Separating operations....

[Brent Wilkerson]

Ok lets see if I can explain this....

 

Ok in mill and or lathe lets say you have 3 operations that all use the same tool. Now when you post it calls out for the tools info and set-up like for mill:

 

T1M6

G0G90G55X1.0Y2.0S1500M3

G43H1M8

.....

 

And for lathe:

G00 T0100

G00 T0101 M25

G50 S1500

G96 S800 M03

.....

 

Now the next operation doesn't change tools so neither G0G90G55.. or the G00T0100G00T0101.. is posted again. I understand it doesn't to recall that out, but if you restart the program not on the first operation but like one of the next operations you screwed. You have to find the location and plug the numbers in.

 

What I'm asking I guess is to be able to have operation post without caring what the previous operation and tool that was used. And just output the code as if it was each single/separate operations.

 

I guess just to post the tool header information at the beginning of each operation always, is the easiest way to say it.

 

I hope that makes sense.

 

Thanks

[Jeremy Grigsby Excelsior Marking]

This is what someone replied to me with the same question you need to know the answer to.

 

jeremy,

 

on the first parameters page of an operation there is a button called "NCI path". If you click it a window opens prompting to save the .NCI to a directory with a check box option to 'force tool change'. Checking the box should get you what your looking for.

 

Steve

 

Hope this is what you mean

[Matthew]

http://www.emastercam.com/ubb/ultimatebb.p...t=006138#000003

 

Above is a link to a topic that I think has the answer your are looking for.

[Matthew]

I guess I need to be quicker!

[Jeremy Grigsby Excelsior Marking]

Yes, I beat you on this one.

[McRae]

Brent,

 

I know what you are trying to accomplish and what you are looking for. For each unique operation, you would like a redundant tool call in order to restart the sequence from any point in the operation. This is a post function and will requre a little bit of logic to accomplish this end. In order for the milling machine not to spit out an error, a block skip must be used to run over the tool change or the program would fail. A better solution and one that Dave Thompson has introduced into his Integrex Post is to keep the tool call consolodated at the top of the operation and then to use the goto feature to skip to a specific block section (ie N1220) to continue machining. The operator will need to edit the goto command at the control to choose the proper sequence.

 

The force tool change would be a better solution for a lathe than the milling machine - and this is dependant on the style of tool changer - Turret configuration. I like to use this feature for check passes and then using the 1005/1006 manual entry functions to insert M00's and dimensional check notes to the operator.

 

[ 05-16-2003, 10:09 AM: Message edited by: Andrew McRae ]

[Brent Wilkerson]

I see it now...I didn't even know what to search for there in the forum. After I read "force toolchange" it made sense.

 

We'll have to try to see if our VMC likes calling for a toolchange when the same tool is already in use. Otherwise using GOTO line number makes sense if it will not do it. Then you are only adding minimal line of code.

 

But I lathe programs, I could see where forcing a toolchange could be used. The Okuma we have here has seq. restart which is what they are comparing it too in the toolroom.

 

Thanks for the quick replies!

[McRae]

Some controls might not like to accept a GOTO line so you may need to use a macro call or something similar. IE M98 P1220 or G65 P1220 or similar.

[Brent Wilkerson]

We use macro calls on that controller now, example:

 

IF[#501-#502GE9.0]GOTO1

and

N30IF[#503EQ0]GOTO32

etc.

 

I just never thought of doing that way before. duh

 

Thanks for the info!!