Newbie- Into the deep end..

[mnewman]

The company I work for recently purchased a woodworking facility to diversify our operating basis.

Prior to about 4 weeks ago I didn't even know what gcode was, now I'm responsible for helping streamline the flow of hand drawn designs into final cut pieces using a Fanuc 15M from 1989.

So far I've got a pretty good handle on how everything works and have successfully used Mastercam X3 to generate code for a few simple pieces.



But enough rambling--

I believe I've got something wrong in my post processor. I'm attempting to post a two contours. I want the code generated in incremental mode, and the first contour does as such, however after it finishes the first cut, it G0 G90 G54 to the start of the next location and then never goes back to G91. At this point I'm clueless as to where to go next.

Help?

[SCRAPWOTSCRAP]

A work around.....you can bring the program file into a word processor software, MS. word, note pad, etc and insert your G91 at the appropriate line, and your file will cut. Maybe modify post processor down the line after you get a real feel for what you're doing. Many of us alter programs generated by post processors....quick and easy fixes.

[mnewman]

Let me clarify that a bit.. The code from that point on is in absolute mode, instead of incremental like the start of the program.

I am aware that in MCEdit there is an Absolute to Incremental convertor, but I cannot communicate to the CNC from within that program like I can with the Mastercam X Editor.

I'm trying to get this process down to the minimal number of steps, as eventually it will be taken over by the workers in the shop, none of whom have much computer experience.

Where in the post processor would I begin to look to correct a problem like this?

[donnelson]

you need to get a hold of mike matera he advertises right here on this post he will fix your post for minimal amount of money just pay the man it is worth it to know that it is right he has helped me and it is good

[Superman]

OK, you've told us you have X3
what modified post are you using ?

Can you put up some code showing the problem ?
( I suggest using just a couple of lines to keep it short )


mark in red the code in error
mark in blue the code you want


example

N4 G30 P1
()
N5 T3
N6 M201 ( pallet #1 )
( 3.0BALL CBD 2FLUTE 4FLUTELENGTH 6SHANK 18OUT )
( TOOL - 3 ; D3 ; H3 ; TOOL DIA. - 3. )
N7 T3 M6
N8 G15 H1
N9 B0. M15
N10 G0 X366.4 Y22.775
N11 S8500 M3
N12 M50 ( thru tool coolant )
N13 G56 G43 H3 Z80.
...
...
...
N107 G0 Z80.
N108 M9
N109 M5
N109 M205 (clear coolant lines )
N110 G17
N111 G15 H0
N112 G30 P1

[Andre' B]

Originally Posted by mnewman I want the code generated in incremental mode,

If I may I have to ask why?
I have been doing this stuff for 25 years and have never found a case where incremental was better, it is almost impossible to read and debug on the floor.

[mnewman]

I've begun using "Generic Fanuc 3X Router", and made a duplicate of the .PST
which I've begun editing to try and fit the needs of our machine.

At the moment the only changes I've made are:
Under NC output, changing 'main program default absolute/incremental' to incremental.
Under Arc, changing the three planes under Arc Center Type to Radius.
Under Misc Int/Real values, changing "Absolute/Incremental, top level" from 0 to 1 (labeled as being 0=Abs, 1=Inc).

.....
N150G0G90G54X-8.0463Y-14.0375
N160S0M5
N170G43H1Z.1
N180G1G91Z-.1F0.
N190X-.0648Y.0435F.01
N200X-.0697Y.0583
N210X-.0692Y.07
N220X-.0689Y.0826
N230X-.0686Y.0962
N240X-.0683Y.1109
N250X-.0677Y.1264
.....
N800X.0597Y.1447
N810X.0582Y.1195
N820X.0569Y.0978
N830X.0562Y.079
N840X.0167Y.0187
N850Z.1F0.
N860M5
N870G0G28Z0.
N880M01
N890G90M5Z0.
N900T2M6
N910G0G90G54X-18.Y-34.25
N920S0M5
N930G43H2Z.1
N940G1Z0.F0.
N950X-14.3521F.01
N960X-14.2902Y-34.21
N970G2X-9.Y-32.65R9.75
N980X-3.7098Y-34.21R9.75
N990G1X-3.6479Y-34.25
N1000X0.
N1010G3X.25Y-34.R.25
N1020G1Y0.
N1030G3X0.Y.25R.25
N1040G1X-18.
N1050G3X-18.25Y0.R.25
N1060G1Y-34.
N1070G3X-18.Y-34.25R.25
N1080G1Z.1F0.
N1090M5
N1100G91G0G28Z0.
N1110G28X0.Y0.
N1120G52X0.Y0.Z0.
N1130G8P0
N1140M30

The code for switching heads and actually starting up the machine is wrong also, but until I understand how to fix that also, I can do that much by hand.

