Need 100's of dedicated work offsets

[Scanfab]

I need to tap into the vast knowledge base of the programming guru wizards here...

I produce with my FADALs over 50,000 steel parts on our 4th axis machine per year. 1st phase is in a 4th axis fixture I built to hold 64 parts(16 pcs at 12, 3, 6 , 9 o'clock). 2nd phase is done in 2 EMC's of ours that cut a dovetail on the bottom side with self-made dovetail tools(steel is mine, mitsu 60' inserts). I have programmed the 4th axis 4020 with G54 being the A0 position, G55 being the A90 and G56 being the A270 for a z height of 10 mm's above my vice. Then G57, G58, and G59 for 13mm family of parts and so on. All parts can be made without EVER changing my work offset table.

Trying to do the same with my EMC (2nd phase) setup. Fixture holds two rows of 12 parts across the table, 24 total. Spacing is 36mm's between parts on X-axis. I want to have a programming system where I can have "dedicated positioning" either within the work offset table or beginning of program that has both X and Y info but also Z info(I zero tools off of LED height block gage.) Problem using E1-E48 is I have more different parts and programs than I have E numbers(48 pcs.) I would rather not use G92 in beginning of program because we have to start mid program alot when testing programs. Right now I use G92 to do my 36mm spacing, any better ways(less prone to startup errors not taking G92 off)

Basically every program would need two work zeros, one for each row of 12-and a total of maybe 50 programs.

I know I can write a note in beginning of every program to tell user what G54 and G55 he should write in work offset page, but there has to be a better way!!!!

G10, G52, G92 what is the best way to get hundreds of dedicated work offsets with least amount of trouble, every program has about ten tools and each tool will have to start with first row of twelve parts then go to other row of 12. In other words, every program will have one X offset and two Y offsets.

P.S. Also a way to do slight "global shift in Z" in beginning of program to compensate for thermal growth ect. by a few 0.01mm's would be great!! Newbie users can modify this number to get correct part height without going into calculate off of bigger dedicated numbers.

[Rekd]

With the Fadal you can save the program and/or the work offsets then reload them like a program. Not sure about the EMC, but it might be worth looking into. If your spacing is the same every time you might consider using a G92 work shift.

HTH

[Scanfab]

All of the programs are kept in the EMC memory, no rs232 used while doing setup. Just choose new program and press cycle start is the idea.

Wondering if G52 can be used with multiple work offset zeros(x and y) or what would be the best way?

[Andre' B]

I have done things like this before, not sure if it can be duplicated in EMC.

O1000(MAIN PROGRAM)
.
.
.
G65P9000A1;
G0G90G54X0.000Y0.000
.
.
.
G65P9000A3;
G0G90G54X0.000Y0.000
.
.
M30


O9000(SET WORK OFFSET)
GOTO#1
N1
(G54 STATION)
#5221=-30.2706(X POS.)
#5222=-10.4260(Y POS.)
#5223=-20.0180(Z POS.)
GOTO9999
N2
(G54 STATION)
#5221=-30.2706(X POS.)
#5222=-10.4260(Y POS.)
#5223=-20.0180(Z POS.)
GOTO9999
N3
(G54 STATION)
#5221=-30.2706(X POS.)
#5222=-10.4260(Y POS.)
#5223=-20.0180(Z POS.)
GOTO9999
N...

N9999
M99

[Andre' B]

P.S. Also a way to do slight "global shift in Z" in beginning of program to compensate for thermal growth ect. by a few 0.01mm's would be great!! Newbie users can modify this number to get correct part height without going into calculate off of bigger dedicated numbers.

That could be done like this.

O1000(MAIN PROGRAM)
.
#501=0.005
#501=-0.001
#503=+0.0023
.
.
.
G65P9000A1;
G0G90G54X0.000Y0.000
.
.
.
G65P9000A3;
G0G90G54X0.000Y0.000
.
.
M30


O9000(SET WORK OFFSET)
GOTO#1
N1
(G54 STATION)
#5221=-30.2706+#501(X POS.)
#5222=-10.4260+#502(Y POS.)
#5223=-20.0180+#503(Z POS.)
GOTO9999
N2
(G54 STATION)
#5221=-30.2706+#501(X POS.)
#5222=-10.4260+#502(Y POS.)
#5223=-20.0180+#503(Z POS.)
GOTO9999
N3
(G54 STATION)
#5221=-30.2706+#501(X POS.)
#5222=-10.4260+#502(Y POS.)
#5223=-20.0180+#503(Z POS.)
GOTO9999
N...

N9999
M99

[Scanfab]

Originally Posted by Andre' B That could be done like this. O1000(MAIN PROGRAM) . #501=0.005 #501=-0.001 #503=+0.0023 . . . G65P9000A1; G0G90G54X0.000Y0.000 . . . G65P9000A3; G0G90G54X0.000Y0.000 . . M30 O9000(SET WORK OFFSET) GOTO#1 N1 (G54 STATION) #5221=-30.2706+#501(X POS.) #5222=-10.4260+#502(Y POS.) #5223=-20.0180+#503(Z POS.) GOTO9999 N2 (G54 STATION) #5221=-30.2706+#501(X POS.) #5222=-10.4260+#502(Y POS.) #5223=-20.0180+#503(Z POS.) GOTO9999 N3 (G54 STATION) #5221=-30.2706+#501(X POS.) #5222=-10.4260+#502(Y POS.) #5223=-20.0180+#503(Z POS.) GOTO9999 N... N9999 M99

The "EMC" is the name of a fadal 2016 machine, has no other meaning btw..

I like and understand(I think) the idea here... But I don't think I have a parameter page to insert numbers in the fadal legacy control?

I could use the #501 to do my "global shifts" but where do I put the #5221 ect info?

[Andre' B]

Originally Posted by Scanfab The "EMC" is the name of a fadal 2016 machine, has no other meaning btw.. I like and understand(I think) the idea here... But I don't think I have a parameter page to insert numbers in the fadal legacy control? I could use the #501 to do my "global shifts" but where do I put the #5221 ect info?

I was thinking EMC2 http://www.linuxcnc.org/ the Linux based CNC control software.


The #5200 variables are just were the Fanuc control I was programming stored the G54,G55, etc. offsets. That info should be in the operators/programers manual.
http://books.google.com/books?id=YKv...iables&f=false

You can also use the G10 comand to load the offsets.

[psychomill]

Does Fadal have a "G10" command? If your sets up repeat and your "2nd" operation is only 24 parts, you can write in your offsets within the program so that when the program starts, it updates all the work offsets you need without having to have the operator make sure he punched them all in......

[Rekd]

Originally Posted by psychomill Does Fadal have a "G10" command? If your sets up repeat and your "2nd" operation is only 24 parts, you can write in your offsets within the program so that when the program starts, it updates all the work offsets you need without having to have the operator make sure he punched them all in......

I think it does, and works like a G92. Been a while though, so check the manual to be sure.