[titchener]

I'm writing some macro code that I would like to be capable of running on as many different controllers as possible, and it makes some assumptions about the location of machine zero.

On my machine (Mach3 controller), the location for Z0.0 in machine coordinates is with the spindle fully raised.

Is that also true on commercial machines (Haas, Fanuc, ...), ie machine Z0.0 is always with the spindle fully up, or do some of these machines use a different convention?

Is this something the user can change or is it always fixed on the machine?

Thanks,

Paul T.

[Geof]

The conventional location for Z machine zero is with the Z axis raised as high as possible or at the tool change position.

On Haas machines with the carousel tool changer Z zero is at the tool change position and the Z axis can actually go positive far enough to left clear of the tool. On some other makes of machines I think Z zero is as high as the Z axis can go and the tool change position is a few inches below this.

[dcoupar]

On Brother and Okuma machines, I believe Z0 is the top of the table. So when you "Home" Z, it goes to the + travel limit, and shows a Z position of whatever the distance from the gage line to the table top is.

[psychomill]

Adding to dcoupar's remarks, there are some exceptions. Toshiba also puts the 0 at the table and Niigata has done this as well.

To answer the question "can it be changed?". Yes, it can but it's not necessarily simple especially as the machine gets more complex or has more automated features that depend on that particular axis. It's probably more tedious than complex and you just have to be sure you get all of the parameters. Then adjust any mechanicals, and correct the programs or macros that rely on this as well.

I've moved the machine 0 positions on several machine types, models and builders. Some were a snap... others took some time.

[titchener]

Thanks for the info fellas, that was helpful.

Paul T.

[Allen Thompson]

I'm writing some macro code that I would like to be capable of running on as many different controllers as possible, and it makes some assumptions about the location of machine zero.

On my machine (Mach3 controller), the location for Z0.0 in machine coordinates is with the spindle fully raised.

Is that also true on commercial machines (Haas, Fanuc, ...), ie machine Z0.0 is always with the spindle fully up, or do some of these machines use a different convention?

Is this something the user can change or is it always fixed on the machine?

Thanks,

Paul T.

Never make any assumptions with your macros. G2 CW G3 CCW should be read from a Machine Parameters sub-routine. From which end of the spindle were they looking when they were looking at a clock? Especially true of lathes but you did say "as many different controls as possible". And if there is one exception, you must always program around it. Mechanical things as well. Each axis travel distance as well as max and min spindle speeds;too low a spindle speed often gives an alarm. I guess you could say that macros that make assumptions are just hard coded programs.:wee:

I've changed parameters in Yasnac MX3s and Hitachi lambda controls to tell the machine that the tool length in Z comes from a spindle gauge point and not the tip of the tool. I think this parameter is the number one would fiddle with if one chose to move how the CNC interpreted Z0.

Any hooo..... just put a variable in your machine independent macro (god love you. you must be young) that asks for the amount and sign of z motion from home. If all the way up is zero then -(minus) and 25.oo inches should give you the working envelope you desire. But what if someone made z-zero all the way up and the motion down is more plus....like Hurco does in their mills....
Macros can keep you up nights:cheers::cheers::banana::cheers::banana:

And in closing I must mention M codes. And different G-Code Series. A G94 is not always a G94 sometimes it is a G98. And G76's Canned Threading Cycle on FANUCs are not always G76s but they do require only one line to execute - except for the FANUC versions that require two G76 lines to execute. Unless the Canned Threading Cycle is not a G76.
Ever programmed G-Codes for a FAGOR ?

I must say that I could not sleep nights if I ever left a macro some where that said it would run on several machines. The crash potential is almost limitless. Make everything universal for the machine you are standing in front of; the portability will then be built in. Mostly....:wave:

[titchener]

Wow, as I'm getting a better understanding of this (thanks for the help fellas) its pretty clear that writing a g code macro that has any complexity at all and expecting it to run reliably on more than one controller type is not going to happen.

I'm surprised that the consumers of machine tools allowed the machine manufacturers to diverge so much on the G code language. Its like the old days of machine tools where every manufacturer had their own proprietary collet and tool holder type. Eventually the market forced them to adopt standards for the tool holders, I wish that would have happened with the controller language.

Oh well, thats the way it goes.

Paul T.