428 Alarm-B

Hello,

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

https://www.cnczone.com/forums/attac...d=426906&stc=1

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?

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

---

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!!!!

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 :)

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

Best regards,

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!!

Quote:

---

Originally Posted by OkumaWiz

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

Quote:

---

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

Quote:

---

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 :)

Quote:

---

Originally Posted by Beefheart

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,

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

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

Quote:

---

Originally Posted by deadlykitten

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?

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

Quote:

---

Originally Posted by deadlykitten

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

---

Yes it was typing error, I have made the last programs without CAM and its working fine.

Thanks