how to post process with incremental O/P

[buddhika]

Hello,

can any one tell me how to post process (or create CNC tool path) to get a incremental (G91) part program out put.
thanks.
Buddhika

 

[cncwhiz]

Buddhika,


Why would you want to do that? This is "BAD" practice and also a PIA to read the program. Are you sure that you want to post the whole program or only some commands in incr?

 

[buddhika]

cncwhiz,
Because I'm slightly changing tool paths in machine it self for some simple jobs. It is easy to make small change in CNC machine and reuse same program than generating whole thing in PRO/E and then transfer it again in to CNC controler.
Anyway thanks for u'r reply. Can u tell me how to generate programs in incremental mode.

Buddhika

 

[dbrainsky]

I am not sure why you would want to do this but Gpost can be setup to output G91 mode automatically. In fil file add MODE/INCR,ON at the end of the MACHIN section.


Ora better way to use incremetal mode is to add the apt words MODE/INCR,ON at the beginning of your proman session. from the menu manager


MACHINING / CL COMMAND / Create / Beginning / Keyboard


type in mode/incr,on


This will add the command to your cldata and the post will now output in G91 mode. Just be careful thatthe post does not switch backto G90 mode at yourtool changes.

 

[marker4x4]

...ora better way to use incremetal mode is to
add the apt words MODE/INCR,ON at the beginning of your proman session.
from the menu manager


MACHINING / CL COMMAND / Create / Beginning / Keyboard


type in mode/incr,on

That's a good one indeed; if I may add someting to it - you can also
insert this CL command in any of your sequences before the cut (turn
G91 ON) and then another one after " mode/incr,off " to turn G91 OFF.

 

[cncwhiz]

I still see this as bad practice. You might as well program by hand. Anytime you use incremental moves you put the machine, part and operator in harms way. If you are editing cl then you also make the whole idea of pro e/ pro man not work as it should be.

 

[ncprog]

Good input on this one!!!


I'm a firm believer in absolute code programming if at all possible, but there are some cases where incremental programming has its benefits. We have a large variety of machine tools in our shop, most programs are absolute from center rotation of pallet (mills x and z) and top of pallet for y. Some are absolute using G92 or G50 coordinate shift. Our laser nest (which mainly is a deleted program when finished) does absolute positioning from part to part and incrementally cuts part using subroutine. Many instances of one partin a nest cut in absolute mode would be a very large program and hard to follow.


View attachment 1332


Another case is multiple instances of intricate geometryusing hard to cut material on a mill where there will be constant editing at the controller until the process is proven out. Usingone subroutine with incrementalcuts allowyou to make fast and easy changes at the controller (depth of cut, chip load, spring passes, etc). Most of these when finished can then be changed in the software back to absolute mode with a final verification inspection.


Yet another case I had was surface milling on a Y-axis lathe. Surface milling takes a lot of code depending on finish requirements (cusp height). The controller didn't have enough memory to hold program of desired result. Lucky the part was symetrical so we broke it down to incrementally cut subroutines to get program size to fit in the machine. (upgrade to more memory on some controllers is ridiculouslly priced base on ROI)


So depending upon manufacturing requirements of the facility, job shop, or even a one time run on a CNC wood router, incremental cuts are avalible on every controller that I've used and can be used to benifit the need of the job at hand.


P.S. We recently switched to Pro/MAN and have a contracted source doing our laser post processor which has the requirements above (plus a few extra). Have not received the post yet, so I don't know the details of automatically posting to this format as of yet (absolute position, incrementally cut).

 

[cncwhiz]

NC,


I think you could do this in absolute. You could "g10" shift A simply absolute shift and it could be changed based on the amount of holes, parts etc. I could understand using incr on this with an loop subroutine. You could have a post built so you only hve to program on part and set some shift amounts at the post level. I have a hex tombstone that I run multiple parts as well. I have all this done in the post and only program one or two parts. Somthing to think about? In the old days of programming by hand I would have programmed the subroutine in incr as well.

 

[ncprog]

CNC,


Good Thinking, I enjoy reading your posts, good information always. This is an old Mazak Laser with a Mazak controller. Previous CAM software was already established prior to my arival. I could have it changed going to Pro/MAN but our "Veteran Employee" who has been running the laser since day one is comfortable with the way it is. I did check the manual though and Mazak has no G10 on this controller version (1992 L32)). They do have the associated "L" word (number of repititions)to use with the M98 subprogram call which we use.


Keeping me on my toes!