[ArtJ]

I have a 95 LNC8 and am learning to use it. I am modeling and camming parts with Fusion 360. I have the machine running facing and profiling just fine. It wants nothing to do with G17 or any G180-18...... cycles for drilling. It throws an error message 680 alarm B T Rad Comp no spec. I have read you can remove G17 from the program. I have done this before only to have it alarm out for a drilling cycle (G181 X0. Z-0.1022 R0.2 F1.66667). My question is what is happening here? I am brand new to CNC lathe, brand new to Okuma control (OSP 5020L) and I am trying to find a workaround here. Is there a parameter I can change to use G17 and G181 cycles? Is there a software update to this machine control? I am unsure of what this generation of lathe wants for drilling cycles. I would like to be able to drill, peck, deep drill with partial and full retraction. I haven't even gotten to any threading so I have no idea what I am in for there. How do I get there with what I have? Any advise would be very much appreciated.

[rcs60]

I would think the the drill cycle you would be using is G74 since you are on the center of the part

G74X0.Z-2.000 D.312K.150L.312F.005

Okumawiz would have a better answer for you but i think that g181 is optional for M tool (live tooling)

G17, G18,G19 Are listed as optional in my manual and would think that unless you have live tooling you didn't get the options of G17,G19 which would be for milling

[ArtJ]

I really appreciate the response. You are correct. No live tooling. I am a mill guy learning lathe. Machine and control are brand new to me. That is great advise. I need to get into some lathe code and see about had writing some stuff. That will teach me what's what in a situation like this. I am going to look into my post processor and see what's going on there as well. I am using the Okuma turn post from Fusion. I would love to try a different post processor but I am not sure where to find a good one. Any suggestions there would be greatly appreciated as well.

[deadlykitten]

hy art j

... Rad Comp no spec

seems to me, that you machine has not the rad comp option installed; i don't have experience with your model, so i can't really check that error, but i wouldn't consider this error as a dead-end

No live tooling

this means that your machine should not execute G17 nor G19 nor other similar codes , thus rad comp G-code groups should not be active, at least for G18, and G18 should be modal ... forever

so, try a simple rad comp program, that only uses G42 41 40

I have read you can remove G17 from the program

if i may ask, where did you read this ?

Is there a parameter I can change to use G17 and G181 cycles?

G17 and G181 belong to different G-groups : 'rad comp plane' and 'cycles'; in their understanding, you should not co-relate them

I would like to be able to drill, peck, deep drill with partial and full retraction.

all you need is the cycle that delivers full retraction, because it can be modified to deliver all the others, like peck and one-shot drilling; pls find attached pfd; is for a newer machine, but okuma's g-codes are pretty similar, so maybe it will work

I haven't even gotten to any threading so I have no idea what I am in for there

it will be ok, just let's fix the drilling for now, and after that you may move to threading, or whatever else

I am using the Okuma turn post from Fusion

can you modifiy the post ?

My question is what is happening here?

i am also asking this almost every day, so ....kindly

[OkumaWiz]

Rcs60 is spot on. You cannot use live tooling commands on your non-live lathe. You also will not need to change planes at all and it will default to the correct XZ plane on booting. His code looks good to for what you are trying to do.

Unfortunately Okuma deleted some very critical options on the LNC8 in search of a better price. Tool comp, user task 2, color crt ,LAP cycles and more were removed to create the 700 model U control ( as in Undesirable;-)) They can be added even today as a software upgrade. If you decide to go that way get all at once to save big $ over doing them 1 at a time.

You will have fun with the G71 threading cycle. It can do virtually any thread in one line of code.

The control is rock solid with the exception of the fiber optic cables and the machine is deadly accurate if maintained properly. Over 10000 of them were made here in the USA back in the day.

Best regards,

[countryguy828]

I agree with the G74 for drilling. I have the same problem using fusion for drilling I always go and change the G181 to G74 and modify what ever is needed to get it running. I have considered editing the post to do G74 but havn't gotten around to it, too many irons in the fire right now. I don't do much in programming maybe once in 3 months so it just hasn't been important to me. Anyways I don't believe the 5000 series controls to have G181, don't think it showed up until the 7000 series controls.

Perhaps we should compile a list of what all needs changed in the post and get a good one together we can both use.

Here at work I have OSP5000L-G, OSP5020L, and OSP700L. to work with, so potentially it could be beneficial.

Recently I bought a machine for personal use at home that has the U10L in it. I don't have it running yet ... as I said too many other things going on right now.

