, you can type in a short test program at the control. But first you have to set your zeros. I assume you know how to home out and origin all axis. Do you know how to set your work coordinate and tool offsets? If not, PM me and I will walk you through it.

    Also, do you have the Fanuc books that came with your machine? You need the programming and parameters manuals for an 11M. If you don't have them, you should get them.

    So...Starting with a homed out machine, all axis origined. Jog the table in X and Y to the middle of the travels. Set G54 X and Y to this location. Leave G54 Z at zero.

    Set Tool 1 height offset to -5.0". Leave the spindle empty, and set your rapid override switch to 25%.

    Go to the program page, In edit mode, type in O1234 <eob> <insert>. This should create an empty program O1234. Note the first letter is the letter "O", not a zero.

    Put the cursor on the ; after O1234. Everything you type in will be added after the cursor, and ach line needs the ; (eob) symbol at the end.

    Simple program to see if the machine moves around okay:

    O1234;
    N1 G90 G17 G40 G49 G80;
    T1 M06;
    S400 M3;
    G0 G54 X0 Y0;
    G43 H1 Z1.0;
    G01 Z0 F20.0;
    Y2.0;
    G03 X0 J-2.0;
    G01 Y-2.0;
    G02 X0 J2.0;
    G01 Y0;
    G0 Z1.0;
    M05;
    M19;
    G91 G28 Z0;
    G28 Y0;
    T2 M06;
    T1M06;
    M30;

    It's been a lot of years since I ran an 11M, so bear with me if I missed something, and don't be afraid to hit the big red button if something looks amiss.

    The program should turn on the spindle, rapid to G54 zero location, rapid to Z 1.0, feed to Z0, feed to Y2.0, feed CCW full circle 4" dia., feed to Y-2.0, feed CW full circle 4" dia., feed to Y0, rapid to Z1.0, turn off spindle, orient spindle, rapid Z axis to tool change position, rapid table all the way to the Y limit, execute tool change to tool 2, execute tool change to tool 1, return to start of the program.
    Thank you very kindly for this I will apply this and get back to you hopefully I can get to it one day this week maybe even tomorrow and I will get back thank you again very much.

  18. #52
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    I read back through your post and recommendation and now understand after homing the machine I need to set the g54 that's correct isn't it?

  19. #53
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    538

    Default

    Quote Originally Posted by Hot Headz Marine View Post
    I read back through your post and recommendation and now understand after homing the machine I need to set the g54 that's correct isn't it?
    Yes. You must set a new G54. Not after every home out- just whenever you run a different part.

    The G54 location is the part zero. It's the spot in the machining envelope you program from. X0 might be the left end of the part, Y0 the fixed jaw of your vise, and Z0 the top of the part, which we set with tool length offsets. I want you to set the tool length offset (H1) to -5.0.

    G54-G59 are work coordinates. You can use them all in the same program if you want to run multiple work locations, etc. But we'll stick with G54 to start.

    You have to set G54 before you run a new program. I want you to set it in the middle of the table and keep the spindle up in the air for the test run.

    edit to add: Don't forget to set the tool length offset (H1) to -5.0 or you'll get a Z+ overtravel.

  20. Likes cwtoyota, Hot Headz Marine liked this post
  21. #54
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    10-4....I will do it. Thank you again for your help.

  22. #55
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by jancollc View Post
    I added a spindle stop and orient.

    I remember that about Kuraki. First 11M I ran was on a KV1000. They want the tool number first because the tool changer pre-stages the next tool and remembers which pot each tool is in. I like that system, there's no waiting on the carousel.
    I have the KV-700 model and I do like the system for pre-staging tools.
    You can issue M16 instead of M6 to change the tools back to their original pot so oversized tools don't crash into each other the carousel too.

  23. #56
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by jancollc View Post
    Yes. You must set a new G54. Not after every home out- just whenever you run a different part...
    This statement brings something to mind... Hot Headz, do you know the proper way to home that machine?
    On some older Fanuc controls, you need to push the origin softkey after all of your homing lights are lit up. The procedure would go like this:

    1) Use the soft-keys to bring up the position display (the one with all four position screens on one page "Machine", "Relative", etc...).
    2) Put the mode selector switch in homing mode.
    3) Use the jog buttons and axis selector switch to home each axis.
    4) Push the right soft-key until you have an "Origin" soft-key.
    5) Push the "Origin" soft-key.
    6) Push the "All-Axis" soft-key.

  24. Likes Hot Headz Marine liked this post
  25. #57
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    Quote Originally Posted by cwtoyota View Post
    Modern computers don't have RS-232 (seria1 COM) ports. I use a USB to RS232 adapter as suggested by jancollc. The one I suggest is made by IOGear and the model number is GUC-232A. It has been 100% reliable with my Fanuc control as well as other RS-232 devices. I tried a crappy (cheap) chinese USB adapter as well as a few others and had nothing but problems with them.

    CADEM has a free software called NC NetLite that makes it pretty easy to communicate to the Fanuc control.
    There are tons of other software out there, but that's a quick download that could get you started.

    There are some settings necessary on the machine (parameters) to get it talking with the PC...
    If you can't get things working, PM me and I'll send you my known good settings from my 11M control.
    Excellent.. Absolutely will take you up on that. Thank you.

  26. Likes cwtoyota liked this post
  27. #58
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    Yes, the way this one works is go to Zero Return in selection switch, xyza +\- to jog off switches and hold xyza one at a time until axis auto homes and lights on + & - light up. This works but feed rates have to be lowered or over travels will alarm.

  28. #59
    Join Date
    Nov 2016
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    580
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    74

    Default

    Perfect explanation for me. I will do it and get back with results. Thank you again for all your help.

  29. #60
    Join Date
    Feb 2010
    Location
    Washington State
    Posts
    342
    Post Thanks / Like
    Likes (Given)
    467
    Likes (Received)
    124

    Default

    Quote Originally Posted by Hot Headz Marine View Post
    Yes, the way this one works is go to Zero Return in selection switch, xyza +\- to jog off switches and hold xyza one at a time until axis auto homes and lights on + & - light up. This works but feed rates have to be lowered or over travels will alarm.
    There's a parameter that slows the feed rate when the homing limit switch touches the homing dog...
    The parameter is something like "Max Rapid F Home" or something like that... I'll see if I can find it this afternoon.

    Do you put the machine back in home position before shutting it off?
    That's the way I was taught as "good practice" and I think it's a good habit to get into.

    If you do it that way, you can home the machine without the jog+ button.
    Simply power it up, switch to homing mode and hold the jog - button for each axis.
    It will rapid away from home position about 4 to 6 inches, then switch directions, decelerate and stop at home position.

  30. Likes Hot Headz Marine 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
  •