New to me Hitache Seiki 3NE-300 Lathe with Fanuc 5t Control. Could you some pointers
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 58
  1. #1
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default New to me Hitache Seiki 3NE-300 Lathe with Fanuc 5t Control. Could you some pointers

    Good Evening Gents,

    This past weekend I took a trip to look at a CNC lathe. I've hemmed and hawed at a lot of cnc mills and lathes, but the price was right so I put down some money and assuming she fires up and runs as expected I'll be pulling this machine home. I've never owned a true cnc machine. I've built a cnc router in college. And I picked up a Bridgeport Boss CNC mill awhile back. Both machines run Mach3. The Boss has actually made a few parts and seems to work ok. Kinda disappointed with the Mach3 control but I digress this thread is about the new (to me) lathe. I expect the age of the lathe is somewhere around 1980 (a good 10 years older than me )

    Supposedly the machine has manuals, but they were in the back cabinet and the door was against a post and couldn't be opened so I currently don't have any literature on the machine. It is a Hitachi Seiki 3NE-300. 10 Hp lathe with hydraulic tailstock, 12 position turret and a small 6" hydraulic chuck. Shop owner was to busy with end of the year work to get to the machine, but wrote me out a bill of sale guaranteeing full power up with opportunity for an inspection prior to Jan 31st. Worked out well for me. I gotta get a space cleaned out for it and run power over etc. My biggest concern is the 5T control.

    Luckily I have a friend at work who seems to remember using a 5T way back when and is willing to come over and start walking me through it when its ready. I got so excited when I came home the first thing I did was pick up an ADR BTR (Behind the tape reader) on ebay. Paid a little less than $150 for the BTR card so I think that was a good deal. From what I have read it should make the control much more usable. I'm thinking I'll try onecnc/cnclink for the softward side.

    Most of what I am looking for out of this thread is what to expect from the control. I have read that the 5T doesn't read decimal points in dimensions. Is this correct? I was also wondering if anyone had an idea of which canned cycles will and wont work. Will G71 work? I really don't know much about programming a lathe, but the before mentioned friend from work is a bit of a guru in my opinion. He tolerates me bugging him during lunch breaks about simple programs and is a wealth of knowledge and seems quite willing to disperse that knowledge. Figured I would try to tap you guys as well though.

    There are about 1/2 dozen threads on here with 5T controls, but they don't get to in depth. Sounds like DOCCNC has some dvds on them, but they look a little expensive for the home shop startup guy.

    Anyway. Any input on either the machine or the control is much appreciated. I find a astonishing shortage of info online for the Hitachi Seiki machines. Thank you all.

  2. #2
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1618

    Default

    The other place has a Funuc 5T sub forum. Rhymes with see n see bone dot com.


    The only person here that mentioned he has a Fanuc 5T that I know of is Garwood.



    Brent

  3. #3
    Join Date
    Oct 2014
    Country
    UNITED KINGDOM
    Posts
    703
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    350

    Default

    Quote Originally Posted by wolfenstien View Post
    ...I have read that the 5T doesn't read decimal points in dimensions. Is this correct?...
    Yes.
    I.e. You would have to write X50.0 as X50000

  4. #4
    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,


    Luckily I have a friend at work who seems to remember using a 5T way back when and is willing to come over and start walking me through it when its ready. I got so excited when I came home the first thing I did was pick up an ADR BTR (Behind the tape reader) on ebay. Paid a little less than $150 for the BTR card so I think that was a good deal. From what I have read it should make the control much more usable. I'm thinking I'll try onecnc/cnclink for the softward side.

    Most of what I am looking for out of this thread is what to expect from the control. I have read that the 5T doesn't read decimal points in dimensions. Is this correct? I was also wondering if anyone had an idea of which canned cycles will and wont work. Will G71 work? I really don't know much about programming a lathe, but the before mentioned friend from work is a bit of a guru in my opinion. He tolerates me bugging him during lunch breaks about simple programs and is a wealth of knowledge and seems quite willing to disperse that knowledge. Figured I would try to tap you guys as well though.
    All of the Multi-repetitive cycles (G71 - G76) are available with the 5T control. They are options, the same as they are on more modern controls, but most machines were supplied with them. G71 Type I is the version supplied; Type II wasn't in existence when the 5T was introduced.

    Its correct that the 5T control doesn't tolerate decimal points. I supply software to my clients who have 5T controls and the Mill equivalent, that displays the program with decimal points included on the PC screen (easier to read), but converts the data to the format that the 5T requires as its drip fed to the control.

