New to me Hitache Seiki 3NE-300 Lathe with Fanuc 5t Control. Could you some pointers - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 58
  1. #21
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,200
    Post Thanks / Like
    Likes (Given)
    4693
    Likes (Received)
    1619

    Default

    Quote Originally Posted by Garwood View Post
    I tried #2, but the 5T won't allow wear comp more than a few hundred thou. I use #1 and it works, but constant editing of programs is a PITA compared to having work offsets in the control.

    Wonder if there's a parameter that limits wear comp that I could change? Hmmm.

    OP, Put up a few pics so we can get a peek at this little booger.

    For the fellas wanting to not use G50's and with a limit on the maximum allowable offset. Does anyone know if these parameters are available in the 5T control?

    Parameter 5013 Maximum value of tool wear compensation.

    Parameter 5014 Maximum value of incremental input for tool wear compensation.

    This will allow larger offsets in the offset table. I believe the limited maximum offset value is a safety precautionary measure because machine applies the offset on the next G0 move instead of at the T call. If turret doesn't shift by the offset amount at the T call it is applied on the next G0 move, if you change the machine to except larger offsets and don't understand this and make large offset adjustment while the machine is running you could be left standing there scratching head wondering wtf just happened..

    Parameter 5002 bit #2 LWT Tool wear compensation is preformed by:

    0: Moving the tool.

    1: shifting the coordinate system.

    Using G50's the machine needs to be started in the exact spot the G50's were figure from. If the program interrupted a couple of safety blocks can be added to the start of each tool with block delete in front to position the machine for automatic operation.

    /G28 U0.
    /G28 W0.
    /G0 W-? (If not running from zero return)
    /G0 U? (If not running from zero return)
    G50 X Z

    Once the machine is running just turn on the block delete to skip those blocks.

    Never change a parameter in your machine without seeing it in your manual yourself first.


    Brent

    http://www.practicalmachinist.com/vb...ml#post2420986

  2. #22
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,135
    Post Thanks / Like
    Likes (Given)
    4442
    Likes (Received)
    2084

    Default

    I think all 5T's use G96/G97 as standard. That would be pretty shitty to have a CNC lathe that didn't.

  3. Likes yardbird liked this post
  4. #23
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    160
    Post Thanks / Like
    Likes (Given)
    27
    Likes (Received)
    52

    Default

    Hi,
    Not sure this is terribly helpful but I have a 3NE-300. I got mine 4 months ago or so but it has a Fanuc/GN 6T (not entirely sure the difference). Year is ~1985. 4000 rpm spindle 1.375" bore. So far it has been good ie everything works. I also have all the manuals, with some of them looking like they covered 5T operation. Or at least 6T without a screen. I took the machine down to the castings and freshened it up best I could. It came with a local contact that operated the machine so I got a couple in person tutorials first. After I understood the basics, the stuff in the manuals fell into place much better. Using something this old with no manuals would be very tricky.
    If you don't mind saying, what did you consider a good deal on your machine?
    You mentioned Mach3 conversion. I have done both Mach and Linuxcnc. I highly recommend Linuxcnc over Mach3 and will do a retrofit on this the first time something of consequence fails. I look forward to hearing about your experience with this. Good luck. img_1948-1-.jpg

  5. #24
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,502
    Post Thanks / Like
    Likes (Given)
    822
    Likes (Received)
    2436

    Default

    Quote Originally Posted by Heinz R. Putz View Post
    .....S500 was automatically RPM, no G96 for SFM.
    This is not correct. G96 may have been an option, but the 5T I ran on a Mori Seiki TL40B had G96.

  6. #25
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,502
    Post Thanks / Like
    Likes (Given)
    822
    Likes (Received)
    2436

    Default

    Quote Originally Posted by vmipacman View Post
    ...it has a Fanuc/GN 6T (not entirely sure the difference).
    No difference between them. General Numeric was a company that sold Fanuc controls in the US. IIRC there was some joint ownership of the company between Fanuc and Siemens?

  7. #26
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,664
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1442

    Default

    Quote Originally Posted by Heinz R. Putz View Post
    Good luck with the 5T, there are still a lot around and working.
    I trained the class for Fanuc in Chicago back then, the 6T came out in about 1980, it was quite an improvement for those days.
    The 5T:
    No screen at all.
    No decimal point, all dimensions, also feedrate written lke: X30000 for X3.0, F100 for F.01.
    S500 was automatically RPM, no G96 for SFM.
    No Program Number, all programs start with block numbers. No noseradius comp.
    Quite reliable.
    This is Heinz at doccnc.com, good luck.
    Hello Heinz,

    Tool Nose Radius comp is most assuredly available with the 5T control, and as Vancbiker points out, Constant Surface Speed is available. How the spindle speed is achieved was up to the MTB, with many machines of this circa having fixed spindle speeds programmable via an S code and number that related to a particular RPM. For example, S1 may have been 50 rpm, S2 100 rpm and so on.

