[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.:idea:

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]

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!

[mmc005]

Nate, Thanks for that info, I never knew of a control that used an L for a Radius. I'll keep that in mind.

Scott, Your welcome, glad to help out and maybe keep some of the frustration down on your end. I don't know if you know about Bobcads support forum but it is pretty good too, here is the link. http://www.bobcadsupport.com/forum/index.php

Dave

[NJC]

Dave,
That post processor seems to work ok, I would like to change the R to L though, what software are you using to edit the post, I can't open it?

Scott

[The Engine Guy]

Dave,
That post processor seems to work ok, I would like to change the R to LK though, what software are you using to edit the post, I can't open it?

Scott

Hi Scott

To edit posts go to C:\Program Files\BobCAD-CAM\BobCAD-CAM V22 and look for the icons for "LatheEditPost" amd "MillEditPost", you can either "double click" to launch them or simply right click on each of them and select "Create a Shortcut" and then drag the shortcut to your desktop or quick launch tool bar and open whichever one you want to use whenever!!

Regards
Rob



.

[mmc005]

Scott,
Exactly what Rob said in the post above, that's what I used. When you start the lathe edit post program, on the left side of the screen you will see a post file drop down box, just click the arrow and the find your processor, Okuma OSP5000L.lathepst. Then click the format tab at the top, then in the arc center type section just click the incremental box. Next go to the Prefixes tab and look for arc Z center and arc X center. Change the arc Z center to L and then click the save button at the bottom of the window. That's it, your done. Then in Bobcad just regenerate the code and it should now have the L and K with the center values in them.
Glad it worked ok for you.

Dave

[NJC]

My bad, I meant change the R to L, not LK, the L seems to work perfectly for arcs. Thanks for the info on the post editor guys, I'll let you know how it turns out

Scott

[NJC]

Two more questions, see attached file from post.

1) In the finishing pass area, the tool that I chose was tool #1 in turret position #1, why does it output as tool #2 in turret #2 position, is this a change in the post or a bug in the software?

2) Why does it say rough in the finishing pass area, can I change the post to say finishing?
Scott

[mmc005]

Scott,
Rob might be a better person to answer this question, but I'll give it try.

Question #1-Did you check the tool orientation and mach info tab after you selected tool 1?
**Edit** I tried it on my post and I had to change the tool number and turrent position for each tool I chose.

Question #2-Did you choose rough/finish(looks like you did) when you edited the parameters for the operation?
**Edit** I tried using the rough/finish pass on mine and it output the same thing as yours did, rouging. I don't think this is an editable feature because it pulls it straight from bobcad.

I'll try it on my post and see how it outputs.

Dave

[The Engine Guy]

Two more questions, see attached file from post.

1) In the finishing pass area, the tool that I chose was tool #1 in turret position #1, why does it output as tool #2 in turret #2 position, is this a change in the post or a bug in the software?

2) Why does it say rough in the finishing pass area, can I change the post to say finishing?
Scott

Hi Scott

Can you post the BobCAD file you saved out for the job please??
Easier for me to try things on the original job.

I know some folks don`t like to post actual jobs up on the Forum for all to see so if you prefer to email it to me then send to "rob (at) alroracing . com" and I`ll see what I can do.

I notice you are using the Tool Tip Rad as well, is this a requirement for the job?? Or can you use a Point (0.00 Rad) Tool.

Your Tool output is showing Turret position T01 then Tool Offset 01 and then Tool Tip Rad 01 on the first cut (Rough) = T010101 which is normally correct, however you have T010202 on your second cut (Finish) so you are using the same tool but a different Offset and a different Tool Tip Rad so could be a BIG problem as the machine could go to a completely different coordinate depending on what you have your tool offsets set to in the machine, for example Offset 02 could easily be a 1/2 inch more towards the X0 and/or 1.0 inch more towards the chuck!!
That could get messy!!

Looks like as Dave said you need to go back into the Edit of your Feature and double check and/or re-set the Tool Turret Number, the Tool Offset and the Tool Tip Radius particularly on the Finish tool.

There is an issue in the software where it outputs "Rough" for both rough and finish cuts and I haven`t found a way to fix it yet, may be a way in the Post Processor to get it to output it differently but I haven`t had time to play with your Post yet!!
If it`s a problem for you at the moment then do what I do and that is select a "Rough" only for the Feature cut and set that up as normal on your contour etc and then do another one with a "Finish" only Feature.
It`s a "workaround" and a little extra work but if it will make things clearer/better at the machine for the operator then worth the few extra minutes.

Hope that helps.

Regards
Rob



.