temporary work offsets. external offset or something else?

I recently retrofitted our cnc router, and one feature i did like about the old controller is that you were able to enter temporary work offsets. 
So if my program started in the x0y0z0 corner of the table and my workpiece was at x3y6z1, i would just have to enter x3.0 y6.0 and z1.0 in the temporary offset boxes and the entire program would be shifted by that amount. It was extremely easy for the new guys who are currently struggling with changing the g5x offsets (they often change the wrong one). I did see the component EXTERNAL OFFSET, but does that actually move the machine when it isn't running a program? Or does it wait until it's actually running a part before it moves to the offset? 

External offsets can be used to move the machine _while_ it is running a program. So if your operators are having problems handling the regular work offsets then that is probably not the way to go. You could use G52 as that applies to all offsets but you would want to make sure it's set to zero before running a new part.

axis.
So what are they used for then? the G5x doesnt work in this case because they just end up changing the wrong one and/or wrong axis and screwing everything up. I need to dumb it down for them. Unfortunately it is what it is.

As an example:
External offset is used to adjust the hight of plasma torches using an eternal voltage signal.

If they can't keep X and Y apart then how would they be able to input the offset?

[edit]
another approach could be to manually jog the machine to the required position, maybe using laser cross hairs, and then have a custom button in the axis gui to zero the x,y position.

Aciera wrote:

As an example:
External offset is used to adjust the hight of plasma torches using an eternal voltage signal.

If they can't keep X and Y apart then how would they be able to input the offset?

gotcha, that makes sense. 
They know the difference between X and Y. but ensuring that they select the axis before changing the G5x value in touch off is a different story. Even I have accidentally had the wrong axis or work offset selected multiple times and had to touch everything off again. It's extremely easy to do.
Basically i just want 3 numerical entry boxes on the screen, one per axis. They can enter the distance to the workpiece from xyz0 in those boxes, and run a program. i dont want them getting confused by work offsets and making mistakes that cause me to have to fix the machine. 

How about using an MDI command:

G10 L2 P0 X<your value> Y<your value>

If you wanted you could also create a custom command like

M123 X<your value> Y<your value>

They can enter the distance to the workpiece from xyz0 in those boxes, and run a program

This can also be done but is a bit more involved.

Aciera wrote:

How about using an MDI command:

G10 L2 P0 X<your value> Y<your value>

If you wanted you could also create a custom command like

M123 X<your value> Y<your value>

They can enter the distance to the workpiece from xyz0 in those boxes, and run a program
This can also be done but is a bit more involved.
 

 

i'd rather spend the time now to figure out how to add the boxes. The operator gets too flustered and makes mistakes when it gets complicated. He JUST got used to the old controller before it took a dump, so i'd really like to make it like it was. Also, i am pretty fond of the way it was as well. The machine has a vacuum table so the workpiece placement is rather arbitrary and it's nice to just plop a piece of wood on the table, measure from the corner of the spoilboard, and just enter the values on the screen into the 3 boxes. 
I can add the boxes via pyvcp, however i assume that somehow either needs to enter an mdi command or change the .var file? That's where i'm a bit lost. 

Your pyvcp boxes should set a halpin value, say 'value_x' and 'value_y' you could then have another pyvcp button that executes an MDI command like this:

G10 L2 P0 X#<_hal[pyvcp.value_x]> Y#<_hal[pyvcp.value_y]>

[edit]
For more information on reading hal pins from gcode see section 4 here:
linuxcnc.org/docs/2.9/html/gcode/overvie...:overview-parameters

Normal workflow would be to go where you want to start your job and just touch off each axis. 
With my plasma machine I had a laser pointer (offset from the torch) which I pointed to where I wanted to start and press one button that moved the cutting tool to the laser point and set the g54 offsets for X & Y. I also had another button called Zero XY which made the current tool position X0Y0. That sounds more like what you want rather than mucking about with entering coordinates.