    Regards,

    Bill
    Last edited by angelw; 12-11-2014 at 03:20 AM.

  8. #27
    Join Date
    Jul 2013
    Location
    Australia
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    25

    Default

    Our machines with 5T had G41 G42 and G96 all worked fine. However our machines were quite large Ikegai's going home for tool changes was not an option.
    Our turrets had tools that was greater than 100mm from turning to boring so G50's for each tool was a must.
    We sold our old machines and they are still running in a plant in Sydney today. There are heaps of 5T's out there. You will get it going and make some cool parts.

  9. #28
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    Thanks for all the replies. I am spending most lunch breaks bugging my friend about this machine. Last time he worked with a 5T was back in 1977. The guy has an incredible memory, and has been a true cnc machinist for that entire period and beyond. When something is broke he is the go to guy. I'm feeling pretty lucky to have someone local willing to work with me one on one. Gonna have to beg the wife for some apple pies I think.

    I only have a couple pics that I snapped with my cell. I'll try to get them up tonight. Machine looks pretty good, but the guy says they did repaint it 12 years ago when he bought it.

    Do those who have a 5t know if G71 is an option on these?

    Thanks again. Getting closer to Jan every day.

  10. #29
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,664
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1442

    Default

    Quote Originally Posted by wolfenstien View Post

    Do those who have a 5t know if G71 is an option on these?

    Thanks again. Getting closer to Jan every day.
    Yes, all of the Multi-repetative cycles (G70 - G76) were available with the 5T control. This suite of cycles are Options (even with current model machines), but most machines were supplied with them. Only Type I version cycles were available.

    Regards,

    Bill

  11. #30
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    20141206_092747.jpg20141206_092747.jpg

    Not sure if this photo is going to work. Like I said crappy quality as its just a snap shot from my phone. I'll get some better pics when it arrives.

    I wasn't sure if I was going to have the G70-G76 commands or if I was going to be limited to the old g9X commands. Thanks again for all the input. I shoulda tried to grab the manual while down there to get some literature on it. Oh well.

  12. #31
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    Machine is Home now. All said and done worked out to be $1500 for the machine and about $250 in moving expenses.

    I've got it all torn down at the moment cleaning it out. Wasn't bad except for the coolant tank. Getting it back together now. Just started playing with the control. Actually I am having a small issue. I can get MDI mode to function well enough, but I am having no luck with writing program and running them. Here is the little program I am trying to run.

    N001 G50 X-20000 Y-50000 S200
    N002 T0101
    N003 G1 X-1000 Y-10000 F10
    N004 M30

    Very short just to see if it does something. Not to mention it doesn't take long to key in. I can get it all keyed in fine in edit mode, but I can't seem to find the program in memory mode. Not sure if I need to look for it or call it up somehow. I've tried pressing almost all the buttons and am getting nothing. No alarms no nada. I got annoyed with it after the first couple nights of getting nowhere and order the operations manual off ebay for $50. Ought to come in handy.

    Also tried to get the BTR going but had no joy there. I installed NClink from onecnc, and built a null modem cable for the unit. I'm getting confirmation that the BTR is receiving a file and has it in its memory, but am not getting any response from the machine control. I may not have my configuration right for that, on the other hand I might have something busted don't know.

    If anyone mind giving me the proceedure step by step for keying in a program and then running said program I would appreciate it. Is there a way to label the program and call it? Does it need to start with some particular header or something. Any help would be great.

    Thanks you all.

  13. #32
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,135
    Post Thanks / Like
    Likes (Given)
    4442
    Likes (Received)
    2084

    Default

    Your lathe has a Y axis? (think you mean Z there)

    You have to call up the tool first with T0100 Then, on the same line as the first rapid move you apply the offset- T0101. I don't think you can just call up the tool and the tool offset at the time with T0101 from the get go. It doesn't work that way on a 5T. I'm pretty sure that the offset apply (T0101 in this case) has to be on a line with a move. T0101 isn't telling the machine to move, it's telling it to comp for the offset in the move on the same line. It adds or subtracts the X and Z wear comp values during the first move.

    If the lathe has a geared spindle you need to set spindle range in the first line like M25 or M37 or some such. The SXXXX number you put on the G50 line is the max spindle speed limit and has to match the gear range you select. Like if the lathe only does 1000 RPM in low gear you can't put G50 S1100. It won't work. The next line will be the G96 or G97 with the tool callup and actual programmed spindle speed or SFM. The next line will be your M03 or M04 by itself and the line after that will have the first move and the tool offset apply.

    I use the BTR for everything on my 5T Mazak. It's an ADR. The baud rate must match exactly. I never use the memory in mine. I just send to the BTR, put the control in tape mode and hit cycle start. If you want to use memory mode I think you need to be in memory mode or edit, hit the read button and then you can run from memory after it's in there.

