Macro Work Coordinate

[firedog]

I am experimenting with shifting my work coordinates for a fixture that has multiple parts on it. This is on a Haas control. I would like to set one when the macine is set up, WC (G54), and use a macro or variable shift to set my other work coordinates. I am using sub programs for all of the machining commands to shorten up the program length. Any suggestions??

Thanks for the help!!

[psychomill]

I'm not sure of the variable numbers on a Haas (a programming book should tell you) but on a Fanuc related control, you can do something like this:

Let's say you have 4 parts, 2 in 'X' and 2 in 'Y', at 4" apart.

O500
G90
#5241=-[#5221+4.0] (G55 X = G54 + 4.0)
#5242=#5222 (G55 Y = G54 Y)
#5243=#5223 (G55 Z = G54 Z)
#5261=#5221 (G56 X = G54 X)
#5262=-[ABS#5222+4.0] (G56 Y = G54 Y + 4.0)
#5263=#5223 (G56 Z = G54 Z)
#5281=-[#5221+4.0] (G57 X = G54 X + 4.0)
#5282=-[ABS#5222+4.0] (G57 Y = G54 Y + 4.0)
#5283=#5223 (G57 Z = G54 Z)
M30

This is provided you've already picked up G54 XYZ.

HTH

[Bent]

You could also temporary shift the WC if you know the distance betwen the parts. Something like this

O0010(TEST)
G90 G40
( T01 DIAM D10.0 ENDMILL)
N1 T01 M06 (ENDMILL USER DEFINED)
T01 G90 M01
(PART NR 1)
M98 P0011
G52 X100.0 Y0.0
(PART NR 2)
M98 P0011
G52 X100.0 Y100.0
(PART NR 3)
M98 P0011
G52 X0.0 Y100.0
(PART NR 4)
M98 P0011
G52 X0 Y0 Z0 (REMEMBER TO SHIFT BACK)
G00 Z100.0 M09
G53 Z0 M5
G53 X-1000. Y0
M30

This program is for a FANUC and in metric( if it matters)

Bent

[miljnor]

seems like alot of work if you already know the distance... why not just type it in???

of course if your making ALOT of parts then i can see it...

[psychomill]

seems like alot of work if you already know the distance... why not just type it in???

My thoughts too.....

Although, with the macro in the program, for repeat set up you'd only have to pick up one offset without someone "fat fingering" the keys.

And I did think of G52, G92,.....

[firedog]

The reason for going this route is for future set-ups. Additionally, we are doing some circular interp moves, so if an adjustment was needed for location, programming the distance wouldn't be the best.
Using a G52 of G92 would add a lot of shift moves to the program, while using a variable means only having to call the appropriate work coordinate.
On the next set-up, the operator will only have to pick up one location, and the rest will fall into place.

Thanks for all the help!!

[miljnor]

I didn't mean to not use the offsets. I meerly ment for 4 offsets i would have just typed them into the offset registers. Although using a macro for future set ups does remove the fumble finger F#$K up. just seamed like alot of code for the amount of fixtured offsets your using.

I ran a job off of a fixture plate with just under 30 fixtures and something like this would have been a huge timesaver..

[deanrach]

Similar to Bent, you can also do as follows (since you already know the locations).

O0010(TEST)
G90 G40
( T01 DIAM D10.0 ENDMILL)
N1 T01 M06 (ENDMILL USER DEFINED)
T01 G90 M01
G54 (PART NR 1)
M98 P0011

G55 (PART NR 2)
M98 P0011

G56 (PART NR 3)
M98 P0011

G57 (PART NR 4)
M98 P0011

G00 Z100.0 M09
M30

G10 is extremely powerful as well ................