rotating 0,0 point to opposite corner.

[Vortex_bits]

Ok, here is another thing I need to figure out.

We have moved our fanuc controller from one side of the machine to the other. On this machine, the bed is the X axis, the Gantry is the Y. So now I want to put 0,0 on the lower left corner of the OTHER side, however, when I did this in tests this weekend, I had to enter all negative axis movements, instead of positive. Because I don't want to re-do all of our single parts, but I DO want to move the 0,0 point, how do I rotate the 0,0 180 degrees, and still keep all the movements positive?

I have heard there is a way to adjust the G53 in the controller to a different spot, but does this affect the movements? And does this mean that I will need to essentially make the machine run OPPOSITE of how it's movements are currently. I.e. make the machine inverse it's Positive and negative moves opposite of what the stickers say?

Never tried this before, so any help is appreciated. thanks.

-Zak

[psychomill]

So, you moved the control to the opposite corner of where it used to be and turned it around? Couldn't just turn the machine around? Just picturing what you're doing here.

If my first guess is right, then yes, your machine will travel in all negative moves now since the coordinate system is still based upon the original corner (or original machine zero) and the signed directions. You could shift this and change the axis direction by parameters but you may have to change a lot of things if you've got tool changers, pallet changers, etc. Sounds like it would be simpler for you to use a G68 (coordinate rotate) command and the control will flip the code around 180°. So, based on your "new" part origin, you could type in the program a "G68X0Y0R180." A G69 at the end will cancel this.

Oh, and this is provided you have the G68 control option....

[Vortex_bits]

Originally Posted by psychomill So, you moved the control to the opposite corner of where it used to be and turned it around? Couldn't just turn the machine around? Just picturing what you're doing here. If my first guess is right, then yes, your machine will travel in all negative moves now since the coordinate system is still based upon the original corner (or original machine zero) and the signed directions. You could shift this and change the axis direction by parameters but you may have to change a lot of things if you've got tool changers, pallet changers, etc. Sounds like it would be simpler for you to use a G68 (coordinate rotate) command and the control will flip the code around 180°. So, based on your "new" part origin, you could type in the program a "G68X0Y0R180." A G69 at the end will cancel this. Oh, and this is provided you have the G68 control option....

Well, the machine is pretty big.. a 5x12 bed, and probably over 12,000 pounds.. plus, then it would be facing the wrong way.

is G68 a modal or non-modal? Sounds like non-modal, and the point of me doing this is so that all over our hundreds of programs that are already in CNC code will work with the new co-ordinate setting. It does have a tool changer, but I can't see why that would change anything, as it's an on-board carosel, not the type with the tools on the sides of the machine.

Anywho, thank you for the idea, I'll have to dig further in and see if there is a semi-easy permanent solution.

-Zak

[psychomill]

You have to add it during the operation and cancel before certain things like tool changes, pallet changes, tool length probes, etc, etc. But it will fix the hundred programs. You're looking to change the grid and axis signed directions so you don't have to edit the programs whic might be a bit complicated.

It does have a tool changer, but I can't see why that would change anything,

You never mentioned the machine you have so I have no idea what yours looks like or is built. But, many machines have mounted tool changers. But the problem is not how the tool changer mounts, is where the machine goes in order to do a tool change. Your wanting to turn around your directions, your tool change motion and position (by parameter and/or M code sub command) may try and send the machine to some strange spot (or worse) when commanded.

Your machine grid should be easy enough to shift. It's the signed direction that will likely cause grief. A G68 would be a simple fix without having to alter the machine settings. As far as the "100s of programs" are concerned, just edit them as they come up or one at a time and not try and attack all of them at once.

a 5x12 bed, and probably over 12,000 pounds

A big XY but doesn't weigh much... is this a router? Changing the grid and axis direction is the "easy fix" coming from the programs standpoint... But my bet, it's going to take more than just a couple parameters...

[Andre' B]

Why would the existing programs need to be changed?
The work offset that you define when doing the setup takes care of that.

Unless you are converting your machine from a right handed coordinate system to a left handed one, which (to be blunt) would be a dumb thing to do.

[Mitsui Seiki]

If you want the machine "home" in the lower left corner you have to move your limit switches.

[psychomill]

Why would the existing programs need to be changed?

If you read what's happening (as I understand it), the signed direction of the machine axes are back wards now relative to the program and from where you now stand to operate the machine. It will take more than just move limit switches but that is one of the several things that will need to happen..... "Home" itself can be moved simple enough I think... a couple switches and some parameters. But moving the machine grid 0,0 (which is easy), changing the axis signed directions and home axis directions and any peripherals affected by the grid can get tricky and involved. Unless, there's a simple parameter to change the signed directions.

Curious though... why did you need to flip the control around? And what machine/control model is it?

[Mitsui Seiki]

I know it takes more. I just pointed out that they need to be moved.
With all that has to be done, it's a lot of work.

[Mitsui Seiki]

Is this what you are doing?
In the old position all movement are - from home and the new one all movements are + from home.

[psychomill]

That's the way I see it Stefan....... but he wants to run the same old programs that are already in his system without re-programming which is why I suggested G68 as an option short of changing a bunch of stuff in the machine/control.....

Vortex... are you there????

[Mitsui Seiki]

Once he has made the necessary changes (limit switches and parameters),isn't all he need new work zeros?

[Andre' B]

Originally Posted by Mitsui Seiki Once he has made the necessary changes (limit switches and parameters),isn't all he need new work zeros?

That is what I am seeing.

Could be he does not know about using work offsets and really did make the programs with the machine zero as the program zero.
If that is the case all that is needed is to add a line at the start of the program with a G54 in it and set the G54 work offsets to the full travel of the machine. Or Fanuc controls have a set of offsets called (EXT) stands for external, on older controls it may be called (COM) for common. This set of offsets gets added to any of the standard G54,G55,...G59..G54.1Px offsets.

Or a quick little program in what ever language he likes to use, could do the translation or even rotation if wanted, off line.