    Regards,

    Bill

  5. #5
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    I have a 5T on my 3NE300 and 4NE400
    I can post some sample programs I use if ya want

    Bill

  6. #6
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1618

    Default

    Quote Originally Posted by BMP View Post
    I have a 5T on my 3NE300 and 4NE400
    I can post some sample programs I use if ya want

    Bill
    Does the 5T use G50's? It would be interesting to look at some of your 5T example programs. Other than single line canned cycles its probably not too much different than the i control. Might help the OP...


    Brent

  7. #7
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,083
    Post Thanks / Like
    Likes (Given)
    4383
    Likes (Received)
    2053

    Default

    Yep, I run a 5T Mazak almost everyday. Mines 1979, 4 years older than me. Mine had an ADR BTR installed when I bought it. The ADR folks are good people. Helped me get the RS232 setup right when I bought it.

    No decimals, no work offsets, no screen. Get used to reading numbers from right to left.

    My 5T has been rock solid reliable. The only issue I have had is running from memory. Sometimes it would lose some Z distance, like inches. I run mine straight from the BTR instead of loading into memory first now. No problems.

    When you get it set up you'll have questions. Ask away. When you run it your butthole will be puckered with no display. After awhile you kinda get used to it. Totally new parts/tooling are always a bit scary.

  8. Likes jdowd liked this post
  9. #8
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by yardbird View Post
    Does the 5T use G50's? It would be interesting to look at some of your 5T example programs. Other than single line canned cycles its probably not too much different than the i control. Might help the OP...


    Brent
    I don't have any programs here I guess
    this is the Smart Cam TMP file

    @START
    %
    #ONBLKM98P100L10
    M30
    #SAFBLK#SPMODE#MOVX#XPOSZ#ZPOST#TOOLS#SPEED
    T#TOFFM8
    #NEXTPT
    #MOVX#XPOSZ#ZPOS#SPNDL
    @TOOLCHG
    #SAFBLK#SPMODE#MOVX#XHOMEZ#ZHOMET#TOOLS#SPEED
    T#TOFFM08
    #NEXTPT
    #MOVX#XPOSZ#ZPOS#SPNDL
    @END
    #SPOFF
    G00X#XHOMEZ#ZHOMET#NTOOLM09
    M01
    M99
    #OFFBLK
    N9999G28X0Z0
    N9991G50X80000Z113000S4000
    N9992M30
    %
    @STPROF
    <#MOV><X#XPOS><Z#ZPOS>
    @RAP
    <#MOV><X#XPOS><Z#ZPOS>
    @LINE
    <#MOV><X#XPOS><Z#ZPOS><F#FEED>
    @ARC
    <#MOV><X#XPOS><Z#ZPOS><I#XCTR><K#ZCTR><F#FEED>
    @FXD1
    G76X#XPASSZ#ZPASS<I#XOV>K#V1D#V2F#FEEDA60
    @FXD4
    G33Z#ZPASSF#FEED
    M04
    G33Z#ZPOSF#FEED
    @TAILIN
    M05
    M12
    G04P250
    M03
    @TAILOUT
    M05
    M13
    M03
    @OPEN
    M05
    M69
    G0Z#ZPOS
    M68
    G4P200
    @STOP
    M0

  10. #9
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,083
    Post Thanks / Like
    Likes (Given)
    4383
    Likes (Received)
    2053

    Default

    That looks absolutely nothing like a 5T post. That barely resembles G-code?

  11. Likes toolmaker96 liked this post
  12. #10
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by Garwood View Post
    That looks absolutely nothing like a 5T post. That barely resembles G-code?
    That is the Smart CAM post processor not a program

  13. #11
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,401
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2371

    Default

    Quote Originally Posted by BMP View Post
    That is the Smart CAM post processor not a program
    You still use SmartCam??? Back in the day it was pretty good, but after all the ownership changes they seemed to lose direction and got left in the dust.



    @yardbird, Yes, the 5T can use G50s. I did on the one I ran back in the late 70s-early 80s. Then your offsets are just used to adjust for tolerance and wear. I pretty sure it would have been possible to set each tools position as an offset but that would have big numbers in the registers and if you fat fingered in a wrong value........