  14. #33
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    Quote Originally Posted by Garwood View Post
    Your lathe has a Y axis? (think you mean Z there)
    Whoops. DUH!.

    Thanks for the reply. Any guesses on what the baud rate may be? I can set the baud rate on the pc, and on the ADR board, but I don't know what the one on the control is. Currently have both pc and BTR set for 9600. are you running 7 or 8 bits?

    Even if my code was wrong I should at least get an alarm or be able to scan through it right? My machine doesn't have a gearbox. I don't really know what I am doing.

    Would you be willing to walk me through it? Could I possible phone you? Sorry to be a bother but would love to get the old girl running.

  15. #34
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    So I've been doing my best to read all post on the 5t and was re-reading some today as I am befuddled by this control. Came across a post by garwood mentioning how to run in MDI, also noted that you only use MDI when you gotta as its so tedious. Anyway, I'm wondering if that is part of my mistake. I am writing my code with the turn switch in edit mode. I'll give it a go in MDI. Didn't realize you could write more than a single line in MDI.

    Also something you referred to in that same post is the cycle start button. Not sure if this is true, but I don't think i have one. I have a "start" button up by the keypad but nothing that says cycle start. Down by my tailstock controls I have a two buttons side by side that say tape with a leader line pointing to each. One says feed hold, the other says start.

    Should my machine have a "Cycle" Start button or just the start??? Maybe I'm blind. I'm going to head out and take a look right now. Back in a few.

  16. #35
    Join Date
    Aug 2006
    Location
    Cape Cod, Ma
    Posts
    454
    Post Thanks / Like
    Likes (Given)
    169
    Likes (Received)
    96

    Default

    I just got the communications running on my 3tf today. I don't know how different the settings are for the 5t but my baud is set for 1200, 7 bit, even parity, 2 stop bit. as for cycle start that should be the green start button next to feed hold.

  17. #36
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    I did get some code running to the machine on Monday night. Despite what I have read about the Pre 1990 Fanuc controls only being able to process at 4800 baud, I've got mine set to 9600 and it seems to be working fine. At least that is what the PC and the BTR are set to. Not sure if the BTR is actually communicating at that rate.

    Found out my initial understanding of g50 was %100 backwards. IE I was giving negative values as I thought it was distance from Home position to part datum. Instead its from part datum to Home. I've only run short little bits of code so who knows if the system is stable yet. I don't even have stick tools for it yet. I'll see if I can't come up with a fairly rigorous program and run the control through its paces and make sure I am not loosing data etc. Then Maybe I'll write something for the single 3/4 inch shank tool I have and see what the machine can do as far as repeat-ability. Being that she is vintage 1978 I would guess there is some wear but I haven't a clue how much.

    Anyway, I've been meaning to change the hydraulic fluid. Manual says to it every 6 months. Is that for real? I suppose that would assume at least 40 hr run times per week? IE approx 1000 hrs of on time? My guess it it take me a few-10 years to do that. I'll try and post my working code and comment on it if anyone finds it useful...

    Thanks for all the help so far. Still excited to see it cut some chips.

    Oh yeah that reminds me. On a machine like this looks like i have the option of running tool upside down or right side up. Currently looks like every thing was run upside down. Any thoughts? I am thinking I am likely to go with all right hand tools and flip em upside down?

    Thanks again.

  18. #37
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Yes tools are upside down
    One thing I did was add to the bar in the back that trips the micro switch for the Z safe tool change point I run all short tools and it is a long ways back to change tools
    I change oil ever 5 years or when it starts looking dirty just make sure to use the right oil.
    I put some Napa brand oil in and ended up replacing every frecking o-ring in the machine
    Check the lube pump make sure all the lube line are getting waylube
    I had one get water in it plugged metering jets
    My machines hold .0002 after there warmed up but from cold to warm I change the offset .0013
    you can call me if ya want @ Benjamin Machine

  19. #38
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    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

  20. #39
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,200
    Post Thanks / Like
    Likes (Given)
    4693
    Likes (Received)
    1619

    Default

    It does seem that if your machine didn't have the G71 option you would get a alarm. Improper G code?

    Nothing about you program jumps out at me as being wrong unless im not seeing it.


    Brent

  21. #40
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    N001 S15000?

    I don't use nose rad comp my machine only has 16 offsets so I just let the cam do the comp
    I don't use the G50 on start line to easy to start in the wrong place I just use the G50 to set zero in morning
    Tool offsets have been working fine the last 27 years
    G71 not sure what that is
    P009 is the call out for for sub to go to line 9
    Q not sure
    D is part of the S76 threading
    And FYI E if your machine has the fine thread option is 6 place thread pitch
    I have never used the U or W call outs


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
  •