New to the Okuma lathe with a U10l control

Hey Everyone I'm in need of desperate help here. I'm very new to CNC lathes I have ran mills my whole career. We recently have purchased a used Okuma Crown with the U10L control I have been able to navigate around the machine relatively easy but when it comes to putting in the program i have had a bit of trouble. I used Fusion 360 to make a simple turn two diameters to get used to the machine I used the Okuma Lathe post and it generated the program after getting the program into the actual machine I have had errors most which have been an easy fix but i have one line that keeps sending an alarm.The alarm is( Alarm 2366 Tool Radius Comp. No spec) the code line that this happens on reads (G90 G18 G3 x2.4992 z-1.5264 k-0.0312).Can anyone help me with this also if anyone has a sample program that they would share with me that runs on the U10L control so I can compare it to what I have to see where I am off. Like I said i am very new to the CNC lathe so any help with this is appreciated .
Thanks

hello

I am also new to okuma u10 L here in the uk ( wales)

MAYBE YOU NEED TO WRITE THE VALUE OF THE RAD eg z- k- r.8) not sure if this will work.

do you have a copy of the post processor for this control as I only use fanuc at present

WORKING WITH EDGECAM ALSO

thanks

tomo1 (peter)

I do have a copy of this post for fusion 360 i have still yet to fully proof the program out to see if the post is correct

Most okumas have to be told what tool nose radius your using and which direction its pointing, do have those options to put in?

I have this information but like i said extremely new to the lathe where would i put this information

on the ones i have run, it is one the same page as the tool offsets. no manuals?

No we didn't receive any manuals with the machine which makes this whole process even more fun as it seems like any time you search for something online Okuma keeps everything under tight wraps are you talking about where you enter the offsets for the machine in the next two columns is where you put the tool radius info in

newton11n:
this was shared here a while back as a resource: Answers and Information - Hartwig, Inc.
there are some pretty useful items on there. Some are "newer" and won't really assist you, but most things, other than the screens you see, are the same.

Okuma is different, however, i've never heard them described as "tight lipped" about their information. I'd suggest contacting your local distributor. Probably Gosiger, Hartwig or Morris companies. Call and ask for someone in applications and ask them to send you copies of the manuals for a U10L. I cannot imagine they would say no or turn you down.

The company linked above has contact info listed and you should be able to get routed to someone who can give whatever manuals you want.

Second:
Try simply deleting the G18 command. Sometimes Okuma is a bit weird about commanding a code that cannot be anything other than what you're commanding.
IE: If you have a twin turret lathe, you start with G13/14 on the first line. Period. Program won't run until it knows which turret to move. Even if you only use G13 and program one turret, you can take that program out of the machine, to a single turret machine, load it, and try to run it, but as soon as it sees the G13 it alarms saying "I don't have 2 turrets, why are you trying to tell me which one to use?" basically. Delete the G13 in this instance, the program runs without flaw.

Third: That alarm specifically states that the machine doesn't have tool nose radius compensation. However, i find that hard to believe on a USA spec machine. Were there any programs left in the machine? I'd refer to those if so.

Fourth: You will not be using: R.1 in a lathe. To command a radius, you use either I/K commands or L. Use L the same way you would use an R command.

Last: Yes, the page in question is the tool data page. The first two columns are for the X/Z offsets. The Second two are the X/Z radius vales. The 5th is a P value. In short, use a 3 for an OD turning tool, or a 2 for an ID turning tool. There are some rules that would mean you only need to put a positive/negative value in the second set of numbers and so forth, however, if you use the P value and numbers in the X/Z radius columns it will always work, however, that is not the case when not using the P values but using G41/42.

Good luck.

Ok I spoke with the People at Great Lakes and they were able to get me what few manuals they had for the machine. They are supposed to be sending them over to me today so hopefully I will be able to get back on the machine tomorrow to try to continue working out the bugs. As far as any programs that were left in the machine no such luck they are all gone . Thanks for the help so far and I will keep you all posted as to how it goes

They community here is pretty helpful and supportive; as much as any internet forum anyway.
Probably above average.
Keep asking questions and someone will give you an answer...

I agree with Teahole that the alarm states that nose comp is not on the machine. Take out the G41/42/40 commands and program without comp by the machine (use the cad to calculate) and it should work. Okuma made the bad decision on the model U controls to not make comp standard, so there is a possibility that the option was not added. Crowns and Cadets had those controls. If you check the Management Data Card located in the electrical cabinet of the machine (hopefully) it will show if the nose comp spec is active.

