Newbie- Multiple set-ups

[RP Designs]

Forgive the ignorance here, I am very new and trying to research as much information as I can. I tried searching and could not find an answer to my questions. I haven't decided on my controller yet (machine is not here yet) so it is more generic. When you are setting up multiple parts for macining, say for instance in three or four vises can you set 3 or 4 different 0,0,0 locations (one for each vise) and then run the program from each location. What I mean is if I set up three vises and want to run the same part in each vise ca I specify three different home locations and run them serially or do I need to run the program, relocate zero's for vise 2 and then re-run the program, etc?
What do you typically do when using a fixture plate? I can certainly build an assembly in cad, export the whole assembly into cam and produce G-code around the whole fixture, but if i am using a generic tool plate is there an easy way to locate the 0,0,0 for a few different parts or is it simpler just to build an assemly in cad and export to cam for g-code?
Thanks for your help with my newbie questions.

[Geof]

The Home position for a VMC is normally when the table is to the full left and forward on its travel and the spindle is raised to its maximum height. These positions are X0,0, Y0.0, Z0.0 and are fixed; i.e. you don't move the home position around.

Normally for machining something a Work Zero, or Work Coordinate is defined at some point on the part. This can be a corner, the center, a hole somewhere and is your choice; you can consider this as the Part Home and it is defined by reference to the machine home.

Normally a machine can have numerous Work Zeroes and these are designated by G54, G55, G56, etc so when you have three vises you define a Work Zero for each one and then run the program using each of the work zeroes in sequence.

For improved efficiency it is better to split a program up and run each tool in each work zero so less time is wasted on tool changes.


When working with a fixture plate simply locate a position on the plate and make it the G54 Work Zero position for that plate; you can think of it as Plate Home. Now the easiest way to locate other Work Zeroes on the plate is to use G52 X, Y, Z (often Z is not needed) where the X and Y values are the plate locations with reference to the G54 position. The G52 command creates 'local work zeroes' and you simply use each tool at each set of X and Y coordinates.

[RP Designs]

Awesome, Geof thanks!

[Joe Engel]

You could also put the tool path into a sub program. Call the tool path, change offsets with the G52, and call the path again...
This way, if editing is needed, you only edit the sub program. Not, each line for each offset. Less chance of errors and quicker to edit.

Generic Ex.
O101(Sub Program)
G98 G73 Z-1.25 R.1 F5.
M99

O100(Main Program)
G0 G90 G54 X0 Y0 S100 M3
G0 H1 Z1.
M98 P101 'Sub Program Call
G52 X4.' Coordinate System Shift From G54, X= 4"
M98 P101
G55 ' Work Offset 2
M98 P101
G28 Z0 H0
M30

So, to change the depth of the peck drilling cylce on all 3 parts, you only change the on line in the sub program.

-Joe