CAM Thread Operation Error 1770002 Help Please 1

[Buckshott00]

Hello All,

I'm using NX 7.5. Windows 32 bit OS XP-Pro I had everything running smoothly, and then I had to add a V-thread to an external diameter of the journal I was working on.

So I added the generation and the simulated path work fine, and the moves list looks good, but when I post process I get:

Error: 1770002
Filename: o:/ugnx751\ip5\src\camsmom\no\ind
mom_td_definitions.c, line number: 503

Error Message: Error recived in do_event. Event Handler: C;\Program Files\UGS\NX 7.5\mach\resource\postprocessor\MS_NL1500Y_turn_master_in.td, Even name: MOM_lathe_thread_move, See

then it just trails off. I'm not sure what to do here. Is there a download to fix UG or does the post need to be altered?

Thanks,

 

[shags72]

Look in the log file in help tab/NX Logfile. Towards the bottom you will see a more complete listing of the error. Then you will have to determine what to do from their.

 

[Buckshott00]

Thanks Shags.

I've now read the log for the error, but I'm no closer to knowing what to do.

Any thoughts?

 

[shags72]

Upload the log file and I will take a look at it and I am sure there are others here who will too.

 

[Buckshott00]

Thanks, I will as soon as I'm back to my work pc!

 

[Arkance/PhoeNX]

The log will make more sense but my guess is that post doesn't like something being output from NX.

Anthony Galante
Senior Support Engineer

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.1.5

 

[Buckshott00]

Yeah Thank you, I think it something it is sending to the post processor or the post processor itself. Because it will verify the thread paths, and it will post process all the other operations, but when I add the thread operation to the rest of the program it doesn't post correctly.

 

[Arkance/PhoeNX]

It may be that the thread milling block is not defined properly in the post. The log will tell a lot more.

Anthony Galante
Senior Support Engineer

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.1.5

 

[Buckshott00]

It's a turning thread operation. I'll be happy to post the log as soon as I'm back to my work pc

 

[Buckshott00]

Here is the log file

 

[Buckshott00]

Whatever it is, it is definitely in the post processor, I changed the:
if {$force_G76_block_once == "0"}
to: MOM_output_literal {$force_G76_block_once == "0"}

I'm attaching the resulting file, maybe someone better with Posts than me (admittedly I'm not very good) could lend me a hand

 

[Arkance/PhoeNX]

Did you create that post?
If that's the case you need to call the variable at the start if the block.

The error in log is as below:

can't read "force_G92_block_once": no such variable
while executing
"if {$force_G92_block_once == "0"} {
set force_G92_block_once "1"
MOM_force once G X Z F

My guess to fix is to add the following lines to the start of the block

global force_G92_block_once
set force_G92_block_once 0


Anthony Galante
Senior Support Engineer

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.1.5

 

[Buckshott00]

Thanks Anthony,

I didn't mean to leave you hanging, but I think I got it working.

I didn't try it your way, but as long as it is working I will be happy to share.

What was odd though was all afternoon I've been getting error files that look like this...

I think my post builder is somehow corrupt.

Thanks everyone for all your help!!!

 

[shags72]

Well just lookin at your log I would guess you info existed it to get it to work and the other issue could be a misuse of some tcl. I had something similar and it ended up being me using ::$var to global variables if I remember the sytax correctly. But what was wierd I had used it before and still had more of the syntax in the same post but in one command it killed it and when you deleted it, I could save. I would send it to gtac to see if they can figure it out.

 

[Buckshott00]

thanks, I'm just going to copy and replace my MACH files and a couple of others with those of a colleague. I think you're right shags there must be a line in there somewhere that's messed up and is wrecking the rest of the posts.

 

[Buckshott00]

In case anyone else has this problem it was these lines that were causing the trouble in the post.


PB_CMD_thread_check custom command from the Rapid Move event

PB_CMD_thread_output custom command from the Lathe Thread event

and an "F" word in the Lathe Thread Event. If anyone needs the post let me know