Question about part offset, G54-59

[Sticky Racing]

I know this is a really basic question, but I am new to this part of g-code. I plan to do some part offsets, or in other words I am going to make several parts at once. I understand that using a G54, 55, 56, etc. essentially moves my table zero to another location. What I am not clear on is where the info is stored. Do the new coordinates for the offset go in the program and look something like:
G54 X4. Y0. (New zero is 4 inches in the X direction from previous zero)
or is the info stored in the machine, and I will have to manually input the coordinates in the machine, and the program just displays the G54?

[Geof]

The G54, 55, etc coordinates are stored in a table in the machine. You put them there in different ways depending on what make of machine you have. You can also enter them from the program using the G10 command.

In your program for the part at G54 you have the G54 command and then all the stuff that happens to that part. Then for G55 you have that command and then the stuff for that part. If all the parts are the same you put the coding for machining the parts in a subroutine. Then you have the G54 followed by a subroutine call M97 P(or O)nnnn where the nnnn is the line n umber your subroutine starts at. The you do G55 M97 Pnnnn, etc through all the work zeroes. If you are using more than one tool you select Tool 1 and step through al the work zeroes, then change to tool 2 and do the same, etc.

If you want an example I can find one.

[Sticky Racing]

Geof,
Thanks, examples would be great, as I am working with a Hurco SM1 and don't have any documentation on what the capabilities of my controller are. So, basically it's all trial and error over here. The last part you posted is my plan. I am planning on doing between 3-5 parts at once for starters, hopefully moving up from there eventually. But yeah, I would like to minimize tool changes, so the first tool would do it's work on each part (all parts are the same for now), then change tools and do that tools operations on each, etc, etc.

Thanks again,

-Ed

[Geof]

Geof,
Thanks, examples would be great, ....-Ed

Don't know if this is what your were expecting . It is a bit big to put in the body of the post so I attached it as a text file you can open in Notepad.

Eleven tools and twelve work zeroes each of which is used at four positions on a four sided rotary fixture so effectively there are 48 work zeroes. Each part uses three work zeroes. I can dig up a picture of the part tomorrow and put it up as well. I thought this shows you how carried away it is possible to get.

[Sticky Racing]

Don't know if this is what your were expecting .

Not exactly
Definitely too sofisticated for my control. But i get the logic, just going to have to figure out which method that my controller can handle. Hopefully it won't be too cumbersome.

[Caprirs]

Maybe a little simpler than Geof's. My machines have Mitsubishi controls so there may be some differences in terms. This program lets me run two parts per tool change located on different vises. If my fixturing allowed me to run more parts per cylce, I could add more work offsets (G56-G59). More than 6 work offsets on my machine requires using a G52 local zero to shift the work offset from inside the program.

An advantage of this style of programming is the ease of editting. If I need to change a dimension, I only have to edit the code in one place, not for every part location.

%
G0G40G90
(ROUGH)
G54
M98H10
G55
M98H10
M9
N2(FINISHOD)
G54
M98H20
G55
M98H20
M9
N3(UNDERCUTDIAMETER"A")
G54
M98H30
G55
M98H30
M9
...
...
...
M9
G0Z6.
G0G53X7.Y0.
M30
N10
T1(.375ROUGHER)
M8
S7500M3
G0X.934Y.95
G43H1Z.05
G1Z-.27F40.
...
...
G0Z.25
M99
N20
T2(.482FINISH)
M8
S5000M3
G0X0.Y0.
G43H2Z.05
G1Z0.F3.
...
...
G0Z.25
M99
N30(FORMTOOL)
T3
M8
S5000M3
G0X.948Y.955
G43H3Z.025
G1Z-.55F40.
...
...
G0Z.25
M99
...

[Geof]

.....An advantage of this style of programming is the ease of editting. If I need to change a dimension, I only have to edit the code in one place, not for every part location.......

This is certainly the programming advantage!!!!

The way we configure ours also allows easy modification to the number of work zeroes because we have machines that can fixture different numbers of parts.

Also on Haas machines, I don't know how applicable this is to other makes, I can copy a subroutine to the clipboard and run it as an individual program from the clipboard. this is how I write and prove these programs; subroutine by subroutine, i.e. tool by tool, and then just paste the proved subroutines onto the bottom of the growing program. And the block deletes before some work zeroes are so that on the next setup just one part is done and checked so the wear can be adjusted for final sizes before taking off block delete and banging ahead on a full machine load.