Posting problem

I need help with a posting problem. Using Mastercam and running on a Milltronics VM15 with Centurion 7 control. When posting a spot drill and peck drill program it will try to send x in a -24 inch move which alarms out. If I change the G91 G28 Z0.0 to a G0 G90 it will run fine. How do fix this with out editing every time? This only happens with drill cycles. If I run pockets and others with the same G91 line it works fine. Any help would be great. Thanks, Al

Are you cancelling the drill cycle before your G91G28 line? Needs G80 perhaps or whatever Centurion 7 uses for cycle cancel.

Yes it does have a G80 before.


O0000(CYLINDERBRACKET)
(DATE=DD-MM-YY - 03-01-20 TIME=HH:MM - 09:55)
(MCX FILE - J:\CYLINDERBRACKET.MCX-8)
(NC FILE - E:\CYLINDERBRACKET.nc)
(MATERIAL - ALUMINUM INCH - 2024)
( T1 | 1/8 DRILL | H1 )
( T2 | 1/4 DRILL | H2 )
N1 G20
N2 G0 G17 G40 G49 G80 G90
N3 T1 M6
N4 G0 G90 G54 X.75 Y-1. A0. S2139 M3
N5 G43 H1 Z1.
N6 G98 G81 X.75 Y-1. Z-.05 R.1 F4.11
N7 X2.25 Y-1.
N8 X3.75 Y-1.
N9 X4.375 Y-1.5
N10 X5.75 Y-.813
N11 G80
N12 M5
N13 G91 G28 Z0.---------here is my issue
N14 A0.
N15 M01
N16 T2 M6
N17 G0 G90 G54 X.75 Y-1. A0. S1069 M3
N18 G43 H2 Z1.
N19 G98 G83 X.75 Y-1. Z-.25 R.1 Q.1 F4.28
N20 X2.25 Y-1.
N21 X3.75 Y-1.
N22 X4.375 Y-1.5
N23 X5.75 Y-.813
N24 G80
N25 M5
N26 G91 G28 Z0.
N27 G28 X0. Y0. A0.
N28 M30
%

Al, do you know how to open and edit your post processors?

Yes, I had to change pxout and pyout to pfxout and pfyout to get it to drill right, but it has the same problem with the original post.

Ha... I know... it's line 13! That's your trouble. Soo unlucky! :-)

Just kidding.

It's like the machine isn't coming out of the drilling cycle properly. For shits and giggles try two things. After the G80 and M5, put a small G0Z move in there and see what happens after with the G28. Before you do that, run your program in the problem area with Single Block mode on and see if the machine runs to an intermediate position on the first push of the green, then home on the second push. Technically there should be no intermediate movement calling G28 with G91 other then a move to where it's already at Z move. So I guess if there are problems it could potentially take 3 green button pushes to get Z home.

Dave

One more thing I though of. Not up to speed on your control, but if you have G53 to use, I would use G53 to send any or all machine axis home. Safer and easier. Some machines will turn the "Z Home" light on with G53Z0, which it will likely need before it will do a tool change, but if it doesn't, throw in a G91G28Z0 right after the G53. That will turn your light on without any machine movement if your axis is already at physical home position. It will happen in an instant so no need to worry about adding time to the process. Don't forget to add a G90 soon after or you'll get yourself in trouble.

Dave

AlPeeso said:

Yes, I had to change pxout and pyout to pfxout and pfyout to get it to drill right, but it has the same problem with the original post.

Click to expand...

If I were in your position I'd play with it a little bit. You'll have to change the post in the pretract post block. Like 13engines said, I would try to swap G28 for G53 and see if that does anything for you.

Personally I wouldn't want to change the post too much knowing that it works with all of your other code well. You could add in some simple logic to basically say, "If it's coming out of a drill cycle, output G0 G90 ZXXX"

I don't have the post documentation right in front of me but in pretract you'd have something like:

if prv_gcode = (73, 74, 83, 84, 85, 86),
pbld, n$, sgabsinc, sgcode, *sg00, *sg90, "ZWHATEVERVALUE", e$
else,
pbld, n$, sgabsinc, sgcode, *sg28ref, "Z0.", e$


(The prv_gcode thing is just an example. It could be something like previous g code or previous op code, can't recall off the top of my head right now. Get with your reseller for the post documentation if you haven't already.)

Thanks for the help. I will give it a try.

Al