428 Alarm-B


Results 1 to 12 of 12

Thread: 428 Alarm-B

  1. #1
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default 428 Alarm-B

    Hello,

    I was trying to program a very simple part using this program on my Okuma LB 15 OSB 3000.

    428 Alarm-B-ohno-jpg

    N10 G00X600.
    N20 g00 Z600.
    N25 G50 S2000
    N30 G96 S120 T0101 M03 M42
    N40 Z97.
    N50 X42.
    N60 G01 X-1.6
    N70 Z98.
    N80 G00 X40. Z99.
    N90 G85 N100 D4. U1. F0.25
    N100 G81
    N110 G01 X0.0 Z97. F0.15
    N120 G03 X40. Z77. K-20
    N130 G01 Z74.
    N140 X42.
    N150 G00 X600
    N180 Z600
    N190 M2

    I get alarm 428-B after N70 is executed, when i read in the manual the alarm means that a "=" is used wrong or a "=" is missing. I'm a Cam guy, and I don't have very much experience typing code on lathes, After two hours changing things in the program and reading manuals I used fusion to make the part. I had a fine cut from the beginning added in the end of the program. What is wrong in my program?

    Similar Threads:
    Attached Thumbnails Attached Thumbnails 428 Alarm-B-ohno-jpg  


  2. #2
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2809
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    hi, pls share tools nose radius; at first glance, without testing, i can say this :
    ... N60 G01 : requies to have a feed value specified ( eq F0.12 G95 )
    ... if you use U1, then try also U1 W0.5, so to leave finish stock on both axis
    ... g80, g42g40 : missing
    ... you cut the face at z97, then you begin the roughing at z99;try to avoid the face cut, and do only the roughing
    ... going from x40(n120) to x42(n140), with U1(n90) requires a radius <0.5, or machine will move towards x- instead of towards x+, during a finish cycle
    ... your program is created for nose rad 0.8 ( N60 G01 X-1.6 )

    your actual cam settings are 'out-of-this-world' ; program should be similar to this / kindly
    Code:
        G50 S2000
        G00 X600 Z600
        NAT01
        G96 S120 M42 M03 M08 G95
        G00 X44 Z99 T010101
        G85 N01 D4 U1 W0.5 F0.25
        N01 G81
        G00 X 0 Z99
        G01 X 0 Z97 G42
        G03 X40 Z77 K-20
        G01     Z74
        G01 X44
        G40
        G80
        M05 M09
        G00 X600 Z600 T0100
        M02


    Last edited by deadlykitten; 09-09-2019 at 01:26 AM.
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


  3. #3
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    Thanks! I tried using G42 and of course G40 but I deleted it to see If it caused any trouble. I will try your program first thing in the morning.

    Thank you very much for helping!!!!



  4. #4
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2809
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    hi, if you intend to eliminate the face-cut operation, then, instead of roughing towards z-( rough od g85 g81 ), try roughing towards x- ( rough od face g85 g82 ); otherwise, if you keep the rough od, be aware that positioning is at z99, and shape begins at z97, thus stock should be <2-0.8mm on z; changing to roughing towards x-, may run on z stock >2mm, because positioning is always above the max diameter

    this is g-code, and you are a cam guy yesterday i checked our previous conversation, and since you work on a cam most of the time (esprit - mori), why don't you try to find an okuma post ? kindly

    Last edited by deadlykitten; 09-09-2019 at 08:54 AM.
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


  5. #5
    Member OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1121
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    I agree with kitty. Your G80 is missing and that is causing your alarm.
    Add it on N145.

    Best regards,

    Experience is what you get just after you needed it.


  6. #6
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    Hi Kitten, I got two jobs. At the company where I'm employed we got a Mori Seiki NTX and Esprit and the license is locked to the machine, Esprit was included when we bought the machine. Besides this I'm working on my own business, I got a HAAS VF-0E and the Okuma. If you got a Haas there is a nice deal on Esprit licenses, they are very cheap to buy and only the simplest functions are activated and they check your machine number. I bought a license and when I checked how much it would cost to lock up the lathe module and convert it to normal license to use it on my Okuma the cost was much higher then I paid for the lathe. I have done some 3D milling in the Haas and my Esprit don't have those functions so I have used Fusion 360 for a while and I think it is a very good Cad/Cam but I don't like it when it comes to the Lathe cam module and that's why I want to learn typing code on simple parts.

    I tried your program without any part in the machine and it worked, but why makes the machine rapid movements in x and z toward the chuck after each cut before it moves back in z to the start point before next cut? Thanks for your engagement!!



  7. #7
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by OkumaWiz View Post
    I agree with kitty. Your G80 is missing and that is causing your alarm.
    Add it on N145.

    Best regards,
    Sorry, I missed the G80 when I wrote the post, i was in the program. Next timme I will transfer the program to my computer so I can post the file. Thanks for your comment



  8. #8
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2809
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    why makes the machine rapid movements in x and z toward the chuck after each cut before it moves back in z to the start point before next cut?
    hi beefheart, here it seems ok, rapids are not toward the chuck; pls check attached image; tool is r0.8P3

    I bought a license
    your lathe does not have igf ?

    there are free cams, also those for which you have to pay, and there is the 3rd option

    Attached Thumbnails Attached Thumbnails 428 Alarm-B-untitled-png  
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


  9. #9
    Member OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1121
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    Quote Originally Posted by Beefheart View Post
    Sorry, I missed the G80 when I wrote the post, i was in the program. Next timme I will transfer the program to my computer so I can post the file. Thanks for your comment
    It is always better to transfer since typo's can frequently happen...that makes me wonder now if what you are seeing is a typo such as GO vs G0 and you are getting the infamous "equal is not exist" alarm...

    The alarm book I have handy doesn't show the 428 alarm. Is it the old green screen OSP 3000 that you have?

    Best regards,

    Experience is what you get just after you needed it.


  10. #10
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    Its color screen, Alarm 428 says "=" error, missing or miss placed.

    It's a 5000, My mistake in the first post

    Last edited by Beefheart; 09-10-2019 at 11:26 PM. Reason: more information


  11. #11
    Member Beefheart's Avatar
    Join Date
    Jul 2016
    Location
    Sweden
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    Quote Originally Posted by deadlykitten View Post
    hi beefheart, here it seems ok, rapids are not toward the chuck; pls check attached image; tool is r0.8P3



    your lathe does not have igf ?

    there are free cams, also those for which you have to pay, and there is the 3rd option

    I will run the program again and check so I didn't misunderstood the movements.

    igf? this lathe is new for me and I haven't read all the manuals yet. I have made some jobs in it programmed in Fusion.

    Can you recommend any cam which have a post processor that will work that not cost a fortune.

    Huuuum 3rd option?



  12. #12
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2809
    Downloads
    0
    Uploads
    0

    Default Re: 428 Alarm-B

    hy beefheart, did you somehow find out why the rapids were towards the chuck ? kindly

    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


Tags for this Thread

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

428 Alarm-B

428 Alarm-B

428 Alarm-B