Best regards,

Ok I was able to run off the last part after adjusting that line of code the rest of the part ran off flawlessly I have since ran a few facing programs with no issues when I went to try running a threading program the machine throws an Error at this line of code G32 z-1.2431 F0.07874 does anyone have an idea why this might do this
I will add text of the whole program that Fusion has generated using the Okuma post

%
(01156.MIN)
N10 G50 S2000
N11 G0 X400.
N12 G0 Z400.
(THREAD1)
N13 T020202
N14 M8
N15 G94
N16 G97 S500 M3 M41
N17 G0 X2.8 Z0.1969
N18 G0 Z0.3181
N19 G1 X1.9496 F39.3701
N20 G32 Z-1.2431 F0.07874
N21 X2.065 Z-1.3009 F0.07874
N22 G0 X2.8
N23 Z0.3181
N24 G1 X1.9311 F39.3701
N25 G32 Z-1.2339 F0.07874
N26 X2.065 Z-1.3009 F0.07874
N27 G0 X2.8
N28 Z0.3181
N29 G1 X1.9168 F39.3701
N30 G32 Z-1.2268 F0.07874
N31 X2.065 Z-1.3009 F0.07874
N32 G0 X2.8
N33 Z0.3181
N34 G1 X1.9049 F39.3701
N35 G32 Z-1.2208 F0.07874
N36 X2.065 Z-1.3009 F0.07874
N37 G0 X2.8
N38 Z0.3181
N39 G1 X1.8943 F39.3701
N40 G32 Z-1.2155 F0.07874
N41 X2.065 Z-1.3009 F0.07874
N42 G0 X2.8
N43 Z0.3181
N44 G1 X1.8943 F39.3701
N45 G32 Z-1.2155 F0.07874
N46 X2.065 Z-1.3009 F0.07874
N47 G0 X2.8
N48 Z0.1969
N49 M9
N50 G90 G0 X400. Z400.
N51 M2
%

Quote:

---

Originally Posted by newton11n

Error at this line of code G32 z-1.2431 F0.07874

---

try F0.0787 ? maybe too many decimals ... i am not sure

0.00004inch > 0.001mm ... hmm

yup, use F0.0787, or use F=7874/100000 :)

Three things. First change the G32 to a G33.
Second it is not a good idea to use G1 with a fast feed rather than a G00. This will screw up your load monitoring if you use it in the future and is much harder on the drives.
Third always post what alarm you are getting and the description so we can better troubleshoot the problem. The Okuma is very detailed and specific in its alarms. (Sometimes with Jinglish though).

Best regards,

Quote:

---

Originally Posted by OkumaWiz

it is not a good idea to use G1 with a fast feed rather than a G00 ... is much harder on the drives

---

hello mr Wizard :) please why "much harder on the drives" ?

... and was there a time when a dual-turret lathe was more affordable ? i dont know the history for such prices, and i started recently to think about an LT2000 ... but i can see that there are few posts about such new lathes, and more about old lathes with 2 turrest ... something tells me that newer ones are too expensive, or something

kindly !

about "harder on the drives", my only guess is that trapezoidal_diagrams are executed more easy at high feeds, compared to round_corners_diagrams

i think that the control struggles to execute those round_corners with increased accuracy, and this is hard, because diff increases at higher feeds

on a trapezoidal_diagram, a sharp corner is executed faster, and i also think / guess that during the linear palier diff is allowed to have more deviations

thus the linear movement may be more accurate during G01 than during G00 :)

... but this is my opinion on it, and i would really apreciate opinions / critics :)

ok I tried to shorten up the f0.07874 to 0.0787 it still throws the same alarm the alarm reads 2250 Alarm Data word 'x','z' anyone know what this means

it may mean that both x&z are required :)

try this :

N20 G32 X1.9496 Z-1.2431 F0.07874

and this

N20 G32 X1.9496 Z-1.2431 F0.0787

Ok I tried this although it did not produce an error it did not cut threads either it basically acted like a turning program

here is my threading program.

(OD THREAD)
NOTHD
T121212(CARBOLOY .33 WIDE INSERT)
G97S1000M3
G0X1.273Z-3.112M8
G71X1.1048Z-4.0015B60.D.003U.001H.064F1/18
G0X1.273M9
X100Z100
M1