What's new
What's new

Bonehead multiple toolpath programming question

bucktruck

Hot Rolled
Joined
Mar 8, 2006
Location
NoCal
I am trying to do some manual programming that I haven't been tasked with in close to 30 years. My question is, how do I run the same toolpath at different locations, within the same work offset. I have the g-code, (a deburring toolpath for a counterbore on a shaft) which is from another machine. The part has 6 identical holes, and the machine holds 4 shafts located at G54 thru G57.

I am attempting to use G52 with a subprogram N500, which contains the deburr toolpath. Something like this:

G0G54X0Y0
G52 X-330. Y7.330 A-133.
M97P500
G52 X-165.
M97P500
G52 X0.
M97P500
G52 X165.
M97P500
G52 X330.
M97P500
M01

N500
(HOLE a1)
N6930 G0 X1.542 Y-1.037
N6940 G0 Z19.5
N6950 G1 Z17.574 F500.
N6960 G1 X1.531 Y-1.346 Z17.932 F2000.
N6970 G1 X1.302 Y-2.129 Z17.896
N6980 G1 X1.029 Y-2.549 Z17.668
N6990 G1 X0.645 Y-2.885 Z17.544
.......
..
M99


What is happening is that the machine seems to skip the G52 X-330 Y7330 A-133 line and go directly to the first line of the subprogram, which then goes to the G52 location. Is there something I'm missing? This would normally take me 5 minutes to program with Mastercam, but my new employer believes that splicing code from another machine, using Notepad, is better than giving us the proper tools to do our jobs.

Machine is a Haas VF6SS if that matters.
 
....This would normally take me 5 minutes to program with Mastercam, but my new employer believes that splicing code from another machine, using Notepad, is better than giving us the proper tools to do our jobs.
Did you get it working? I have nothing on this but perhaps your dealer's application guys can help, I call mine up once in a while and they have always been a great resource.
I believe it's great for operators to have manual editing skills so they know how code works but there's no getting around what you said about taking you 5 minutes in MC, or any half-way decent cam system, not to mention less mistakes and having a lot of cad cam power at your fingertips. How's notepad working out for you boss at this point? I feel for ya. Sorry man, I can't seem to keep my mouth shut in face of antiquated low-tech management.
 
I am trying to do some manual programming that I haven't been tasked with in close to 30 years. My question is, how do I run the same toolpath at different locations, within the same work offset.
This is easy. Create the toolpath using only incremental moves. You can do your Z moves in Absolute if it makes you more comfortable, (and all your work offsets share the same Z setting), but overall, completely Incremental is your easiest bet. Just like you might do when using a threadmill routine all over. The only thing you need is the proper start location for each iteration of the Incremental code. And it won't matter if you're in the same Work Offset or any other Work Offset. You can even hold the toolpath in a Subroutine if that shortens to program file.
 
I know... but don't get me started on folks lost without their CAM. Even after 30 years if I'm reading right. On second reading, I think goooose actually solved his problem, and he did sorta have the right idea. The ability to program a fixed set of moves anywhere on a part using any work offset is about as easy as it comes, even done manually. (Not manual XYZ coords. I'm not that old of a fart)
Incremental is your friend...
 
Try this:
G54 ( don't make any moves here as it's bogus anyway )
G52 X-330. Y7.330 A-133.
M97P500
G52 X-165.
M97P500
G52 X0.
M97P500
G52 X165.
M97P500
G52 X330.
M97P500
M01
G52 X0 Y0 A0 ( cancel all G52 shifts within your program, else you get screwed! )
M30 ( must put it before the sub, else the sub will run once more at the end!)
N500
(HOLE a1)
G0 X1.542 Y-1.037
G0 Z19.5
G1 Z17.574 F500.
G1 X1.531 Y-1.346 Z17.932 F2000.
G1 X1.302 Y-2.129 Z17.896
G1 X1.029 Y-2.549 Z17.668
G1 X0.645 Y-2.885 Z17.544
M99

Otherwise I don't see why that wouldn't run.
I do have CAM, but simple shit like this is always fingered and G52 shifts are typically part of it.
 








 
Back
Top