Nakamura as200l index turret while b axis is not home

[Leon82]

Is there an mcode to allow this to happen? Asking for a co worker.

 

They are using the sub as a center and it won't index with it not home

[Leon82]

Well, he removed the g28 b0 and it works as expected.

[Colin Gilchrist]

3 hours ago, Leon82 said:

Well, he removed the g28 b0 and it works as expected.

G28 can cause strange behavior, as it cancels many machine modes when you use it. My preference for moving the machine around is to always use G53, since it is non-modal, and won't cancel any of your active machine functions (Work Offset, Cutter Compensation, Tool Length Compensation), whereas G28 cancels all of those modes, and it is left up to you to recall the correct machine modes before resuming cutting.

[Colin Gilchrist]

G28 can also be problematic in other ways as well.

• G28 implementation can vary between machine builders, and even between individual machines, based on the unique combination of parameter settings on each machine.
• G28 cancels active machine modes (G54-59, G43, G41/42), as mentioned, so these modes must all be recalled after the G28,
• G28 responds differently, depending on the current ABS/INC state of the machine. DANGEROUS in ABS mode, because G28 X0. Y0. Z0., is now interpreted as an "Intermediate move", before going "Home". This means the machine will try to smash the "Spindle Gauge Line" to your current Work Offset Origin, (totally ignoring the fact there is a tool present in the spindle), before returning safely to the home position.
• On some machines, G28, executed on a line by itself, will cause "Home Return" motion. Some machines require the Axis Address (X,Y,or Z), on the line, and will only return the axes that are included on the G28 line.
• With "most" Fanuc style machines, G00 G91 G28 Z0. will move the spindle to the home position, without going to the Intermediate "zero" position first, but again, it depends on the mixture or combination of Parameter Settings on the machine. But, if you use "G00 G91 G28 Z0.", you have now cancelled all of your active machine modes, and put the machine into INC mode.
• Many machine tool builders (MTB's) will also include a "Secondary Reference Point" -> G30, or even several "additional points", with G30 P1, G30 P2, G30 P3, and G30 P4. Often the G30 X0. Y0. Z0. Position is used for the Tool Change Position, whereas the G91 G28 position is set to "Machine Home".

But that said, I hate having the risk of a crash when using G91 G28, which is why I immensely prefer to use G53 Machine Home Position Commands.

• G00 G90 G53 G49 Z0.
• That line above will move the gauge line of your spindle, to the machine home position, without cancelling any active machine modes.
• Including the G49 will cancel any active TLO, "as the spindle moves to the home position". I have yet to encounter a problem with this.
• G00 G90 G53 Z0. will make the same "home move", but will leave the current 'TLO' active, if one has been enabled. (G43 Hxx or G43.4 Hxx is still active, unless explicitly cancelled by G49).

 

[civiceg]

G28 burns you once....G53 for the rest of my life.