Need Help!- G28 to G54

[pointcloud]

I have finally gotten around to installing my home switches, and now have a Question...

If I set my G54 in my controller, and my program reads

g1x12y5z2f50
g28
g54
g1x12y5z2f50

Will this run to xyz then touch off home and return to the offset and basically go back to where it was???

[aa8vs]

The machines I worked with if a G28 was on a line alone, nothing would happen.
if in G90 mode the G28 X0 Y0 Z0 would force the xyz to the zero position first then
to the values setup in Ref1 register. In G91 mode the G28 X0 Y0 Z0 the machine would move incrementally to positions of xyz and then to home. Note the x0y0z0 would be incremental motions of naught. It would just go home.

[pointcloud]

Machine home or part 0,0,0???

[aa8vs]

Generally machine home is setup in REF1 x, y, z
The alternate is setup in REF2 x, y, z [fuzzy on ref2] we never used

WE only used G28 in incremental mode G91 Programs always ran in G90 absolute mode. Using in G90 it was to easy to make a mistake and when the rapid plane is about 4 /6 mm off the part you don't want to mess up

G28 was the t/c position which was also the machine home position

N... [G90] G1 Z220.18 [mm] M9 (Clear part)
N... G91 G28 X0 Y0 Z0 T1300 M19 (preselect stop spindle)
N.. T1300 B... M6
N.. G90 G54 X... Y... Z... S... B... H1 M3 M8
N.. G1 Z.... F.....

If the move had to be squared due to fixture in the way;

N... G91 G28 Z0
N.. G28 X0 Y0
N.. G90 .......

[aa8vs]

O3501 (T709183 95.50 SEMI FINISH BORE)
N10 G21 G0 G90 G94 G80 G40 G49 G17 (B 5-JAN-2004 10:29)
N20 M606 T709183 B45.
N30 G54 M26
N40 G65 P1014 B45.
N50 G0 G43 X0. Y-144.94 Z354.7 B45. S3349 H1 M3 M10 M8 T709192
N60 Z238.45
N70 G1 Z90.3 F3547
N80 Z238.45
N90 G0 Y-33.18
N100 G1 Z90.3 F3547
N110 Z238.45
N120 G0 Y78.58
N130 G1 Z90.3 F3547
N140 Z238.45
N150 G0 Y190.34
N160 G1 Z90.3 F3547
N170 Z238.45
N180 G0 Z354.7
N190 G65 P1014 B135.
N200 G0 X0. Y166.24 Z354.7 B135. M11
N210 Z238.45 M10
N220 G1 Z90.3 F3547
N...
N...
N320 Z238.45
N330 G0 Z358.45 M319
N340 G91 G28 X0. Y0. Z0. M554 M558
N350 G90 M99


Any questions I can go over it with you ... Chuck

[pointcloud]

I want to have several fixtures.. and do one part referance all, then another part in a different fixture... Or since I do not have a tool changer I would like to referance all, STOP, change the tool and start again...

[aa8vs]

We have done both, Using extended offsets G54.1 P1 .. P48 can store the specific zero offsets for each fixture. The G54 offset would be the program zero that is common to all fixtures. A sub program would be used to combine based on Fixture # the zero offsets from the extended table [unique to each fixture] with the program zero G54 offset and provide a custom adjustment for each fixture used. If this seems like what you might consider, I can send you some code to review and adapt for your use.

Chuck