  14. #12
    Join Date
    Jul 2013
    Location
    Australia
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    25

    Default

    Had 5T lathes for years. You really need to get your head around the G50. When you change tools you need to call G50 for each tool as the wear offsets only go 100mm. I would only suggest using these for tolerancing.
    If you send me a pgm you make I can edit it for you no prob.
    Its really only G50X....Z....(This usually home in X and I generally used Z 200mm from the face of your part.)
    T0101
    ..
    ..
    G00G40 X (must be the same as last G50) Z (must be the same as last G50)
    T0202
    G50X....Z.... This G50 is the position that Tool 2 is from X 0 Z 0 on your part.
    And repeat for each tool.
    NOTE. If you pull the turret forward or move in Z to change or check tips between parts you MUST manually drive the turret back to the original start position. (Home in X and Z200 from the face of the part.)
    There are many ways you may choose to set as a pgm method but basically you NEED to remember that wherever the tool is when the pgm reads the G50 the machine thinks that is where it is. BIG crashes if you are not diligent with your checking. BTW thes old electronics and DC motors take a few seconds to pull up when you crash so damage is never small.
    Cheers

  15. #13
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by Vancbiker View Post
    You still use SmartCam??? Back in the day it was pretty good, but after all the ownership changes they seemed to lose direction and got left in the dust.



    @yardbird, Yes, the 5T can use G50s. I did on the one I ran back in the late 70s-early 80s. Then your offsets are just used to adjust for tolerance and wear. I pretty sure it would have been possible to set each tools position as an offset but that would have big numbers in the registers and if you fat fingered in a wrong value........
    Ya I'm old still running it on a 486-66 with windows 3.1 lol
    Still works for me all that matters

    I'm sure I will get bashed for my poor programing skills but here is the code

    %
    N100G97G00X50000Z30000T0100S1000
    N101T0101M8
    N102G00X15001Z1000M03
    N103X14001
    N104G01Z-38810F40
    N105G00X14501Z1000
    N106X13501
    N107G01Z-38810
    N108G00X14001Z1000
    N109X13001
    N110G01Z-38810
    N111G00X13501Z1000
    N112X12501
    N113G01Z-37450
    N114G00X13001Z1000
    N115X12001
    N116G01Z-37450
    N117G00X12501Z1000
    N118X11501
    N119G01Z-37450
    N120G00X12001Z1000
    N121X11001
    N122G01Z-37450
    N123G00X11501Z1000
    N124X10501
    N125G01Z-37450
    N126G00X15000Z1000
    N127X11100Z50
    N128G01X-520
    N129X8389
    N130G03X8898Z-55K-360
    N131G01X9939Z-576
    N132G03X10150Z-831I-255K-255
    N133G01Z-37450
    N134X11920
    N135G03X12740Z-37860K-410
    N136G01Z-38810
    N137G00X15000Z1000
    N138X50000Z30000
    N200G97G00X50000Z30000T0300S1300
    N201T0303M08
    N202G00X11000Z0M03
    N203G01X600F30
    N204X8209
    N205G03X8704Z-103K-350
    N206G01X9745Z-623
    N207G03X9950Z-870I-247K-247
    N208G01Z-37490
    N209G02X9970Z-37500I10
    N210G01X11740
    N211G03X12540Z-37900K-400
    N212G01Z-38800
    N213G00X50000Z30000
    N300G97G00X50000Z30000T1100S500
    N301T1111M08
    N302G00X10600Z2000M03
    N303G76X9100Z-9000K500D100E71428A60
    N310G00Z2000
    N311X50000Z30000
    N312M05
    N313G00X50000Z30000T0100M09
    N314M30
    N9999G28X0Z0
    N9991G50X89556Z93000S3000
    N9992M30
    %
    Program 2
    %
    N10M98P100L10
    N11G97G00X70000Z60000T0100
    N12M30
    N100G97G00X50000Z30000T0100S2500
    N101T0101M8
    N102G00X10000Z0M03
    N103G01X-300F40
    N104X7524
    N105X8000Z-238
    N106Z-3150
    N107G00X50000Z30000
    N200G97G00X50000Z30000T0200S2500
    N201T0202M08
    N202G00X0Z1000M03
    N203G01Z-2500F80
    N204G00Z1000
    N205X50000Z30000
    N300G97G00X50000Z30000T0400S2500
    N301T0404M08
    N302G00X6000Z500M03
    N303G01Z0F20
    N304X5582
    N305X5200Z-191
    N306Z-3070
    N307G00X5000Z500
    N308X50000Z30000
    N400G97G00X50000Z30000T0900S2500
    N401T0909M08
    N402G00X9000Z-2500M03
    N403G01X8000F20
    N404Z-2800
    N405X7600Z-3000
    N406X4600
    N407G00X9000
    N408X50000Z30000
    N500G97G00X50000Z30000T1000S2500
    N501T1010M08
    N502G00X0Z-2000M03
    N503M05
    N504M69
    N505G0Z500
    N506M68
    N507G4P200
    N508X50000Z30000
    N509M05
    N510G00X50000Z30000T0100M09
    N511M01
    N512M99
    N9999G28X0Z0
    N9991G50X89556Z113000S3000
    N9992M30
    %

