top of page

Which is better, G53 or G28?

Suggested by Jason Michaud of Chippewa Valley Community College

Mike: We are having a discussion in our department if we should have students send the axis home with a G28 or a G53. For some reason I like using the G28 but others prefer G53. Is there an advantage of one over the other and which one promotes better programming practice?

  • G28 G91 Z0 or G53 Z0

One advantage to using G28 is that the axis origin lights will come on which was very important in the days of using G92 to assign program zero - when the machine had to be in a planned position before the cycle was activated. This made it possible for an operator to check whether the machine was at the zero return position (the lights would be on). But with fixture offsets (or geometry offsets on lathes) this is no longer so important.

Another "advantage" is that G28 is universal. For companies that have very old machines (no fixture offsets - or possibly G52 is not allowed), they can use the same command for all machines.

Finally, even today, I think some machine tool builders don't make G53 part of there standard package, meaning the G28 method will always work (or G53 would have to be purchased as an option).

The biggest reason some people don't like G28 is the G91 that goes with it. If they forget it, the machine will first go to the program zero point (possibly crashing) then go home. Or if they subsequently forget the G90 in upcoming motion commands, the machine will still be in the incremental mode.

Generally speaking, if a company is sure that they can use G53 on all of their machines (maybe the company is just getting started in CNC), I'd recommend using G53. But if they have any concern about compatibility, I'd recommend using G28.

One last point about using G53. I'm not sure if it is influenced by the common fixture offset (fixture offset number zero). I don't think it is, but it would be worth testing. When a value is placed in the common fixture offset, the point of reference for fixture offset entries is moved from the zero return position to a more logical place - possibly a location point on a sub-plate.

To test, simply put a -3.00 value in the Z axis register of the common fixture offset (don't forget to clear it after the test!). Then give the command G53 Z0 in MDI mode. Does the machine still go to the zero return position, or is it three inches below? If G53 is affected by the common offset, I would NEVER recommend using it. Someday, the user may need to use the common offset, which would mean they'd have to change lots of programs.

159 views0 comments

Recent Posts

See All

Can you speed up your tool change time?

Machining centers, of course, have automatic tool changing devices to automate the tool changing process. Current models boast very fast tool changing times and you may be quite satisfied with tool ch


bottom of page