Resetting the Coodinate System

[rweatherly]

I would like to make a sign with a three lines of text using Mach 3. The "text wizard" only produces one line at a time. What I would like to do is to take the G-code for the three lines and paste them to one file.

When the machining for the first line is finished, I would like to move to a new position on the sign, zero out the X & Y, and start the second line, and so on for the third line.

Is there a way to do this with G Code?

Thanks,

Richard

[HuFlungDung]

Yes there is. This would be a good breaking in exercise for you, to learn to use work offsets.

Pick a reference point (called a datum) for the first line of text. The difference between machine home and this datum in terms of the X and Y axis, would be entered into your G54 offset table.

Then, pick a similar reference point wherever you want the second line of text to begin. Again, establish where this reference point is relative to your machine home. The X and Y values go in the G55 offset table.

Likewise, the third line of text's reference point is entered in the G56 offset table.

Then, when machining the first line of text, near the beginning of that operation, you insert a G54 into your gcode, and move to your first reference point.

When completed, then insert a G55 in your gcode and move to the second reference point at the beginning of your second line of text.

And so forth.

Always be mindful that the current work offset is modal, that means it stays in effect until you change it to another one. Most of the time, you would want to work a single part in the G54 work offset. It is standard practise to insert a G54 near the very beginning of every program in the start lines, just to ensure that the proper work offset is being used.

This way, the operator then establishes a habit of looking in the offset tables whenever a new job is set up, to make sure that the G54 is correct.

[rweatherly]

I believe that I understand the offset table. Say I machining two holes and have X=0 Y=0 for G54, and X = 1 Y = 1 for G55. Say after machining the first hole the tool ends up at 0,0. If the next lines are:

G55
G00 X0 Y0

Then does the G00 move the machine to 1,1 where the new 0,0 location is?.

[HuFlungDung]

Yes, it should. It makes it easier to understand if you remember that the value of the numbers used in the offset tables are based from the machine coordinate system, which is known as G53. When you home your machine at startup, the G53 coordinate system is in effect until the first work offset coordinate system is called.