New to me Hitache Seiki 3NE-300 Lathe with Fanuc 5t Control. Could you some pointers - Page 3
Close
Login to Your Account
Page 3 of 3 FirstFirst 123
Results 41 to 58 of 58
  1. #41
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1618

    Default

    G71 is a rough turning canned cycle. P & Q is the first and last bolck of profile to be roughed U & W are finish allowances D is depth of cut for the rough cycle.


    Brent

  2. #42
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by wolfenstien View Post
    Good evening Gents,
    Haven't got much to show for the last couple weeks. I can start the machine and drip feed consistently, but my format is shaky. I run through a ton of time before I get a piece of code to run right. Currently am trying to get a G71 cycle to run. Problem is I don't get an alarm instead the machine reads down to line 008 jumps to line 012 (moving -.010 in X) and then stops. No alarms no nothing. Just sits there. I dunno whats going on.

    I am hopeful that since it didn't alarm out that it may be capable of using G71. Do I have the wrong format going on?

    Any help would be appreciated.

    N001 G50 X40000 Z70000 S15000
    N002 T0100
    N003 X35000 T0101
    N004 G96 S350 M03
    N005 M08
    N006 30000
    N007 Z500
    N008 G71 P009 Q12 D0050 F0040 U0000 W0000
    N009 G00 X20000
    N010 G01 Z-5000
    N011 X22000 Z-10000
    N012 X30000
    N013 G00 Z1000
    N014 M09
    N015 M01
    Hello wolfenstien,
    With reference to your code above
    1. as already been mentioned by another, S15000 in Block N001 should be S1500. Its unlikely that this old machine has more than 15000 revs available to be able to limit the Spindle Revs to that amount.

    2. perhaps a Typo when listing your program here, but there should be an address before 3000 in the N006 30000 Block; probably X

    3. make sure you specify Feed per Rev mode before launching your G71 cycle. If by chance the control is in Feed per Minute mode (G98), a Feed Rate of F0040 may appear that the slide is stopped, when in reality the slide is moving very, very slowly. Look at the position readout to see if there is any movement in the X or Z slide. Accordingly, ensure that G99 has been programmed before the G71 block is executed.

    Your control will have the G71, Multi-Repetitive cycle:
    1. a p/s 010 alarm would be raised if G71 was not a function of the control
    and
    2. by the cursor jumping down to Block N012 indicates that the profile described by blocks between the P and Q referenced blocks inclusive is being processed.

    Regards,

    Bill
    Last edited by angelw; 03-17-2015 at 07:04 AM.

  3. Likes yardbird liked this post
  4. #43
    Join Date
    Aug 2006
    Location
    Cape Cod, Ma
    Posts
    452
    Post Thanks / Like
    Likes (Given)
    169
    Likes (Received)
    96

    Default

    Don't you need a G00 up at line N003? There are 3 movement before the G71 but no travel command. I only use g50 for spindle speed limit so.... I don't know if it acts as a traveling command.

  5. #44
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    Yeah it doesn't help when I through typos in the code I post.

    Spoke with some friends at work and they mentioned two things. One. older controls tend to like to have the cycle boxed in. Meaning that the last line of the cycle moves back to the exact position the cycle started at. (It was noted that that last move should be in a single axis only)

    The more likely culprit was pointed out by the second friend. Being that I am likly in G99 and I had taken out the spindle start line (Again not shown in my post) The machine was trying to move at .004/Rev and the spindle was turning at 0 revs therefore actual feed speed was 0.

    Don't know if these two items will make everything better, but I just got home from work I am about to go punch these in and see.

    Will let you know.

  6. #45
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default



    IT WORKED. G71 is out there running right now. Will take a picture of the code I am running. No typos that way.

