Understanding RS274/NGC overview....(not)

[greybeard]

In the RS274/NGC language view, a machining center has an absolute coordinate system and nine program coordinate systems.

...from the NIST pages, which I'm reading as a prelude to understanding how to write Gcode !

Can anyone tell me why a machine should need nine program coordinate systems with a real world example ?
Or any number of them, come to that !

John

[samco]

9 vise locations? I use 2 when I make circuit boards - on for the front and one for the back (2 different zero locations on my vacuum table)

sam

[samco]

like this - then you can have a zero point or such at each vice...

[vlmarshall]

Good question! Here's a few more examples:

Just like Samco posted... I've got 4 vises in a machine at work right now, two of them with a single work offset, and two with two offsets, all set around the parts in them.

In another machine, I've almost always got 4 or 6 of the System 3R clamping blocks set up, as well as a work stop in a single vise.

When I've got a 4th axis set up, I'll usually leave a work offset with the Y axis set for that, even between jobs.

At home, I've machined the first operation of a few parts in a vise, and the second operation on a fixture plate nearby, each with it's own coordinate system.

I've used my mill as a lathe, with tools on the table, each with it's own zero point.

Samco's example gets even more complex with softjaws, holding two parts in each vise, when 9 offsets aren't enough.

[greybeard]

So, if I've got it right, the 9 coordinate systems are allowing you to set up multiple jobs on the table, then run one routine on one job, while loading/unloading others. Then having finished job one, the machine can run routine 2 on fixture 2, where routines 1 and 2 could be the same or different, but are within a program that has been set up to run up to nine different jobs.
So you can write routines, store them till needed, then drop them into any program, just giving the coordinates for that fixture in that routine?

Please expand the above if there are other important facilities it gives.
Many thanks
John

[vlmarshall]

Well, I almost never mess around in/on a machine while i's running, but the bit about multiple jobs is correct.
I see you're developing a V-Carve-like program (very impressive, by the way), so I'll use sign engraving as an example. Let's say that you mass-produce wooden wall plaques. Some of them hang vertically, and some with the long dimension horizontal, "landscape", as my printer calls it.

You've got a fixture that locates the upper edge and one corner in the same place every time you put a part on the table, no matter the orientation. Also assume you want to dimension all of your work from the center of the plaque. That center point will be in a different table location for each of the two plaque styles, and you might not want to go back and find the center each time you engrave one. Set G54 for the center of the plaque when sitting vertically, G55 for the center of a horizontal plaque, G56 for the keyhole hanger on the back of the vertical style, and G57 for the hanger location on the "landscape" plaque.

Now you can write one program for the keyhole hanger, which may start:
G56 G00 G90 G17 G21
T1 M6
G43 H1
S5000 M3
X0 Y0 Z1.
etc...
A quick edit of the G56 to G57 will move your entire keyhole-cutting routine to the alternate location.

Likewise for the front side, save two "templates" in your CAD program, or in your case, maybe make your carving program find the center of a block of text, and dimension from there... either way, a switch in the finished g-code between G54 and G55, will move your engraving to the correct pre-set location.

Just an example, one of many. I hope I've made things a little clearer. That's the fun of this trade/hobby, all of this is like a big pile of Lego, Meccano, or such; a huge set of tools, and no single "correct" way to use them.

[greybeard]

Many thanks for giving me real world detail.
Just the sort of example that makes all the difference.

I must see if I can convert my coreldraw vector files to something a bit clearer than jpegs, then I can post better diagrams of what I'm trying to do, and any progress I make.
Thanks again for the help.
John

[jmelson]

Originally Posted by greybeard ...from the NIST pages, which I'm reading as a prelude to understanding how to write Gcode ! Can anyone tell me why a machine should need nine program coordinate systems with a real world example ? Or any number of them, come to that ! John

The machine coordinate system is based on the machine itself. You don't wan to have to write your G-code to know that the corner of your part is at (1.234 , 2.456) inches from the machine home position, you want to be able to set your part to be at (0,0) or some logical coordinates.

There has to be a machine coordinate system because the machine has physical ends of travel, and may have leadscrew error compensation based on the machine position. So, you can't just set the machine coordinates as you please. That's why there is a part coord system that can be arbitrarily set. Well, if you have one system, why not a couple more, for different fixtures on your table? You don't have to use them ALL, I never have. But, I can use a couple for different parts on a multi-part fixture, for instance.

Jon