Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

Broken NX OOTB Fanuc Posts

[ Edited ]

I am trying to configure a post for the two CMS/Fanuc180i 5 axis (dual rotary head) machines at our shop.  I have a few newbie questions-forgive me if the answer is obvious.  And yes, I have seen the tutorials!

 

I tried to start using the sim05 generic Fanuc post, first thing I tried to do was change axis names from from A/C to C/B, but when I go to save it gives me an error.  Hardly seems like I changed enough to mess something up!

I tried again, this time without changing anything and I see the same error; is this broken right out of the box!?

 

Error(s) say:

"PB_CMD_check_block_cycle_plane_change_for_wcs_rotation":

can't read "g68_first_vect(0)":no such variable while executing "set dpp_ge(g68_first_vec,$i)"....blah blah blah

AND

"PB_CMD_check_block_output_rotary_before":

can't read "g68_first_vect(0)":no such variable while executing "set dpp_ge(g68_first_vec,$i)"....blah blah blah

This is a little intimidating; PB itself is not very intuitive for me, and the tutorials don't really cover debugging...Any ideas where to start?

 

I'm also wondering if is it typical to create a post for use with Machine Code Simulation and a different one for actual output?  When I try to run the MCS it gives me errors when it doesn't see G43 and/or hits G43.4.  It sounds like using the Machine Configurator you can change Gcodes, do I need to use this to modify G43?  I am having trouble getting the MC to run as well, go figure...

 

One other thing, while running MCS I get to an in process tool change I get a "command 'grasp' called with invalid argument" error, this is using the sim01 toolchange.prg file slightly modified to drive the X axis rather than spin the umbrella C axis.

It works fine when it first goes to grab a tool (empty spindle), it errors out when it gets to the point that it should release the tool, before it goes to get the next one.

EDIT:  Fixed this one!  I replaced the entire sim01 release IF statement with the one from the sim05 that actually says 'release' in it instead of 'grasp'

 

Again, sorry if these are silly questions.  If I could take a PB course I would, but I don't think it in the cards!

 

Attached are the error messages, and just FYI I am using NX/PB ver9.0, and will update to 9.0.3 tomorrow, so maybe this will fix everything!

29 REPLIES

Re: Broken NX OOTB Fanuc Posts

hi ,

 

I have a solution to this problem:-

 

Error(s) say:

"PB_CMD_check_block_cycle_plane_change_for_wcs_rot​ation":

can't read "g68_first_vect(0)":no such variable while executing "set dpp_ge

Can you remove

 

--first copy the post process files to any other folder.

--remove the vnc.tcl file as height in the attachment(PFA)

--now open the post and change the axis and save .It will work.

--Also if you need only post processor file then uncheck the option in post(mentioned in attachment 1.png).

 

Re: Broken NX OOTB Fanuc Posts

[ Edited ]

I updated to 9.0.3 yesterday and saw that the sim05 fanuc template had been updated, so one of those things seems to have resolved my post builder saving issue!

 

I also found that I can change the length compensation G-Code to G43.4 and the MCS seems to read it fine (the first time at least).  Was this the correct way to do this, or is it just a fluke?

I ask because I noticed that the second tool it uses only get a G43 despite changing the above setting.  In both my first and initial move I included a block "G00 G43.4 H01 S M03" witch force output on, but the second tool change gives me "G00 G43 Hxx Sxxxxx M03"

In this particular example it also goes and does a G68.2 move and then throws out a bunch of other errors which is odd because there is no plane or WCS change...

Everything in post builder is so cryptic, I sincerely doubt that a couple hour training course would be enough to make me competent with this...

 

I also have another issue with the tool change CSE subprogram.  It places Tn in the correct pocket,  shifts over to grab Tn+1, and goes off to cut just fine, but when the tool magazine retracts Tn stays in space where it was unclamped.  Its not a 'real' problem, just annoying to see a big tool floating in space.

