end of nc sequence

[pesau-2]

Dear all ,

At end of Sequence I require following command "G0G80G90Z100.0M05M09" , Currently for every sequence I add CL command  INSERT/G0G80G90Z100.0M05M09.

Can this be done in post processor , like how we add for start and end program using "Start/End of Program".

Can you please suggest best method to handle the End of Nc sequence

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[KenFarley]

By "at end of sequence" do you mean "at next tool change"?

I'd start by looking at all the options available in the NC Post Processor Java application. If you don't find anything there that addresses your specific needs, you will need to delve into the FIL code world to handle the outputting of your NC code.

[pesau-2]

I am trapping the spindle stop and writing the end sequence using the FIL code is there any other simple method to capture the END OF SEQUENCE.

[KenFarley · Accepted solution]

So, I guess the answer to my question is that you are actually trying to output some special code at the next tool change. The reason I asked is because in the manufacturing module, a "sequence" is one particular defined set of motions. I could have a number of consecutive sequences right after each other, like "cut outside shape", then "cut inside shape", etc. which use the same tool. In the generated CL code, I won't see a SPINDL / OFF until the second "sequence" is done.

For what you are doing, it seems like responding to the "SPINDL / OFF"  via

CIMFIL/ ON, SPINDL

...

(check if it's an "off" command, process as usual otherwise)

...

CIMFIL/ OFF

is the way to go. It's far better than having to add CL Commands to your sequences to take care of it, because those tend to be something I'd forget, eventually.

[joshuataylor]

If you are just inserting code at the tool change you can do that through the Option File Generator.  Applications tab ->NC Post Processor->Machine Codes ->Tool Change Sequence-> User Blocks tab. Try it and see if it inserts them where you want, otherwise you get to play with FIL.

Josh

[pesau-2]

thank you all for your valuable input