Need Help!- v22 won't post correctly to Okuma OSP 5000L

[NJC]

I have an Okuma LB-15 with an OSP 5000L. I can send programs too and from the PC, but can't get Bobcad to post a toolpath that will work correctly. The program will transfer and I can edit it, but when I try to dry run it, it comes up with a 425 B alarm- unusable gcode. Does anybody have a post for this that works well? I don't know g-code so I'm a little in the dark with this, I just want to be able to generate a toolpath and cut parts.

Thanks,
Scott

[mmc005]

Do you have a working program with the same g-code that your trying to use now? Can you post it? I'm sure it's just a few minor problems with the processor that we can probably fix. Which post processor are you using to generate the code?
Dave

[harley4ever]

It's simple. If it dont work then spend more and upgrade to 23.

[NJC]

harley4ever, I could do without the neg comments, I'm trying to get a problem resolved.

Dave, I'm using the post for a 5000L that I downloaded off of bobcadsupport.

I have attached 2 programs, 1st one is how it was generated by bobcad, second one is after I modified it.

I found that if I edit out the first line and just put a % instead of the all of the other crap that was there it will load into the machine.

I was coming up with an alarm for unusable g-code in line #N01- I deleted the whole line, not sure if I needed it, but the alarm is gone

Now the only problem is on line # N12, alarm #452- data word Arc Cal., not sure what this meens, I tried changing a few things without any luck

Any thoughts?

Thanks,
Scott

[The Engine Guy]

Originally Posted by NJC harley4ever, I could do without the neg comments, I'm trying to get a problem resolved. Dave, I'm using the post for a 5000L that I downloaded off of bobcadsupport. I have attached 2 programs, 1st one is how it was generated by bobcad, second one is after I modified it. I found that if I edit out the first line and just put a % instead of the all of the other crap that was there it will load into the machine. I was coming up with an alarm for unusable g-code in line #N01- I deleted the whole line, not sure if I needed it, but the alarm is gone Now the only problem is on line # N12, alarm #452- data word Arc Cal., not sure what this meens, I tried changing a few things without any luck Any thoughts? Thanks, Scott

Hi Scott

Dave is right, probably won`t take a lot to "tweak" your Post Processor, if you have a running program for the machine or even a list of the "G" codes assigned to the machine control from the Manual if you have one I reckon it won`t take long to get you running right.

Regards
Rob

.

[mmc005]

Scott,
I downloaded your files and I will download the post off Bobcad later tonight and maybe we can get you a post that will work for morning. Unless someone else can get to it first, that is.
Dave

[mmc005]

Scott,
I can't find the 5000L post processor on the bobcad site, can you post it here or email it to me?

Thanks,
Dave


**Edit**
Nevermind, I found it, under lathe. I thought it was a Mill.

[mmc005]

Scott,
Line 12 didn't work in either of the programs that you posted? Do you have a program using the G03 or G02 command that you can upload? Do you have the manual for the control, it will tell you what the alarm means. My bet is that it might need an "R" with a radius size and not the I and K positions.
Dave

[mmc005]

Scott,
Try this post, I took out the header info that was causing you a problem when sending to the control, I also changed the I and K to R. Use this new post for the same program file and then try to send it to the machine. Then see if the machine still gives you the same alarm code. Let me know if it works for you.

Dave

[The Engine Guy]

.

Hi Scott

My 2 cents worth, some pics of Post Editing that may help you do this yourself.

I think this is probably what Dave has done for you.

Regards
Rob

.

[nlh]

Hey guys,

Don't bother with I,J,K with this control, unless of course you want to. In the post editor change it to output an L instead of an R value. For some reason this control uses the L for radius.

Hope this helps.

Nate

[NJC]

Yep, you guys are right on!!

I looked through a list of g-code for this machine this morning and also came to the conclusion to use an L instead of I and K, I just put in L.25 and whalla, worked great.

Dave, thanks for helping out with the post, I'll try it in the morning and let you know how I make out.

Rob, thanks, maybe I can tweak the post that Dave started for me.

Nate, worked perfectly!

I really appreciate all of the help, the information on this site is incredible and of course the individuals that share it absolutely rock, Thanks!