As you can see, in green, it starts out in Incremental mode, as desired, however when it fast planes to the next chain further down the program, it switches to absolute and never goes back to incremental. This is not the desired behavior. I want all the code in incremental.

[mnewman]

Originally Posted by Andre' B If I may I have to ask why? I have been doing this stuff for 25 years and have never found a case where incremental was better, it is almost impossible to read and debug on the floor.

Because we are doing a low number of each cut, usually only a few at a time spread out over a very long period of time, they need to be able to reposition where on the table the piece is cut without having to re-write half the code.

Edit: And if there's an easier way to do that then having all incremental code, I'm all ears. I just need it to work (:

[Superman]

Originally Posted by mnewman Under Misc Int/Real values, changing "Absolute/Incremental, top level" from 0 to 1 (labeled as being 0=Abs, 1=Inc).

Before altering the post
Have you altered all misc values in all operations to output in increm.
or did you alter only the 1st op. ?

And if there's an easier way to do that then having all incremental code, I'm all ears. I just need it to work (:

The G54 is the zero point datum, adjust this X & Y and the program is set from that.

If the output is inc. or abs you get the same part- absolute is more user freindly and can be followed & edited.

adjust an address in incremental-the code following is junk.

you can put the G54 anywhere and run the absolute output, you will get the same part .

[mnewman]

Originally Posted by Superman Before altering the post Have you altered all misc values in all operations to output in increm. or did you alter only the 1st op. ?

I dunno Where do I even check that?

Originally Posted by Superman The G54 is the zero point datum, adjust this X & Y and the program is set from that.

That's sounding like a more reasonable way to do this. I'll have to look into that.

Originally Posted by Superman If the output is inc. or abs you get the same part- absolute is more user freindly and can be followed & edited. adjust an address in incremental-the code following is junk.

As I understand it, they'd only alter the first coordinate to reposition it,
but getting G54 as part of the routine will be more reasonable.

[g-codeguy]

I program lathes. Very little experience with mills. Woodworking? What's that? I'm going out on a limb here trying to help, and don't doubt someone will cut it off from under me. But...I'll try anyway.

I modified a v9 mill post for incremental. Boss complained that it wouldn't output incremental now that it is in X3. I checked it out, and the post still said incremental output. Apparently X3 doesn't care what the output is set for in the post. You have to select incremental in each operation where it is desired.

For mills look in the area where the tool depth, approach, etc. is defined. There is a place there to select incremental if that is what you want. I believe this is the solution to your problem. A side note: On a mill or lathe, if you have G54 you will also have G55 through G59 work offsets at a minimum. Hope I used the correct words there (work offsets) else I will get flamed.

Be sure to let us know how you make out. I always like to know "the rest of the story." Too often the OP never lets you know if his problem was solved or not.

________________

“It stands to reason that where there's sacrifice, there's someone collecting sacrificial offerings. Where there's service, there's someone being served. The man who speaks to you of sacrifice, speaks of slaves and masters. And intends to be the master."
--Ayn Rand

[Matt Berube]

Originally Posted by g-codeguy I program lathes. Very little experience with mills. Woodworking? What's that? I'm going out on a limb here trying to help, and don't doubt someone will cut it off from under me. But...I'll try anyway. I modified a v9 mill post for incremental. Boss complained that it wouldn't output incremental now that it is in X3. I checked it out, and the post still said incremental output. Apparently X3 doesn't care what the output is set for in the post. You have to select incremental in each operation where it is desired. For mills look in the area where the tool depth, approach, etc. is defined. There is a place there to select incremental if that is what you want. I believe this is the solution to your problem. A side note: On a mill or lathe, if you have G54 you will also have G55 through G59 work offsets at a minimum. Hope I used the correct words there (work offsets) else I will get flamed. Be sure to let us know how you make out. I always like to know "the rest of the story." Too often the OP never lets you know if his problem was solved or not. ________________ “It stands to reason that where there's sacrifice, there's someone collecting sacrificial offerings. Where there's service, there's someone being served. The man who speaks to you of sacrifice, speaks of slaves and masters. And intends to be the master." --Ayn Rand

I got the impression you'd be disappointed if nobody flamed you so here you go !