 

I have a feeling I know the answer to this... but is it possible to post a toolpath, edit that posted code, and then feed it back into the Machine Code Simulation?  Just in case we have issues with the head angle or a retract that just wont cooperate and we have to hand edit the post, or we do some 100% handwritten programs.

EDIT: Yes this is possible via Tools->Simulate Machine Code File

Re: Broken NX OOTB Fanuc Posts

Don't everyone reply all at once! By myself, talking to myself

I fixed the toolchanger issue, used the grasp command from sim01, except it only works with 0-9 tools, so I nested another if statement inside of it and removed the 0 from "pocket_0" for tools 10+.

I also am pretty sure that the G68 was being generated from somewhere in Op Start->First Move, so I removed a lot of the junk that I didn't recognize as being absolutely necessary and now the G68 IJKR G69 are gone!

Except it still calls out G43, NOT G43.4 Robot Mad

Can someone PLEASE provide some insight?  I'm starting to pull my hair out!

Re: Broken NX OOTB Fanuc Posts

[ Edited ]

Not much to add. I have worked on this configuration a few times (dual head rotary) but didn't rely on OTB code much - so I don't know what is there in the sim kits (in the posts) - let alone what is changing between versions. It makes sense to use them though (like you are) for the ISV and for the latest coding that they do in posts. I have generally lied to NX about the kinematic (prefer TT) because it has been difficult to get 3+2 circle output otherwise - but that is a more complicated post project.For 5 axis - I would switch to HH. My experience has been more prismatic application. Anyway - I assume the questions you have are directed to Siemens (expectations for OTB code.)

NX10.03
Windows 7 Pro

Re: Broken NX OOTB Fanuc Posts

Most of the parts we run are large 'organic' shapes like wind turbine blades, and aside from roughing the programmers stick to full 5-axis motions.  

I think I managed to resolve all of my major issues, though it is far from perfect.  Considering it was a Fanuc post and we have Fanuc controllers, and that Siemens said the OOTB posts were ready to run, it took a lot more effort than I had expected.

 

I know they want people to pay for training, but I think more documentation beyond a couple 10 minute long videos would go a long way in helping people prepare for the training courses, or decide if its even worth while. 

Re: Broken NX OOTB Fanuc Posts

You can just open the post (with VNC) in PB, then uncheck the VNC toggle; the VNC file will be removed.

Re: Broken NX OOTB Fanuc Posts

Thats a good workaround to know.  Fortunately after applying the update to 9.0.3 whatever bug that was has been fixed so that was resolved without having to disable the VNC.

Re: Broken NX OOTB Fanuc Posts

[ Edited ]

Just when I thought I was done...one last problem is popping up.  I have programmed a helical approach into a cavity milling operation, but I only want it to output XYZ moves, no IJK.

Just as a wild guess I tried removing the entire block of code, it ignores the helix and and just does a plunge move.  Since that didn't work I tried replacing the helix move codes with the same values in linear, but then I get an error:

 

"
Event: MOM_helix_move
Error Info: Error code 1745007: MOM given an invalid expression in a block template; MOM: Invalid address expression: $mom_cutcom_adjust_register
while executing
"MOM_do_template helix_move"
(procedure "MOM_helix_move" line 5)
invoked from within
"MOM_helix_move"
Error Code: NONE

"

 

EDIT:

Resolved through changing PB_CMD_init_helix "set mom_kin_helical_arc_output_mode LINEAR"

And I have the same code blocks in helical moves as I do in linear.

Re: Broken NX OOTB Fanuc Posts

[ Edited ]

evanser89 -

 

You would not get such an error if the D word in the Block has been set to "Optional" (with a little red "o" symbol at the upper-right corner). However, if the helix move is your first engage move where CUTCOM needs to be turned on along the way, you will want make sure the tool change has occurred already; and mom_cutcom_adjust_register should have been set.

Learn online





Solution Information