Dave in Ohio

[deadlykitten]

Perhaps we should compile a list of what all needs changed in the post and get a good one together we can both use

hy cg if changes can be done using replace function, then all you need is to macro a text editor

if also arguments require editing, then it may still be possible

if you wish, share your list of desired changes, and maybe i can help you

it's easier to translate a post output, than configure the post itself / kindly

[ArtJ]

I am getting G180-G191 and also G17 out of the Fusion Okuma turning post processor. From what I am reading from you all I really need to get a post that utilizes G71 and G74. G17 I think should be disabled. The profiling and facing is working great and that is all I have done so far. As I have stated previously,I am as green as it gets with lathe and Okuma control. I just got this machine running. So assume I know nothing. I am learning alot here and I really appreciate you all helping. I am open to suggestions on how to edit the post processor and make any parameter changes on the machine. I am also wondering if there is a software update for this machine and how I would go about check and updating.

[ArtJ]

I was able to find this in the post editor. Not sure what to do there as I have never done this before, but it looks like its set to use 181 and so on for drilling cycles. I kinda feel like I would be poking around in something I shouldnt be without guidance.

[kurmay]

This postprocessor is run only live tooling cycle.
Please try this postproc
https://forums.autodesk.com/autodesk...ning_Mod-1.cps

[deadlykitten]

hy i can't help with the post edit, but i suggest to search on any autodesk forum, like this one : https://www.cnczone.com/forums/autod...st-processors/

out there are many other such forums, but not all of them are 'active', so don't stick too much arround those where you won't receive an answer; considering that fusion is growing fast, you should have more chances to find someone to help with your post editing

about threading, just make your cam to spit code, doesn't matter if it's not compatible with okuma; then, if you wish, create a program that drills a hole and cuts a thread, then share the min file here; i will check it, and see if i can create a small application, that you simply run after you generate the program with your cam, in order to change it to be okuma compatible

there are also other solutions to your issue, like to talk with kurmay, or to wait a bit until i finish my programing application / kindly

[countryguy828]

I was able to find this in the post editor. Not sure what to do there as I have never done this before, but it looks like its set to use 181 and so on for drilling cycles. I kinda feel like I would be poking around in something I shouldnt be without guidance.

ArtJ ...

You are in the right neighborhood, I have looked at it in the past but not actually edited it or tested anything yet. Worst comes to worst ...trial and error make sure there is a backup of the post file. Run in dry mode/machine lock and see if there is any errors, if that works cut air and see if that works, if good that far try it with plastic or aluminum scrap piece.

I'm sorry I can't do anymore at this point, I just have too much of higher priority right now, else I would get it going for you.

Dave in Ohio

[ArtJ]

This postprocessor is run only live tooling cycle.
Please try this postproc
https://forums.autodesk.com/autodesk...ning_Mod-1.cps

This post works with the drilling and is the best woking one I have used so far. I am seeing that I have lost constant surface speed even though I asked for it in the toolpath pre post. And the pecking cycle is not pecking. But I am closer now than I have been so far.

Here is a screen shot of the current code layout from this post processor.

[deadlykitten]

have lost constant surface speed

look better, ccs is still there

[ArtJ]

I see G97. But then it goes to G96 right before the cutting moves which is constant cutting speed on. The spindle stays at one rpm even while diameter changes. Its not keeping constant surface speed. I just ran this program on the lathe and thats what its doing. Pretty stoked though. I am closer to having the recipe dialed in with your help.

[deadlykitten]

ok if you wish to see your lathe delivering ccs, then try g96 s50 instead of your actual values; if ccs is 2 high, then spindle will stay at G50 limit, otherwise will fly-off

random tips :
... when overriding spindle to 90-110%, if it doesn't change your actual rpm, then your rpm is > G50 limit
... sometimes, if you face cut small dia stock in g96 + reposition for od turning, you may loose precious seconds, because rapid is executed faster than spindle deceleration

[ArtJ]

You are right. It is still there. It wasnt changing rpm because it was in low range. I missed the setting of low range to 850 rpm in the post options. That was my mistake. Still getting used to posting lathe code. Here is a pic side by side in visual studio of the code generated by Fusions Okuma post processor and the post processor tweaked by Kurmay. I see the M42 on the first and the M41 on the second. I will remedy this and give it a go again in the morning.

[ArtJ]

I thought there was a user selectable (or identifiable) low range rpm in the post processor settings. It turns out there is not. So there is something in this post that is automatically selecting low range (G41). I am currently working on find the spot in the processor to edit that and then I think I am home free. Once this is all done I am planning on doing a series of videos to help anyone that was in my shoes get going with this machine. Its been a heck of a journey to this point and I want to thank everyone for all the help. Could not have done this without you guys.

[kurmay]

Hi ArtJ

Line1268 in postprocessor file

var spindleRange = (_spindleSpeed <= 1000) ? 41 : 42;

Thats mean is M42 active only if spindle speed bigger than1000rpm.

[Voss_Machine]

He has M41 called...low range rpm is like 1000rpm. He needs M42 to get the max 4200rpm, unless limited by the G50 line.