Help with G52,G53, G92,G10

[rtpeters]

I have a couple Haas vf3's. Have always used their G54-G59 and 100-120 work offsets. I am interested in learning exactly how and why G52, G53, G92, G10 codes are used. My machines and more importantly my manuals are about 8 years old and really lack good explanations. Example "G52 Set local coordinate system (child)" I don't know what this means...
A good summary(definitions) of the codes, reasons for using one as opposed to the other, and some example code would be a great help.
Thanks

[DAB_Design]

rtpeters, I'm kind of in the same boat. I just started a new job, and they use G54-59. I have never used these. I have always used G92. Throw in the fact that I have never ran a Haas, and it makes things just a bit more confusing. Their machine is only about 8 months old I think, and the only manual doesn't seem to get into things as much as I'd like.

Since I'm not too familiar with the Haas, I'm kind of hesitant to give any info on the G92. I'm not sure if it's handled the same as the controls I'm used to (Cincinnati Milicron)

[rtpeters]

I'm game for your input. The haas manual does state how their codes differ from standard Fanuc. It just doesn't give any explanation of how or why to use them. Basically I'm just trying to get educated on all the ways to machine a matrix of parts from a single plate, or multiple plates in different vices or even multiple fixtures. I want to know ALL of the different methods. Maybe not All, I don't have macros.
As for the G54-59 and 110-120, we simply indicate a part/fixture, position the table at the x0y0 for that part and press the "work offset" for x,y. That stuffs the coordinates into the register, of course, you choose which register...G54,G55 and so on. Then in your program you call up one of these offsets. I have only ever manually set these offsets, and never manipulated them from inside the program. And I guess thats what I want to learn about.

[firedog]

There are several ways to "manipulate" or set the work co-ordinate sytems on the Haas machines. The most common way is to use the work co-ordinate system, G54-G59 and G110-G120. As you have done, you can set them with the machine. If you know what the co-ordinate is you can use a G10 statement to set it as well. Here is an example of such a statement:
G10 L2 P1 X-2.1472 Y-8.2893 Z0
I place this near the top of my program, before any machining commands. When the control reads this line, it inserts this co-ordinate into the work offset page, in this example, G54. Each time the control reads this line of the program, it resets the work co-ordinate to what is in the G10 line. Any adjustments need to be made to the G10 line to be effective. You can also use a G10 statement to set cutter comp, wear values, tool length offets as well. All of these can only be adjusted by changing the G10 line in the program.

A G52 works by shifting the parent work co-ordinate. For instance, if the G54 co-ordinate is X-5.0, Y-3.0, and Z0, you could use the following line to put in a shift to another part zero.
G52 X-2.00 Y1.00 Z0.
Your new part zero is now X-7.00, Y-2.00, Z0. To go back to your original part zero, you could use this line:
G52 X0 Y0 Z0.
The work co-ordinate has now shifted back to the original G54 location.

An example of how I use a G52 is when I have multiple parts on a fixture plate, with a indicating hole on the plate. Since I can figure out the distance to each part on the fixture plate from the indicating hole I set my main work co-ordinate (G54) on the indicating hole. The G52 value is then the distance from the indicating hole to each part zero in an incremental value. When this fixture plate is put back on the machine, the G52 values are still correct, and the only thing that needs to be changed is the indicating hole value(G54).

I never use a G92 anymore, because using the other work co-ordinate callups gives me more flexibility.