Fanuc 4th axis questions

I'm trying to write a post for a Fanuc based machine with a 4th axis rotary table.

Currently the operators position their part relative to the pivot of the table. I would like to change that, if possible, and use RTCP so that the operator can just pick up the datum of the block (like using M128 on a Heidenhain controller).

Is this possible in Fanuc?

Also, they have requested that the tool move to the max Z and max Y positions before rotating. In Heidenhain I would just use M91 or M92 and use values that are relative to the machine. Is there a counterpart of this method in Fanuc language?

Thanks,

Dan

More machine dependent than anything. in MOST cases a g91 g28 x0y0z0 sends the machine home but you may want a g91g28 z0; g91g28 xoyo on a different line

I program for 4th axis in Fanuc quite frequently.I need a little clarification on your RTCP, but I always use the centerline of the 4th axis as the datum for my 4th axis parts. Touch off on a known diameter(chuck) for work offset and tool length, and away you go.
MaxZ and maxY? I would assume you are referring to the spindle all the way up and away from the part and table. G91G28ZO in one line, then G28Y0 in the next line does that simply enough. Be sure to revert back to G90 after your home , before you start approaching the part.
I may be missing something here in your question, but Fanuc is about the most simple dialect I've encountered for programming. I write a bit of Okuma as well, but in this shop, those are lathes, 2 axis, so that wouldn't apply at all.

If your writing a post for a CAM system you have several options.

Myself: I always attempt to mount the part or fixture as close to COR as possible. Then I will indicate the part in the machine to see where it's at in space relative to center line of 4th.
Next all you have to do is draw or move the part in CAM relative to how it's actually in the machine. Done.

I've heard of fancy Macro's written for picking up offsets in the machine too.... That's above my head a lil

4th axis rotary table... which kind? "A" on a VMC (rotates about X) or "B" in a HMC (rotates about Y)? For A, the simplest thing is to set Y & Z at center of rotation, and X & A where it makes sense. If B, could be from center of rotation, or you could just pick up the desired X,Y,Z at each rotation (takes longer). But as Rstewart said, you can pick up a known point somewhere in the setup, then use a macro to set offsets for the other rotations (such as a part on a tombstone or bolted straight to the rotary table). I have used such a macro. You have to know how far it is from X,Y,Z home to the center of rotation. You then edit these values into the macro, along with the rotation angles for each work offset (G54, G55, etc). The macro then trigs out the X,Y.Z for all the rotations. Only thing is, that program zero ends up being the same program zero from all rotations so you have to work to that when you do your program. Not hard if you're using a CAM system and origin off a common point.

Thanks for the replies. The process described is what is currently happening. I come from the 5-axis world where RTCP is common, and we don't need to concern ourselves with where the rotation points are. Either M128, CYCL DEF 19 or PLANE SPATIAL will allow us to rotate and transform the locations onto that plane. I'm a bit surprised that with a 4th axis (rotating about the X) that this isn't being done too. I realize I'm talking apples and oranges here (Heidenhain vs Fanuc) but I'm going to keep pursuing this until I either make it work or hit a dead end.

Dan

Some models of Fanuc control have "Rotary Table Dynamic Fixture Offset" available as an option. This function allows the control to "track" the zero as the rotary moves. It is an option and not available on the lower end models.

G53 allows the programmer to position the axes using the machine coordinate system rather than the part coordinate system.