Changing line number increment in post.

[RandleXX]

How do I change the default starting line number from "N100" to "N1" and the increments settings in the MPOKUMA post? I found the Max line number setting but no starting number or increment amount.

Thank You.

Randle

[Guest CNC Apps Guy 1]

Screen, Configure, NC Settings...

[Christian Raebild]

If you want to hardcode them in the post, instead of setting the defaults as James describe, then you need to set the following variables at the top of the pheader postblock:

 

seqno and n : starting line number

seqinc : line number increment

 

If you set those variables earlier than the pheader postblock, then they will be overwritten with the values from the NCI file, and if you set them later, then you will already have output line numbers, which means your line numbers will be messed up.

[RandleXX]

Thanks. I am going with the hardcode method for a machine specific DNC type post for large drip feed surfacing programs with line numbers from N1 to N10000+.

Randle

[Jim at Gentex]

Question:

 

Why use line numbers at all if drip feeding?

 

They only make the nc file bigger. I always strip the line numbers in Cimco edit before sending the file, and it seems to run smoother without all that extra information. Just a suggestion...

 

*************************************************

Jim teh been there done that CNC programmer.

[Brendan P]

I have all my posts set up to post one line number for each tool and that's it.

I personally cant stand having all those N#'s.

The guys have never complained,and if for any reason they need to skip down to a certain line number,it takes 2 seconds to throw one in where you need it.

 

 

Just my personal preference.

[RandleXX]

When drip feeding with our Okuma DNC-B an operator cannot start in the middle of a program he must start from the beginning, so if he bails out in the middle, he needs to know which line number to edit the program from on the host PC. Drip feeding memory size is only limited by the host pc so huge programs are no problem.

Randle

[richardtraver]

without changing the post you can set the increment in the tool parmeters to start with this number and go up by that number. look on the page where you set your speeds and feeds for the tool. the max however will still be set by your post parameters

[Jim at Gentex]

I see, Randle. Thanks. I didn't understand what you meant at first.

 

I drip feed large surface files to my 2 Fadals too, but if I need to abort a program in the middle, I usually just start over from the beginning if it's not too far along, or I will rotate the program 180 degrees to start from the opposite end and overlap where the aborted program left off.

 

I noticed that if I run the nc file without the line numbers, it runs smoother because the controller has less incoming information to process. My controllers are more than 10 years old and have a max baud rate of 9600, so they can only process the data at that speed. Knowing this, I try to make my nc files as lean as possible so I don't get any choppiness in the program caused by the buffer trying to keep up.