  7. #46
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by wolfenstien View Post

    The more likely culprit was pointed out by the second friend. Being that I am likly in G99 and I had taken out the spindle start line (Again not shown in my post) The machine was trying to move at .004/Rev and the spindle was turning at 0 revs therefore actual feed speed was 0.
    Hi wolfenstien,
    Your above statement is not correct. You turned the spindle on in N004 G96 S350 M03, long before launching the G71 cycle. Accordingly, the spindle would have been running and G99 is the correct Feed Motion code to use. As I suggested back in Post #42, it could have been that your control was in G98 (Feed per Minute) mode. In this case it would have taken one minute for the slide to travel 0.004", and could have been mistaken for stopped.

    Your N012 X30000 for the last block in the Profile Description is correct. There is no need to have the cycle Boxed in, as you put it.

    Regards,

    Bill

  8. #47
    Join Date
    Oct 2018
    Country
    CANADA
    State/Province
    Ontario
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Yes , please post some program with G71
    Thank

  9. #48
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1618

    Default

    Quote Originally Posted by m1234a1 View Post
    Yes , please post some program with G71
    Thank
    G28 U0
    G28 W0
    G50 X0 Z0
    M41
    G0 T0101
    G99
    G97 S M
    G0 X6. Z.5
    G50 S
    G96 S
    G0 X2. Z.1 M8
    G71 P1 Q2 U W D F
    N1 start of part profile

    Part profile

    N2 end of part profile
    G0 X2.
    M9
    G0 X6. Z.5 T0100 M5
    G28 U0
    G28 W0
    M30

    I think that's pretty much everything but the numbers. Should run on a 5T

    Brent

  10. #49
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by yardbird View Post
    G28 U0
    G28 W0
    G50 X0 Z0
    M41
    G0 T0101
    G99
    G97 S M
    G0 X6. Z.5
    G50 S
    G96 S
    G0 X2. Z.1 M8
    G71 P1 Q2 U W D F
    N1 start of part profile

    Part profile

    N2 end of part profile
    G0 X2.
    M9
    G0 X6. Z.5 T0100 M5
    G28 U0
    G28 W0
    M30

    I think that's pretty much everything but the numbers. Should run on a 5T

    Brent
    Hello Brent,
    It should be mentioned that the N1 Block in your example can only contain an X address, as G71 Type II was not available with the FS 5T control.

    Regards,

    Bill

  11. #50
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1618

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    It should be mentioned that the N1 Block in your example can only contain an X address, as G71 Type II was not available with the FS 5T control.

    Regards,

    Bill
    Hello Bill,

    Good catch! I hadn't given that any thought. I didn't reread the thread but I believe I remember someone somewhere mentioning the 5T doesn't use decimals either. Maybe that was the 3T?

    Brent

  12. #51
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by yardbird View Post
    Hello Bill,

    Good catch! I hadn't given that any thought. I didn't reread the thread but I believe I remember someone somewhere mentioning the 5T doesn't use decimals either. Maybe that was the 3T?

    Brent
    Hello Brent,
    That's correct that the 5T control can't use decimal point format, the the 3T control can. I had a quick read through this Thread and there was a lot of incorrect information put forward.

    Regards,

    Bill

  13. #52
    Join Date
    Feb 2010
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    I have purchased this Machine from the OP. There are not a lot of threads about these machines out there so I thought I may keep it going a bit instead of starting a new one.

    The OP is a great guy and we have had a few dealings and even keep loosely in touch. I knew exactly what I seemed to have gotten. Or as much as he honestly knew as he never really produced more than a single item on it (as I gather).

    I have mixed experience manual and cnc. Honestly on the shop floor I usually didn't do much more than setup and simple program edits. I have an Eagle knee mill that was Anilam cnc outfitted and a year or so before I purchased it it was updated to run mach 4 with a win 7 PC. The mill is running daily and I really need to have the 3NE-300 up to speed as I'm doing all that work manually. The last cnc lathe I ran was a Haas vl2, and numerous other brands and controls (all pretty similar though).

    I will admit I have a bit more studying to do to understand the 5t interface. I spent an afternoon with the 5t manual and it is beginning to make sense. I have the btr board reinstalled and it seems to recognize the computer. I seem to be able to send the board programs and receive them back.