  16. #14
    Join Date
    Jul 2013
    Location
    Australia
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    25

    Default

    Quote Originally Posted by BMP View Post
    Ya I'm old still running it on a 486-66 with windows 3.1 lol
    Still works for me all that matters

    I'm sure I will get bashed for my poor programing skills but here is the code

    %
    N100G97G00X50000Z30000T0100S1000
    N101T0101M8
    N102G00X15001Z1000M03
    N103X14001
    N104G01Z-38810F40
    N105G00X14501Z1000
    N106X13501
    N107G01Z-38810
    N108G00X14001Z1000
    N109X13001
    N110G01Z-38810
    N111G00X13501Z1000
    N112X12501
    N113G01Z-37450
    N114G00X13001Z1000
    N115X12001
    N116G01Z-37450
    N117G00X12501Z1000
    N118X11501
    N119G01Z-37450
    N120G00X12001Z1000
    N121X11001
    N122G01Z-37450
    N123G00X11501Z1000
    N124X10501
    N125G01Z-37450
    N126G00X15000Z1000
    N127X11100Z50
    N128G01X-520
    N129X8389
    N130G03X8898Z-55K-360
    N131G01X9939Z-576
    N132G03X10150Z-831I-255K-255
    N133G01Z-37450
    N134X11920
    N135G03X12740Z-37860K-410
    N136G01Z-38810
    N137G00X15000Z1000
    N138X50000Z30000
    N200G97G00X50000Z30000T0300S1300
    N201T0303M08
    N202G00X11000Z0M03
    N203G01X600F30
    N204X8209
    N205G03X8704Z-103K-350
    N206G01X9745Z-623
    N207G03X9950Z-870I-247K-247
    N208G01Z-37490
    N209G02X9970Z-37500I10
    N210G01X11740
    N211G03X12540Z-37900K-400
    N212G01Z-38800
    N213G00X50000Z30000
    N300G97G00X50000Z30000T1100S500
    N301T1111M08
    N302G00X10600Z2000M03
    N303G76X9100Z-9000K500D100E71428A60
    N310G00Z2000
    N311X50000Z30000
    N312M05
    N313G00X50000Z30000T0100M09
    N314M30
    N9999G28X0Z0
    N9991G50X89556Z93000S3000
    N9992M30
    %
    Program 2
    %
    N10M98P100L10
    N11G97G00X70000Z60000T0100
    N12M30
    N100G97G00X50000Z30000T0100S2500
    N101T0101M8
    N102G00X10000Z0M03
    N103G01X-300F40
    N104X7524
    N105X8000Z-238
    N106Z-3150
    N107G00X50000Z30000
    N200G97G00X50000Z30000T0200S2500
    N201T0202M08
    N202G00X0Z1000M03
    N203G01Z-2500F80
    N204G00Z1000
    N205X50000Z30000
    N300G97G00X50000Z30000T0400S2500
    N301T0404M08
    N302G00X6000Z500M03
    N303G01Z0F20
    N304X5582
    N305X5200Z-191
    N306Z-3070
    N307G00X5000Z500
    N308X50000Z30000
    N400G97G00X50000Z30000T0900S2500
    N401T0909M08
    N402G00X9000Z-2500M03
    N403G01X8000F20
    N404Z-2800
    N405X7600Z-3000
    N406X4600
    N407G00X9000
    N408X50000Z30000
    N500G97G00X50000Z30000T1000S2500
    N501T1010M08
    N502G00X0Z-2000M03
    N503M05
    N504M69
    N505G0Z500
    N506M68
    N507G4P200
    N508X50000Z30000
    N509M05
    N510G00X50000Z30000T0100M09
    N511M01
    N512M99
    N9999G28X0Z0
    N9991G50X89556Z113000S3000
    N9992M30
    %
    Sorry neither of these pgms will work.
    1. No G50
    2. Tool offsets need to be canceled eg T0100 Before the next tool is called.
    Otherwise tool offsets are added.
    On a T5 when a tool offset is called and then not cancelled it is added to the the next tool called. And without a G50 all tools would need to be same X & Z value.
    Again.....be Very careful with pgms for a 5T
    Quote Originally Posted by BMP View Post
    Ya I'm old still running it on a 486-66 with windows 3.1 lol
    Still works for me all that matters