    Any how... If any has one of these machines or comparable. I have a port of some sort that has nothing in it that is leaking a good deal of way oil. It looks to me like it probably had a plug but I don't want to block it off if that is not what should be happening with it. I inspected for lines that may have been unhooked but see no obvious signs of such. Thanks in advance for and informed advice.


    Sent from my SM-G960U using Tapatalk

  14. #53
    Join Date
    Feb 2010
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    [QUOTE=Tuff Luck Tom;3356742]I have purchased this Machine from the OP. There are not a lot of threads about these machines out there so I thought I may keep it going a bit instead of starting a new one.

    The OP is a great guy and we have had a few dealings and even keep loosely in touch. I knew exactly what I seemed to have gotten. Or as much as he honestly knew as he never really produced more than a single item on it (as I gather).

    I have mixed experience manual and cnc. Honestly on the shop floor I usually didn't do much more than setup and simple program edits. I have an Eagle knee mill that was Anilam cnc outfitted and a year or so before I purchased it it was updated to run mach 4 with a win 7 PC. The mill is running daily and I really need to have the 3NE-300 up to speed as I'm doing all that work manually. The last cnc lathe I ran was a Haas vl2, and numerous other brands and controls (all pretty similar though).

    I will admit I have a bit more studying to do to understand the 5t interface. I spent an afternoon with the 5t manual and it is beginning to make sense. I have the btr board reinstalled and it seems to recognize the computer. I seem to be able to send the board programs and receive them back.

    Any how... If any has one of these machines or comparable. I have a port of some sort that has nothing in it that is leaking a good deal of way oil. It looks to me like it probably had a plug but I don't want to block it off if that is not what should be happening with it. I inspected for lines that may have been unhooked but see no obvious signs of such. Thanks in advance for and informed advice.


    An update on the last post. I put a fitting in the hole and ran a hose from it to a bucket. It seems to be way oil and some coolant. I am going to leave as is.

  15. #54
    Join Date
    Feb 2010
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default BTR Board Update

    I finally seem to have the btr board operating. I have been hand entering programs into the memory. While that works it is cumbersome and time consuming. Not a big deal if it will be set up to run production but I do short runs here.
    I am not 100% sure that the btr is operating as intended. But I can send programs to the board and run them on the lathe in tape mode. I can read/download (to computer) the program I have hand entered in memory.

    I can not edit the program in the memory through the btr and computer. And am not sure if that is an intended option.

    Operating off the btr in tape mode is ok. But the M30 at the end of the program doesn't return me to the top of the program. Probably because it's acting as a tape would? It's ok but I don't love it. It will gladly take the trade in set up time and program editing.

    I can not seem to get the btr to echo the program back to the computer or show NC block.

    I have never used a BTR so it may be my mistake. I figured I'd at least update this for any lurkers on the subject.

    This morning I pulled the punch cable and ribbon cable and tested continuity. I had previously done this to all the serial cabling between the computer and the btr. Today I also changed the usb/serial cable for a new (in package) one that I have had. I just needed the machine/btr to work so I did not try as I went and it working now could be a result of any of those 3 changes. I did not find faults in any cables.

  16. #55
    Join Date
    Feb 2010
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    20191009_122513.jpg

    My terminal settings using NC Link. The BTR Board is from Advanced Digital Research. I did reach out to them and they were polite but mostly unwilling to clarify my questions about operation. I do have the manual and it is ok but leaves room for questions when things are not going 100%.

  17. #56
    Join Date
    Feb 2010
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    And the receive settings.

  18. #57
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,401
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2371

    Default

    You might try substituting M2 for the M30 at the end of the program.

  19. #58
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,081
    Post Thanks / Like
    Likes (Given)
    4382
    Likes (Received)
    2053

    Default

    I used an ADR on a %T for about a decade and never had an issue. ADR was always great if I had a question.

    I think you're overestimating what you can do with a tape reader and the 5T. You can send a program, that's it.


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
  •