    I'm sure I will get bashed for my poor programing skills but here is the code

    %
    N100G97G00X50000Z30000T0100S1000
    N101T0101M8
    N102G00X15001Z1000M03
    N103X14001
    N104G01Z-38810F40
    N105G00X14501Z1000
    N106X13501
    N107G01Z-38810
    N108G00X14001Z1000
    N109X13001
    N110G01Z-38810
    N111G00X13501Z1000
    N112X12501
    N113G01Z-37450
    N114G00X13001Z1000
    N115X12001
    N116G01Z-37450
    N117G00X12501Z1000
    N118X11501
    N119G01Z-37450
    N120G00X12001Z1000
    N121X11001
    N122G01Z-37450
    N123G00X11501Z1000
    N124X10501
    N125G01Z-37450
    N126G00X15000Z1000
    N127X11100Z50
    N128G01X-520
    N129X8389
    N130G03X8898Z-55K-360
    N131G01X9939Z-576
    N132G03X10150Z-831I-255K-255
    N133G01Z-37450
    N134X11920
    N135G03X12740Z-37860K-410
    N136G01Z-38810
    N137G00X15000Z1000
    N138X50000Z30000
    N200G97G00X50000Z30000T0300S1300
    N201T0303M08
    N202G00X11000Z0M03
    N203G01X600F30
    N204X8209
    N205G03X8704Z-103K-350
    N206G01X9745Z-623
    N207G03X9950Z-870I-247K-247
    N208G01Z-37490
    N209G02X9970Z-37500I10
    N210G01X11740
    N211G03X12540Z-37900K-400
    N212G01Z-38800
    N213G00X50000Z30000
    N300G97G00X50000Z30000T1100S500
    N301T1111M08
    N302G00X10600Z2000M03
    N303G76X9100Z-9000K500D100E71428A60
    N310G00Z2000
    N311X50000Z30000
    N312M05
    N313G00X50000Z30000T0100M09
    N314M30
    N9999G28X0Z0
    N9991G50X89556Z93000S3000
    N9992M30
    %
    Program 2
    %
    N10M98P100L10
    N11G97G00X70000Z60000T0100
    N12M30
    N100G97G00X50000Z30000T0100S2500
    N101T0101M8
    N102G00X10000Z0M03
    N103G01X-300F40
    N104X7524
    N105X8000Z-238
    N106Z-3150
    N107G00X50000Z30000
    N200G97G00X50000Z30000T0200S2500
    N201T0202M08
    N202G00X0Z1000M03
    N203G01Z-2500F80
    N204G00Z1000
    N205X50000Z30000
    N300G97G00X50000Z30000T0400S2500
    N301T0404M08
    N302G00X6000Z500M03
    N303G01Z0F20
    N304X5582
    N305X5200Z-191
    N306Z-3070
    N307G00X5000Z500
    N308X50000Z30000
    N400G97G00X50000Z30000T0900S2500
    N401T0909M08
    N402G00X9000Z-2500M03
    N403G01X8000F20
    N404Z-2800
    N405X7600Z-3000
    N406X4600
    N407G00X9000
    N408X50000Z30000
    N500G97G00X50000Z30000T1000S2500
    N501T1010M08
    N502G00X0Z-2000M03
    N503M05
    N504M69
    N505G0Z500
    N506M68
    N507G4P200
    N508X50000Z30000
    N509M05
    N510G00X50000Z30000T0100M09
    N511M01
    N512M99
    N9999G28X0Z0
    N9991G50X89556Z113000S3000
    N9992M30
    %

  17. Likes Garwood liked this post
  18. #15
    Join Date
    Oct 2009
    Location
    Maine
    Posts
    111
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    12

    Default

    Good Morning all,

    Thank you for all the replies. I gotten mixed messages from different people. Some say working with a control this age is just not worth it, but others say there is nothing wrong with the control and as long as you learn to work with it, then it can be quite usable. Maybe not particularly user friendly, but usable. No matter what anyone says I'm still a little giddy to have a real cnc lathe. Probably won't get it moved and under power till late in January.

    BMP, if you have this exact machine with the same control is it likely that the parameters will be the same? The machine has been powered down for about a year so its possible they are gone. I hope not, but we shall see. Not sure how I'm going to proceed if there parameters are gone. Can't really do an inspection without those.

    Oh yeah I was also meaning to ask. I have seen two different sets of specs for the 3ne-300 machines. Some have a higher speed spindle speed (6000RPM I think) with a smaller through bore somewhere around 1.7" diameter and the others have around a 3500RPM max with a 2.0" Spindle. Which one do you have? I am pretty sure that the one I am getting is the higher speed smaller spindle bore model. I think the large spindle model also had 8 stations in the turret vs 12 on the high speed. I cannot confirm these specs though.

    Again thanks for the support and input. Really looking forward to seeing how this turns out.

  19. #16
    Join Date
    Mar 2006
    Location
    Columbus, Ohio
    Posts
    1,115
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    124

    Default

    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.

  20. #17
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by nupress View Post
    Sorry neither of these pgms will work.
    1. No G50
    2. Tool offsets need to be canceled eg T0100 Before the next tool is called.
    Otherwise tool offsets are added.
    On a T5 when a tool offset is called and then not cancelled it is added to the the next tool called. And without a G50 all tools would need to be same X & Z value.
    Again.....be Very careful with pgms for a 5T
    I knew someone would bash my program
    Sorry to say that is a working Program
    G50 is on line N9991 I just use it in the morning to set zero point
    Offsets are canceled when next tool is called N200G97G00X50000Z30000T0300S1300
    Dry run is your friend
    I have had this machine scene 88

  21. #18
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    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.

    Hmm mine uses G96 and G97

    Bad thing only 16 tool offset's

  22. #19
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by wolfenstien View Post
    Good Morning all,

    Thank you for all the replies. I gotten mixed messages from different people. Some say working with a control this age is just not worth it, but others say there is nothing wrong with the control and as long as you learn to work with it, then it can be quite usable. Maybe not particularly user friendly, but usable. No matter what anyone says I'm still a little giddy to have a real cnc lathe. Probably won't get it moved and under power till late in January.

    BMP, if you have this exact machine with the same control is it likely that the parameters will be the same? The machine has been powered down for about a year so its possible they are gone. I hope not, but we shall see. Not sure how I'm going to proceed if there parameters are gone. Can't really do an inspection without those.

    Oh yeah I was also meaning to ask. I have seen two different sets of specs for the 3ne-300 machines. Some have a higher speed spindle speed (6000RPM I think) with a smaller through bore somewhere around 1.7" diameter and the others have around a 3500RPM max with a 2.0" Spindle. Which one do you have? I am pretty sure that the one I am getting is the higher speed smaller spindle bore model. I think the large spindle model also had 8 stations in the turret vs 12 on the high speed. I cannot confirm these specs though.

    Again thanks for the support and input. Really looking forward to seeing how this turns out.
    My 3NE is 4000 rpm. 1 3/8 thru 12 station turret
    4NE is a 3200 gear head 2" thru 12 station turret
    I didn't know they had others
    I have put a spindle in this machine don't remember them asking which one I had.
    Parameters should still be there battery keeps them there
    Mine has 3 AA's for parameters and 3 D's for program
    Change them only with the power ON

  23. #20
    Join Date
    Jan 2013
    Location
    CA
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    17

    Default

    Quote Originally Posted by nupress View Post
    NOTE. If you pull the turret forward or move in Z to change or check tips between parts you MUST manually drive the turret back to the original start position. (Home in X and Z200 from the face of the part.)
    There are many ways you may choose to set as a pgm method but basically you NEED to remember that wherever the tool is when the pgm reads the G50 the machine thinks that is where it is. BIG crashes if you are not diligent with your checking. BTW thes old electronics and DC motors take a few seconds to pull up when you crash so damage is never small.
    Cheers

    This is why I only use G50 to set zero point from machine zeros
    No need to remember where you are at
    I use tool offsets to set from the G50 zero
    My G50 X zero is the distance from machine zero (G28 X0 Z0) and center of boring tool blocks. That number never changes. (unless the encoder is removed for cleaning or replaced)
    G50 on Z changes depending on tool and part length


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
  •